User Manual Fine Turbo v6.2-9

June 28, 2018 | Author: jap_Bello | Category: Computational Fluid Dynamics, Graphical User Interfaces, Navier–Stokes Equations, Icon (Computing), Fluid Dynamics
Share
Report this link


Description

FINEUser Manual ™ Flow Integrated Environment contains: FINETM GUI v6.2 Euranus v5.1 NUMERICAL MECHANICS APPLICATIONS ™ FINE User Manual Version 6.2-d (May 2005) NUMECA International 5, Avenue Franklin Roosevelt 1050 Brussels Belgium Tel: +32 2 647.83.11 Fax: +32 2 647.93.98 Web: http://www.numeca.com NUMERICAL MECHANICS APPLICATIONS Contents CHAPTER 1: Getting Started 1-1 Overview 1-2 Introduction What is CFD? Components Multi-tasking Project Management 1-3 How To Use This Manual Outline Conventions 1-4 First Time Use Basic Installation Expert Graphics Options 1-5 How to start FINE™ Interface 1-6 Required Licenses Standard FINE™ License Additional Licenses CHAPTER 2: User Interface 2-1 Overview 2-2 Project Selection Creating a New Project Opening of an Existing Project Grid Units and Project Configuration 2-3 Main Menu Bar File Menu Mesh Menu Solver Menu Modules Menu 2-4 Icon Bar File Buttons Grid Selection Bar Solver Buttons Module Buttons User Mode 2-5 Computations Button 2-6 Parameters Button 2-7 View Area 2-8 Mesh Information 2-9 Parameters Area 2-10 Graphics Area Viewing Buttons 2-11 File Chooser 2-12 Profile Manager 1-1 1-1 1-1 1-1 1-3 1-3 1-3 1-5 1-5 1-5 1-6 1-6 1-6 1-7 1-8 1-8 1-8 2-1 2-1 2-2 2-2 2-3 2-4 2-4 2-4 2-8 2-9 2-10 2-10 2-10 2-11 2-12 2-12 2-12 2-12 2-13 2-13 2-15 2-15 2-16 2-16 2-19 2-19 FINE™ iii Contents CHAPTER 3: Fluid Model 3-1 Overview 3-2 The Fluid Model in the FINE™ Interface Properties of Fluid Used in the Project List of Fluids Add Fluid Delete Fluid from List Edit Fluid in List Showing Fluid Properties Filters Import Fluids Database Expert Parameters 3-3 Theory Transport Properties Fluid Models CHAPTER 4: Flow Model 4-1 Overview 4-2 Time Configuration The Interface for an Unsteady Computation Expert Parameters for Unsteady Computations Best Practice on Time Accurate Computations Theoretical Aspects for Unsteady Computations 4-3 Mathematical Model Euler Laminar Navier-Stokes Turbulent Navier-Stokes Expert Parameters for Turbulence Modelling Best Practice for Turbulence Modelling Theoretical Aspect of Turbulence Modelling Gravity Forces Low Speed Flow (Preconditioning) 4-4 Characteristic and Reference Values Reynolds Number Related Information Reference Values CHAPTER 5: Rotating Machinery 5-1 Overview 5-2 Rotating Blocks 5-3 Rotor/Stator Interaction in the FINE™ Interface 5-4 How to Set-up a Simulation with Rotor/Stator Interfaces? Mixing Plane Approach Frozen Rotor Domain Scaling Method Phase Lagged Method 5-5 Theoretical Background on Rotor/Stator Interfaces 3-1 3-1 3-2 3-2 3-2 3-3 3-7 3-7 3-8 3-8 3-8 3-8 3-9 3-9 3-10 4-1 4-1 4-2 4-2 4-5 4-6 4-9 4-15 4-15 4-15 4-16 4-16 4-19 4-27 4-41 4-42 4-47 4-47 4-47 5-1 5-1 5-2 5-3 5-5 5-5 5-9 5-11 5-13 5-15 iv FINE™ Contents Introduction Default Mixing Plane Approach Full Non-matching Technique for Mixing Planes Domain Scaling Method CHAPTER 6: Throughflow Model 6-1 Overview 6-2 Throughflow Blocks in the FINE™ Interface Global Parameters Block Dependent Parameters Mesh for Throughflow Blocks Boundary Conditions for Throughflow Blocks Initial Solution for Throughflow Blocks Output for Throughflow Blocks 6-3 File Formats for Throughflow Blocks One-dimensional Throughflow Input File Two-dimensional Throughflow Input File Output File 6-4 Expert Parameters Related to Throughflow Blocks Under-relaxation Process Others. 6-5 Theoretical Background on Throughflow Method The Time Dependent Approach Basic Equations and Assumptions The Tangential Blockage Factor The Blade Force CHAPTER 7: Optional Models 7-1 Overview 7-2 Fluid-Particle Interaction Introduction Fluid-Particle Interaction in the FINE™ Interface Outputs Specific Output of the Fluid-Particle Interaction Model Expert Parameters for Fluid-Particle Interaction Theory References 7-3 Conjugate Heat Transfer Introduction Conjugate Heat Transfer in the FINE™ Interface Theory 7-4 Cooling/Bleed Introduction Cooling/Bleed Model in the FINE™ Interface Expert Parameters Theory Cooling/Bleed Data File: ’.cooling-holes’ 5-15 5-16 5-19 5-21 6-1 6-1 6-2 6-2 6-2 6-6 6-7 6-8 6-8 6-9 6-9 6-11 6-11 6-12 6-12 6-12 6-13 6-13 6-13 6-13 6-14 7-1 7-1 7-1 7-1 7-3 7-6 7-7 7-8 7-9 7-11 7-11 7-11 7-11 7-13 7-15 7-15 7-16 7-31 7-32 7-33 FINE™ v Contents 7-5 Transition Model Introduction Transition Model in the FINE™ Interface Expert Parameters Theory CHAPTER 8: Boundary Conditions 8-1 Overview 8-2 Boundary Conditions in the FINE™ Interface Inlet Condition Outlet Condition Periodic Condition Solid Wall Boundary Condition External Condition (Far-field) 8-3 Expert Parameters for Boundary Conditions Imposing Velocity Angles of Relative Flow Extrapolation of Mass Flow at Inlet Outlet Mass Flow Boundary Condition Torque and Force Calculation Euler or Navier-Stokes Wall for Viscous Flow Pressure Condition at Solid Wall 8-4 Best Practice for Imposing Boundary Conditions Compressible Flows Incompressible or Low Speed Flow Special Parameters (for Turbomachinery) 8-5 Theory on Boundary Conditions Inlet Boundary Conditions Outlet Boundary Conditions Solid Wall Boundary Conditions Far-field Boundary Condition CHAPTER 9: Numerical Model 9-1 Overview 9-2 Numerical Model in FINE™ CFL Number Multigrid parameters Preconditioning Parameters 9-3 Expert Parameters for the Numerical Model Interfaced Expert Parameters Non-interfaced Expert Parameters 9-4 Theory Spatial Discretization Multigrid Strategy Full Multigrid Strategy Time Discretization: Multistage Runge-Kutta Implicit residual smoothing 7-37 7-37 7-38 7-39 7-40 8-1 8-1 8-1 8-4 8-6 8-9 8-10 8-13 8-13 8-13 8-14 8-14 8-14 8-15 8-15 8-15 8-15 8-16 8-16 8-16 8-17 8-22 8-26 8-29 9-1 9-1 9-2 9-2 9-2 9-3 9-3 9-3 9-5 9-7 9-7 9-13 9-16 9-17 9-20 vi FINE™ Contents CHAPTER 10:Initial Solution 10-1 Overview 10-2 Block Dependent Initial Solution How to Define a Block Dependent Initial Solution Examples for the use of Block Dependent Initial Solution 10-3 Initial Solution Defined by Constant Values 10-4 Initial Solution from File General Restart Procedure Restart in Unsteady Computations Expert Parameters for an Initial Solution from File 10-5 Initial Solution for Turbomachinery 10-6 Throughflow-oriented Initial Solution CHAPTER 11:Output 11-1 Overview 11-2 Output in FINE™ Computed Variables Surface Averaged Variables Azimuthal Averaged Variables ANSYS Global Performance Output Plot3D Formatted Output 11-3 Expert Parameters for Output Selection Azimuthal Averaged Variables Global Performance Output 11-4 Theory Computed Variables Surface Averaged Variables Azimuthal Averaged Variables Global Performance Output CHAPTER 12:Blade to Blade Module 12-1 Overview 12-2 Blade-to-Blade in the FINE™ Interface Start New or Open existing Blade-to-Blade Computation Blade-to-Blade Data Boundary Conditions Numerical Model Initial Solution Menu Output Parameters Control Variables Page Launch Blade-to-Blade Flow Analysis 12-3 Expert Parameters 12-4 Theory Mesh Generator Flow Solver 10-1 10-1 10-1 10-2 10-2 10-3 10-4 10-4 10-5 10-5 10-6 10-7 11-1 11-1 11-2 11-2 11-7 11-9 11-10 11-15 11-17 11-18 11-18 11-18 11-20 11-20 11-21 11-21 11-24 12-1 12-1 12-2 12-2 12-3 12-8 12-10 12-10 12-10 12-10 12-11 12-11 12-11 12-11 12-12 FINE™ vii Contents 12-5 File Formats used by Blade-to-Blade Module Input Files Output Files CHAPTER 13:Design 2D Module 13-1 Overview 13-2 Inverse Design in the FINE™ Interface Start New or Open Existing Design 2D Project Creation of Inverse Design Input Files Initial Solution Menu Launch or Restart Inverse Design Calculation Expert Parameters 13-3 Theory 13-4 File Formats used for 2D Inverse Design Input Files Output Files CHAPTER 14:The Task Manager 14-1 Overview 14-2 Getting Started The PVM Daemons Multiple FINE™ Sessions Machine Connection from UNIX/LINUX Platforms Machine Connection from Windows Platforms Remote Copy Features on UNIX/LINUX Remote Copy Features on Windows 14-3 The Task Manager Interface Hosts Definition Tasks Definition 14-4 Parallel Computations Introduction Modules Implemented in the Parallel Version Management of Inter-block Communication How to Run a Parallel Computation Troubleshooting Limitations 14-5 Task Management Using Scripts Launch IGG™ Using Scripts Launch AutoGrid using Scripts Launch EURANUS in Sequential using Scripts Launch EURANUS in Parallel using Scripts Launch CFView™ Using Scripts 14-6 Limitations CHAPTER 15:Computation Steering and Monitoring 15-1 Overview 12-13 12-13 12-15 13-1 13-1 13-2 13-2 13-3 13-5 13-6 13-6 13-7 13-8 13-8 13-9 14-1 14-1 14-1 14-1 14-2 14-2 14-4 14-4 14-4 14-5 14-5 14-6 14-11 14-11 14-12 14-12 14-13 14-14 14-14 14-14 14-15 14-15 14-16 14-17 14-21 14-22 15-1 15-1 viii FINE™ Contents 15-2 Control Variables 15-3 Convergence History Steering Files Selection and Curves Export Available Quantities Selection New Quantity Parameters Definition Quantity Selection Area Definition of Global Residual The Graphics View 15-4 MonitorTurbo Introduction The Residual File Box Quantities to Display 15-5 Best Practice for Computation Monitoring Introduction Convergence History MonitorTurbo Analysis of Residuals APPENDIX A:Governing Equations A-1 Overview A-2 Reynolds-Averaged Navier-Stokes Equations General Navier-Stokes Equations Time Averaging of Quantities Treatment of Turbulence in the Equations Formulation in Rotating Frame for the Relative Velocity A-3 Formulation in Rotating Frame for the Absolute Velocity APPENDIX B:File Formats B-1 Overview B-2 Files Produced by IGG™ The Identification File: project.igg The Binary File: project.cgns The Geometry File: project.geom The Boundary Condition File: project.bcs B-3 Files Produced by FINE™ The Project File: project.iec The Computation File: project_computationName.run B-4 Files Produced by the Flow Solver EURANUS The cgns file: project_computationName.cgns The mf file: project_computationName.mf The res file: project_computationName.res The log file: project_computationName.log The std file: project_computationName.std The wall file: project_computationName.wall The aqsi file: project_computationName.aqsi The Plot3D files The me.cfv file: project_computationName.me.cfv 15-1 15-2 15-3 15-3 15-4 15-5 15-5 15-6 15-7 15-7 15-9 15-9 15-10 15-10 15-11 15-11 15-12 A-1 A-1 A-1 A-1 A-2 A-2 A-3 A-3 B-1 B-1 B-1 B-2 B-2 B-2 B-2 B-2 B-2 B-3 B-3 B-3 B-4 B-4 B-5 B-5 B-5 B-6 B-6 B-7 FINE™ ix Contents B-5 Files Used as Data Profile Boundary Conditions Data Fluid Properties B-6 Resource Files Boundary Conditions Resource File euranus_bc.def Fluids Database File euranus.flb Units Systems Resource File euranus.uni APPENDIX C:List of Expert Parameters C-1 Overview C-2 List of Integer Expert Parameters C-3 List of Float Expert Parameters APPENDIX D: Characteristics of Water (steam) Tables D-1 Overview D-2 Main Characteristics B-7 B-7 B-9 B-10 B-10 B-10 B-10 C-1 C-1 C-1 C-2 D-1 D-1 D-1 x FINE™ CHAPTER 1: Getting Started 1-1 Overview Welcome to the FINE™ User’s Guide, a presentation of NUMECA’s Flow INtegrated Environment for computations on structured meshes. This chapter presents the basic concepts of FINE™ and shows how to get started with the program by describing: • what is CFD, • what FINE™ does and how it operates, • how to use this guide, • how to start the FINE™ interface. 1-2 1-2.1 Introduction What is CFD? All the mathematical sciences are founded on relations between physical laws and laws of numbers, so that the aim of exact science is to reduce the problems of nature to the determination of quantities by operations with numbers. James Clerk Maxwell, 1856 In the late 1970’s, the use of supercomputers to solve aerodynamic problems began to pay off. One early success was the experimental NASA aircraft called HiMAT, designed to test concepts of high manoeuvrability for the next generation of fighter planes. Wind tunnel tests of a preliminary design for HiMAT showed that it would have unacceptable drag at speeds near the speed of sound; if built that way the plane would be unable to provide any useful data. The cost of redesigning it in further wind tunnel tests would have been around $150,000 and would have unacceptably delayed the project. Instead, the wing was redesigned by a computer at a cost of $60,000. Paul E. Ceruzzi, 1989 Computational Fluid Dynamics (CFD) is commonly accepted as referring to the broad topic encompassing the numerical solution, by computational methods, of the governing equations that describe FINE™ 1-1 Getting Started Introduction fluid flow related conservative equations (for instance involving energy or species concentration). It has grown from a mathematical curiosity few decades ago, to become an essential tool in almost every branch of fluid dynamics, from aerospace propulsion to weather prediction. Key elements of CFD are briefly described below. Please notice these informations have mostly been extracted from the web at http://www.crankfield.ac.uk/sme/cfd/whatiscfd.htm and http:// ltp.larc.nasa.gov/aero/login.htm. The reader is invited to consult the web at www.cfd-online.com for more insight in CFD theory. By 1900, theoretical and mathematical developments in fluid dynamics had not achieved significant progress as quickly as experimental efforts. Although the Navier-Stokes equations describing fluid behaviour had existed for over 75 years before the Wright brothers' first flight, they were simply too complex to solve in their complete form for anything but simplified problems under specific conditions. Even today, theoretical solutions to the Navier-Stokes equations are rare and only suited to specific classes of problems. As a developing science, CFD has received extensive attention throughout the international community since the advent of the digital computer. CFD interests are mainly driven by the desire to model complex physical fluid phenomena, that couldn't be easily or cost effectively simulated with a physical experiment. Computational techniques differ from analytical or theoretical solutions in the sense that they only solve equations at a finite number of points rather than for the entire flow field. Choosing these points may become quite difficult - especially for a complex geometry and may require hundreds of thousands or even million of points. In general, a dense grid with many points will give a solution of great detail, but require more computer memory and time to reach a solution. Since this trade-off in computer resources and solution quality is required, the current trend is often to use a dense grid in areas where the solution may change rapidly such as in the boundary layer or near a shock wave, but use of a coarser grid with fewer computational points in areas where the solution is expected to change more gradually. The selection of grid nodes is the science of grid generation. It is a complex field on its own and has many applications outside CFD, such as in constructing solid models for stress, vibration and heat transfer analysis. There are several different techniques that are commonly used to develop computational grids for CFD. Grid nodes can be arranged either in a regular or irregular pattern. Depending on the pattern selected, the method of generation is referred to as structured or unstructured. Both techniques have their own advantages and disadvantages. Basically, structured methods enable the generation of regular grids, with high quality standards and good control in the distribution of grid nodes in shear and boundary layers. However, they may sometimes be hard to generate for very complex geometries. On the contrary, unstructured methods allow a limited control in the grid quality (and thus in the grid solution) but the grid generation process does usually require limited user resources, even for complex geometries. It is thus important that the user recognizes these so that the best grid can be created for a particular geometry. The quality of the grid is definitely important, since it strongly influences the solution including whether or not a solution can be found at all. FINE™/Turbo and FINE™/Design3D environments developed by NUMECA rely on structured grid methods, based on AutoGrid and IGG™ software tools. NUMECA offer also includes unstructured capabilities, through HEXPRESS™ hexahedral grid generator and FINE™/HEXA environment. More details can be provided upon request. 1-2 FINE™ Introduction Getting Started Usually, about 4 to 5 unknowns are computed at each grid node. This makes methods of presenting CFD results a difficult matter, mainly due to the large number of data to manage. Adequate postprocessing is then required to easily and quickly outline the major characteristics of the flow. This is usually done through surface color techniques and particle paths/ribbons. The latter method is mostly used to depict vortices and complex flow-wall interactions. The user is invited to refer to CFView™ manual for a detailed information on NUMECA offer in that area. 1-2.2 Components The resolution of Computational Fluid Dynamics (CFD) problems involves three main steps: • spatial discretization of the flow domain, • flow computation, • visualization of the results. To perform these steps NUMECA has developed three software systems. The first one, IGG™, is an Interactive Geometry modeller and Grid generation system for multiblock structured grids. The second software system, the flow solver EURANUS, is a state of the art 3D multiblock flow solver able to simulate Euler or Navier-Stokes (laminar or turbulent) flows. The third one, CFView™, is a highly interactive Computational Field Visualization system. These three software systems have been integrated in a unique and user friendly Graphical User Interface (GUI), called FINE™, allowing the achievement of complete simulations of 3D internal and external flows from the grid generation to the visualization, without any file manipulation, through the concept of project. Moreover, multi-tasking capabilities are incorporated, allowing the simultaneous treatment of multiple projects. 1-2.3 Multi-tasking FINE™ has the particularity of integrating the concept of multi-tasking. This means that the user can manage a complete project in FINE™ interface; making the grid using IGG™, running the computation with EURANUS and visualizing the results with CFView™. Furthermore, the user has the possibility to start, stop and control multiple computations. Please note that the flow simulation can be time consuming, therefore the possibility of running computations in background has been implemented. See chapter 13 for more detail on how to manage multiple tasks through the interface or in background. 1-2.4 Project Management To manage complete flow analyses, FINE™ integrates the concept of project. A project involves grid generation, flow computation and visualization tasks. The results of each of these tasks are stored in different files that are automatically created, managed and modified within FINE™: • The grid files: The grid generation process, IGG™, creates files containing the representation of the geometry and the grid related to the project. The definition of the types of boundary conditions is also done during this process. The four files that contain the information about the mesh have the extensions .igg, .geom, .bcs and .cgns. • The project file: The project file is created by FINE™. It has the extension .iec and contains the input parameters needed for the flow computations. • The result files: FINE™ creates a new subdirectory for each computation where it stores the following files: — a file with extension .run containing all computation input parameters used by the solver and by CFView™, FINE™ 1-3 Getting Started Introduction — a .cgns file that contains the solution and is used for restarting the solver, — a .res file used by the Monitor to visualize the residual history (see Chapter 15), — two files used to visualize the convergence history in the Steering with extensions .steering and .steering.binary (see Chapter 15). — two files with extensions .mf and .wall that contain global solution parameters. — two files with extensions .std and .log that contain information on the flow computation process. — a .batch file used to launch the computation in batch (see Chapter 15). • The CFView™ visualization files: In addition to the .run file, the flow solver creates a series of files, which can be read by CFView™. These files have different extensions. For example in case of turbomachinery flow problem, the solver will create a file for the azimuthal averaged results with extension .me.cfv. Through the interface, the user can modify all the information stored in the files associated to the project. When creating a new project a new directory is made, e.g.; \project. In this directory the project file is stored: \project\project.iec and a directory is created called \project\_mesh. In this directory the grid files used for the computations can be stored. It is however also possible to select a grid that is located in another directory. Only one mesh file should be used for all computations in a project. If computations need to be done on another mesh file it is advised to duplicate the project (see section 23.1.4) or to create a new project (see section 2-3.1.1) for those computations. batch FIGURE 1.2.4-1 Example of file management for a FINE™ project 1-4 FINE™ How To Use This Manual Getting Started 1-3 1-3.1 • • • • • • • How To Use This Manual Outline Chapters 1and 2: introduction and description of the interface, Chapters 3 to 13: computation definition, Chapter 14: task management, Chapter 15: monitoring capabilities, Annex A: the Navier-Stokes equations, Annex B: used file formats, Annex C: list of supported non-interfaced expert parameters. This manual consists of five distinct parts: At first time use of FINE™ it is recommended to read this first chapter carefully and certainly section 1-4 to section 1-6. Chapter 2 gives a general overview of the FINE™ interface and the way to manage a project. For every computation the input parameters can be defined as described in the chapters 3 to 13. Chapter 14 gives an overview of how to run computations using the Task Manager or using a script. Chapter 15 finally describes the available tools to monitor the progress on a computation. The expert user finds in chapter 3 to 13 a section describing advanced options that are available in expert user mode. Additionally Annex C provides a list with all supported expert parameters on the page Computation Steering/Control Variables in expert user mode. For each parameter a reference is given to the section in the manual where it is described. The use of non-supported parameters is at own risk and will not guarantee correct results. 1-3.2 • • • • • Conventions Some conventions are used to ease information access throughout this guide: Commands to type in are in italics. Keys to press are in italics and surrounded by <> (e.g.: press <Ctrl>). Names of menu or sub-menu items are in bold. Names of buttons that appear in dialog boxes are in italics. Numbered sentences are steps to follow to complete a task. Sentences that follow a step and are preceded with a dot (•) are substeps; they describe in detail how to accomplish the step. The hand indicates an important note The pair of scissors indicates a keyboard short cut. A light bulb in the margin indicates a section with a description of expert parameters. FINE™ 1-5 Getting Started First Time Use 1-4 1-4.1 First Time Use Basic Installation When using FINE™ for the first time it is important to verify that FINE™ is properly installed according to the installation note. The installation note provided with the installation software should be read carefully and the following points are specifically important: • Hardware and operating system requirements should be verified to see whether the chosen machine is supported. • Installation of FINE™ according to the described procedure in a directory chosen by the user and referenced in the installation note as ‘NUMECA_INSTALLATION_DIRECTORY’. • A license should be requested that allows for the use of FINE™ and the desired component and modules (see section 1-6 for all available licenses). The license should be installed according to the described procedure in the installation note. • Each user willing to use FINE™ or any other NUMECA software must perform a user configuration as described in the installation note. When these points are checked the software can be started as described in the installation note or section 1-5 of this users guide. 1-4.2 Expert Graphics Options a) Graphics Driver The Graphics area of FINE™ interface uses by default an OPENGL driver that takes advantage of the available graphics card. When the activation of OPENGL is causing problems, FINE™ uses an X11 driver (on UNIX) or MSW driver (for Windows) instead. It is possible to explicitly change the driver used by FINE™ in the following ways: On UNIX: in csh, tcsh or bash shell: setenv NI_DRIVER X11 in korn shell: NI_DRIVER=X11 export NI_DRIVER The selection will take effect at the next session. On Windows: • Log in as Administrator. • Launch regedit from the Start/Run menu. • Go to the HKEY_LOCAL_MACHINE/SOFTWARE/NUMECA International/Fine# register. • Modify the DRIVER entry to either OPENGL or MSW. The selection will take effect at the next session. 1-6 FINE™ How to start FINE™ Interface Getting Started b) Background Color The background color of the Graphics area can be changed by setting the environment variable NI_IGG_REVERSEVIDEO on UNIX/LINUX platforms or IGG_REVERSEVIDEO on Windows platforms. Set the variable to ’ON’ to have a black background and set it to ’OFF’ to have a white background. The variable can be manually specified through the following commands: On UNIX: in csh, tcsh or bash shell: setenv NI_IGG_REVERSEVIDEO ON in korn shell: NI_IGG_REVERSEVIDEO=ON export NI_IGG_REVERSEVIDEO The selection will take effect at the next session. On Windows: • Log in as Administrator. • Launch System Properties from the Start/Settings/Control Panel/System menu. • Go in the Environment Variables. • Modify or add the IGG_REVERSEVIDEO entry to either ON or OFF. The selection will take effect at the next session. 1-5 How to start FINE™ Interface In order to run FINE™, the following command should be executed: On UNIX and LINUX platforms type: fine -print <Enter> When multiple versions of FINE™ are installed the installation note should be consulted for advice on how to start FINE™ in a multi-version environment. On Windows click on the FINE™ icon in Start/Programs/NUMECA software/fine#. Alternatively FINE™ can be launched from a dos shell by typing: <NUMECA_INSTALLATION_DIRECTORY>\fine#\bin\fine <Enter> where NUMECA_INSTALLATION_DIRECTORY is the directory indicated in section 1-4.1 and # is the number corresponding to the version to be used. FINE™ 1-7 Getting Started Required Licenses 1-6 1-6.1 Required Licenses Standard FINE™ License The standard license for FINE™ allows for the use of all basic features of FINE™ including: • IGG™ (see separate IGG™ manual), • AutoGrid (see separate AutoGrid manual), • CFView™ (see separate CFView™ manual), • Task Manager (see Chapter 14), • Monitor (see Chapter 15). 1-6.2 Additional Licenses Within FINE™ the following features are available that require a separate license: • parallel computations (see Chapter 14), • treatment of unsteady rotor-stator interfaces (see Chapter 5), • transition (see Chapter 7), • fluid-particle interaction (see Chapter 7), • conjugate heat transfer (see Chapter 7), • steam tables (see Chapter 3), • cooling/bleed flow (see Chapter 7), • throughflow (see Chapter 6), • blade to blade and 2D inverse design (Chapter 12 and Chapter 13). Next to FINE™ other products are available that require a separate license: • FINE™/Design 3D (3D inverse design, see separate user manual). 1-8 FINE™ CHAPTER 2: User Interface 2-1 Overview When launching FINE™ as described in Chapter 1 the interface appears in its default layout as shown in Figure 2.1.0-1. An overview of the complete layout of the FINE™ interface is shown on the next page in Figure 2.1.0-2. In the next sections the items in this interface are described in more detail. Together with the FINE™ interface a Project Selection window is opened, which allows to create a new project or to open an existing project. See section 2-2 for a description of this window. A File Chooser window is available for browsing through the file system and to select a file. More detail on the File Chooser window is given in section 2-11. To define a profile through the FINE™ interface a Profile Manager is included. The Profile Manager is described in more detail in section 2-12. FIGURE 2.1.0-1 Default FINE™ Interface FINE™ 2-1 User Interface Project Selection Computations button (Section 2-5) Main menu bar (Section 2-3) Icon bar (Section 2-4) Parameters button (Section 2-6) View button (Section 2-7) Mesh information (Section 2-8) Parameters area (Section 2-9) Graphics area (Section 2-10) FIGURE 2.1.0-2 Complete overview of the FINE™ interface 2-2 Project Selection When the FINE™ interface is started the Project Selection window is appearing together with the interface. This window allows to create a new project or to open an existing one as described in the next sections. After use of this window it is closed. To open a project or to create a new one without the Project Selection window is also possible using the File menu. 2-2.1 1. Creating a New Project To create a new project when launching the FINE™ interface: click on the Create a New Project... icon. A File Chooser will appear, which allows to select a name and location for the new project (for more detailed information on the File Chooser window see section 2-11). In the Directories text box on UNIX a name can be typed or the browser under the text box may be used to browse to an appropriate location. On Windows, the browser under the Save in text box is used to browse to an appropriate location. Once the location is defined type on UNIX and on Windows a new name in the text box under respectively Files and File name, for example project.iec (it is not strictly necessary to add the extension .iec, FINE™ will automatically create a project file with this extension). Click on OK (on UNIX) or Save (on Windows) to accept the selected name and location of the new project. 2. 3. 4. 2-2 FINE™ Project Selection User Interface 5. A new directory is automatically created with the chosen name as illustrated in Figure 2.3.1-5 indicated by point (1). All the files related to the project are stored in this new directory. The most important of them is the project file with the extension .iec, which contains all the project settings (Figure 2.3.1-5, no. 2). Inside the project directory FINE™ creates automatically a subdirectory "_mesh" (Figure 2.3.1-5, no. 3). A Grid File Selection window (Figure 2.2.1-3) appears to assign a grid to the new project. There are three possibilities: • to open an existing grid click on Open Grid File. A File Chooser allows to browse to the grid file with extension .igg. Select the grid file and press OK to accept the selected mesh. A window appears to define the Grid Units and Project Configuration. Set the parameters in this window as described in section 2-2.3 and click OK to accept. • if the grid to use in the project was not yet created use Create Grid File to start IGG™. Create a mesh in IGG™ or AutoGrid (Modules/AutoGrid) and save the mesh in the directory "_mesh" of the new project. Click on Modules/Fine Turbo to return to the FINE™ project. Select the created mesh with the pull down menu in the icon bar. A window will appear to define the Grid Units and Project Configuration. Set the parameters in this window as described in section 2-2.3 and click OK to accept. • When using the AutoBlade™ or Design 3D Module it is not necessary to select a grid. In that case close the Grid File Selection window and select Modules/AutoBlade or Modules/ Design 3D menu to use these modules. 6. 2.2 3 1.1 2.1 1.2 FIGURE 2.2.1-3 Grid File Selection window. 2-2.2 Opening of an Existing Project To open an existing project the two following possibilities are available in the Project Selection window: • Click on the icon Open an Existing Project... A File Chooser will appear that allows to browse to the location of the existing project. Automatically the filter in the File Chooser is set to display only the files with extension .iec, the default extension for a project file. • Select the project to open in the list of Recent Projects, which contains the five most recently used project files. If a project no longer exists it will be removed from the list when selected. To view the full path of the selected project click on Path... To open the selected project click on Open Selected Project. FINE™ 2-3 User Interface Main Menu Bar 2-2.3 Grid Units and Project Configuration The Grid Units and Project Configuration window shows some properties of the selected mesh when linking the mesh to the project: • Grid Units: the user specifies the grid units when importing a mesh. The user may define a different scale factor to convert the units of the mesh to meters. The scale factor is for instance 0.01 when the grid is in centimetres. • Space Configuration: allows the user to specify whether the mesh is cylindrical or Cartesian and the dimensionality of the mesh. In case the mesh is axisymmetric the axis of symmetry should be defined. FIGURE 2.2.3-4 Grid Units and Project Configuration window. The mesh properties are always accessible after linking the mesh to the project through the menu Mesh/Properties... 2-3 2-3.1 Main Menu Bar File Menu 2-3.1.1 New Project The menu item File/New allows to create a new FINE™ project. When clicking on File/New a File Chooser window appears as described in section 2-11. Browse in the Directory list to the directory in which to create a new project directory (in the example of Figure 2.3.1-5 the directory /fermat was selected). Give a new name for the project in the File list, for example project.iec and click on OK to create the new project. When starting a new project a new directory is automatically created with the chosen name (1). All the files related to the project are stored in this new directory. The most important of them is the project file with the extension .iec, which contains all the project settings (2). Inside the project directory FINE™ creates automatically a subdirectory "_mesh" (3). As all the computations of the project must have the same mesh it is advised to store the mesh in this specially dedicated directory. 2-4 FINE™ Main Menu Bar User Interface Each time the user creates a new computation, a subdirectory is added (4). The output files generated by the flow solver will be written in the subdirectory of the running computation. (1) project directory (2) (3) automatically created _mesh directory (4) computation directory FIGURE 2.3.1-5 Directories managed through FINE™ After the new project is created a Grid File Selection window (Figure 2.2.1-3) appears to assign a grid to the new project. There are two possibilities: • to open an existing grid click on Open Grid File. A File Chooser allows to browse to the grid file with extension .igg. Select the grid file and press OK to accept the selected mesh. A window appears to define the Grid Units and Project Configuration. Set the parameters in this window as described in section 2-2.3 and click OK to accept. • if the grid to use in the project was not yet created use Create Grid File to start IGG™. Create a mesh in IGG™ or AutoGrid (Modules/AutoGrid) and save the mesh in the directory "_mesh" of the new project. Click on Modules/Fine Turbo to return to the FINE™ project. Select the created mesh with the pull down menu in the icon bar. A window will appear to define Grid Units and Project Configuration. Set the parameters in this window as described in section 2-2.3 and click OK to accept. 2-3.1.2 Open Project There are two ways to open an existing project file: a) Using the File/Open Menu Item: 1. 2. 3. Click on File/Open. A File Chooser window appears. Browse through the directory structure to find the project file to open. This file has normally the .iec extension. If this is not the case, the file filter in the input box named `List Files of Type', has to be modified. Select the project file. 4. 5. Click on the file name and press the OK button. The opened project becomes the active project. All subsequent actions will be applied to this project. b) Selecting the File From the List of Files in the File Menu. The File menu lists the names of the five most recent projects that have already been opened. Click on a project name from this menu to open this project. FINE™ 2-5 User Interface Main Menu Bar FINE™ will check the write permission of the project directory and the project file and will issue a warning if the project or directory is read only. In both cases the project can be modified, but the changes will not be saved. Only one project can be active. Opening a second project will save and close the first one. An attempt to open a no longer existing project will remove its name from the list in the File menu. 2-3.1.3 Save Project The File/Save menu item stores the project file (with extension .iec) on disk. The project file is automatically saved when the flow solver is started, when FINE™ is closed, or when another project is opened. 2-3.1.4 Save As Project File/Save As is used to store the active project on disk under different name. A File Chooser opens to specify the new directory and name of the project. When this is done a dialog box asks whether to save all the results files associated with the project. If deactivated, only the project file (with the extension .iec) will be saved in the new location. 2-3.1.5 Save Run Files File/Save Run Files is used to store all the information needed for the flow solver in the .run file of the active computation. This menu is mainly useful when the Task Manager is used (see chapter 14 for a detailed description of the Task Manager). If more than one computation is selected in the Computations list, then all parameters in the Parameters area will be assigned to all selected (active) computations. This may be dangerous if the parameters for the currently opened information page are not the same for all the selected computations. To avoid this it is recommended to select only one computation at a time. The run file is automatically updated (or created if not existing) when starting a computation through the main menu (Solver/Start...). 2-3.1.6 Preferences When clicking on File/Preferences... the Preferences window appears that gives access to some project specific and global settings: a) Project Units In this section the user can change the units system of the project. The units can be changed independently for a selected physical quantity or for all of them at the same time. To change the units for one specific quantity select the quantity in the list (see (1) in Figure 2.3.1-6). Then select the unit under Select New Units (2). To change the units for all physical quantities at the same time use the box Reset Units System To (3). The default system proposed by NUMECA is the standard SI system except for the unit for the rotational speed, which is [RPM]. When the user changes the units, all the numerical values corresponding to the selected physical quantity are multiplied automatically by the appropriate conversion factor. The numerical values 2-6 FINE™ Main Menu Bar User Interface are stored into the project file in the same units as they appear in the interface, but in the .run file, which is used by the flow solver, the numerical values are always stored in SI units. The results can be visualized with the flow visualization system CFView™ in the units specified in FINE™.The change of the units can be done at any stage of the creation of the project. User-defined units can be defined through a text file euranus.uni. Please contact NUMECA support team at [email protected] for more information. (1) (2) (3) FIGURE 2.3.1-6 Project Units in the Preferences Window b) Global Layout Under the Global Layout thumbnail the user may specify project independent preferences for the layout of the interface. More specifically the user may activate or deactivate the balloon help, which gives short explanation of the buttons when the mouse pointer is positioned over them. By default balloon help is activated. Deactivation of the balloon help will only be effective for the current session of FINE™. When FINE™ is closed and launched again the balloon help will always be active by default. 2-3.1.7 Quit Select the File/Quit menu item to quit the FINE™ integrated environment. The active project will be saved automatically. Note that this action will not stop the running calculations. A TaskManager window will remain open for each running computation. Closing the TaskManager window(s) will kill the running calculation(s) after confirmation from the user. 2-3.1.8 Limitations in File Names If the name of an already existing project is specified, this project file will be overridden. All other files and subdirectories will remain the same as before. By default, no IGG™ file is associated with the new project and it is indicated "usr/unknown" in the place of the grid file name. The procedure to link a mesh file to the project is explained in section 24.2. FINE™ 2-7 User Interface Main Menu Bar 2-3.2 Mesh Menu 2-3.2.1 View On/Off This toggle menu is used to visualize the grid in FINE™. It may take few seconds to load the mesh file for the first time. The parameters area will be overlapped by the graphic window, and the small control button on the upper - left corner of the graphic window can be used to resize the graphics area in order to visualize simultaneously the parameters and the mesh (see section 2-10). Once the mesh is opened, the same menu item Mesh/View On/Off will hide it. Note that the mesh will stay in the memory and the following use of the menu will visualize it much faster than the first time. When the mesh is loaded the following items appear in the FINE™ interface: • the View sub-pad (see section 2-7 for more details), • the Mesh Information Area (see section 2-8 for more details), • the Graphics Area will appear in the FINE™ interface (see section 2-10 for more details), • The Viewing buttons will appear on the bottom of the Graphics Area. Their function is described in section 2-10.1). The Graphics Area and the Viewing buttons will disappear when the mesh is hidden (Mesh/View On/Off). All the three tools will disappear when the mesh is unloaded (Mesh/Unload). 2-3.2.2 Tearoff graphics This menu transfers the graphics area and its control buttons into a separate window. Closing this window will display the graphics area back in the main FINE™ window. Currently this feature is only available on UNIX systems. 2-3.2.3 Unload Mesh/Unload clears the mesh from the memory of the computer. 2-3.2.4 Properties Clicking on Mesh/Properties... opens a dialog box that displays global information about the mesh: • Grid Units: the user specifies the grid units when importing a mesh. When importing a mesh the Grid Units and Project Configuration window appears, which allows the user to check the mesh units (see section 2-2.3). The chosen units can be verified and, if necessary, changed. • Space Configuration: allows the user to verify whether the mesh is cylindrical or Cartesian and the dimensionality of the mesh. When importing a mesh the Grid Units and Project Configuration window allow the user to check these properties. Those chosen properties can be verified and, if necessary, changed. • The total number of blocks and the total number of points are automatically detected from the mesh. • For each block: the current (depending on the current grid level) and maximum number of points in each I,J and K directions, and the total number of points are automatically detected from the mesh. 2-8 FINE™ Main Menu Bar User Interface FIGURE 2.3.2-7 Mesh Properties dialog box 2-3.3 Solver Menu This menu gives access to the NUMECA flow solver EURANUS, which is a powerful 3D code dedicated to Navier-Stokes or Euler computations. EURANUS uses the computational parameters and boundary conditions set through FINE™ and can be fully controlled both from FINE™ Solver Menu and from the Task Manager (see chapter 13). In this section, the information is given on how to start, suspend, interrupt and restart the flow solver. All these actions may be simply performed by using the pull down menu appearing when the button Solver of the Menu bar is clicked. 2-3.3.1 Start the Flow Solver To start the flow solver, select the menu item Solver/Start.... It is not recommended to start the flow solver before setting the physical boundary conditions and the computational parameters. Using the Start item to run the flow solver on active computation implies that the result file produced by a previous calculations on that computation will be overwritten with the new result values. It also implies that the initial solution will be created from the values set in the Initial Solution page. 2-3.3.2 Save To save an intermediate solution while the flow solver is running click on Solver/Save.... 2-3.3.3 Stop the Flow Solver There are two different ways to stop the flow solver: • Solver/Suspend... interrupts the flow computation after the next iteration. This means that the flow solver stops the computation at the end of the next finest grid iteration and outputs the current state of the solution (solution file + CFView™ files) exactly as if the computation was finished. This operation may take from few seconds to few minutes depending on the number of grid points in the mesh. Indeed, if the finest grid is not yet reached, the flow solver continues the full multigrid stage and stops only after completion of the first iteration on the finest grid. FINE™ 2-9 User Interface Icon Bar • Solver/Kill... allows to stop immediately the computation for the active project.In this case no output is created and the only solution left is the last one that was output during the run. This may become a dangerous choice if asked during the output of the solution. The output is then ruined and all the computation time is lost. To avoid this, it is better to use Solver/Suspend... or to kill the computation some iterations after the writing operations. 2-3.3.4 Restart the Flow Solver To restart a computation from an existing solution the solver should be started using the Solver/ Start... menu. On the Initial Solution page the initial solution has to be specified from an existing file (’.run’). See Chapter 10 that describes the several available ways to define an initial solution. 2-3.4 Modules Menu Clicking on the menu item Modules shows a pull down menu with the available modules. The first three items are related to geometry and mesh definition: • AutoBlade™ is the parametric blade modeller, • IGG™ is the interactive geometry modeller and grid generator, • AutoGrid is the automated grid generator for turbomachinery. Furthermore two design modules are available: • Design2D is a tool for two-dimensional blade analysis and design. • Design3D is a product for three-dimensional blade analysis and optimization. The Task Manager is accessible with Modules/Task Manager. For more detailed information on the Task Manager consult Chapter 14. To start the flow visualization from FINE™, click on the Modules/CFView button and confirm to start a CFView™ session. Wait until the layout of CFView™ appears on the screen. CFView™ automatically loads the visualization file associated with the active computation. To visualize intermediate results of a computation, wait until the flow solver has written output. For more information about the flow visualization system, please refer to the CFView™ User’s Guide. 2-4 Icon Bar The icon bar contains several buttons that provide a short cut for menu items in the main menu bar. Also the icon bar contains a File Chooser to indicate the mesh linked to the project and a pull down menu to choose between Standard Mode and Expert Mode. 2-4.1 File Buttons The New Project icon is a short cut for the menu item File/New. The four buttons on the left of the icon bar are short cuts for items of the File menu: 2-10 FINE™ Icon Bar User Interface The Open Project icon is a short cut for the menu item File/Open. The Save Project icon is a short cut for the menu item File/Save. The Save RUN Files icon is a short cut for the menu item File/Save Run Files. 2-4.2 Grid Selection Bar By clicking on the open envelope on the right of the bar a File Chooser is opened, which allows to select the grid file (with extension .igg) of the mesh to use for the project. To select a grid not only the grid file with extension .igg needs to be present but all four files (with extensions .igg, .geom, .bcs and .cgns) need to be available in the same directory with the same name for the chosen mesh. If a mesh has already been linked to the current project and another mesh is opened, FINE™ will check the topological data into the project against the data into the mesh file and will open a new dialog box (Figure 2.4.2-8) The dialog box will inform the user that a merge of the topologies has been performed and will also show at which item the first difference was detected. FIGURE 2.4.2-8 Merge Topology Dialog Box The three following possibilities are available: • Merge Mesh Definition will merge the two if needed. For example, if a new block has been added to the mesh, linked with the current project. The existing project parameters have been kept for the old blocks, and the default parameters have been set for the new block. • Open Another Grid File will open a File Chooser allows to browse to the a new grid file with extension .igg. Select the grid file and press OK to accept the selected mesh. Then the dialog box Mesh Merge Information will appear. • Start IGG will load automatically the new mesh into IGG™. FINE™ 2-11 User Interface Computations Button The merge may also occur when opening an existing project, or when switching between IGG™ and FINE™, because the check of the topology is performed each time when a project is read. In case the mesh file is no longer existing, or not accessible, an appropriate warning will pop-up when opening the project. In this case it will not be possible to start the flow solver, so the user needs to locate the mesh by means of the File Chooser button on the right of the Grid Selection bar. Once the grid file selected and its topology checked the Grid Units and Project Configuration window appears. This window allows to check the properties of the mesh and to modify them if necessary. See section 2-2.3 for more detail on this window. 2-4.3 Solver Buttons The Start Flow Solver icon is a short cut for the menu item Solver/Start.... Three buttons allow to start, suspend and kill the active computation: The Suspend Flow Solver icon is a short cut for the menu item Solver/Suspend.... The Kill Flow Solver icon is a short cut for the menu item Solver/Kill.... 2-4.4 Module Buttons The Start IGG icon is a short cut for the menu item Modules/IGG. Two buttons allow to start the pre- and post processor: The Start CFView icon is a short cut for the menu item Modules/CFView. 2-4.5 User Mode By clicking on the arrow at the right the user may select the user mode. For most projects the available parameters in Standard Mode are sufficient. When selecting Expert Mode parameters area included additional parameters. These expert parameters may be useful in some more complex projects. The next chapters contain sections in which the expert parameters are described for the advanced user. 2-5 Computations Button When clicking on the Computations button at the top left of the interface a list of all the computations of the project is shown. The active computation is highlighted and the corresponding parameters are shown in the Parameters area. All the project parameters of the computation can be controlled separately by selecting (from this list) the computation on which all the user modifications are applied. 2-12 FINE™ Parameters Button User Interface When selecting multiple computations, the parameters of the active page in the Parameters area are copied from the first selected computation to all other computations. With the buttons New and Remove computations can be created or removed. When clicking on New the active computation is copied and the new computation has the same name as the original with the prefix new_ as shown in the example below. In this example computation_2 was the active computation at the moment of pressing the button New. A new computation is created called new_computation_2 that has the same project parameters as computation_2. To rename the active computation click on Rename, type the new name and press <Enter>. 2-6 Parameters Button The Parameters button is the second button on the left, below the Computations button. When clicking on this button a directory structure appears allowing the user to go through the available pages of the project definition. The Parameters area shows the parameters corresponding to the selected page in the Parameters list. To see the pages in a directory double click on the name or click on the + sign in front of the name. 2-7 View Area When the mesh is loaded with Mesh/View On/Off, a third button is shown in the list on the left: the View button. This button is used in order to show or hide the View sub-pad. By default the View subpad is opened. It consists of three pages and controls the viewing operations on the geometry and the grid. The two first pages show the created geometry and/or block groups of the mesh and allow to create new groups. This possibility is only useful in FINE™ for visualization purposes (for example, to show only some blocks of the mesh to get a clearer picture in the case of a complex configuration). FINE™ 2-13 User Interface View Area FIGURE 2.7.0-1 The View sub-pad The third page provides visualization commands on the grid. It consists of two rows: a row of buttons and a row of icons. The row of buttons is used to determine the viewing scope, that is the grid scope on which the viewing commands provided by the icons of the second row will apply. There are five modes determining the scope, each one being represented by a button: Segment, Edge, Face, Block, Grid. Only one mode is active at a time and the current mode is highlighted. Simply left-click on a button to select the desired mode. • • • • • : in Segment mode, a viewing operation applies to the active segment only. : in Edge mode, a viewing operation applies to the active edge only. : in Face mode, a viewing operation applies to the active face only. : in Block mode, a viewing operation applies to the active block only. : in Grid mode, a viewing operation applies to all the blocks of the grid. The icons of the second row and their related commands are listed in the following table: Icon Command Toggles vertices. Toggles fixed points. Toggles segment grid points. Toggles edges. Toggles face grid. Toggles shading. 2-14 FINE™ Mesh Information User Interface The display of vertices should be avoided since it allows to modify interactively in the Graphics area the location of the vertices and therefore alter the mesh. The Graphics area is for display purposes only and any modification on the mesh in the Graphics area will not be saved in the mesh files and therefore not used by the flow solver. 2-8 Mesh Information Active block, face, edge and segment indices Number of blocks, faces, edges and segments for the active topology When the mesh is loaded also the Mesh Information Area is shown containing the following information for the selected section of the mesh: FIGURE 2.8.0-1 Mesh Information Area • Active Block, Face, Edge and Segment indices. • Number of grid blocks, active block faces, active face edges, active edge segments. • Block: — Number of active block points. — Number of grid points. — Name of the block. — Number of points in each block direction. • Face: constant direction and the corresponding index. • Edge: constant direction according to the active face and the corresponding index. • Segment: number of points on the segment. 2-9 Parameters Area The Parameters area displays a page containing the parameters related to the selected item of the Parameters list. Depending on the selected User Mode the available expert parameters will be displayed. FINE™ 2-15 User Interface Graphics Area 2-10 Graphics Area The Graphics area shows the mesh of the open project. The Graphics area appears and disappears when clicking on Mesh/View On/Off. When the Graphics area appears it is covering the Parameters area. Use the button on the left boundary of the Graphics area to reduce its size and to display the Parameters area. The View items on the left and the grid icons in the Graphics area can be used to influence the visualization of the mesh. The View items are described in section 2-7 and the icons in the Graphics area are described below. button to resize Graphics area FIGURE 2.10.0-2 Resizing of Graphics Area 2-10.1 Viewing Buttons The Viewing buttons are used to perform viewing manipulations on the active view, such as scrolling, zooming and rotating. The manipulations use the left, middle and right buttons of the mouse in different ways. The sub-sections below describe the function associated with each mouse button for each viewing button. For systems that only accept a mouse with two buttons, the middle mouse button can be emulated for viewing options by holding the <Ctrl> key with the left mouse button. 2-10.1.1 X, Y, and Z Projection Buttons These buttons allow to view the graphics objects on X, Y or Z projection plane. Press the left mouse button to project the view on an X, Y or Z constant plane. If the same button is pressed more than one time, the horizontal axis sense changes at each press. 2-16 FINE™ Graphics Area User Interface 2-10.1.2 Coordinate Axes The coordinate axes button acts as a toggle to display different types of coordinate axes on the active view using the following mouse buttons: • Left: press to turn on/off the display of symbolic coordinate axis at the lower right corner of the view. • Middle: press to turn on/off the display of scaled coordinate axis for the active view. The axis surrounds all objects in the view and may not be visible when the view is zoomed in. • Right: press to turn on/off the display of IJK axis at the origin of the active block (in Block Viewing Scope) or of all the blocks (in Grid Viewing Scope). For more informations about the viewing scope, see section 2-7. 2-10.1.3 Scrolling This button is used to translate the contents of active view within the plane of graphics window in the direction specified by the user. Following functions can be performed with the mouse buttons: • Left: press and drag the left mouse button to indicate the translation direction. The translation is proportional to the mouse displacement. Release the button when finished. The translation magnitude is automatically calculated by measuring the distance between the initial clicked point and the current position of the cursor. • Middle: press and drag the middle mouse button to indicate the translation direction. The translation is continuous in the indicated direction. Release the button when finished. The translation speed is automatically calculated by measuring the distance between the initial clicked point and the current position of the cursor. 2-10.1.4 3D Viewing Button This button allows to perform viewing operations directly in the graphics area. Allowed operations are 3D rotation, scrolling and zooming. After having selected the option, move the mouse to the active view, then: • Press and drag the left mouse button to perform a 3D rotation • Press and drag the middle mouse button to perform a translation • Press and drag the middle mouse button, while holding the <Shift> key, to perform a zoom • To select the centre of rotation, hold the <Shift> key and press the left mouse button on a geometry curve, a vertex or a surface (even if this one is visualized with a wireframe model). The centre of rotation is always located in the centre of the screen. So, when changing it, the model is moved according to its new value. This 3D viewing tool is also accessible with the <F1> key. 2-10.1.5 Rotate About X, Y or Z Axis The rotation buttons are used to rotate graphical objects on the active view around the X, Y or Z axis. The rotations are always performed around the centre of the active view. Following functions can be performed with the mouse buttons: • Left: press and drag the left mouse button to the left or to the right. A clockwise or counterclockwise rotation will be performed, proportional to the mouse displacement. Release the button when finished. • Middle: press and drag the middle mouse button to the left or to the right. A continuous rotation will be performed, clockwise or counter-clockwise. Release the button when finished. FINE™ 2-17 User Interface Graphics Area 2-10.1.6 Zoom In/Out This button is used for zooming operations on the active view. Zooming is always performed around the centre of the view. Following functions can be performed with the mouse buttons: • Left: press and drag the left mouse button to the left or to the right. A zoom in - zoom out will be performed, proportional to the mouse displacement. Release the button when finished. • Middle: press and drag the middle mouse button to the left or to the right. A continuous zoom in - zoom out will be performed. Release the button when finished. 2-10.1.7 Region Zoom This button allows to specify a rectangular area of the active view that will be fitted to the view dimensions. After having selected the button: 1. 2. 3. Move the mouse to the active view. Press and drag the left mouse button to select the rectangular region. Release the button to perform the zoom operation. These operations can be repeated several times to perform more zooming. Press <q> or the right mouse button to quit the option. This tool is also accessible with the <F2> key. 2-10.1.8 Fit Button The fit button is used to fit the content of the view to the view limits without changing the current orientation of the camera (which can be interpreted as the user's eyes). 2-10.1.9 Original Button The original button is used to fit the content of the view and to give a default orientation to the camera. 2-10.1.10Cutting Plane This option displays a movable plane that cuts the geometry and the blocks of the mesh. The plane is symbolically represented by four boundaries and its normal, and is by default semi-transparent. After having selected the button: • Press and drag the left mouse button to rotate the plane • Press and drag the middle mouse button to translate the plane • Press < x >, < y > or < z > to align the plane normal along the X, Y or Z axis • Press <n> to revert the plane normal • Press < t > to toggle the transparency of the plane (to make it semi-transparent or fully transparent). It is highly advised to deactivate the plane transparency when using X11 driver to increase the execution speed. 2-18 FINE™ File Chooser User Interface 2-11 File Chooser For file management (opening and saving of files) FINE™ uses the standard File Chooser window. The layout of the File Chooser depends on the used operating system but a typical layout is shown in Figure 2.11.0-3. The Directories list allows to browse through the available directory structure to the project directory. Then the Files list can be used to select the file name. In the case a file needs to be opened an existing file should be selected in the list of available files. In the case a new file needs to be created the user can type a new file name with the appropriate extension. In the List Files of Type bar the default file type is set by default to list only the files of the required type. For a description of all available file types in FINE™ see section 1-2.4. FIGURE 2.11.0-3 Typical layout of a File Chooser window 2-12 Profile Manager When a law is defined by a profile clicking on the button right next to the pull down menu will invoke a Profile Manager. FIGURE 2.12.0-4 Profile Manager for fluid parameters FINE™ 2-19 User Interface Profile Manager The Profile Manager is used to interactively define and edit profiles for both fluids and boundary conditions parameters. The user simply enters the corresponding coordinates in the two columns on the left. The graph is updated after each coordinate (after each pressing of <Enter> key). The button Import may be used if the profile exists already as a file on the disk. The Export button is used to store the current data in the profile manager as a file (for example to share profiles between different projects and users). The formats of the profile files are explained in Appendix B where all file formats used by FINE™ and EURANUS are detailed. If the mouse cursor is placed over a point in the graph window, this point is highlighted and the corresponding coordinates on the left will be also highlighted, giving the user the possibility to verify the profile. The button OK will store the profile values and return back to the main FINE™ window. 2-20 FINE™ CHAPTER 3: Fluid Model 3-1 1. 2. 3. Overview Every FINE™ project contains a fluid with the corresponding properties. In FINE™ the fluid to use for a computation can be defined by: Using the fluid defined in the project file of which the properties are shown on the fluid selection page (see section 3-2.1), or selecting a fluid from the fluid database included in the release that contains a set of pre-defined fluids (see section 3-2.2), or creating a new fluid (see section 3-2.3). In the next section the interface is described in detail including advice for use of the fluid definition. The theoretical background for the different fluid models is described in section 3-3. FINE™ 3-1 Fluid Model The Fluid Model in the FINE™ Interface 3-2 The Fluid Model in the FINE™ Interface list of pre-defined fluids filters list of properties FIGURE 3.2.0-1 Fluid Selection page 3-2.1 Properties of Fluid Used in the Project Every FINE™ project contains a fluid with the corresponding properties that are displayed in the interface (see Figure 3.2.0-1). When a new project is created the used fluid is a default fluid. When an existing project is opened the used fluid is defined by the properties as defined in the project file ’.iec’. The first listed fluid property is the fluid type. Four fluid types are available: • perfect gas, • real gas, • incompressible gas or liquid, • condensable fluid. For more detail on each of these types see section 3-3. For the first three fluid types the properties can be defined through the interface as described in section 3-2.3. For the use of the condensable fluid contact NUMECA to obtain the appropriate tables to add a condensable fluid to the list of fluids. To modify the properties of the used fluid a fluid may be selected from the list of pre-defined fluids (section 3-2.2) or a new fluid may be defined (where the new fluid is based on the current one, see section 3-2.3 for more detail). 3-2.2 List of Fluids The list of fluids (see Figure 3.2.0-1) contains pre-defined fluids in a database with for each fluid the fluid type and the permissions. 3-2 FINE™ The Fluid Model in the FINE™ Interface Fluid Model Every fluid is associated with the user who created it and can be modified or removed only by its owner (the owner has Read Write Delete permissions). All other users will have Read Only permissions only. The user may select a fluid from the list. The selection will be highlighted and the properties of the selected fluid are displayed in the information box below the fluid list. Those fluid properties will be saved in the project file ’.iec’ as soon as the project is saved. 3-2.3 Add Fluid To add a fluid to the database click on the Add New Fluid... button. A new fluid is then created with the current properties as shown in the list of properties. A wizard will appear allowing the user to modify those properties. On the first page of this wizard the user can enter the name and the type of the new fluid. The name should be entered by moving the mouse to the text box for the Fluid Name and to type the name on the keyboard. By default a name is proposed like new_fluid_1. The fluid type can be entered by selecting the appropriate check boxes. First make a choice for a compressible or incompressible fluid. For a compressible fluid select a perfect gas or a real gas. The fluid type corresponding to the selected checkboxes is shown in the text box for the Fluid Type. To cancel the modifications to the fluid definition and close the wizard click on the Cancel button. Once the fluid name and type are correctly set, click on Next>> to go to the next page of the wizard. On this page the following properties have to be defined: • Specific Heat Law, • Heat Conduction Law, • Viscosity Law, • Density Law (for an incompressible fluid only). The possible values to enter for these laws depend on the selected fluid type as described in the next paragraphs. In the case a law is defined by a constant value, type the value in the corresponding dialog box. In the case a law is defined by a profile, the Profile Manager can be opened by clicking on the button ( ) right next to the pull down menu (see section 3-2.3.6 for more detail). In the case a ) right law is defined by a formula, the Formula Editor can be opened by clicking on the button ( next to the pull down menu (see section 3-2.3.5). Information linked to fluid creation is stored in the fluid database only when closing the FINE™ interface. As a consequence, this information will not be available to other users as long as this operation is not completed. 3-2.3.1 Definition of a Perfect Gas For the definition of a perfect gas the user has to specify: • The specific heat at constant pressure. For a perfect gas only a constant Cp is allowed. • The specific heat ratio (Cp/Cv) characteristic of the fluid. • The heat conductivity which may be constant, defined by a polynome in temperature or specified through a constant Prandtl number. FINE™ 3-3 Fluid Model The Fluid Model in the FINE™ Interface • The viscosity law which may be constant, temperature dependent or specified by the Sutherland law. In case the viscosity depends on the temperature the user can specify the law through a polynome or as a profile through the Profile Manager. Furthermore, when the viscosity law is defined by the Sutherland law, the Sutherland parameters are accessible by clicking on the button ( ) right next to the pull down menu. The user can select a law for the dependence of the laminar viscosity in function of the static temperature. The default is the Sutherland’s law that imposes a temperature dependence of the dynamic viscosity. The viscosity may also be maintained constant. 3-2.3.2 Definition of a Real Gas A real gas is defined by laws for the dependence of Cp and/or γ with the temperature. The user can either define a profile, using the Profile Manager, or impose a polynomial approximation using the Formula Editor. In this last case, the polynomes take the following form: Cp ( T ) = A0 T γ ( T )= B0T –3 –3 + A1 T –2 –2 + A2T –1 –1 + A 3 + A 4 T + A5 T + A 6 T 1 2 3 1 2 3 , (3-1) + B1 T + B2 T + B 3 + B4 T + B 5 T + B6 T , (3-2) where the coefficients A0, A1, A 2, A 3, A 4, A5, A6, B 0, B 1, B 2, B 3, B4, B5 and B 6 are chosen by the user and set in the dialog box for Cp and γ respectively. In the definition of real gas properties, lower and upper bounds of temperature variations [Tmin-Tmax] allowed in the domain must be provided. Depending on the local temperature during the iterative process, the physical properties will then be able to vary according to the laws defined in the fluid database. Note that it is necessary to cover the whole temperature range occurring in the system otherwise some inaccuracy in the results might be introduced. In addition, the local temperature may not fit at some occasion in the prescribed range; this is especially true during the transient. If so, as indicated by the formula editor (section 3-2.3.5), the physical properties are kept constant, at a value that corresponds to the lower/upper bound allowed by the range. For the default definition of a real gas, involving a compressibility factor, the user has to specify: • The specific heat at constant pressure characteristic and the specific heat ratio (γ=Cp/Cv) of the fluid, that can be dependent on the temperature through a polynome or a profile. In both cases, the user has to specify the temperature range over which the specific heat is defined. For alternative modelling methods for a real gas see section 3-2.9 and section 3-3.2.2. • The heat conductivity which is constant, defined by a polynome or profile in temperature or specified through a constant Prandtl number. • The viscosity law which may be constant, dependent on temperature or specified by the Sutherland law. In case the viscosity depends on the temperature the user can specify the law through a polynome or as profile. Furthermore, when the viscosity law is defined by the Sutherland law, the Sutherland parameters are accessible by clicking on the button ( down menu. ) right next to the pull Compared to a perfect gas computation (Cp and γ constant), the real gas option results in an increase of about 25% of the CPU time. Real gas calculations are usually robust enough to avoid any use of preliminary run with average physical properties. However, convergence difficulties may arise in the transient (say the first 100-200 iterations) if either the temperature range allowed is too large or if the properties are expected to vary very significantly in the temperature range allowed. At these occasions, it is often useful to run an equivalent perfect gas, with average proper- 3-4 FINE™ The Fluid Model in the FINE™ Interface Fluid Model ties, in order to remove any temperature dependency and ease the convergence process in the transient. 3-2.3.3 Definition of a Liquid For the definition of a liquid two models are available: • a ’pure’ liquid with constant density, • a barotropic liquid for which the density varies with pressure. Depending on the type of liquid the user has to specify: • The specific heat at constant pressure. For liquids only a constant Cp is allowed. • The heat conductivity which may be constant, defined by a polynome in temperature or specified through a constant Prandtl number. • The viscosity law which may be constant or depend on temperature. In case the viscosity depends on the temperature the user can specify the law through a polynome or as a profile through the Profile Manager. • The density law can be pressure dependent (using a polynomial law or as a profile through the Profile Manager) or follow Boussinesq law. In this latter case the density is constant and the Boussinesq coefficients are taken into account only if the button Gravity Forces (Flow Model page) is activated. These coefficients are used in source terms of the density equation in order to modelize the gravitational effect (i.e. natural convection) although the density is assumed to be strictly constant. For liquids, the reference temperature and pressure must lie in the expected range of the static temperature and pressure of the flow field. The reference pressure and temperature are defined on the Flow Model page (Eq. 4-85). 3-2.3.4 Definition of a Condensable Gas The aim of the Condensable Fluid module is the modelling of the real thermodynamic properties of the fluid by means of interpolation of the variables from dedicated tables. The module can be used for a single-phase fluid whose properties are too complex to be treated with a perfect or real gas model. It can also be used in order to treat thermodynamic conditions that are close to the saturation line. Note that the model can be used on the liquid or on the vapour side of the saturation curve. In case the thermodynamic state lies inside the two-phase region a homogeneous equilibrium two-phase mixture of vapour and liquid is considered. The hypothesis of an equilibrium mixture is however not valid if the dryness (wetness) fraction exceeds 20%. The module can not be used above these fractions, as it completely ignores evaporation-condensation phenomena. The approach that has been adopted in EURANUS consists of using a series of thermodynamic tables, one table being required each time a thermodynamic variable must be deduced from two other ones. This implies the creation of many tables as input, but presents the advantage that no iterative inversion of the tables is done in the solver, with as a consequence a very small additional CPU time. The thermodynamic tables are provided by NUMECA, upon request. The tables corresponding to water steam have been generated on basis of literature. NUMECA has also developed a tool for the generation of the thermodynamic tables on basis of equations presented in the literature. In order to use a condensable gas as fluid model, the user has to copy the provided tables in a userdefined subdirectory called /tables_username/ in /NUMECA_INSTALLATION_DIRECTORY/ COMMON/steam_tables on UNIX or in /NUMECA_INSTALLATION_DIRECTORY/bin/ FINE™ 3-5 Fluid Model The Fluid Model in the FINE™ Interface steam_tables/ on Windows before launching FINE™. When the subdirectory is created, the condensable gas is recognized by FINE™ and the fluid will appear in the list with respectively Fluid Name and Fluid Type as "_name" and Condensable Fluid. 3-2.3.5 Formula Editor When a law is defined by a formula clicking on the button right next to the pull down menu will invoke a formula editor. When a law is defined by a formula clicking on the button right next to the pull down menu will invoke the Formula Editor. FIGURE 3.2.3-2 The Formula Editor for polynomials in the fluid properties The Formula Editor is used to define polynomial values for the fluid properties. The user has to define the seven coefficients of the polynomial according to the displayed formula on the top, and also the lower and upper limits of the range, in which the polynomial function is defined. Press <Enter> after each entry. The constant values equal to the minimal and maximal values will be considered outside of this range (as shown in the graph). If a fluid with "Read Only" permissions contains formulas they may be visualized by means of the Show Fluid Properties... button that opens the Formula Editor window, but they can not be modified - a message will warn the user that the selected fluid can not be modified. 3-2.3.6 Profile Manager When a law is defined by a profile clicking on the button right next to the pull down menu will invoke a Profile Manager. The Profile Manager is used to interactively define and edit profiles for both fluids and boundary conditions parameters. The user simply enters the corresponding coordinates in the two columns on the left. The graph is updated after each coordinate (after each pressing of <Enter> key). The button Import may be used if the profile exists already as file on the disk. The Export button is used to store the current data in the profile manager as a file (for example to share profiles between different projects and users). The formats of the profile files are explained in detail in Appendix B. 3-6 FINE™ The Fluid Model in the FINE™ Interface Fluid Model FIGURE 3.2.3-3 Profile Manager for fluid parameters If the mouse cursor is placed over a point in the graph window, this point is highlighted and the corresponding coordinates on the left will be also highlighted, giving the user the possibility to verify the profile. The button OK will store the profile values into the fluid definition. If a fluid with "Read Only" permissions contains profiles they may be visualized by means of the Show Fluid Properties... button that opens the Profile Manager window, but they can not be modified - a message will warn the user that the selected fluid can not be modified. 3-2.4 Delete Fluid from List When the user has the permission to delete a fluid the button Delete Fluid... allows to remove the selected fluid from the list of fluids. Information linked to fluid removal is stored in the fluid database only when closing the FINE™ interface. As a consequence, this information will not be available to other users as far as this operation is not completed. A message will however warn users that the fluid properties have been modified (up to removal in the present situation) by the owner. 3-2.5 Edit Fluid in List When the user has the permission to write for a fluid, the properties of the selected fluid can be modified by clicking on Edit Fluid.... A wizard will appear allowing to modify the name, the type and the laws defining the selected fluid. The two pages of this wizard and the laws to define are described in detail in section 3-2.3. Information linked to fluid edition is stored in the fluid database only when closing the FINE™ interface. As a consequence, this information will not be available to other users as far as this operation is not completed. A message will however warn users that the fluid properties have been modified by the owner. FINE™ 3-7 Fluid Model The Fluid Model in the FINE™ Interface 3-2.6 Showing Fluid Properties When the user does not have the write permission (Read Only) for a fluid the Show Fluid Properties... button opens the wizard with the properties of the fluid. In this case it is not possible to modify any of the properties in the wizard but the user has access to visualize the fluid properties including the defined profiles and formulae. 3-2.7 Filters On the Fluid Model page two filters are available to display only a limited amount of fluids in the list of fluids. Select the owner(s) and fluid type(s) to display from the pull down menus to limit the list of fluids. Please notice that under Windows™ the fluid database is not owner-oriented. The database is stored locally and user defined fluids is accessible with full permissions to all Windows™ users. 3-2.8 Import Fluids Database When the user has is own fluid database, the Import Fluids Database... enables to load a user defined database through a File Chooser window to select the ’.flb’ file containing the properties of all the fluids. When loading an existing project and opening the Fluid Model page, please notice that FINE™ is automatically checking if the fluid is existing or not in the fluid database. If the fluid name is existing but the properties are different, a comparison window will invite the user to select the fluid to use (the default fluid in the database or the fluid defined in the project). 3-2.9 Expert Parameters A list of the expert parameters which can be used in the definition of the fluid type follows hereafter. It is only a summary to know directly the expert parameters related to the definition of a fluid. More details about these expert parameters are given in section 3-3. All expert parameters related to fluid definition are available in Expert Mode on the Control Variables page. For these expert parameters the default values are appropriate ones that only have to be changed in case the user has specific wishes concerning the fluid modelling. PRT: Allows to define the turbulent Prandtl number. For the real gas (thermally perfect gas): IRGCON: defines how the real gas is modelled (default IRGCON = 0) = 0: a compressibility factor is used: two laws have to be entered to define the dependence of Cp and γ with the temperature. = 1: constant r model, γ is calculated from r and Cp. The dependence of Cp with temperature needs to be entered. RGCST: value of the gas constant r used with IRGCON equal to 1 (default RGCST = 287) 3-8 FINE™ Theory Fluid Model For condensable fluid: IHXINL = 0 (default), = 1: activation of special inlet boundary condition. 3-3 3-3.1 Theory Transport Properties 3-3.1.1 The Laminar Viscosity In general the kinematic viscosity (in m2/s) is defined in FINE™. The laminar kinematic viscosity may be • constant, • given in terms of a polynomial function of the temperature, • given by a profile for a certain temperature range, • varying according to Sutherland’s law. The dynamic viscosity is then computed within the code by multiplying the kinematic viscosity by the reference density. The Sutherland law is given by: For T ∞ ≥ 120K T µ ( T ) = µ ( 120 ) -------120 ⎝ ⎛ ⎠ ⎞ ⎝ ⎛ T ≤ 120 K (3-3) 0 For T ∞ ≤ 120K T µ ( T ) = µ ∞ ----T∞ ⎝ ⎛ ⎠ ⎞ T ≤ 120 K (3-4) The viscosity µ ∞ in Eq. 3-3 and Eq. 3-4 is the dynamic viscosity specified in the Fluid Model page or is obtained from the kinematic viscosity and the density both specified in the Fluid Model page, while T ∞ and TSUTHE are respectively the reference temperature and the Sutherland temperature specified also in the Fluid Model page. FINE™ ⎠ ⎞ T µ ( T ) = µ ( 120 ) -------120 ⎝ ⎛ 1.5 120 + TSUTHE -------------------------------------T + TSUTHE ⎠ ⎞ 0 µ( T) = µ∞ T ----T∞ 1.5 T ∞ + TSUTHE ----------------------------------T + TSUTHE T ≥ 120 K 0 T ≥ 120 K 0 3-9 Fluid Model Theory 3-3.1.2 The Heat Conductivity The laminar heat conductivity may be • constant, • given in terms of a polynomial function of the temperature, • given by a profile for a certain temperature range, • specified through the Prandtl number. In case the Prandtl number Pr is specified, the laminar thermal conductivity is obtained as: µC p κ = --------Pr (3-5) The turbulent viscosity is calculated iteratively using one of the turbulence models discussed in section 4-3.3. The turbulent conductivity is obtained from the turbulent viscosity and a turbulent Prandtl number whose value can be controlled through the expert parameter PRT (default: 1.0): µt Cp κ t = ---------- . Pr t (3-6) 3-3.2 Fluid Models In this section, details are provided about the different fluid types available in FINE™: • perfect gas, • real gas, • liquid, • condensable fluid. 3-3.2.1 Calorically Perfect Gas The perfect gas law is used as constitutive equation: p = ρrT with r the gas constant for the perfect gas under consideration: R r = ---- = c p – c v , M with R the universal gas constant and M the molecular weight of the perfect gas. γ is the specific heat ratio, C p the specific heat at constant pressure, and C v the specific heat at constant volume with: Cp γ = ----- . Cv (3-9) (3-8) (3-7) When the gas temperature is so low that the vibrational and electronic modes are frozen, the internal energy of the gas will be proportional to the temperature and the specific heats as well as γ are constant. The gas is "calorically perfect". This is the usual assumption of moderate speed aerodynamics. 3-10 FINE™ Theory Fluid Model The relation between r and C p is given by γ–1 r = ---------- C p . γ bles through the following relation: ( ρw ) p = ( γ – 1 ) ρE – -------------- . 2ρ 2 (3-10) The values of γ and C p are user input. The static pressure is obtained from the conservative varia- (3-11) 3-3.2.2 Real Gas For real gases or more precisely thermally perfect gases, C p and γ depend on the temperature T. The corresponding values can be entered either through a polynomial approximation or through a profile. The thermally perfect gas model is based on two equations: • the perfect gas relation, still valid: R p = ρrT = ρ ---- T , M (3-12) • the enthalpy equation: h = C v dT + rT , T0 where T0 is a reference temperature. In practice T0 is set equal to the minimum temperature of the temperature range specified in the Fluid Model page. These two equations lead to: rT = ( C p – C v ) dT . T0 In the case of a real gas with varying specific heats one can notice that it is not possible to respect the 2 above equations with a constant value of r, unless the difference (Cp-Cv) does not vary with temperature. Two solutions are proposed in EURANUS in order to model real gases: • Perfect gas with compressibility factor (expert parameter IRGCON=0) — the equation of state is modified to include a compressibility factor Z: R p = ZρrT = Zρ ---- T M ( C p – C v ) dT T0 Z = ------------------------------------------rT • Constant r model FINE™ ⎠ ⎟ ⎞ ∫ T ⎠ ⎟ ⎞ ∫ T ⎭ ⎬ ⎫ ⎩ ⎨ ⎧ ⎝ ⎜ ⎛ ⎝ ⎜ ⎛ ⎠ ⎟ ⎞ ∫ T p C p dT = e + -- = ρ T0 ∫ T ⎝ ⎜ ⎛ (3-13) (3-14) (3-15) (3-16) 3-11 Fluid Model Theory — the user specifies the gas constant r (expert parameter RGCST). Then Cp is provided and γ calculated as Cp γ = -------------Cp – r (expert parameter IRGCON=1). 3-3.2.3 Incompressible Fluid a) Liquid The density is user input: ρ = Cst . (3-17) This implies a decoupling of the mass and momentum conservation equations from the energy conservation equation, since no term in the mass and momentum equations depends on the temperature. b) Barotropic Liquid The density is a user defined function of the pressure: ρ = f(p) . (3-18) The corresponding values can be entered either through a polynomial approximation or through a profile (see section 3-2.3.5 and section 3-2.3.6). The particularity of the barotropic liquid formulation is that although the density is not constant, a decoupling of the energy equation is still adopted, exactly as in the full incompressible formulation. Modification of the treatment of the energy equation A modification of the treatment of the energy is required in order to account for the density variations. The temperature equation for any type of fluid can be written as: ⎠ ⎞ ⎝ ⎛ ⎠ ⎞ ⎝ ⎠ ⎛ ⎞ V dT ∂p ρc v ----- = – T ----dt ∂T ⎝ ⎛ ∇V + ∇ k∇T + ε v , (3-19) where εv is the viscous dissipation term and V is the specific volume (inverse of density). Since for a barotropic fluid there is a unique relation between the pressure and the density the first term on the right hand side of the above equation vanishes and the temperature for a barotropic fluid becomes: dT ρc v ----- = ∇ k∇T + ε v . dt In addition, since we have from classical thermodynamics that ⎠ ⎟ ⎞ 2 ∂c v ∂ p ------- = T -------2 ∂V ∂T the specific heat at constant volume depends only on the temperature cv=cv(T). Note that we also have as for an incompressible fluid that the specific heats at constant pressure and at constant volume are equal (cv=cp). The modification of the formulation of the energy for a barotropic fluid can be derived from the above relations. Since we have for a barotropic fluid: 3-12 ⎠ ⎞ ⎝ ⎜ ⎛ ⎝ ⎛ (3-20) , V (3-21) FINE™ Theory Fluid Model V The barotropic relation can be integrated from a reference state to obtain finally T p e ( p, T ) = e 0 + T0 ∫ c dT + ∫ ----- ------ dp . ρ ∂p v 2 p0 Compared to an incompressible formulation the energy depends on both pressure and temperature. 3-3.2.4 Condensable Fluid a) Introduction The aim of the Condensable Fluid module is the modelling of the real thermodynamic properties of the fluid by means of interpolation of the variables from dedicated tables. The module can be used for a single-phase fluid whose properties are too complex to be treated with a perfect or real gas model. It can also be used in order to treat thermodynamic conditions that are close to the saturation line. Note that the model can be used on the liquid or on the vapour side of the saturation curve. In case the thermodynamic state lies inside the two-phase region a homogeneous equilibrium two-phase mixture of vapour and liquid is considered. The hypothesis of an equilibrium mixture is however not valid if the dryness (wetness) fraction exceeds 20%. The module can not be used above these fractions, as it completely ignores evaporation-condensation phenomena. For a real fluid the equation of state may be a complicated and usually implicit expression, generating unacceptable computational overhead if the corresponding equations are explicitly introduced in the solver. Similarly when an equilibrium mixture of vapour and droplets (wet steam for instance) is considered as a single fluid, the calculation from the saturation properties of thermodynamic variables must be done iteratively. The approach that has been adopted in EURANUS consists of using a series of thermodynamic tables, one table being required each time a thermodynamic variable must be deduced from two other ones. This implies the creation of many tables as input, but presents the advantage that no iterative inversion of the tables is done in the solver, with as a consequence a very small additional CPU time. This additional time corresponds to the one that is needed by the bilinear (or bicubic) interpolation procedures through the tables. In order to optimize the efficiency of these interpolations the input tables are always built on basis of a Cartesian mesh in the plane of the input variables (V1,V2) (N1 and N2 values for the variables V1 and V2 respectively). b) Thermodynamic Tables Tables are generated based on NUMECA internal tools, based on various sets of well-known equations as described below: • Benedict-Webb-Rubin equation (usually used with refrigerants), • Modified Benedict-Webb-Rubin model (selected equation for hydrogen), • Vander Waals equation. Single tables are generally used, which means that the tables cover both single-phase and two-phase regions, as for instance depicted in the figure 3.3.2-4, showing one of the tables used to model hydrogen. A bilinear interpolation approach is well adapted to these tables, providing an adequate smoothing of the saturation region. Bicubic interpolation techniques have also been implemented and tested. They provide a higher accuracy for a given number of data points but tend to create spu- FINE™ ⎠ ⎟ ⎟ ⎞ ⎠ ⎞ ⎠ ⎞ ∂p de = c v dT + T ----∂T ⎝ ⎝ ⎛ ⎛ – p dV = c v dT – pdV . (3-22) p ∂ρ ⎝ ⎜ ⎜ ⎛ (3-23) 3-13 Fluid Model Theory rious oscillations in the saturation region. These oscillations can be avoided by adopting separated tables covering respectively the single and the two-phase regions, these two tables intersecting along the saturation line. Five categories of tables are used by the solver 1. Basic tables: p(e,ρ) and T(e,ρ) The numerical scheme being based on a formulation of the equations on basis of the energy and the density, the basic tables are used in order to update the pressure and the temperature after each update of the formulation variables. 2. Entropy tables: p(h,s), ρ(h,s), s(h,p), h(s,p) The entropy tables are used at the inlet/outlet boundary conditions, and are required in order to calculate the total (static) thermodynamic conditions from the static (total) ones. 3. The (p,T) tables: e(p,T) and ρ(p,T) These tables are required in order to allow the use of the inlet boundary conditions based on total pressure and temperature. They are also required by the turbomachinery initial solution procedure. ρ [kg/m3] FIGURE 3.3.2-4 Thermodynamic Table: ρ(p,Τ) 4. The viscosity and conductivity tables: µ(e,ρ) and κ(e,ρ) 3-14 FINE™ Theory Fluid Model The viscosity and conductivity can also be interpolated from tables. If these tables are not present the other laws available within the user interface can be used. 5. The saturation table This table contains the liquid and vapour values of all thermodynamic variables along the saturation line. It is only required if the user activates the dryness fraction output and/or if the inlet boundary condition based on total enthalpy and dryness fraction is selected. c) Integration of Thermodynamic Tables in the Solver Provided that all the input tables are present, the full functionality of the basic solver is accessible. All boundary conditions are available, as well as the initial solution procedures. The numerical schemes are not different, making use of the same acceleration techniques (multigrid, local time stepping, residual smoothing) providing robust and fast convergence to steady state. The evaluation of the advective, viscous and artificial dissipation fluxes involves the pressure in the momentum and energy equations and the temperature in the energy equation. For a perfect gas both are easily deduced from the equation of state, the conversion being so rapid that only the pressure and the density are stored and the other variables recalculated from these whenever they are needed. In the condensable fluid module the density, the pressure, the temperature and the energy are stored in order to limit the number of interpolations. Only one interpolation is made in order to deduce the new values of pressure and temperature after the update of the density and the energy. The speed of sound which enters the numerical solution process through the spectral radius in the time step and in the residual smoothing and artificial dissipation coefficients is also required. It can either be interpolated from a table or computed from the partial derivatives of the p(e,ρ) table: ∂p 2 c = ----∂ρ ⎝ ⎛ The Baldwin-Lomax, Spalart-Allmaras and (k,e) turbulence models can be used. The turbulent conductivity calculation is based on the usual relation: µt κ t = ------- c p Prt The specific heat at constant pressure can either be constant (the value being provided in the user interface) or deduced from the specific table. Condensable fluid option is not compatible with the use of cooling/bleed module and/or upwind schemes for space discretization. By default, a set of thermodynamic tables for water (steam) is proposed starting FINE™/ Turbo v6.2-9. More details can be found in Appendix D. The installation of the thermodynamic tables must be performed as described in section 3-2.3.4 d) Specific Output Specific outputs can be created by the condensable fluid module: • enthalpy: static, total absolute and total relative • dryness fraction (0<x<1), and generalised dryness fraction FINE™ ⎠ ⎞ p ∂p - + ---- ----2 e ρ ∂e ⎝ ⎛ ⎠ ⎞ (3-24) ρ (3-25) 3-15 Fluid Model Theory Below is a list of the buttons appearing in the Outputs/Computed Variables page under the thumbnail Thermodynamics when the condensable gas is selected as fluid model. n FIGURE 3.3.2-5 Condensable Gas Outputs e) Selection of the Viscosity, Conductivity, and Specific Heat As mentioned above the viscosity and conductivity can be specified in two-dimensional tables. If it is not the case the other laws can be used (constant, polynomial expression or user profiles). Unfortunately because of the incomplete integration of the condensable fluid module in the user interface the selection of these laws is no longer available as soon as a condensable fluid is chosen. The way to select these laws is the following: 1. 2. 3. 4. create a perfect gas, enter the desired properties for the viscosity and conductivity, save the corresponding computation, change the fluid type by selecting the condensable fluid. The same procedure applies to the specific heat at constant pressure, that is used in order to derive the turbulent conductivity from the turbulent viscosity. 3-16 FINE™ CHAPTER 4: Flow Model 4-1 Overview The Flow Model page, as displayed in Figure 4.1.0-1, can be used in order to specify several characteristics of the flow: • the time configuration to define time dependence of the equations to solve, • the mathematical model to: — choose between viscous and non-viscous flow, — choose between laminar and turbulent flow, — activate gravity, — activate pre-conditioning for low speed flow, • characteristic scales defining the Reynolds number of the flow, • reference values of the temperature and pressure in the flow. This chapter is organised in the following way: • section 4-2 describes the interface, best practice and theoretical background for unsteady computations, • section 4-3 describes the interface, best practice and theoretical background for the definition of the mathematical model and especially the available turbulence models, • section 4-4 provides details on the Reynolds number related information and reference values. FINE™ 4-1 Flow Model Time Configuration FIGURE 4.1.0-1Flow Model page. 4-2 Time Configuration To perform time independent computations it is sufficient to select Steady. In case time dependence needs to be included in the simulation Unsteady should be selected which gives access to additional parameters for unsteady flow simulation. All parameters in the FINE™ interface related to unsteady computations are described in the following section. For more theoretical information on unsteady flow simulation section 4-2.4 should be consulted. 4-2.1 The Interface for an Unsteady Computation When selecting Unsteady time configuration in the Flow Model page the following additional parameters become accessible in the FINE™ interface: a) Rotating Machinery On the Rotating Machinery page, under the Rotor-Stator thumbnail, the domain scaling rotor/stator interaction is activated. Furthermore, the Phase Lagged capability can be activated on the top of the page. When activated, the phase-lagged rotor/stator interaction will be applied. Finally in both cases, the Number of Angular Positions (in one periodicity) is requested in the Computation Steering/Control Variables page instead of the time step. b) Time Dependent Boundary Conditions On the Boundary Conditions page the boundary conditions at inlet and outlet may be defined as a function of time. To define a time dependent boundary condition go to the Boundary Conditions page and change the default (Constant Value) with the pull down menu to: 4-2 FINE™ Time Configuration Flow Model • fct(time) to define a constant value in space but varying in time. Click on the profile data button ( ) to activate the Profile Manager. • fct(space-time) to define a space and time dependent variation of the boundary condition value. In this case a one-dimensional space profile has to be defined. The time profile to impose is a scaling factor that is applied to the space profile. This means that the profile in space is only varying in time with a certain scaling factor. Another way to define an inlet/outlet unsteady boundary condition is to set an absolute rotational speed to the boundary condition by activating Rotating Boundary Condition and specifying the rotational speed in Rotational Speed Unsteady respectively under the INLET and OUTLET thumbnails, and to set the periodicity of the signal entered in FINE™ through the expert parameter NPERBC. It is important to notice that EURANUS allows only one rotation speed (combined with a zero rotation speed). It is important that the inlet/outlet unsteady boundary condition circumferential profile is imposed on a range covering the initial blade passage location and the blade passage location after one period of the signal. Example T 0 θ1 θ2 π θ3 θ4 2π θ v2.2 t0 t0+T The blade channel is initially (t0) located at θ1,θ2 and will after one period of the signal (T) be located at θ3,θ4. Τhe circumferential signal has thus to be imposed from at least θ1 to θ4. When Rotating Boundary Condition is activated, the time step is no longer specified by the physical time step in the FINE™ interface in the Computation Steering/Control Variables page. Instead the time step is imposed by defining the Number Of Angular Positions. c) Phase Lagged When activating Rotating Boundary Condition in the Boundary Conditions page to rotate the reference system of the boundary condition at the inlet and/or outlet, the period of the boundary condition should be compared to the blade passing period. In the case of a single blade row calculation with the period of the varying inlet or outlet boundary conditions different from the blade passing period, the Phase Lagged option should be activated in the Configuration/Rotating Machinery page FINE™ 4-3 Flow Model Time Configuration and the periodicity of the signal entered in FINE™ has to be specified through the expert parameter NPERBC. See section 4-2.3.2 and section 4-2.4.5 for more detailed information on the phase lagged boundary condition. In the case of phase lagged approach, the Number Of Angular Positions is the number of time iterations per full machine rotation. It is important to notice that EURANUS allows only one rotation speed (combined with a zero rotation speed). It is important that the inlet/outlet unsteady boundary condition circumferential profile is imposed on a range covering the initial blade passage location and the blade passage location after one period of the signal (see example on page 4-3). d) Control Variables On the Computation Steering/Control Variables page the following parameters appear when selecting an unsteady time configuration non-turbomachine: • Physical Time Step: in general cases the user specifies the magnitude of the physical time step in seconds. This time step is constant through the whole calculation. In cases of turbomachinery applications where Rotor/Stator interfaces are detected or Rotating Boundary Condition activated, the Number Of Angular Positions is requested instead of the time step as described in section 4-2.2. • Number Of Physical Time Steps: to define the number of time steps to perform. In cases of turbomachinery applications where Rotor/Stator interfaces are detected or Rotating Boundary Condition activated, the Number of Periods can also be specified. • Save Solution Every: allows to save the solution after a constant number of time steps. By default the solution is overwritten in the same output files. In order to keep the successive unsteady solutions, the multiple output (Multiple Files) option has to be activated. • Outputs For Visualization: — Output For Visualization/At end only and Multiple Files: multiple set of output files saved for restart of the unsteady computation and visualization in CFView™ only available at the end of the computation. — Output For Visualization/At end only and One Output File: one set of output files saved for restart of the unsteady computation and visualization in CFView™ only available at the end of the computation. — Output For Visualization/Intermediate and Multiple Files: multiple set of output files saved for restart of the unsteady computation and visualization in CFView™ during the computation. — Output For Visualization/Intermediate and One Output File: one set of output files saved for restart of the unsteady computation and visualization in CFView™ during the computation. • Number Of Steady Iterations: the number of iterations to initialize the unsteady computation. Such initialization is performed with the steady state algorithm, using fixed geometry and mesh as well as constant inlet/outlet boundary conditions. In case this initialization procedure is used the steady state iterations can even be preceeded by a full multigrid process allowing a rapid initialization of the flow (see section 9-4.3). • Save Steady Solution Every: the number of iterations at which the solution of steady initialization is saved By default only one output file is created. For the generation of multiple output files, 4-4 FINE™ Time Configuration Flow Model Multiple Files option has to be selected. e) Second Order Accurate in Time EURANUS performs second order accurate simulations in time. In order to allow to do a second order restart it is necessary to select Multiple Files in the Computation Steering/Control Variables page. When Multiple Files option is selected, in unsteady calculations the ’.cfv’ and ’.cgns’ are saved at the requested time steps and only a part of the ’.cgns’ file is saved for the previous time step. When requesting a restart of an unsteady computation EURANUS will automatically find this second solution file to use. If this file is not found, a first order scheme is used for the first time step. Note that only limited output is saved when selecting Multiple Files with Output For Visualization/At end only and a solution is requested every x time steps, only solution files with extension ’.cgns’ are written every x time steps instead of the full set of solution files. This limited output still allows to restart from this solution (see section 15-2). 4-2.2 Expert Parameters for Unsteady Computations 4-2.2.1 Numerical Model in Expert User Mode On the Numerical Model page, two new parameters appear in the user expert mode when selecting the Dual time stepping technique. They are the control variables for the inner iterations of this last technique. For each physical time step a certain amount of iterations is performed in pseudo time leading to a converged solution independent of the pseudo time (see section 4-2.4 for detailed information). • Convergence criteria of the inner iterations (orders of magnitude of reduction). The inner iterations are stopped if the reduction of the residuals reaches the specified value. • Maximum number of inner iterations: it allows to define the maximum number of iterations to perform for each time step. In general the default of 100 iterations per time step is sufficient. The inner iterations is automatically stopped after this maximum number of iterations if the convergence criteria has not been satisfied. 4-2.2.2 List of Non-interfaced Expert Parameters The following expert parameter related to unsteady computations are accessible on the Control Variables page by selecting the Expert Mode. Please consult section 4-2.4 for more theoretical detail on this parameter. ICYOUT can be equal to 0 or 1 (the default): • ICYOUT=0: name of output changes with suffix _t#iter, • ICYOUT=1(default): each solution is overwritten every cycle (every NOFROT time steps). IFNMB can be equal to 0 (the default) or 1: • IFNMB=0 (default): to keep all PERNM boundaries, • IFNMB=1(default): to transform all PERNM boundaries into periodic full non matching ones. NPERBC can be equal to 1 (the default) or integer value: • NPERBC=1 (default): when the inlet/outlet unsteady boundary condition is a rotating circumferential profile (activating Rotating Boundary Condition and specifying the rotational speed in Rotational Speed Unsteady respectively under the INLET and OUTLET thumbnails) and the boundary condition is entered in the FINE™ interface for the full range [0,2π]. FINE™ 4-5 Flow Model Time Configuration • NPERBC= N: when the inlet/outlet unsteady boundary condition is a rotating circumferential profile (activating Rotating Boundary Condition and specifying the rotational speed in Rotational Speed Unsteady respectively under the INLET and OUTLET thumbnails) and the boundary condition is entered in the FINE™ interface for part of the range [0,2π/N] covering one or multiple periods of the signal. RELPHL =0.5 0.5 if necessary, under-relaxation factor can be applied on Periodic and R/S boundary conditions by reducing the two values of the expert parameter for respectively the periodic and the R/S boundary conditions. NPLOUT =0 (by default) enables to visualize multiple non periodic passage output in CFView™ by loading the corresponding ’.cfv’ file. 4-2.3 Best Practice on Time Accurate Computations To perform time accurate computations, general advice is provided in this section. For advice on how to perform a time accurate turbomachinery calculation including rotor/stator interactions see section 5-4.3. 4-2.3.1 General Project Set-up for Time Accurate Computations 1. 2. 3. Create a new project, Select the fluid to use in the Fluid Model page, Select Unsteady time configuration in the FINE™ Flow Model page and set all the other parameters on this page in the same way as for a steady computations as detailed in section 4-3 and section 4-4. On the Rotating Machinery page set all the parameters (Phase-Lagged option) in the same way as for a steady computation as described in Chapter 5. Set the steady or unsteady boundary conditions. For more detail on time dependent boundary conditions and phase lagged approach see section 4-2.3.2. Concerning the initial solution for unsteady computations there are three possibilities: 4. 5. 6. — to start from a steady solution, — to start from an unsteady solution, — to use constant values, initial solution for turbomachinery or throughflow as an initial guess with or without steady state initialisation. For more detail on these initalisation procedures see section 4-2.3.3. 7. 8. All outputs available in steady mode are also available in unsteady mode (see Chapter 11). On the Control Variables page set: — the physical time step or number of angular position (see section 4-2.3.4) and the number of time steps or periods, — the amount of output files (see section 4-2.3.5), — amount of iterations in steady state initialisation (see section 4-2.3.3). 4-2.3.2 Time Dependent Boundary Conditions Unsteadiness can be generated by means of time varying inlet/outlet boundary conditions. Two different situations can be encountered: 1. 2. The time variation is imposed as an amplitude factor of the space variation, The time variation is imposed by rotating the inlet and/or outlet boundary condition. The absolute rotation speed of the boundary condition(s) is imposed in the Boundary Conditions page. 4-6 FINE™ Time Configuration Flow Model Depending on the periodicity of the boundary condition the phase lagged approach needs to be used: 1. The circumferential distribution of the imposed inlet/outlet conditions has the same period as the blade row. The calculation of such time-dependent flow does not require to activate phase lagged approach. The period of the time varying inlet/outlet boundary condition is different from the blade passing period. The calculation of such time-dependent flow requires to activate the Phase Lagged approach at the top of the Rotating Machinery page. A circumferential profile must be entered in the FINE™ interface for the full range [0,2π] and NPERBC = 1 or for part of the range [0,2π/N] covering one or multiple periods of the signal and NPERBC = N. The profile should be based either on θ, z-θ or r-θ. The profile is automatically rotating at the speed of rotation that is specified through the rotation speed specified in the Boundary Conditions page. It is important that the inlet/outlet unsteady boundary condition circumferential profile is imposed on a range covering the initial blade passage location and the blade passage location after one period of the signal (see example on page 4-3). A profile as a function of r-θ must be structured. The profiles must be given at stations of constant θ for increasing r. Also θ must be increasing going from one station to the next in the file. 2. 4-2.3.3 Initialisation Procedure a) Start From a Steady Solution In most cases it is first required to perform a preliminary steady state computation. The objective might be to ensure that the problem naturally depicts the unsteady behaviour and/or to get an adequate guess solution before going towards time accurate calculations depicting periodic behaviours. The steady state initialisation may be done in a separate computation, performed in steady mode using a time-marching approach based on local time stepping by default. The time accurate calculation is then started using this solution as an initial solution. To set up the time accurate calculation in this case follow the steps 1 to 8 as detailed in section 4-2.3.1. In step 6 select in the Initial Solution page from file and select the solution of the steady computation. In step 8 (section 4-2.3.1) it is possible to select additional steady state initialisation in the Control Variables page (see paragraph c). b) Start From Time Accurate Solution It is possible to start from a previously performed time accurate solution. For general information about starting from an initial solution see section 10-4. In order to allow to do a second order accurate restart it is necessary that Multiple Files option is selected in the Control Variables page in the Output Files parameters. When the option is activated in unsteady calculations the ’.cfv’ and ’.cgns’ are saved at the requested time steps and only a part of the ’.cgns’ file is saved for the previous time step. When requesting a restart of an unsteady computation EURANUS will automatically find this second solution file to use. If this file is not found, a first order scheme is used for the first time step. FINE™ 4-7 Flow Model Time Configuration c) Steady State Initialisation in Unsteady Computation The steady state initialisation is automatically performed before starting the time accurate computation (that means within the same computation). To perform a steady state initialisation in an unsteady computation, the number of iterations has to be entered in Steady Initialization parameters on the Control Variables page. 4-2.3.4 Physical Time Step The physical time step should be entered on the Control Variables page. The time step to choose depends on the expected frequency of the flow phenomena to capture. In general it is recommended to compute at least 10 to 20 time steps per period. When working with turbomachines, using a Number Of Angular Positions of 10 points per blade passage is giving a coarse but reasonable result. To have a more accurate (but more CPU consuming) result choose 20 to 30 points per passage (see chapter 5 for more details). Under the phase lagged option, the Number Of Angular Positions is the amount of stations per 2π and therefore it should be 10 to 20 times the number of blades (see chapter 5 for more details). Example 1: single blade row calculation involving phase-lagged boundary conditions When working with N1 blades turbomachine and a periodic signal at inlet presenting a periodicity of N2 and plotted on [0,2π/N2] range. • Number Of Angular Positions = i x N1 where i is an integer imposed so that (i x N1) is around 30. • Number Of Time Steps = j x (Number Of Angular Positions) where j is the number of full revolution. Usually j is set to 20. • NPERBC = period of the signal (N2) (Number Of Angular Positions)x(NPERBC) corresponds to the number of time steps per full revolution (2π) Example 2: complete row calculation involving sliding boundary conditions When working with N1 blades turbomachine and a periodic signal at inlet presenting a period of N2 and plotted on [0,2π] range. • Number Of Angular Positions = i x N1 x N2 where i is an integer so that (i x N1) and (i x N2) are around 30. • Number Of Time Steps = j x (Number Of Angular Positions) where j is the number of full revolution. Usually j is set to 20. • NPERBC = 1 (Number Of Angular Positions)x(NPERBC) corresponds to the number of time steps per full revolution (2π) 4-2.3.5 Amount of Output By default only one set of output files is created that is periodically overwritten. Activate Multiple Files in the Control Variables page to create a set of output files for each time step that an output will occur (that depends on the Save solution Every entry available in the Control Variables page). ’.cgns’ files will be generated. The files are automatically renamed accordingly to the time step computed using the suffix ’_t#.’ that is thus determining the #th physical time step. The corresponding ’.cfv’ files can be read in CFView™ only if in addition of the Multiple Files the Intermediate has been selected in the Output For Visualization option. 4-8 FINE™ Time Configuration Flow Model Note that the ’.run’ and ’.cgns’ files (without ’_t#.’ suffix) are linked to the initial state of calculation. 4-2.4 Theoretical Aspects for Unsteady Computations Unsteady flow phenomena may arise intrinsically as for example in separated flows, wake flows or may be caused by an external time dependent driving force as for example an oscillating structure. In any case an efficient time-accurate solver has to be employed to obtain time dependent solutions within a reasonable computational time. At present, the most effective approach is called the dual time stepping approach proposed by Jameson, (1991) and it consist in adding to the time dependent Navier-Stokes equations pseudo-time derivative terms. At each physical time step, a steady state problem is solved in a pseudo time and all available acceleration techniques such as multigrid, local time stepping and implicit residual smoothing can be applied. This approach has been used for compressible flow simulations by several authors, Arnone, (1995), Melson et al., (1993), Pierce et al., (1997), Eliasson et al., (1995) and has shown to be an important improvement over the classical global time stepping approach. 4-2.4.1 Standard Time Accurate Solver (Non-preconditioned Formulation) For unsteady flow simulations the Reynolds-Averaged Navier-Stokes equations are expressed as: ∂ ---∂t ∫ ∫ ∫ U dV + ∫ ∫ ∫ ------- dV + ∫ ∫ F ⋅ dS = ∫ ∫ ∫ ST dV , ∂τ V V S V ∂U (4-1) where t is the physical time and τ is pseudo time, U is the solution vector of the conservative variables, V is the volume, F are the conservative fluxes and ST are the source terms. The time discretization of the derivative of the conservative variables with respect to the physical time t is made to meet the desired accuracy in time. Two formulations are available: First order upwind in time: U dV ⎠ ⎟ ⎞ ∂ ---∂t ∫∫∫ V n+1 U V –U V = -------------------------------------------- . ∆t n+1 n+1 n n This first order scheme is used only for the first time step of the unsteady computation except for a restart when the two previous solutions are available (see section 4-2.2). Second order upwind in time: U dV ⎠ ⎟ ⎞ ∂ ---∂t ∫∫∫ V All other terms in Eq. 4-1 are computed at time n+1. The equation is then treated as a modified steady state problem in the pseudo time τ: ∂U ------ V n + 1 + R TA ( U ) = 0 . ∂τ (4-4) Denoting by R the residual corresponding to the steady state problem, the new residual used for time accurate computations RTA is given by: + β 0 U V + β –1 U V β 1 UV R TA ( U ) = R ( U ) + ---------------------------------------------------------------------------------------- . ∆t n+1 n n n–1 n–1 FINE™ ⎝ ⎜ ⎛ ⎝ ⎜ ⎛ (4-2) n+1 1.5U V – 2U V + 0.5U V = ----------------------------------------------------------------------------------------------- . ∆t n+1 n+1 n n n–1 n–1 (4-3) (4-5) 4-9 Flow Model Time Configuration For the second order upwind scheme we have β1=1.5, β0=-2, β-1=0.5 while for the first order scheme we have β1=1, β0=-1, β-1=0. The new residual contains terms that depend only on the solution of previous time steps, all other terms depend on the current solution vector U. When steady state is reached at each physical time step, the left hand side of Eq. 4-5 tends to zero and the time accurate solution is obtained. a) The Time Stepping When integrating equation Eq. 4-4 in the pseudo time τ, it is recommended, Arnone et al. (1995), Pierce and Alonso (1997) to treat the term ( β 1 U n+1 n+1 V ) ⁄ ( ∆t ) implicitly. This is obtained by developing the solution vector U in a Taylor expansion: U l+1 ∂U l = U + ------ ∆τ . ∂τ (4-6) Putting Eq. 4-6 into Eq. 4-5, a modified pseudo time step is introduced: ∆τ ∆τ mod = --------------------- . ∆τ 1 + β 1 ----∆t (4-7) The pseudo time step is modified by an additional term containing the physical time step. This term becomes dominant if the physical time step is significantly smaller than the pseudo time step. This situation does not often happen since the physical time step is taken as large as possible. However, in the far field where mesh dimensions are increased the pseudo time step might reach high values and the contribution of the physical time step will have a stabilizing effect there. The physical time step ∆t is limited by the level of desired accuracy. For periodic flows the time step is usually taken a fraction lying between 1/20-1/40 of the expected period. b) Initial Solution at Each Physical Time Step The simplest way to obtain an initial solution on the next time level is to choose the latest available solution: U initial V n+1 n+1 = U V n n (4-8) Vn+1 being the cell volume evaluated at the next time step. The volume evaluation at each physical time step is only performed for moving meshes. In Jameson (1991) it is suggested to take as initial solution an extrapolated solution from the previous time steps. This is obtained by a Taylor expansion: (U ⋅ V) n+1 ∂(U ⋅ V ) n 2 = ( U ⋅ V ) + ---------------------- ∆t + O ( ∆t ) ∂t n (4-9) This expression leads to the following initial solution: U initial V n+1 n+1 = ( U ⋅ V ) + β1 ( U ⋅ V ) + β0 ( U ⋅ V ) n n n–1 + β –1 ( U ⋅ V ) n–2 . (4-10) In practice however, using this expression does not show any convergence enhancement for the next time step compared to the convergence obtained with Eq. 4-8. Eq. 4-8 is therefore implemented. 4-10 FINE™ Time Configuration Flow Model In the particular case of turbomachinery applications a discretization in time of the blade passing period is performed by the unsteady algorithm, and once one full period has been accomplished by the algorithm, the solution may be initialised using the solution obtained at the same position at the previous rotation. This requires the storage of all the intermediate solutions and the experience has shown that it did not bring significant convergence improvements. The approach has however been implemented in EURANUS, and can be activated by setting the expert parameter PREROT to 1. 4-2.4.2 Density Based Time Accurate Solver and Preconditioning Application of the dual time stepping approach along with low speed preconditioning to variable and constant density flows is presented in Hakimi, (1997). For unsteady flow simulations the preconditioned Reynolds-Averaged Navier-Stokes equations are expressed as: ∂ ---∂t ∫ ∫ ∫ U dV + ∫ ∫ ∫ Γ V V – 1 ∂Q ------ dV + ∂τ ∫ ∫ F ⋅ dS = ∫ ∫ ∫ ST dV , S V (4-11) where t is the physical time and τ is pseudo time, U is the solution vector of the conservative variables, Q is the solution vector of chosen dependent variables, Γ is the preconditioning matrix, V is the volume, F are the conservative fluxes and ST are the source terms. For all fluids we have: Q = ( p g, u, v, w, E g, ρ k, ρε, Y i ) . (4-12) The time discretization of the derivative of the conservative variables with respect to the physical time t is made to meet the desired accuracy in time. The equation is then treated as a modified steady state problem in the pseudo time τ: ∂Q n + 1 ------ V + R TA ( Q ) = 0 , ∂τ with + β0 U V + β–1 U V ) Γ ( β 1 U ( Q )V R TA ( Q ) = R ( Q ) + ---------------------------------------------------------------------------------------------------------- . ∆t n+1 n n n–1 n–1 (4-13) (4-14) The residual RTA in Eq. 4-14 being the preconditioned residual. The new residual contains terms that depend only on the solution of previous time steps, all other terms depend on the current solution vector Q. When steady state is reached at each physical time step, the left hand side tends to zero and the time accurate solution is obtained a) The Time Stepping When integrating Eq. 4-14 in the pseudo time τ, we treat the term ( Γβ 1 UV This is obtained by developing the solution vector U in a Taylor expansion: U l+1 n+1 ) ⁄ ( ∆t ) implicitly. ∂U ∂Q l - = U + ------ ------ ∆τ ∂Q ∂τ (4-15) Putting this relation into equations Eq. 4-13 we obtain the following updating procedure: ∆Q n + 1 ∂U ∆τ ------- V - = – I + Γβ 1 ------ ----∆τ ∂Q ∆t ⎝ ⎛ –1 R (U) TA where I is the identity matrix. The updating procedure has been modified and includes now the time steps ratios, leading to a stabilizing effect. FINE™ ⎠ ⎞ (4-16) 4-11 Flow Model Time Configuration b) Initial Solution at Each Physical Time Step The initial solution on the next time level is the latest available solution: U initial V n+1 n+1 n+1 = U V n+1 n n (4-17) Q initial = Q ( U initial ) Since the dependent variables are Q, these variables have to be computed at the beginning of each physical time step from the conservative variables U. 4-2.4.3 Unsteady Inlet and Outlet Boundary Conditions For a steady state flow problem, to any quantity imposed at the inlet section or at the outlet section corresponds a space distribution on the surface that is uniform, one dimensional (x,y,z,r,θ,z) or two dimensional (xy,xz,yz,rθ,rz,θz). These distributions are written in a file and the code performs a linear interpolation to obtain the desired quantity on the cell face centre of the section. For an unsteady flow problem, the inlet and outlet imposed quantities may vary in time. Two possibilities are available within EURANUS: 1) user specified time function For a fixed system of reference with time dependent boundary conditions, the boundary conditions for a quantity q is given by: q(t)=qo f(t), where qo is a space distribution (uniform, 1D or 2D) and f(t) is a scaling function read from a file: (tn, f(tn)). 2) rotation of the reference system In turbomachinery the relative motion between stator and rotor blades induces an unsteadiness, due to the fact that for instance in a turbine stage the flow conditions that a rotor sees at the inlet are time dependent, whereas these conditions would be fixed for a fixed reference system. If one of the imposed variable along the inlet or the outlet is not uniformly distributed in the tangential direction in the fixed space the inlet/outlet section sees a boundary condition that changes in time. In this case, the space distribution of the imposed quantity being defined by qo (1D or 2D), each cell face centre coordinate is rotated by an angle ∆θ = Ω relative • ∆t at each time step, before performing a new space interpolation. The activation of this procedure along the inlet and/or the outlet is obtained by activating Rotating Boundary Condition in the Boundary Conditions page and specifying the rotational speed in Rotational Speed Unsteady respectively under the INLET and OUTLET thumbnails. The use of a Rotating Boundary Condition imposes a limitation for the specified profiles at the inlet and outlet. Only θ profiles (f(θ), f(r-θ) or f(θ-z)) are allowed and the 2D space profile f(r-θ) must be structured (profile f(r) with the same number of points for different θ) 4-2.4.4 Unsteady Turbomachinery Calculations The relative motion between successive blade rows together with boundary layers, wakes, shocks and tip leakage jets are the major sources of unsteadiness that may affect a turbomachinery flow locally or as it travels through the next rows. All these interactions are strongly coupled, increasing 4-12 FINE™ Time Configuration Flow Model in magnitude as the gap between successive blade rows is decreased, and affecting consequently the performance of the machine. Three types of unsteady simulations are available within EURANUS: • single blade row calculation, periodic boundary conditions: the unsteadiness is created by a time varying inlet or outlet conditions. The circumferential distribution of the imposed inlet/ outlet conditions has the same periodicity as the blade row, which permits to avoid the introduction of any time periodicity in the periodic boundary conditions. The activation of this unsteady mode requires to activate Rotating Boundary Condition in the Boundary Conditions page and specifying the rotational speed in Rotational Speed Unsteady respectively under the INLET and OUTLET thumbnails. • single blade row calculation, phase-lagged periodic boundary conditions: contrary to the previous case, the period of the varying inlet or outlet boundary conditions is different from the blade passing period, and phase-lagged periodic boundary conditions have to be used. To activate this mode, on the Rotating Machinery page, the Phase Lagged capability has to be activated on the top of the page. • multi-stage calculations with unsteady rotor/stator interactions: the domain scaling or phase lagged approach are used within EURANUS. The theoretical background and implementation of this approach are presented in the chapter 5. 4-2.4.5 Phase Lagged Periodicity Boundary Conditions If the inlet and/or outlet boundary conditions present a pitchwise variation with a period different from the blade passing period, a time periodicity has to be introduced along the periodic boundary conditions upstream and downstream of the blade passage, leading to the so-called "phase-lagged" boundary conditions (Fatsis, Pierret and Van den Braembussche, 1995). Ω D C n∆t F Y G E A H B Z X n= NumberOfAngularPositions NOFROT -------------------------------------------------------------------------- = --------------------------NumberOfBlades NBLADES FIGURE 4.2.4-2Illustration of a typical pump with periodicity conditions FINE™ 4-13 Flow Model Time Configuration Let us consider that the computational domain is the one defined by ABCDHGFE as shown in Figure 4.2.4-2, where the solid blade walls correspond to the segments BC and FG. Under the context of phase-lagged boundary conditions, the scalar variables (density, pressure, turbulent viscosity,...)on AB, EF and CD, GH are not equal and the velocity vectors are not related by a simple rotation operator, since the flow is not periodic. Boundary conditions for segments EF and GH: Since, in the absolute system of reference, the actual positions of segments EF and GH correspond respectively to the positions of segments AB and CD n time steps earlier, the variables at time t on segments EF, GH are obtained from those on segments AB, CD at time t- n ∆t: U GH ( t ) = U CD ( t – ( n ⋅ ∆t ) ) , (4-18) Therefore, the flow variables of segments AB and CD need to be stored for the n preceding time steps. Boundary conditions for segments AB and CD: In the absolute system of reference, the actual positions of segments AB and CD correspond respec2π – ϕ tively to the positions of segments EF and GH, -------------------------------------- time steps earlier, with ϕ the angle ( NOFROT – n ) between D and H. The variables at time t on segments AB, CD are obtained from those on segments EF, GH using: 2π – ϕ U CD ( t ) = U GH t – -------------------------------------- ∆t .. ( NOFROT – n ) ⎠ ⎞ ⎝ ⎛ (4-19) 2π – ϕ Therefore, the flow variables of segments EF and GH need to be stored for the -------------------------------------- pre( NOFROT – n ) ceding time steps. Since at the beginning of the computation no solution is available at the previous time steps, standard periodic boundary conditions are applied at the first iteration and then frozen during n time steps for segments EF, GH and (NOFROT-n) time steps for segments AB and CD. Although this procedure is the simplest, it might contribute to slow down the convergence to a periodic state. The current implementation of the phase-lagged boundary conditions only allows matching and full non matching periodic boundary conditions. This option can be used with non matching periodic boundary conditions (PERNMB) if they are automatically transformed into full non matching boundary by setting the expert parameter IFNMB to 1. 4-2.4.6 Choice of the Physical Time Step For a general case the user specifies the amplitude of the physical time step. This time step is constant through the whole calculation. In the case of turbomachinery applications the user defines the time step in another manner, by imposing the Number Of Angular Positions that the unsteady algorithm should solve within one period. The time to accomplish one full rotation being equal to 2π /Ω (Ω the rotation speed of the domain as defined in the Rotating Machinery page), the time step is computed using the relations: 2π ∆t = -------------------------------------------------------------- , Ω ⋅ Nperiods ⋅ NOFROT (4-20) 4-14 FINE™ Mathematical Model Flow Model where Nperiods is the number of blades, or in case of phase lagged option: 2π 1 ∆t = ----- ------------------------ . Ω NOFROT (4-21) 4-2.4.7 References Arnone, A., Liou, M. and Povinelli, L., 1995, " Integration of Navier-Stokes Equations using dual time stepping and multigrid method:, AIAA-Journal, Vol. 33, No. 6, 1995, pp. 985-990. Eliasson, P., and Nordstrom, J., 1995, " The development of an unsteady solver for moving meshes ", FFA/TN 1995-39. Fatsis, A., Pierret, S., Van den Braembussche, R., 1995, " 3D unsteady flow and forces in centrifugal impellers with circumferential distortion of the outlet static pressure ", ASME, 95-GT-33. Hakimi N. (1997) ’Preconditioning methods for time dependent Navier-Stokes equations’, PhD Thesis, Dept of Fluid Mechanics, Vrije Universiteit Brussel. Hirsch Ch. (1990) 'Numerical Computation of Internal and External Flows. Volume 2', John Wiley & Sons. Jameson, A., 1991, "Time dependent calculations using multigrid, with applications to unsteady flows past airfoils and wings", AIAA-Paper 91-1596. Melson, N.D., Sanetrik, M.D., Atkins, H.L., 1993, "Time accurate Navier-Stokes calculations with multigrid acceleration", AIAA paper, pp. 1041-1042. Pierce, N.A., Alonso, J.J., 1997,"A preconditioned implicit multigrid algorithm for parallel computation of unsteady aeroelastic compressible flows:, AIAA-Paper 97-0444. 4-3 4-3.1 Mathematical Model Euler When selecting Euler on the Flow Model page an inviscid calculation will be performed. In such a case all solid walls are considered as Euler walls and the (non-zero) velocity is tangential to the wall. Euler walls do not require any boundary conditions (in contrast to viscous walls). Since the Reynolds number has no meaning for Euler calculations this number is not displayed when Euler flow is selected. See section 8-5.3 for more detailed information on the boundary conditions. 4-3.2 Laminar Navier-Stokes When selecting Laminar Navier-Stokes equations the only effect is on the thermodynamic property of the flow. The viscosity will be the laminar kinematic viscosity and thus does not contain any turbulent component. FINE™ 4-15 Flow Model Mathematical Model 4-3.3 Turbulent Navier-Stokes When selecting Turbulent Navier-Stokes equations, turbulence is taken into account depending on the chosen turbulence model. In FINE™ several turbulence models are available: • Baldwin-Lomax, • Spalart-Allmaras, • Chien (low Reynolds number k-ε), • Extended wall function k-ε, • Launder-Sharma (low Reynolds number k-ε), • Yang-Shih (low Reynolds number k-ε), • Non Linear k-ε (high Reynolds number), • Non Linear k-ε (low Reynolds number). In this section the parameters in the interface related to the turbulence models are described. In section 4-3.6 more theoretical information is provided on those models. For the Baldwin-Lomax model, algebraic formula are used to compute the turbulent data and consequently no additional input are needed in the interface. For the Spalart-Allmaras model and the k-e models, additional equations are solved and consequently suitable initial and boundaries conditions must be defined in the interface. a) Boundary Condition Inlet • Spalart-Allmaras: the value of the turbulent viscosity must be defined. It might be constant or varying in space and time. The user can specify the time or spatial variation through the profile manager. • k-ε models: the values of the turbulent quantities (k and ε) must be defined. They might be constant or vary in space and time. The user can specify the time or spatial variations through the profile manager. b) Initial Condition • Spalart-Allmaras: a constant initial value of the turbulent viscosity is defined through the expert parameter NUTFRE on the Control Variables page under the Expert Mode. • k-ε models: the initial values of the turbulent quantities (k and ε) are specified by the user if constant or turbomachinery initial solutions are chosen. 4-3.4 Expert Parameters for Turbulence Modelling 4-3.4.1 Interfaced Expert Parameters In expert mode additional parameters related to turbulence modelling are available when using the k-ε models with wall functions (extended wall function k-ε and high Reynolds non linear k-ε models). For these turbulence models the wall type can be defined as smooth or rough: • For a smooth solid wall (default) only the von Karman constant and Bo have to be specified (κ and B on page 35 of this chapter). • When selecting a rough solid wall two additional parameters have to be specified: the equivalent roughness height and the zero-displacement plane (k0 and d0, see page 35 of this chapter). 4-16 FINE™ Mathematical Model Flow Model 4-3.4.2 Non-interfaced Expert Parameters All non-interfaced expert parameters related to the turbulence models are accessible on the Control Variables page by selecting the Expert Mode. Please consult section 4-3.6 for more theoretical detail on those parameters. Calculation of the wall distances NREPET: repetition of the computed domain to find the closest wall (default value =1). NSUBM: maximum number of subdomains a domain is split into (default value = 1000). NTUPTC: number of patches whose sub-patches will be searched (default value = 20). RTOL: maximum angle allowed between two normals of a patch (default value = 1.8). When problems occur during the wall distance calculation (wall distance not equal to 0 on the wall), we recommend to rise the value of NTUPTC to 40. Furthermore, RTOL has to be decreased to 0.9 if the wall distance gradient is not smooth. Baldwin-Lomax IATFRZ: multigrid parameter = 0: apply the turbulence model on all grid levels, = 1: freeze turbulence on coarser grids (default), = 2: freeze turbulence on all grids (see ITFRZ and RESFRZ). ITFRZ: freeze the turbulent viscosity field if the fine grid iteration exceeds ITFRZ (default value = 1000000). RESFRZ: freeze the turbulent viscosity field if the fine grid residual is lower than RESFRZ (default value = -12). Spalart-Allmaras MUCLIP: controls the maximum allowable value for the ratio MUT/MU (default value = 5000). NUTFRE: constant to initialize the turbulent viscosity field (default value = 0.0003). k-ε models CMU: constant for the k-ε model in Eq. 4-59 (default value = 0.09). CE1: constant for the k-ε model in Eq. 4-57 (default value = 1.44 automatically set to 1.35 for the Chien k-ε model). CE2: constant for the k-ε model in Eq. 4-57 (default value = 1.92 automatically set to 1.8 for the Chien k-ε model). SIGK: constant for the k-ε model in Eq. 4-56 (default value = 1.). SIGE: constant for the k-ε model in Eq. 4-57 (default value = 1.3). PRT: constant for the k-ε model - the turbulent Prandtl Number (default value = 1.). INEWKE: defines the high Reynolds k-ε model when k-epsilon (Extended Wall Function) is selected: = 0: standard formulation of the wall functions, = 10 (default): mesh independent formulation of the wall functions (extended wall functions). ICOPKE: (= 1) applies the pressure gradient-velocity model to take into account a compressibility correction. It is useful only for high Mach number flows (M>3). The default value is 0. FINE™ 4-17 Flow Model Mathematical Model SIGRO: constant in the k-ε model when ICOPKE =1 in Eq. 4-70 and Eq. 4-72 (default value = 0.5). C3: constant for the k-ε model when ICOPKE = 1 in Eq. 4-72 (default value = 2.). ICODKE: parameter to active the compressible dissipation, = 0 (default): no compressible dissipation, = 1: Sarkar model for compressible dissipation (Eq. 4-75), = 2: Nichols model for compressible dissipation (Eq. 4-77). ALF: constant of Sarkar model for compressible dissipation when ICODKE=1 (default = 0.5). CP1: constant of Nichols model for compressible dissipation when ICODKE=2 (default value = 4.). MAVRES: allows to control the update of k and ε (default = 0.95), > 0: according to the restrictions defined by Eq. 4-78 and Eq. 4-79, = 0: according to the restriction defined by Eq. 4-78, < 0: according to the restriction defined by Eq. 4-80. MAVREM: allows to control the multigrid corrections for k and ε (default = 0.95), > 0: according to the restrictions defined by Eq. 4-78 and Eq. 4-79, = 0: according to the restriction defined by Eq. 4-78, < 0: according to the restriction defined by Eq. 4-80. MUCLIP: controls the maximum allowable value for the ratio MUT/MU (default value = 5000). LTMAX: maximum turbulent length scale (default = 1.E+6), = -1: control of turbulent length scale with automatic clipping. IYAP: (= 1) applies the Yap’s modification to control the turbulent length scale (default value = 0). The value of the expert parameter LTMAX must be the default value. TEDAMP: parameter to improve the robustness of the k-ε models (default value = -1), > 0: a minimum of TEDAMP multiplication factor of the clipping value (EKCLIP) is used for k in the factor 1 ⁄ T in Eq. 4-57, a minimum of TEDAMP multiplication factor of the clipping value (EPCLIP) is used for ε to compute the turbulent viscosity (Eq. 4-59), <= 0 : the minimum values used for k and ε correspond to the expert parameter EPS, GAMMAT: introduces the turbulence time scale in the computation of the local time step to control stability (default value = 10). PRCLIP: sets an upper bound for the ratio between production and dissipation (default value = 50). LIPROD: (= 1) corresponds to a linearization of the production term (default value = 0) when strain rate is large (i.e. impinging flow) and PRCLIP has no more effect on the flow field. EKCLIP: clipping value for the turbulent kinetic energy k (default value = 1.E-5). EPCLIP: clipping value for the turbulent dissipation rate ε (default value = 1E-5). KEGRID: Full multigrid parameter corresponding to the finest grid level on which the BaldwinLomax model is used (default = 2). On the lower grid levels, the k-ε model is used. IUPWTE: (= 1) uses an upwind scheme for the convection of k-ε instead of a centre scheme (default = 1). 4-18 FINE™ Mathematical Model Flow Model IKENC: (= 1) solves the k-ε equations with a non-conservative approach (default = 1). IKELED: (= 1) actives the LED scalar scheme for k-ε instead of the standard central scheme (default = 0). IOPTKE: (= 1) optimized implementation for k-ε (Yang-Shi, Wall function, Lauder Sharma) (default = 1). 4-3.5 Best Practice for Turbulence Modelling 4-3.5.1 Introduction to Turbulence Turbulence can be defined as the appearance of non-deterministic fluctuations of all variables (velocity u", pressure p", etc ...) around mean values. Turbulence is generated above a critical Reynolds number that may range in values from 400 to 2000 depending on the specific case. In 95% of industrial applications the critical Reynolds number falls above that range. That is why it is in general necessary to predict adequately the turbulence effects on the flow-field behaviour. Τo model turbulent flow in a satisfactory way, four steps should be performed: • choosing a turbulence model, • generating an appropriate grid, • defining initial and boundary conditions, • setting expert parameters to procure convergence. 4-3.5.2 First Step: Choosing a Turbulence Model. A turbulence model is chosen based on the specific application. Table 4-1 states the most appropriate turbulence models to use for different types of flows. Although these are the "most appropriate" this does not mean that certain turbulence models cannot be used for the flow types listed, but just that they are "less appropriate". TABLE 4-1 Recommended turbulence models for different flow types Three main kinds of turbulence models exist: • algebraic models (e.g. Baldwin-Lomax), • one-equation models (e.g. Spalart-Allmaras), • two-equation(s) models (k-ε). When quick turbulence calculations are required, for example, in design-cycle analysis, it is recommended that the Baldwin-Lomax model is used due to its high numerical stability and low computational expense. To simulate more precisely the turbulent quantities with also a good rate of convergence the Spalart-Allmaras model should be preferred. FINE™ 4-19 Flow Model Mathematical Model Another model often used in design is "standard" k-ε. This model employs an empirically based logarithmic function to represent the near-wall physics and requires a lower grid resolution in this region as a result. One drawback of this treatment is that the logarithmic function does not apply for separated flows, although the NUMECA extended wall function will still work. If it is expected that a significant amount of separation will have to be predicted, one of the low-Reynolds number turbulence models would be more appropriate. All of the listed turbulence models employ constant turbulent Prandtl numbers which is somewhat of a restriction when performing heat transfer calculations. However, experience has shown quite successful prediction of heat transfer coefficients when using Baldwin-Lomax and Launder-Sharma k-ε. 4-3.5.3 Second Step: Generating an Appropriate Grid. a) Cell Size viscous sub-layer buffer layer log layer Separating flow logarithmic law Data of Lindgren (1965) Note that the sublayer extends up to y+=5 but 10 is an acceptable approximation for design calculations. Note: The variable v* displayed in the figure is uτ. Picture from White, F.M., Viscous Fluid Flow, McGraw Hill, 1991. FIGURE 4.3.5-3Boundary layer profiles When calculating turbulence quantities it is important to place the first grid node off the wall within a certain range (ywall). This can be done for the blade and the endwalls (hub and shroud) independently. When doing computations including viscosity (Navier-Stokes equations) the boundary layer near a solid wall presents high gradients. To properly capture those high gradients in a numerical simulation it is important to have a sufficient amount of grid points inside the boundary layer. When Euler computations are performed no boundary layer exists and therefore the cell size near solid walls is of less importance. 4-20 FINE™ Mathematical Model Flow Model To estimate an appropriate cell size ywall for Navier-Stokes simulations including turbulence, the local Reynolds number based on the wall variable y+is computed. The value of y+ associated with the first node off the wall will be referred to here as y1+: y1+ where uτ is the friction velocity: uτ = τ wall ----------- = ρ 1 -- ( Vref ) 2 C f 2 (4-23) ρu τ y wall = -------------------µ (4-22) Note that the value of ywall depends on the value of y1+. In Figure 4.3.5-3 is represented the evolution of u+ against y+ from the measurements of Lindgren(1965) with: u+= u / u τ Low-Re models resolve the viscous sublayer and are well suited for y1+ values between 1 and 10 whereas high-Re models apply analytical functions to the log-layer and are appropriate to y1+ values ranging from 20 to 50 (it depends on the extension of the buffer layer for the considered flow). Moreover one can notice that the logarithmic function does not apply for separated flow. So whether it is expected that a significant amount of separation will have to be predicted, one of the low-Reynolds number turbulence models would be more appropriate. Recommendations are given in the table below for ranges of y1+ specific to the different types of models. Turbulence Models High-Re: Standard k-ε, Extended wall-function k-ε (will accept lower values) Low-Re: Baldwin-Lomax, SpalartAllmaras, LaunderSharma k-ε, Yang-Shih k-ε, Chien k-ε, Extended wall-function k-ε. 1-10 + Non-linear k-e (Suited for research, not design-cycle analysis) High-Re Y1 + Low-Re 1-10 20-50 TABLE 4-2 Appropriate y1 20-50 values for available turbulence models One way to estimate ywall as a function of a desired y+ value is to use a truncated series solution of the Blasius equation: ⎠ ⎞ ⎝ ⎛ ⎠ ⎞ Vref y wall = 6 --------ν ⎝ ⎛ –7 / 8 L ref -------2 1/8 y+... (4-24) Note that the reference velocity, Vref, can be taken from an average at the inlet. For instance, if the mass flow is known the value can be calculated using density and the cross-sectional area of the inlet. If the mass flow is not known the reference velocity may be calculated from the inlet total pressure and an estimated static pressure using isentropic relations. The reference length, Lref, should be based on streamwise distance since an estimation of boundary layer thickness is implied FINE™ 4-21 Flow Model Mathematical Model in this calculation. For instance, in the case of a turbomachinery simulation one could use the distance of hub and shroud curves that exist upstream of the first row of blades. This is approximate, of course, as the thickness of boundary layers will vary widely within the computational domain. Fortunately it is only necessary to place y+ within a range and not at a specific value. Another method of estimating ywall is to apply the 1/7th velocity profile. In this case the skin friction coefficient Cf is related to the Reynolds number: 0.027 Cf = ------------1 Re x / 7 (4-25) where Rex should be based on average streamwise values of Vref and Lref as discussed above. Since uτ is based on Cf it may be calculated based on Eq. 4-23, and ywall may then be calculated from Eq. 4-22. Note that either method is not exact but they will yield results that are quite close to each other. In fact, it can be instructive to calculate ywall using both methods as a check. Since only one wall distance is being calculated, the particular flow being studied should be kept in mind. For instance if it is a diffusing flow Cf, and hence y+, can be expected to drop. Since a certain range is desired (e.g., 20< y+<50 for high-Re Standard k- ε) the user may choose to base the calculation of wall distance on an average of that range (e.g., 40). b) Things to Look Out For These instructions should provide reasonable estimates but it is always wise to plot y+ once a solution has finished. Spot checks should be made to ensure that most y+ values fall within the desired range. For instance it is useful to plot y+ contours over the first layer of nodes from a given wall. There are some special cases where such checks do not strictly apply. For instance, skin friction approaches zero at points of separation so it is expected that y+ will be low in such regions. It is generally recommended that turbomachinery blade tip clearances are meshed with uniform spanwise node distributions. In such cases, the y+ values will tend to be higher within the gap than elsewhere in the computational domain near-wall regions. This should not raise concern as the tip clearance flow consists of thoroughly sheared vortical fluid that undergoes significant acceleration and is therefore quite different than a standard boundary layer. It is expected that the skin friction will be high in this region due to the acceleration. c) General Advice • What grid resolution is adequate? The resolution method employed in the EURANUS flow solver requires approximately 9 nodes across a free shear-layer and approximately 15 across a boundary layer to provide grid-independent results for turbulent flows. If wall functions are used the boundary layer only requires approximately 9 nodes. Of course the flow field under study will realistically consist of shear layers of which the width varies substantially throughout the flow field. The user must therefore decide what is important to capture and what is not. For instance, in the design-cycle analysis of a compressor with a volute it would probably be acceptable to choose a fully-developed boundary layer. The number of nodes across the diameter would therefore be approximately 29. However, it would be wise to select a number like 33 to maintain a a large number of multi-grid levels. The selection of nodes in the streamwise direction should be governed by what resolution adequately represents the studied geometry. Regions of concentrated high gradients, such as airfoil leading or trailing edges or any geometrical corners should contain a relatively high clustering of nodes. 4-22 FINE™ Mathematical Model Flow Model • What determines the grid quality? After the various grid resolution concerns are addressed, the level of skewness must be analysed. Providing clustering in a curved geometry can often lead to internal angles of grids cells of 10o. It is important to minimize the number of cells containing such low angles as the calculation of fluxes can become significantly erroneous under such conditions. More information concerning how to check the quality of a grid can be found in the IGG™ or AutoGrid manual. If the adjustment of node numbers and clustering does not reduce the level of skewness, local smoothing should be applied. The expansion ratio, or the ratio of adjacent cell sizes, should also be checked. It is particularly important to keep this value within an absolute range of about 0-1.6 in regions of high gradients, such as boundary layers, free shear-layers and shocks. If it is evident that adjacent cells are different in size by factors significantly greater than two, the clustering in this region should be reduced or the number of nodes should be increased. d) Verification of y1+ By following this instructions it should be possible to generate a grid of reasonable quality for turbulent flows. It is recommended however, that the user checks values of y1+ after approximately one hundred iterations on the fine grid to ensure the proper range has been specified. At the same time, it can be useful to plot contours of residuals (continuity, momentum, energy and turbulence) over selective planes. If the level of skewness is too high, this will be indicated by local peaks in residuals that are orders of magnitude greater than the rest of the flow field. If a multi-block grid is used, the residual levels in each block can be compared in the monitor. 4-3.5.4 Defining Initial and Boundary Conditions Turbulence is commonly modelled by emulating molecular diffusion with a so-called "eddy-viscosity" (µT). A standard method for determining µT is based on turbulent-eddy length and time scales that are modelled through turbulence kinetic energy (k) and dissipation (e.g. ε) equations. It is important to note that the level of turbulence quantities (i.e. turbulence intensity, µT, k, ε) specified at the inlet boundary can have a strong effect on the flow-field prediction for quantities like the total pressure, velocity profiles, flow angles, total temperature etc. Since the measurement of turbulence is rarely conducted in a design and test environment, the designer faces the problem of setting these quantities without knowing the correct values. a) Spalart-Allmaras Model When the Spalart-Allmaras model is selected the user should specify in the inlet boundary condition the kinematic turbulent viscosity νΤ (m2/s). If no information is available on the turbulence properties of the flow, estimates can be made based on the following assumptions that: T • For internal flows (e.g. turbomachinery): ----- = 1 to 5. ν ν T • For external flows (e.g. vehicle aerodynamics): ----- = 1 . ν ν b) K-ε Models • Estimation of k The value of the turbulent kinetic energy can be derived from the turbulence intensity Tu or from the wall shear stress. FINE™ 4-23 Flow Model Mathematical Model — From the turbulence intensity. The turbulence intensity Tu can be expressed against the streamwise fluctuating velocity u" and the streamwise velocity Uref: u T u = ----------- . U ref ″2 (4-26) For internal flows the value of Tu is about 5% and for external flows it is reduced to 1%. With these considerations k can be calculated in considering an isotropic turbulence: 3 ″2 2 k = -- ( u ) 2 (4-27) — From the wall shear stress. If the wall shear stress is known, the user can use the wall functions defined for the fully turbulent flow: wall k = ----------ρ Cµ τ (4-28) This value of k could be used as an initial value and also for the inlet boundary condition. • Estimation of ε The value of the turbulent dissipation can be specified through one of the following rules: — Specify the ratio of the turbulent viscosity to the laminar viscosity µ ρref k ε = C µ ----- ------------µ it µ For internal flows (such as turbomachinery flow), typical values are µ it ⁄ µ = 50 . For external flows (in aerodynamics computations), typical values are µ it ⁄ µ = 1 . 2 (4-29) — Specify the turbulent length scale (only for internal flows). A typical values is l = 0.1D H . where DH is the hydraulic diameter of the inlet section 3 3 -- -- 4 2 cµ k ε = --------- . l (4-30) — Derive ε from the asymptotic turbulent kinetic equation: In a free uniform flow the turbulent kinetic energy equation reduces to ∂k u ---- = – ε . ∂x (4-31) This relation can be used to specify the value of the turbulent dissipation in the following way: ∆k ε = – u ----- , L (4-32) where u is the inlet velocity, ∆k the decay of the turbulent kinetic energy over a length L. For example, in a turbomachine, L is the maximum geometric length and ∆k could be set to 10% of the inlet value of k. 4-24 FINE™ Mathematical Model Flow Model Using this method, the user must make sure that the value of the turbulent viscosity obtained from these values of k and ε is not too big or too small. i.e. 1 < ----t < 1000 . If this condition is not satisfied, it is advised to scale down or up the value of k inlet or the ∆k and compute again the turbulent dissipation µ µ — Specify the wall shear stress. If the wall shear stress is known, the user can use the wall functions defined for the fully turbulent flow. ( τ wall ⁄ ρ ) ε = -----------------------l 3 -2 (4-33) If there is an initial solution file containing k and ε , the k and ε values of this file are used to initialize the fields. The initial values mentioned above can also be used to set the inlet boundary conditions for the k and ε fields. However, to reduce the possibility of oscillations in skin friction due to non-physical relaminarisation during convergence, it is recommended to insure ε ≈ 0.1 ε inlet . Either of the above methods can be applied for setting the boundary conditions in turbomachine applications. However, if the given values of k and ε lead to the killing of the turbulence shortly after the inlet section, we suggest to apply Eq. 4-32 and select an inlet values of k such that the ratio of the turbulent viscosity to the laminar viscosity equals 50. In some cases a cross-check between Eq. 4-29 and Eq. 4-31 may result in very different values for ε. In such a case it is recommended to re-evaluate k and ε in the following manner: 1. Use relation Eq. 4-32: 0.1k ∆k ε = – u ------ = u --------- . ∆L ∆L (4-34) This relation expresses that k0 (k at the inlet) is expected to be decreased by about 10% over a length ∆L that is characteristic to the size of the domain. 2. 3. Use relation Eq. 4-29. In this relation Cµ=0.09 and ν represents the laminar viscosity of the fluid. Combine the relations of the two previous steps to remove ε0, leading to: ⎠ ⎞ 0.1U µ T ν - k 0 = ----------- ----- -----∆L µ C µ 4. ⎝ ⎛ . (4-35) Using either relation Eq. 4-29 or Eq. 4-32 then easily leads to an estimation of ε0. 4-3.5.5 Setting Expert Parameters to Procure Convergence Several expert parameters may be set to procure convergence. FINE™ 4-25 Flow Model Mathematical Model a) Cut-off (Clipping) of Minimum k Value The float parameter EKCLIP controls the minimum allowable value of k. This is done to prevent non-physical laminarisation and remove the possibility of negative values being calculated during numerical transients. Setting this value to a reasonable level has been shown to significantly increase convergence rate. EKCLIP: clipping k to about 1% of inlet value maintains minimum residual turbulence in the domain. b) Minimizing Artificial Dissipation in the Boundary Layer An alternative treatment of the dissipation terms in the k and ε equations has been introduced to overcome difficulties related to turbulence decay in boundary layers observed in some specific test cases. Currently, the dissipation terms are scaled with the spectral radius of the equations and are further damped in an exponential manner across the boundary layer. The major drawback of this formulation is that it introduces an excessive amount of artificial dissipation into the boundary layer, leading to non-physical relaminarisation problems. A different implementation, based on the L.E.D. (Local Extrema Diminishing) version of the Jameson-Schmidt-Turkel treatment introduces better monotonicity properties of the k and ε equations. IKELED = 0 (default): Dissipation scaled with spectral radius. = 1: Less diffusive L.E.D. scheme activated. c) Wall Function for the k-ε Turbulence Model INEWKE = 0: Wall function applies for first node off the wall at Y+ =20-50, Launder & Spalding. = 10 (default): Mesh-independent formulation of the wall function. d) Full Multigrid k-ε / Baldwin-Lomax Model Switch KEGRID = 2(default) Grid 222 - Baldwin Lomax, Grid 111 - Baldwin Lomax, Grid 000 - k-e Model. KEGRID = 3: Grid 222 - Baldwin Lomax, Grid 111 - k-e Model, Grid 000 - k-e Model. Example: k-ε run on the finest grid level (000) with 3 levels of grid (222, 111 & 000) in the multigrid procedure. The Baldwin-Lomax model remains active on levels 222 and 111 before k-e is automatically switched on when the finest grid is reached. This is controlled through the expert parameter KEGRID whose value is set to 2 by default, meaning that the Baldwin Lomax model is used up to the second level of grid. The µt / µ field computed using the Baldwin-Lomax model is then transferred to the finest mesh and used to calculate initial k and ε values. The use of a KEGRID value higher than the number of grid levels available enables the k and ε equations to be solved on all grid levels. A similar procedure can be followed when a calculation on 111 mesh is first desired. Providing KEGRID is set to 2 (default value), the Baldwin-Lomax is then active on level 222 before the k-ε model is automatically switched on when the finest grid level (111 in this case) is reached. However, the question then arises when a restart procedure on the 000 level is required. How to restart on 000 while transferring strictly the k and ε fields already computed on 111? By default, since KEGRID=2, the solution computed on 111 is seen as a Baldwin-Lomax solution. The k and ε fields 4-26 FINE™ Mathematical Model Flow Model are then reset using the classical procedure while the other variable fields (density, velocity and energy) are transferred adequately. To overcome this difficulty, KEGRID must again be set to a value higher than the number of grids. This procedure results in a much better initialization of k and ε, thus preventing some relaminarisation while enhancing convergence. e) Cut-off (clipping) of Maximum Turbulence Production/Destruction Value The float parameter PRCLIP controls the maximum allowable value of turbulence production/ destruction (=production/density*dissipation in k-e model). Limiting this to a finite value enhances convergence rate by removing the possibility of unbounded turbulence spikes occurring during the numerical transient. However, care must be taken to apply a reasonable limit. Recommended values are: PRCLIP (Float): For most flows: 50 (default), In turbulent diffusion dominated flows (e.g., seals): 200. f) Linearization of Turbulence Production/Destruction Value The integer parameter LIPROD activates the linear production (PRCLIP is no more used if LIPROD set at 1). This linearization of the turbulence production is relevant for impingement flows for which the standard model is well known to overestimate the production of kinetic energy at stagnation point. LIPROD = 1: activate the linear production (PRCLIP no more used in that case). 4-3.6 Theoretical Aspect of Turbulence Modelling An algebraic (Baldwin-Lomax), an one-equation (Spalart-Allmaras) and several two-equation turbulence models ( k – ε ) are available. Wall distance All turbulence models need to compute the wall distances everywhere in the computed domain. It is a rather time consuming process so that they are saved in the *.cgns mesh file at the beginning of the first computation. These values will be read and used for the next computations. If the mesh file is modified or saved again, they are erased and will be computed again. Different important expert parameter are used in the calculation of the wall distance. The default values are generally sufficient and they have to be changed only if a problem arises. The expert parameter NREPET allows to take into account the periodicity of the computed domain. Indeed, at each point of the domain, the closest wall is not always in the computed domain if periodic boundary conditions are used. Consequently the domain is repeated beyond the periodic boundaries to compute correctly the wall distance. The default value is 1 and can be increased to 2 in very particular cases. The expert parameter NSUBM is the maximum number of subdomains a domain is split into. Its value is sufficiently high and it must be changed only if an error message tells you to increase it. The expert parameter NTUPTC is the number of patches whose sub-patches will be searched. In a very complex geometry, the value of this parameter can be increased if the calculation of the wall distances fails. Another expert parameter can be decreased in parallel with the increase of NTUPTC. This parameter is the real RTOL. It is the maximum angle allowed between two normals of a patch. If a larger value is found, the patch is subdivided. FINE™ 4-27 Flow Model Mathematical Model 4-3.6.1 Baldwin-Lomax The Baldwin-Lomax algebraic turbulence model, Baldwin & Lomax (1978) is a two layer model where the turbulent viscosity in the inner layer is determined using Prandtl’s mixing length model, and the turbulent viscosity in the outer layer is determined from the mean flow and a length scale. The strain-rate parameter in Prandtl’s mixing length model is taken to be the magnitude of the vorticity. The influence on the mean flow equations through the turbulent kinetic energy is neglected. The turbulent viscosity is given by µt = ( µ t ) i, n ≤ n c ( µ t ) 0, n > n c ⎩ ⎨ ⎧ (4-36) where n is the normal distance to the wall, and n c is the smallest value of n at which the inner and outer viscosity is equal. The inner viscosity is ( µ t ) i = ρl ω where l = kn ( 1 – e ⎝ ⎜ ⎛ –y ⁄ A + + 2 (4-37) ) (4-38) ρwτw + y = --------------- n µw and ω i = ε ijk with ε ijk the Kronecker symbol. The outer viscosity is ( µ t ) 0 = KC cp ρF wake F Kleb ( n ) where F wake is the smaller of n max F max 2 ∂u j ∂ xk and C wk n max ( u + v + w )max – ( u + v + w ) min 2 2 2 The term n max is the value of n corresponding to the maximum value of F , F max , where F(n) = n ω (1 – e and – n /A + + 4-28 ⎠ ⎟ ⎞ (4-39) (4-40) (4-41) 2 2 2 /F max (4-42) ) (4-43) FINE™ Mathematical Model Flow Model 6 F Kleb = 1 + 5.5 ( nC Kleb /n max ) + –1 (4-44) The constants used are hard coded and equal: A = 26 , C wk = 1. , C cp = 1.6 , k = 0.41 , C kleb = 0.3 , K = 0.0168 .The turbulent Prandtl number, needed to calculate the turbulent conductivity, is accessible through the expert parameter PRT (see section 3-3.1.2). The expert parameter IATFRZ allows to control the interaction of the model with the multigrid system. When IATFRZ is set to 0, the model is applied separately on all grid levels. When it is set to 1, the model is only applied on the finest grid and the turbulent viscosity is restricted (through the restriction operator) to the coarser grids where the turbulent viscosity is frozen. It is possible to freeze the turbulent viscosity field on all grid level by setting IATFRZ to 2. The value can be automatically changed by using a criteria based on a maximum iteration number or on a minimum convergence. The maximum iteration number is specified by the expert parameter ITFRZ. The minimum reduction of order of magnitude is set in the expert parameter RESFRZ. 4-3.6.2 Spalart-Allmaras The Spalart-Allmaras turbulence model is a one equation turbulence model which can be considered as a bridge between the algebraic model of Baldwin-Lomax and the two equation models. The Spalart-Allmaras model has become quite popular in the last years because of its robustness and its ability to treat complex flows. The main advantage of the Spalart-Allmaras model when compared to the one of Baldwin-Lomax is that the turbulent eddy viscosity field is always continuous. Its advantage over the k-ε model is mainly its robustness and the lower additional CPU and Memory usage. The principle of this turbulence model is based on the resolution of an additional transport equation for the eddy viscosity. The equation contains an advective, a diffusive and a source term and is implemented in a non conservative manner. The implementation is based on the papers of Spalart and Allmaras (1992) with the improvements described in Ashford and Powell (1996) in order to ˜ avoid negative values for the production term ( S in Eq. 4-50). The turbulent viscosity is given by ˜ ν t = ν f v1 ˜ where ν is the turbulent working variable and f v1 χ f v1 = -----------------3 χ + c v1 ˜ with χ is the ratio between the working variable ν and the molecular viscosity ν , ˜ ν χ = -ν The turbulent working variable obeys the transport equation ˜ ∂ν 1 ˜ ˜ ˜ ˜ ˜ ----- + V ⋅ ∇ν = -- { ∇ ⋅ [ ( ν + ( 1 + c b2 )ν ) ∇ν ] – c b2 ν ∆ν } + Q ∂t σ where V is the velocity vector, Q the source term and σ , c b2 constants. (4-48) 3 (4-45) a function defined by (4-46) (4-47) FINE™ 4-29 Flow Model Mathematical Model The source term includes a production term and a destruction term: ˜ ˜ ˜ ˜ Q = νP( ν) – νD(ν ) where ˜˜ ˜ ˜ ν P ( ν ) = c b1 Sν ˜ ν ˜ ˜ ν D ( ν ) = c w1 f w -d 2 (4-49) (4-50) The production term P is constructed with the following functions: ˜ ν ˜ S = Sf v3 + ---------- f v2 ; 2 2 κ d 1 f v2 = ------------------------------ ; 3 ( 1 + χ ⁄ c v2 ) ( 1 + χf v1 ) ( 1 – f v2 ) f v3 = ------------------------------------------χ where d is the distance to the closest wall and S the magnitude of vorticity. In the destruction term (Eq. 4-51), the function f w is 1 + c w3 = g -----------------6 6 g + c w3 ⎝ ⎜ ⎛ 6 1 -6 fw with g = r + c w2 ( r – r ) ; The constants arising in the model are 6 c w1 = c b1 ⁄ κ + ( 1 + c b2 ) ⁄ σ , c w2 = 0.3 , c w3 = 2. , c v1 = 7.1 , c v2 = 5. c b1 = 0.1355 , c b2 = 0.622 , κ = 0.41 , σ = 2 ⁄ 3 2 The equation Eq. 4-48 is solved with the appropriate boundary conditions: ˜ ˜ on solid wall ν = 0 , along the inflow boundaries the value of ν t is specified ( ν is obtained by using a Newton-Raphson procedure to solve Eq. 4-45) and along the outflow boundaries it is extrapolated from the interior values. 4-30 ⎠ ⎝ ⎞ ⎛ (4-51) (4-52) (4-53) ˜ ν r = ------------˜ 2 2 Sκ d ⎠ ⎟ ⎞ (4-54) (4-55) FINE™ Mathematical Model Flow Model 4-3.6.3 k-ε Turbulence Models a) General Formulation In the k – ε turbulence model two additional transport equations for the turbulent kinetic energy, k , and the turbulent dissipation rate, ε , are solved. In EURANUS, 4 linear and 2 non-linear models are currently used. In the following, the trace of the tensor X will be written {X} In the k – ε turbulence model two additional differential equations need to be solved respectively for k and ε . These additional equations can be put in the following general form: µ ∂ρk -------- + ∇• ρwk – µ + ----t ∇k = – ρw″ ⊗ w″ S – ρε ∂t σk ˜ µ 1 ∂ρε ˜ ˜ - ˜ -------- + ∇• ρwε – µ + ----t ∇ε = – -- C ε1 f 1 ρw″ ⊗ w″ S + C ε2 f 2 ρε + E T ∂t σε where S is the mean strain tensor and – ρw″ ⊗ w″ the turbulent Reynolds stress tensor. ˜ The variable ε is the modified dissipation rate ˜ ε = ε–D and the turbulent viscosity µ t is given by the following relation µ t = ρC µ f µ kT (4-59) (4-58) ⎠ ⎟ ⎞ ⎭ ⎬ ⎫ ⎩ ⎨ ⎧ ⎝ ⎜ ⎛ ⎠ ⎞ ⎝ ⎛ ⎭ ⎬ ⎫ ⎩ ⎨ ⎧ ⎠ ⎞ ⎝ ⎛ (4-56) (4-57) b) Linear Models In the linear models, the turbulent Reynolds stress tensor is related to the mean strain tensor in a linear way. 2 ( – ρ w″ ⊗ w″ )ij = 2µ t S ij – 2 ( ∇w )δ ij – -- ρkδ ij -3 3 (4-60) ⎠ ⎟ ⎞ ˜ ˜ 1 ∂w i ∂w j + S ij = -2 ∂ xj ∂ x i The implemented linear models are: ⎝ ⎜ ⎛ - Chien, low Reynolds number k-ε model (Chien, 1982). - Extended wall functions (Hakimi, 1997) = Standard high Reynolds (Launder & Spalding, 1974) if the expert parameter INEWKE is set to 0. - Launder-Sharma, low Reynolds number k-ε model (Launder & Sharma, 1974). - Yang-Shih, low Reynolds number k-ε model (Yang & Shih, 1993). FINE™ 4-31 Flow Model Mathematical Model The constants or functions Cµ, Cε1, Cε2, σk, σε, fµ,f1, f2, D, E and T are model dependent and they k k y are defined in the Table 4-3 where Re t = ----- and Re y = ---------νε ν TABLE 4-3 Coefficients 2 0.5 of the k-ε models Standard high-Re Launder & Sharma 0.09 1.44 1.92 1.0 1.3 – 3.4 -------------------------------------2 ( 1 + ( Re t ) ⁄ 50 ) k-ε Model Cµ Cε1 Cε2 σk σε fµ x A a B b C c d f1 f2 T D Chien 0.09 1.35 1.80 1.0 1.3 1–e – 0.0115y + Yang & Shih 0.09 1.44 1.92 1.0 1.3 [1 – e a b c – ( Ax + Bx + Cx ) d 0.09 1.44 1.92 1.0 1.3 1.0 e ] Rey 1.5 10-4 1 5 10-7 3 10-10 5 0.5 1.0 1 – 0.22e – Re t ⁄ 36 2 1.0 1.0 k⁄ε 2 + 1.0 1 – 0.3e – Re t 2 1.0 1.0 k ⁄ ε + (ν ⁄ ε) 2 0.5 ˜ k⁄ε 2νk ⁄ y ˜ k⁄ε 2ν ( ∇ k ) 0. 0. νµ t ( ∇•S ) 2 E ˜ – 2µε e ---------------------------2 y 0. – 0.5y 0. uτ ⁄ Cµ / DNS u τ ⁄ ( κy ) / DNS 3 2 0.5 2νµ t ( ∇•S ) 2 kw 0. 0. εw 0. 0. 2ν ( ∇ k ) 2 The constants Cµ, Cε1, Cε2, σk, σε can however be changed by the user (respectively the expert parameters CMU, CE1, CE2, SIGK, SIGE in the Computation Steering/Control variables page. The turbulent Prandtl number, needed to calculate the turbulent conductivity, is also an expert parameter (PRT). 4-32 FINE™ Mathematical Model Flow Model Two variants of the high Reynolds k-ε with wall functions (section d) Solid Boundary and Wall Functions) exist: • If the expert parameter INEWKE=10 (Default), the wall functions are derived from DNS (Direct Numerical Simulation) curve fitting. The k-ε model is in that case derived from the Yang-Shih model. This new model, named extended wall functions, allows to obtain accurate results on fine mesh contrary to the standard high Reynolds k-ε model. • if the expert parameter INEWKE=0, standard wall function are applied and the y+ value of the near wall cell should be greater than 20. The Chien and the Launder-Sharma models belong to the same family (zero value of ε at the wall) while the standard model and Yang-Shih model belong to a second family (non zero value of ε at the wall). Launching the restart is allowed as long as the user sticks to the same family. c) Non Linear Models The non-linear models are based on two linear models: the Yang and Shih model for low Reynolds variant and the Standard k-ε model for high Reynolds variant. c.1) The low Reynolds model The production term is modified through: fµ γRi t 4 2 – ρw″ ⊗ w″ = -- ---------------------- 1 – --------------------- kTS – -- ρkI i 3A + f s 3 1 + γRi 1 µ t i where T is defined in Table 4-3 and: T' = 1 ⁄ ( f t1 ⁄ T w + f t2 ⁄ T ) 1 f t1 = 1 – --------------------------------------------2 2 ( 1 + 2 { S }ν ⁄ ε ) ⎠ ⎟ ⎞ ; A2 T w = -----------------2 2{S } ; f t1 f t2 = 1 – -------------------------1 + Re t ⁄ 70 ˜ ˜ 1 ∂w i ∂w j Ω ij = -– 2 ∂ xj ∂ xi 2 1⁄3 ; s = T' 2 { S } ; ω = T' – 2 { Ω } ; Ri t = – ωs – ω and Cτ2 = 46; Cτ3 = -7; A1 = 4; A2 = 1000 and γ = 0.2 c.2) The high Reynolds model The model is modified in the following way: 2 2 • f µ is set to unity FINE™ ⎠ ⎟ ⎞ ⎝ ⎜ ⎛ ˜ ˜ 1 ∂w i ∂w j S ij = -+ 2 ∂ xj ∂ xi ⎝ ⎜ ⎛ ⎠ ⎞ C τ3 2 2 2 2 – ----------------------------- kT' 2S + SΩ – Ω S – -- { S } 3 3 3 A2 + s + ω ⎝ ⎛ ⎠ ⎞ C τ2 2 2 2 2 – ----------------------------- kT' 2S – SΩ + ΩS – -- { S } 3 3 3 A2 + s + ω ⎝ ⎛ ⎠ ⎟ ⎞ ⎝ ⎜ ⎛ (4-61) 4-33 Flow Model Mathematical Model • T’ is replaced by T The production term becomes: γRi t 4 1 2 – ρw″ ⊗ w″ = -- ------------- 1 – --------------------- kTS – -- ρkI i 3 A1 + s 3 1 + γRi t i where s and ω are modified according to: s = T 2{ S } ω = T –2 { Ω } The coefficients Cτ2, Cτ3, A1, A2 and γ remain unchanged. Note that the High Reynolds non-linear model uses the wall functions as it is based on the standard k-ε model. Before launching the non-linear model, it is recommended to apply first the linear model and restart from this solution. This procedure will provide a good initial solution for the non-linear model and prevent the non-linear terms to cause divergence of the code at the early stage. Since the non-linear model is from Yang-Shih, the restart can be done only from the Yang-Shih model (linear or not) and the Standard model with wall functions. 2 2 d) Solid Boundary and Wall Functions The values of kw and εw are imposed at the boundary for the Chien, Launder & Sharma and Low Reynolds non-linear models, while for the Standard and non-linear High Reynolds number models, it is imposed in the first inner cell. The wall friction velocity uτ is calculated through a wall function (Eq. 4-64 or Eq. 4-65) from the velocity at the cell center and the normal distance to the wall. For the models that do not use wall functions (Chien, Launder Sharma, Yang & Shih and Low Reynolds non linear model), the profile of the boundary layer is directly inferred from the input values at the wall. Consequently, particular attention must be paid to the grid refinement in this region in order to capture the viscous sublayer. A typical + value is given by 1 < y < 10 at the first node from the wall. The wall functions are used to mimic the presence of the walls by reflecting the effect of the steep, non-linear variations of the flow properties through the turbulent boundary layer. They define the shear stress and the heat flux on the cell faces lying on solid boundaries as well as the values of k and ε in the vicinity of the wall. The wall functions are applied in the Standard (see kw and εw in Table 4-3 ) and in the High Reynolds non linear k-ε models. For the extended wall functions model, the wall functions for k and ε are fitted with polynomials to the DNS data. 4-34 ⎠ ⎞ C τ3 2 2 2 2 – ----------------------------- kT 2S + SΩ – Ω S – -- { S } 3 3 3 A2 + s + ω ⎝ ⎛ ⎠ ⎞ C τ2 2 2 2 2 – ----------------------------- kT 2S – SΩ + ΩS – -- { S } 3 3 3 A2 + s + ω ⎝ ⎛ ⎠ ⎟ ⎞ ⎝ ⎜ ⎛ (4-62) (4-63) FINE™ Mathematical Model Flow Model d.1) Velocity For smooth walls: The wall function in the viscous sublayer is given by: u + ---- = y uτ + τ with y = ------- , the dimensionless normal distance from the walls and u τ = (4-64) yu ν τ wall ⁄ ρ , the wall friction velocity directly related to the wall shear stress. While in the turbulent layer, the wall function becomes: u 1 + ---- = -- ln y + B κ uτ (4-65) where κ is the von Karman constant (default value 0.41) and B another constant (default value 5.36). They can be modified by the user in the Boundary Condition page. For rough walls: The wall function is given by (no viscous sublayer considered): u 1 y – d0 ---- = -- ln ------------- + B uτ κ k0 (4-66) where κ and B are defined just above and k0 and d0 are constants asked for each rough wall. The constant k0 is the equivalent roughness height while d0 is known as the height of the zero displacement plane, defined by u ( k 0 + d 0 ) = 0. (if B=0). For small roughness elements, d 0 = 0 . For high roughness elements, the flow behaves as if the wall was located at a distance d0 from the real wall position. ks k 0 = ----30 where ks is the average roughness height + For rough walls, the constant B is usually zero (when ks+ > 70 with value of B is evolving as presented in below graph. + ks y k s = ----------y ). Otherwise the + s FINE™ 4-35 Flow Model Mathematical Model When a rough wall is specified, the distance from the wall to the cell-centre of the first inner cell should be bigger than k0 + d0. In general, the first inner cell should be located within the fully turbulent layer. d.2) Temperature Similarly, for isothermal walls, the following laws are considered in the code: T = Pr y + + in the viscous sublayer (4-67) where Pr is the laminar Prandtl number and: + + Pr t y T = ------- ln --------- + 13.2Pr κ 13.2 + Tw – T T = --------------- . Tτ ⎠ ⎞ ⎝ ⎛ in the turbulent layer (4-68) where The heat flux at the wall is defined as: q w = ρCpuτ T τ (4-69) A complete description of the available thermal boundary conditions at walls is provided in section 8-5.3. The "law of the wall" distributions of velocity, temperature and other variables are assumed to prevail across the boundary layer. They are imposed at the node of a single + grid cell for which the user is advised to check that 20 < y < 100 . As a result, if the first cell node from the wall is placed too close, calculation is conducted in the viscous sublayer and the law is no longer valid. Similarly, if the first node is placed too far away, then a discrepancy may exist between the profiles and their assumed shape. e) Numerical Concerns This paragraph provides a description of the numerical method used to deal with the k and ε equations. e.1) Choice of the initial and boundary conditions Initial values for k and ε must be specified by the user, as well as the inlet boundary condition. The specified values at the inlet boundary can have a strong effect on the flow-field prediction. Several methods are proposed in section 4-3.5.4 to help the user in the choice of suitable values. e.2) Compressibility correction The compressibility correction is present only in the k-ε model of Chien and is useful only for high Mach number flows (M>3). Two kinds of compressibility effects are implemented: 1) the contributions from the modelled pressure gradient-velocity term and 2) the compressible dissipation. They can be activated by using respectively the expert parameters ICOPKE or ICODKE. The first compressibility correction is associated with the modelling of pressure gradient-velocity term in the equation of the turbulent kinetic energy, and, according to Zhang et al. (1991), leads to the source term Rk: 4-36 FINE™ Mathematical Model Flow Model µ t ∂ρ ∂p R k = – ----------, 2 ρ σp ∂ xi ∂ xi which modifies the term D of Eq. 4-58: µ t ∂ρ ∂p D' = D + ----------. 3 ρ σp ∂ xi ∂ xi Similarly a term R ε can be added to the ε equation. After Vandromme (1991) one has: µ t ε ∂ρ ∂p R ε = – C 3 ----------- , 2 ρ σ k ∂ xi ∂ xi p (4-70) (4-71) (4-72) which modifies the term E of Eq. 4-57: µ t ε ∂ρ ∂p E' = E – C 3 ----------- . 2 ρ σ k ∂ xi ∂ x i p (4-73) The above terms are included in the k – ε equations if the expert parameter ICOPKE is set to 1; if ICOPKE=0 (Default) they are set to zero. The empirical constants in these equations are two expert parameters (SIGRO and C3), with default values: σ p = 0.5 C 3 = 2.0 . (4-74) The second correction concerns the modelling of compressible dissipation. The physical foundation for this correction is the observation of decreased turbulent viscosity with increased Mach number (Nichols, 1990). The type of compressible dissipation is controlled by the expert parameter ICODKE. For ICODKE=0 no correction for compressible dissipation is done. In the correction of Sarkar (1989) (ICODKE=1), the dissipation of k is expressed as the sum of solenoidal ( ε ) and dilatational ( ε d ) components. The dissipation in the source term of the k -equation (Eq. 4-56) is then corrected according to: ε corr = ε ( 1 + αM t ) with M t a turbulent Mach number defined as M 2 t 2 (4-75) k= ---2 a (4-76) where a is the speed of sound.The constant α is an expert parameter (ALF), with default value =0.5. Nichols (1990) developed a model that corrects the production term in the turbulent kinetic energy equation (ICODKE=2): ⎠ ⎞ ⎝ ⎛ ⎠ ⎞ – ρw″ ⊗ w″ S ( corr ) k = – ρw″ ⊗ w″ S 1 – C p1 ( γ – 1 )M ---2 a FINE™ ⎝ ⎛ (4-77) 4-37 Flow Model Mathematical Model where a is the local speed of sound, γ is the specific heat ratio and C p1 an empirical constant (CP1 in the list of expert parameters available on the Control Variables page, with default value =4.). This correction improves the prediction of the turbulent production level by directly taking the effect of the Mach number (M) into account. e.3) Limiters for the turbulence variables Successive limitations are set for the turbulence variables to ensure physical values and the stability of the calculation. Indeed, the term sources in the k-ε equations can vary strongly especially at the beginning of the computation and lead to unphysical values and divergence. 1. To control the stability of the calculation, the expert parameter MAVRES, denoted here ζ , is used This parameter limits the variation of the turbulence variables for each Runge-Kutta stage. Denoting the new value of k or ε as q > 0: q n+1 n+1 , the following restrictions are imposed when MAVRES = max ( q n+1 , EPS,ζq ) , ( 2 – ζ )q ) n n (4-78) q n+1 = min ( q n+1 (4-79) where EPS is an expert parameter with a small value, default 1E-28, also used to avoid possible divisions by zero. The restriction defined in Eq. 4-79 is not applied to the turbulent dissipation rate (ε) when this tends to increase, in order to avoid excessive values of the turbulent viscosity. If MAVRES = 0, only the restriction defined in Eq. 4-78 is applied (avoiding negative values) If MAVRES < 0, the restriction is: q n+1 (1 + ζ)(q –q ) n – q = -------------------------------------------n+1 n q –q 1 + ------------------------n q ⎠ ⎟ ⎞ ⎝ ⎜ ⎛ n+1 n (4-80) 2. A similar system is applied to the multigrid corrections with the expert parameter MAVREM, denoted below as ζ : If MAVREM > 0: q n+1 – q < ( 1 – ζ )q n n If MAVREM = 0: restriction to positive values If MAVREM < 0: q n+1 –q ) (1 + ζ )( q n – q = -------------------------------------------n+1 n q –q 1 + ------------------------n q ⎠ ⎟ ⎞ ⎝ ⎜ ⎛ 3⁄2 n+1 n k 3. The expert parameter LTMAX is used to limit the turbulence length scale L turb = --------- to a ε value compatible with the domain scale. If Lturb>LTMAX and MAVRES > 0, the value of ε is set to respect the maximum length scale. If Lturb>LTMAX and MAVRES <= 0, the values of k and ε are set to a small value EPS. The default value for LTMAX is 1E+6. 4-38 FINE™ Mathematical Model Flow Model 4. An automatic control of the turbulent length scale is possible by setting the expert parameter LTMAX to a negative value (LTMAX = -1). In this case, the following length scale control is proposed: L = min ( kT, 5le max ) with le max the maximum equilibrium length scale in the computation, defined by le max = κd max C µ –3 ⁄ 4 (4-81) (4-82) where d max is the maximum distance to the wall among all grid points of all blocks. The factor 5 in Eq. 4-81 is set to avoid to clip the length scale too early. The turbulent viscosity is then written as ν t = C µ f µ kL For the update of turbulent variables (previous paragraph), LTMAX is replaced by 5le max 5. Another way to control the turbulent length scale is the Yap’s modification. It is applied by setting the expert parameter IYAP to 1. In this case, the expert parameter LTMAX should be set to its default value (1.E+6) to avoid conflicts. Yap’s modification consists of adding to the epsilon equation a source term that control the turbulent length scale. It can be applied to all k-ε models. The source term to be added writes: ll- 2 ε S YAP = 0.83max -- – 1, 0 -- -le le T where l and l e are respectively the turbulent length scale ( l = length scale ( l e = κdC µ –3 ⁄ 4 ). A weakness of Yap’s correction is that it might conflict with Inlet boundary conditions if these are set without respecting a turbulent length scale criteria. 6. The expert parameter TEDAMP is another parameter to control stability. This parameter prevents the factor 1 ⁄ T in the ε equation from being singular as k tends to zero (see Eq. 4-57 and the relationship between k and T in Table 4-3 ). A minimum of TEDAMP multiplication factor of the clipping value (expert parameter EKCLIP) is used for k . The same parameter is used to damp 1/ε coming from T in the calculation of the turbulent viscosity, Eq. 4-59: a minimum of TEDAMP multiplication factor of the clipping value (expert parameter EPCLIP) is used for ε . If TEDAMP<=0, the minimum values used for k and ε correspond to the expert parameter EPS. The default value of TEDAMP is -1. Irrespective of the value of TEDAMP, this strategy always avoids the use of possible negative values of k in the source term and of ε in the turbulent viscosity. FINE™ ⎠ ⎝⎠ ⎞ ⎛⎞ ⎝ ⎛ (4-83) kT ) and the equilibrium 4-39 Flow Model Mathematical Model 7. Another control on the stability is available through the parameter GAMMAT which introduces the turbulence time scale Tturb in the computation of the local time step: 1 1 GAMMAT --------- = ---- + ------------------------∆t kε ∆t T turb The default value of GAMMAT is set to 10. 8. Another important consideration is the amount of turbulence production compared to its dissipa· tion, Prod ⁄ ( ρε ) . This quantity should stay within physically admissible ranges so that the turbulence production remains limited. The parameter PRCLIP allows the control of this ratio. As an example, Prod ⁄ ( ρε ) ≈ 1 for homogeneous core flows and thin shear layers, whereas Prod ⁄ ( ρε ) < 1 for separated shear layers and wakes. Flows of high shear, such as jets in cross · flow, can exhibit much higher values of Prod ⁄ ( ρε ) . An upper bound of PRCLIP=50 is recommended to the user. However, this control is removed by the use of a linearised turbulent production model introduced in all linear k-ε models. This simple modification is relevant for impinging flows, for which the turbulence models are well known to overestimate the turbulent production of kinetic energy. It corresponds to a linearisation of the production term when the strain rate is large when the expert parameter LIPROD is set at 1. 9. The expert parameters EKCLIP and EPCLIP are respectively the minimum allowable values of the turbulent kinetic energy (k) and the turbulent dissipation rate (ε). They avoid non-physical negative values. Moreover the minimum value of k (EKCLIP) allows to maintain a minimum residual turbulence in the domain. The default value is 1.E-5. The minimum value of ε is chosen so that the computed value of the turbulent viscosity is reasonable. With a default value set to 1.E-5, the turbulent viscosity has a value of the order 1.E-6. 10. The input parameter KEGRID allows the use of a particular full multigrid strategy for k-ε computations. The Baldwin-Lomax model is used on the coarse grids during the full multigrid stage and the k and ε initial solution is obtained from the Baldwin-Lomax model solution. KEGRID corresponds to the last grid level on which the algebraic model is used. For example, if the computation is done with 4 levels of multigrid and KEGRID is equal to 2, the Baldwin-Lomax model is used on the 333 (or level 4), 222 (or level 3) and 111 (or level 2) and the k-ε computation is initiated when transferring to the finest grid. If KEGRID is set to 3, the k-ε computation will be initiated when transferring to 222. If KEGRID is greater than the number of multigrid levels, the computation will be started on the coarsest level with k-ε. 11. The expert parameter IKENC allows solving k-ε equations with a non-conservative approach. This settings avoids the appearance of an artificial source term in the k-ε equations during the convergence process. This artificial term comes from the residuals of the equation of the mass conservation that can be non-negligible at the beginning of the convergence process. This approach is new and not sufficiently tested to ensure that the loss of conservation is not excessive in all cases. 12. The expert parameter IKELED allows to avoid an excessive artificial dissipation of the standard central scheme into the boundary layer. Indeed this scheme can lead to a non-physical relaminarisation in some specific test cases. An alternative computation of the artificial dissipation, based on the Local Extrema Diminishing (LED) version of the Jameson-Schmidt-Turkel treatment has been implemented. It is active when the expert parameter IKELED is set to 1. All the above mentioned limiters are very important for the robustness of k-ε computations. With the exception of the length scale LTMAX all limiters are given appropriate defaults and we do not recommend to modify them. For LTMAX we recommend to set it to ten times the geometrical length scale. (4-84) 4-40 FINE™ Mathematical Model Flow Model 4-3.6.4 References Ashford G.A. , and Powell K.G. 1996, "An unstructured grid generation and adaptative solution technique for high-Reynolds number compressible flow", VKI (Von Karman Institute) Lecture Series 1996-06. Baldwin B., Lomax H. (1978) 'Thin Layer Approximation and Algebraic Model for Separated Turbulent Flows', AIAA-78-257. Chien K.Y. (1982) 'Predictions of Channel and Boundary-Layer Flows with a Low-ReynoldsNumber Turbulence Model', AIAA J., Vol. 20, No. 1. Hakimi N. (1997) ’Preconditioning methods for time dependent Navier-Stokes equations’, PhD Thesis, Dept of Fluid Mechanics, Vrije Universiteit Brussel. Jameson A., Schmidt W., Turkel E. (1981) 'Numerical Solutions of the Euler Equations by Finite Volume Methods using Runge-Kutta Time-Stepping Schemes', AIAA-81-1259. Jameson A., 1995, "Positive schemes and shocks modelling for compressible flows", International Journal for Numerical Methods in Fluids, Vol 20, pp 773-776. Launder B.E. and Sharma B.I., 1974,"Application of the Energy-Dissipation Model of turbulence to the Calculation of Flow Near a Spinning Disc", Letters in Heat and Mass Transfer, Vol. 1, pp. 131138. Launder B.E. and Spalding D.B., 1974, "The numerical computation of turbulent flow", Comput. Methods App. Mech. Eng., vol. 3, pp. 269-289. Nichols R.H. (1990) 'A Two-Equation Model for Compressible Flows', AIAA paper 90-0494. Sarkar S., Erlebacher G., Hussaini M.Y., Kreiss H.O. (1991) 'The analysis and modelling of dilatational terms in compressible turbulence', J Fluid Mech, Vol.227, pp.473-493. Spalart P.R. and Allmaras S.R. (1992),"A one equation turbulence model for aerodynamic flows",, AIAA 92-0439 Vandromme D. (1991) 'Turbulence Modelling for Compressible Flows and Implementation in Navier-Stokes Solvers', VKI Lecture Series 1991-02. Yang Z. and Shih T.H., 1993, "A k-e model for turbulence and transitional boundary layer", NearWall Turbulent Flows, R.M.C. So., C.G. Speziale and B.E. Launder(Editors), Elsevier-Science Publishers B. V., pp. 165-175. Zhang H.S., So R.M.C., Speziale C.G., Lai Y.G. (1991) 'A Near-Wall Model for Compressible Turbulent Flow', ICASE Report 91-82. 4-3.7 Gravity Forces When gravity should be taken into account the box marked Gravity Forces should be checked. If gravity is activated by checking this box three input dialog boxes appear to define the Gravity Vector. The default gravity vector is defined as: (gx,gy,gz)=(0,-9.81,0) [m/s2], representing the gravity on Earth where the y-axis is oriented normal to the ground. When the gravity is taken into account in the Navier-Stokes equations, the source terms ρg and ρ ( g ⋅ V ) are respectively introduced in the momentum and energy conservation equations where ρ is the density, g the gravity vector and V the velocity vector. FINE™ 4-41 Flow Model Mathematical Model If the fluid is a liquid, the density is constant and you do not have any influence of the pressure or temperature on the flow by interaction with the gravity. To simulate these interactions, one can use the Boussinesq approximation in the gravity source terms. With this approximation, the density is developed in the first order of the MacLaurin series. It becomes: ρ = ρ ref + α ( p – p ref ) – β ( T – T ref ) with α the compressibility and β the dilatation coefficients specified in the fluid properties. This variation of the density is only applied to the gravity source term (Boussinesq approximation). Otherwise, the density is kept constant in the conservation equations. The value of ρ ref is the characteristic density specified in the Flow Model page. p ref and T ref are the reference values in the Flow Model page. When the gravity is taken into account, a reference pressure must be specified at a reference altitude to add the hydrostatic pressure in the initial pressure field. The reference pressure is the reference value in the Flow Model page. The reference altitude is specified in the expert parameter IREFPT. (4-85) 4-3.8 Low Speed Flow (Preconditioning) This option appears in the Flow Model page only if the fluid type is compressible. Indeed, the preconditioning is automatically used for an incompressible fluid. This option is only implemented for central schemes. Consequently, the upwind spatial scheme (Numerical Model page) is not available if the preconditioning option is chosen. 4-3.8.1 General Description In the low subsonic Mach number regime, time-marching algorithms designed for compressible flows show a pronounced lack of efficiency. When the magnitude of the flow velocity becomes small in comparison with the acoustic speeds, time marching compressible codes converge very slowly. The problems faced by compressible codes at low Mach number are: • High disparity between the convective eigenvalues u and the acoustic eigenvalues u+c, u-c leading to a much too restrictive time step for the convective waves causing thus poor convergence characteristics. • Round off errors mostly due to the use of absolute pressure in the momentum equations. • Impossibility to treat strictly incompressible flows. Therefore the development of a low speed preconditioner was motivated in order to provide fast convergence characteristics and accurate solutions as the Mach number approaches zero. Over the past years and up to now, many attempts have been made to solve nearly incompressible flow problems within available compressible codes and with minor programming efforts. The corrective action brought to the discretization of the conservation equations is called preconditioning and is derived from the artificial compressibility method introduced for incompressible flows by Chorin, (1967). 4-42 FINE™ Mathematical Model Flow Model For steady state applications solved by time marching algorithms the time derivatives of the unknowns arising in the flow equations are of no physical meaning and can thus be modified without altering the final steady state solution. The idea of preconditioning precisely uses this property and consists of multiplying the time derivatives of the dependent variables with a matrix called preconditioning matrix. The main property of this matrix is to remove the stiffness of the eigenvalues. In addition, reduced flow variables such as the dynamic pressure and the dynamic enthalpy are introduced, reducing drastically the round off errors at low Mach numbers. The acoustic wave speed c is replaced by a pseudo-wave speed c’ of the same order of magnitude as the fluid speed. To be efficient the selected preconditioning matrix should be valid for inviscid computations as well as for viscous computations with heat transfer. The preconditioning methodology developed (Hakimi, 1997) is of sufficient generality and can treat any type of fluids including perfect gases and incompressible Newtonian and non Newtonian fluids. On the numerical level, the solution procedure including space discretization, time integration and boundary conditions have been adapted to the new transient behaviour of the conservation equations. The low speed preconditioner has been validated for inviscid flows, viscous flows, turbulent flows and unsteady flows. Efficient convergence rates and accurate solution have been obtained for Mach numbers from M=0.1 to M=10-6, Reynolds numbers from Re=106 to 10-6 and aspect ratios from 1 to 2000. 4-3.8.2 Basic Equations The preconditioned equations considered for a compressible fluid are: 1- ∂p ∂ρu -------- ∂ρw ---- ----- + --------- + ∂ρv + ---------- = 0 2 ∂x ∂y ∂z β ∂t ∂τ xx ∂τ yx ∂τ zx αu ---------- ∂p + ρ du + ∂p = --------- + --------- + --------- ----- ----2 ∂t dt ∂x ∂x ∂y ∂z β dv ∂p ∂τ xy ∂τ yy ∂τ zy αv ∂p ----- ----- + ρ ----- + ----- = --------- + --------- + --------- – ρg - 2 ∂t ∂x ∂y ∂z dt ∂y β αw ∂p dw ∂p ∂τ xz ∂τ yz ∂τ zz ------- ----- + ρ ------ + ----- = --------- + --------- + -------- 2 ∂t ∂x ∂y ∂z dt ∂z β de ρ ----- + p ∇ ⋅ V = ∇ ⋅ k∇T + ε v dt Compared to the unpreconditioned Navier-Stokes equations a pressure time derivative is added to the continuity equation and also to the momentum equations. The internal energy equation is con∂v i sidered to build the system and εv is a dissipation term defined as: ε v = τ ⋅ ∇ ⋅ V = τ ij ------ ; ∂x j V = ( u, v, w ) is the velocity vector. At this stage the eigenvalues as well as the eigenvectors associated with the preconditioned method defined by Eq. 4-86 are already completely defined. ⎠ ⎞ ⎝ ⎛ ⎠ ⎞ ⎝ ⎛ ⎠ ⎞ ⎝ ⎛ (4-86) 4-3.8.3 General Form of the Preconditioning Matrix The Preconditioned Reynolds-Averaged Navier-Stokes equations including turbulence and species transport equations written in a Cartesian frame of reference and integrated over a control volume Ω are expressed as: FINE™ 4-43 Flow Model Mathematical Model ∫∫∫Γ Ω – 1 ∂Q ------ dΩ + ∂t ∫ ∫ F ⋅ dS = ∫ ∫ ∫ ST dΩ S Ω (4-87) with ˜ T Q = ( p g, u, v, w, E g, ρk, ρε ) . (4-88) The variable p g = p – p ref is the gauge pressure and the variables E g is the total gauge energy. For a perfect gas with constant Cv , E g is given by: V E g = C v ( T – T ref ) + ----2 2 (4-89) For an incompressible fluid with constant C p , Eg is given by: V E g = C p ( T – T ref ) + ----- . 2 2 (4-90) The extension of the preconditioning matrix to the turbulence transport equations is then given in its general form both for compressible and incompressible fluids by: ⎠ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎞ ⎝ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎛ 1 ---2 β ( 1 + α )u -------------------2 β ( 1 + α )v -------------------2 β ( 1 + α )w --------------------2 β 2 0 0 0 0 0 0 0 . . 0 ρ 0 0 0 0 0 0 . . 0 0 ρ 0 0 0 0 0 . . 0 0 0 ρ 0 0 0 0 . . 0 Γ –1 = (4-91) αv + Eg --------------------- ( – 1 )∗ 0 0 0 ρ 0 0 0 . . 0 2 β 0 0 0 0 0 1 0 0 . . 0 0 0 0 0 0 0 1 0 . . 0 * the term -1 should be added in compressible cases only. We notice from Eq. 4-91 that the preconditioning matrix does not apply to the transport equations of k and ε. This choice is the simplest and did not cause any particular instability for turbulent test cases run so far. 4-3.8.4 Eigenvalues of the System The eigenvalues of the preconditioned system defined by Eq. 4-86 are determined from the Euler part and can be obtained easily if the equations are written in terms of the primitive variables (p,u,v,w,p or e ). 4-44 FINE™ Mathematical Model Flow Model Their expression is given in 3D for compressible fluids by: λ 1 ,2, 3 = V ⋅ n ⎠ ⎟ ⎞ ⎝ ⎜ ⎛ ⎠⎠ ⎟⎟ ⎞⎞ ⎝ ⎜ ⎛ ⎝ ⎜ ⎛ 1 β λ 4 ,5 = -- V ⋅ n 1 – α + ---- ± 2 2 c ⎠ ⎟ ⎞ ⎝ ⎜ ⎛ 2 β V ⋅ n 1 – α + ---2 c 2 2 2 ( V ⋅ n) - 2 + 4 n – ----------------- β 2 c 2 (4-92) The two parameters α and β are chosen so that the stiffness of the eigenvalues is minimised at low speed. The corresponding eigenvalues for incompressible fluids are: λ 1 ,2, 3 = V ⋅ n 2 2 2 1 λ 4 ,5 = -- V ⋅ n ( 1 – α ) ± ( V ⋅ n ( 1 – α ) ) + 4n β 2 (4-93) Compared to preconditioned system of compressible fluids, the first three eigenvalues are unchanged and the eigenvalues of the acoustic waves can be obtained by setting in Eq. 4-92 the speed of sound to infinity. We note in particular that the acoustic eigenvalues are always of opposite sign showing that the flow remains subsonic with respect to the pseudo-sonic speed. As for the compressible preconditioner the two parameters α and β are chosen so that the stiffness of the eigenvalues is minimised at low speed. Note that if a k-ε model is considered, the corresponding eigenvalues will be: λi = V⋅n (4-94) k-ε 4-3.8.5 Choice of the Parameters α, β and the Reference Velocity The user control variables are P ref, T ref ,α ,β . Pref ,T ref are accessible through the Flow Model page and are referred to as reference pressure and reference temperature. A value of Tref of the order of magnitude of the expected temperature field will reduce the machine round-off errors influence on the temperature field. The value of Pref fixes the absolute level of the pressure in the field. This value is used in the equation of state for a compressible fluid and in the second order artificial dissipation term. A value of Pref close to the real pressure level is therefore recommended. The parameter α is accessible in the ‘Expert parameters’ list of the Control variables page as ALPHAP. According to several computations accomplished with the central scheme, good convergence rates were obtained for values of α lying in the range [-1,1]. So far the best value is found to be α=-1. This optimal value is not surprising since it increases the spectral radius and therefore adds an additional amount of artificial dissipation. Τhe preconditioning parameter β is imposed by the user in the Numerical Model page through a coefficient β∗ and a characteristic velocity U ref such that FINE™ 4-45 Flow Model Mathematical Model 2 2 β = β∗ U ref (4-95) U ref is representative of the maximum velocity in the flow field. For example, in external flows, Uref could be taken as the free stream velocity whereas in internal flows it could be taken as the maximum inlet velocity. For the user’s convenience, the constant Uref is however always set equal to the reference velocity specified in the Flow Model page and used in the calculation of the Reynolds Number. The choice of Uref has an influence on the convergence. The default value of β∗ is 3. Based on our experience with the presented low speed preconditioner the parameter β∗ can be taken of order unity for inviscid flow computations. For viscous computations associated with Reynolds numbers greater than about Re=1000, a constant value β∗ of order unity is also adequate. If convergence difficulties are encountered at the very beginning of a computation, it is recommended to increase the value of the parameter β∗. Remember however that a too large value of β∗ will introduce excessive artificial dissipation into the solution. For lower Reynolds number the parameter β∗ has to vary in order to preserve numerical stability and a good convergence rate. The parameter β∗ should increase as the Reynolds number decreases and may vary over several orders of magnitude (see Figure 4.3.8-4). If the local velocity scaling option is activated in the Numerical Model page, another definition of β is used: 2 2 2 β = β∗ max ( Uref, Uloc ) (4-96) where U loc is the local velocity. * β 10000 1000 100 10 1 1 10 100 1000 10000 Re FIGURE 4.3.8-4 Typical variation of the preconditioning parameter β* with Reynolds number For high Reynolds flows it is suggested to choose β among the following values: • β=3 • β=30 • β=300 Too small or too big values of β may lead to divergence and to a too dissipative solution (if β is too high) 4-46 FINE™ Characteristic and Reference Values Flow Model 4-3.8.6 References Chorin, A. J. (1967) ’A numerical method for solving incompressible viscous flow problems’, J. of Comput. Phys., Vol 2, pp. 12-26. Hakimi N. (1997) ’Preconditioning methods for time dependent Navier-Stokes equations’, PhD Thesis, Dept of Fluid Mechanics, Vrije Universiteit Brussel. 4-4 4-4.1 Characteristic and Reference Values Reynolds Number Related Information The user has to specify some characteristic values (length, velocity and density). These values are used to calculate the Reynolds Number (only plotted when the kinematic viscosity is constant) that provides an useful information to choose the suitable model (section 4-3.5). These characteristic values can be used for other purposes as well. The characteristic length is used: — in the outlet boundary condition for which the mass flow is imposed with pressure adaptation, — in the computation of CP1 and CP3 for cylindrical cases. The characteristic velocity is used: — in the preconditioning method to compute the parameter β (see section 4-3.8.5), 2 — in the computation of the solid data Cf (normalized by ( ρ ref U ref ⁄ 2 ) ). The characteristic density is used: — in the Boussinesq approximation for incompressible fluid (Eq. 4-85), 2 — in the computation of the solid data Cf (normalized by ( ρ ref U ref ⁄ 2 ) ), — in the evaluation of the Reynolds number only when the dynamic viscosity of the fluid is specified in the Sutherland law on the Fluid Model page. 4-4.2 Reference Values The reference values have been introduced for the precoditioning to define a gauge pressure and a gauge total energy. Now these reference values have some additional uses which are described hereafter: — in the Boussinesq approximation for incompressible fluid (Eq. 4-85), — in the outlet boundary condition for which the mass flow is imposed with pressure adaptation. FINE™ 4-47 Flow Model Characteristic and Reference Values 4-48 FINE™ CHAPTER 5: Rotating Machinery 5-1 Overview The Rotating Machinery page contains the following thumbnails: • Rotating Blocks defining for each block typical information concerning cylindrical cases. This thumbnail is only available when the mesh is cylindrical (see Mesh/Properties... to see whether the mesh is cylindrical or Cartesian). See section 5-2 for more detail on this thumbnail. • Rotor/Stator defining the properties of each rotor/stator interface. This thumbnail is only available when the mesh contains Rotor/Stator interfaces. Rotor/Stator interfaces are defined in IGG™ as ROT boundary condition. For more detail on this thumbnail see section 5-3. • Throughflow Blocks giving access to two-dimensional throughflow Euler simulation and this is only accessible for non-viscous flow (Euler selected as mathematical model on the Flow Model page). See Chapter 6 for more detail on the options available under this thumbnail. FINE™ 5-1 Rotating Machinery Rotating Blocks 5-2 Rotating Blocks FIGURE 5.2.0-1 Rotating Blocks on Rotating Machinery Page When selecting the Rotating Blocks thumbnail the page appears as shown in Figure 5.2.0-1. On the left a list of all blocks is displayed. It is possible to group the blocks that have the same properties on this page: 1. Select several blocks in the list of blocks by simply clicking on them. Clicking on a block deselects the currently selected block(s). It is possible to select several blocks situated one after another in the list by clicking on the first one and holding the left mouse button while selecting the next. To select a group of blocks which are not situated one after another in the list, click on each of them while keeping the <Ctrl> key pressed. Click on the Group button. A text box will appear just below the Group button. Place the cursor in the text box and type the name of the group and press <Enter>. The name of the group will appear on the list of blocks in red with a plus sign on the left of the name. To see the blocks that are included in a certain group double click on the name of the group or click on the + symbol in front of the name. To remove a group of blocks select the group and click on the Ungroup button. The group will be removed and the blocks that were in this group will be listed again in the list as separate blocks. 2. 3. On the right of the list with blocks the information is given for the selected block or group of blocks. If multiple blocks are selected the information is only displayed for the first selected block. For each block the current and maximum number of nodes in the three grid directions is given. Four items need to be defined by the user: the streamwise direction, the spanwise direction, the azimuthal direction and the rotational speed: — The streamwise, spanwise and azimuthal directions allow to determine the block orientation. Remark that if the AutoGrid module is used for the grid generation, the streamwise direction is automatically taken as being the k-direction, the spanwise direction as the j-direction and the azimuthal direction as the i-direction. — EURANUS flow solver solves the equations in a relative frame of reference. This implies that the mesh blocks surrounding rotating blades rotate with the blades and should therefore been set as "rotating" in this page. The rotational speed of the block has to be given in RPM (Revolutions Per Minute). A positive value for the rotation speed indicates a rotation in pos- 5-2 FINE™ Rotor/Stator Interaction in the FINE™ Interface Rotating Machinery itive θ-direction with θ positive according to a right handed coordinate system. In Figure 5.2.0-2 this is illustrated for the case where the z-axis is the axis of rotation which is automatically the case in a mesh created with AutoGrid. FIGURE 5.2.0-2 Positive rotation speed The different computations in a project can not have different configuration settings. If any of the settings in this area is changed, the modifications will be taken for all (active and not active) computations. The rotation axis should be the z-axis in order to be compatible with the EURANUS flow solver. 5-3 Rotor/Stator Interaction in the FINE™ Interface The Rotor-Stator thumbnail gives access to the definition of the rotor/stator interfaces as shown in Figure 5.3.0-3. This thumbnail is only accessible when the mesh contains rotor/stator interfaces. Rotor/stator interfaces are defined in IGG™ as ROT boundary condition. Consult the IGG™ manual for more detailed information on how to define this boundary condition. For more theoretical information on rotor/stator interfaces see section 5-5. The rotor/stator patches should not include R=0 regions. On the left the list of patches is displayed which are defined as part of a rotor/stator interface in IGG™ (boundary condition type: "ROT"). It is possible to display only a limited amount of patches by using the Filter. Type in the text box the part of the name that is common to all patches to display and press <Enter>. All patches containing in the name the entered text will be displayed. Note that the filter is case insensitive. It is possible to group patches that have the same definition by selecting them in the list and clicking on the Group button. A text box will appear below this button which allows to enter a name for the group. The group will be displayed in red in the list of patches. Double click on the group name to see which patches are in the group. To select multiple patches select them while keeping the <Ctrl> key pressed. To remove the group simply select the group from the list and click on Ungroup. The patches in the selected group will be put back into the list of patches and the group name will be removed from the list. FINE™ 5-3 Rotating Machinery Rotor/Stator Interaction in the FINE™ Interface Multiple rotor/stator interfaces can be treated in one single project. Each rotor/stator interface is indicated by an ID number and each of them may contain an arbitrary number of upstream and downstream patches. For each patch in the list the ID number of the corresponding rotor/stator interface has to be provided by the user. Also it should be specified whether the patch is located in the upstream or downstream side of the interface. It should be mentioned that no hypothesis is made on the direction of the flow through the interface. The purpose of the upstream and downstream denominations is only to establish the two groups of patches belonging to respectively the rotor and the stator side. .The ID number of the rotor/stator interface cannot be higher than the total number of rotor/stator interfaces. FIGURE 5.3.0-3 Rotor/stator Interface Definition In addition to the ID number and the upstream/downstream side specifications the user has to select also: • the order of extrapolation (zero or first order). Zero order extrapolation (default) is used in most cases and usually provides satisfactory results. First order extrapolation may be useful in case of important flow gradients in the direction normal to the interface together with a relatively coarse mesh. • one of the four available steady state techniques (for steady state applications only), i.e. the Local Conservative Coupling, Conservative Coupling by Pitchwise Rows, Full Non Matching Mixing plane and Full Non Matching Frozen Rotor approaches. 1. The first approach is only recommended for the rotor/stator interface between an impeller and a volute. Experience has shown that in cases where significant flow variations are observed in the circumferential direction (as for instance in the case of rotor-volute interactions) it is more stable to base the flux decomposition on the local flow direction as it is done in the Local Conservative Coupling. Small conservation errors can be observed with this technique, which is therefore only used for special configurations. 5-4 FINE™ How to Set-up a Simulation with Rotor/Stator Interfaces? Rotating Machinery 2. The second approach is recommended due to its capability to provide an exact conservation of mass flow, momentum and energy through the interface. This approach adopts the same coupling procedure for all the nodes along the circumferential direction, even if the local flow direction is different from the averaged one. This technique offers the advantage of being able to guarantee a strict conservation of mass, momentum and energy through the interface. Moreover it shows to be very robust and is therefore used by default. 3. The third approach is respecting an exact conservation of mass flow, momentum and energy through the interface as the second approach but has less constraint on the interface geometry. 4. The fourth approach is considering the rotor/stator interface as a perfect connection and is neglecting the rotor movement in the connecting algorithm. In this approach, the periodicities must be equal between the rotor and the stator. 5-4 How to Set-up a Simulation with Rotor/Stator Interfaces? Three different approaches are available in FINE™ to simulate the interaction between rotating and non-rotating blocks: Steady state: • Mixing plane approach: a pitchwise averaging of the flow solution is performed at the rotor/ stator interface and the exchange of information at the interface depends on the local direction of the flow. See section 5-4.1 for more detail on how to use this approach and section 5-5.3 and section 5-5.3 for the theoretical background. • Frozen rotor: a steady simulation of one specific position of the rotor with respect to the stator. For more information on how to set up a project according to this method see section 5-4.2. For its theoretical background see section 5-5.4.4. Unsteady: • Domain scaling method: unsteady simulation in which the mesh periodicities are constrained to be identical on both sides of the interface. See section 5-4.3 for more detail on how to use this approach and section 5-5.4 for the theoretical background. • Phase lagged method: unsteady simulation in which the mesh periodicities are not constrained to be identical on both sides of the interface. See section 5-4.4 for more detail on how to use this approach and section 5-5.3 for the theoretical background. 5-4.1 Mixing Plane Approach In the mixing plane approach the flow solution at the rotor/stator interface is azimuthally averaged and the exchange of information at the interface depends on the local direction of the flow. In this section it is described how to use this approach in FINE™. For more theoretical detail on the mixing plane approach itself consult section section 5-5.2 and section 5-5.3. 5-4.1.1 Geometrical Constraints The default mixing plane method (Local Conservative Coupling and Conservative Coupling by Pitchwise Rows) used in FINE™ imposes the following geometrical constraints: FINE™ 5-5 Rotating Machinery How to Set-up a Simulation with Rotor/Stator Interfaces? • The patches on both sides of the rotor/stator interface must cover the same range in spanwise direction, • The meshes need not to match in the spanwise direction, but the azimuthal mesh lines on the boundary must be circular arcs. An illustration of these constraints is given in Figure 5.4.1-4. Consisting of two stripes, the depicted configuration provides a complete description of the capabilities. The upstream side of the quasisteady interface consists of three blocks, represented by the bold frames and the surface meshes, while a single block is assumed for the downstream side. A gap may exist between two blocks, e.g., if the mixing plane coincides with the exit plane of a blade row having a blunt trailing edge. The grid points distribution are different for each of the boundary patches involved, but the pitchwise grid lines have constant radius and the pitchwise line along which two patches of the same side join (e.g., BC 1 and BC 3) exists as an inner grid line on all other boundaries. In the example, the interface is thus decomposed into two stripes, stripe 1, consisting of BC 1 and BC 2 on the upstream side and BC 5 on the downstream side, and stripe 2, consisting of BC 3 and BC 4 on the upstream side and BC 6 on the downstream side. . FIGURE 5.4.1-4 Example of stripe configuration A new interpolation technique (Full Non Matching Mixing plane) has been implemented to avoid those geometrical constraints. This new technique is based on the full non-matching algorithm and has clear advantages: • The geometrical constraints have been removed, the only remaining constraint being that the rotor/stator patches belonging to a given interface should lie on the same common axisymmetric surface. 5-6 FINE™ How to Set-up a Simulation with Rotor/Stator Interfaces? Rotating Machinery • An exact conservation of the mass flow, momentum and energy is guaranteed. In special configurations such as rotor-volute interaction it is preferable to use Local Conservative Coupling and thus it may be required to use the previous approach (IRSNEW=0). When setting the expert parameter IRSNEW=1 only Full Non Matching Mixing plane approach will be applied on all rotor/stator interfaces even if another mixing plane approach has been selected in the Rotating Machinery page under Rotor-Stator thumbnail. 5-4.1.2 Constraints on the Mesh Only one blade passage needs to be meshed for both the rotor and the stator, regardless of their respective periodicity. The boundary condition type must be set to "ROT" in IGG™ for all grid patches belonging to a rotor/stator interface. 5-4.1.3 Settings in FINE™ 1. 2. The mixing plane approach is a steady simulation technique which requires to set on the Flow Model page the Time Configuration to Steady. The patches that have boundary condition type "ROT" in the mesh are listed in FINE™ on the Rotating Machinery page under the Rotor-Stator thumbnail. The user has to specify for each of these patches: • an ID number that will identify the rotor/stator interface (useful when multistage), • a switch to indicate if the patch is belonging to the "upstream" or "downstream" part of the rotor/stator interface. ID = 2 Upstream Downstream Upstream Downstream ID = 1 Flow Direction FIGURE 5.4.1-5 Aachen Turbine: Upstream/Downstream and ID number identification • the boundary condition: Local Conservative Coupling, Conservative Coupling by Pitchwise Rows or Full Non Matching Mixing plane as described in section 5-3. When setting IRSNEW=1 only conservative coupling by pitchwise rows is available. Selecting local conservative coupling in the FINE™ interface will have no effect when IRSNEW=1. FINE™ 5-7 Rotating Machinery How to Set-up a Simulation with Rotor/Stator Interfaces? 5-4.1.4 Illustrative Example To illustrate the mixing plane approach the flow around a cube is considered as shown in Figure 5.4.1-6. The flow is entering the domain at the bottom of the figure. The upstream portion of the domain is the 'rotor' with a cube fixed on it. The second part is a 'stator'. Due to the pitch wise averaging process one can see that the vortex occurring slightly downstream the 'trailing edge' of the cube is spread when entering in the 'stator' component. If the rotational speed of the cube is high, this approximation is acceptable since one can consider that the stator "sees" a more statistically average flow. If the rotational speed is low, this approximation is essentially invalid and thus another method should be considered. FIGURE 5.4.1-6 Flow around a cube: Mixing Plane approach 5-4.1.5 Expert Parameters This section provides a summary of the expert parameters related to mixing plane approach. a) Selection of Technique IRSNEW = 0: default mixing plane interpolation technique imposing geometrical constraints as listed in section 5-4.1.1. = 1: new full non-matching algorithm for rotor/stator interfaces removing the geometrical constraints of the default mixing plane technique. More detail on this interpolation technique can be found in section 5-5.3. When setting IRSNEW=1 only conservative coupling by pitchwise rows is available. Selecting local conservative coupling in the FINE™ interface will have no effect when IRSNEW=1. 5-8 FINE™ How to Set-up a Simulation with Rotor/Stator Interfaces? Rotating Machinery b) Under-relaxation with Default Mixing Plane Approach NQSTDY gives the possibility to the user to update the rotor-stator boundary conditions every NQSTDY iterations. If the parameter NQSTDY is set to zero (default), the update is done at every Runge-Kutta step. This is an under-relaxation technique that is rarely used. Before the mixing process, the averaged variables can be under-relaxed to stabilize the calculation: RQSTDY= 1 (default): no relaxation = 0 to 1: under-relaxation This is another under-relaxation technique that allows to limit the changes in the variables from one iteration to the next. This technique is used in special cases where stability problems are encountered. 5-4.2 Frozen Rotor The basic idea at the origin of the frozen rotor technique consists of neglecting the rotor movement in the connecting algorithm. The governing equations are solved for the rotor in a rotating frame of reference, including Coriolis and centrifugal forces; whereas, the equations for the stator are solved in a absolute reference frame. The two components are literally connected, and hence a rotor-stator approximation is not required, rather the continuity of velocity components and pressure is imposed. As a result, the final steady solution will be depending on the relative position of the rotor and the stator. Unsteady 'history effect' (such as shedding separated zones) are neglected. It is usually well accepted that the frozen rotor approach is an appropriate solution for the treatment of rotor-volute interactions, where pitchwise variations of the flow are too important to be neglected. However, it requires the meshing of the complete impeller (all passages). Another drawback is that the flow solution depends on the rotor position. 5-4.2.1 Constraints on the Mesh Exactly as for the domain scaling approach a constraint must be satisfied on the mesh periodicity. The pitchwise distance must be the same for both side of the rotor/stator and coincident (no gap allowed between rotor and stator components in the pitchwise direction). For each different position of the rotor with respect to the stator a new mesh will have to be created in IGG™ and a new steady calculation has to be performed. 5-4.2.2 Settings in FINE™ There are three ways to run a frozen rotor calculation: 1. To mesh all blade rows completely and to use matching connections (CON) in IGG™ for the patches at the interface of the rotor and the stator. The blocks of the rotor should be made rotating, as well as the boundary conditions. A steady calculation can be run for this configuration. A non matching (NMB) connection or periodic non matching (PERNM) connection can not be used in this case: even though the computation might run the result would not be correct. This was previously the only way to perform frozen rotor calculations in FINE™. This approach is no longer used as the constraint on matching connections is too restrictive. Only CON matching connections are allowed in this first method. 2. To create a mesh covering the same pitchwise distance on both sides of the interface and to impose Full Non Matching Frozen Rotor in the Rotating Machinery page under the Rotor-Stator thumbnail. Furthermore the user has to specify for each of these patches the ID and the FINE™ 5-9 Rotating Machinery How to Set-up a Simulation with Rotor/Stator Interfaces? upstream/downstream location as described in section 5.4.1.3 at step 2. Therefore, the boundary condition type must be set to "ROT" in IGG™ for all grid patches belonging to a rotor/stator interface. 3. To start an unsteady computation by imposing iterations as a steady initialization in the Control Variables page. Note that for example for an impeller-volute computation the complete impeller would need to be meshed in all three cases since the periodicity of the volute is 1. 5-4.2.3 Illustrative Example Results obtained from frozen rotor calculations usually look similar to unsteady ones. More detailed analysis shows that the approximation introduced in the connection algorithm induces a deviation of the wake when passing through the interface. FIGURE 5.4.2-7 Aachen Turbine: Frozen Rotor approach As an illustration the frozen rotor method is compared to the sliding mesh approach for the Aachen Turbine in Figure 5.4.2-7 and Figure 5.4.2-8. FIGURE 5.4.2-8 Aachen Turbine: Domain Scaling (Sliding Mesh) approach 5-10 FINE™ How to Set-up a Simulation with Rotor/Stator Interfaces? Rotating Machinery 5-4.2.4 Expert Parameters The only expert parameter in case of a frozen rotor simulation is IRSNEW. This parameter should always be set to 2 when performing a frozen rotor simulation. 5-4.3 Domain Scaling Method The Domain Scaling Method is an unsteady simulation technique for rotor/stator interfaces. The effect of displacement due to rotation is taken into account. At each time step, the rotor is set at its correct position and equations are solved for that particular time step for the whole computation domain. The final solution is therefore a succession of instantaneous solutions for each increment of the rotor position. 5-4.3.1 Constraints on the Mesh The boundary condition type must be set to "ROT" in IGG™ for all grid patches belonging to a rotor/stator interface. The blade passages of each blade row to include in the mesh should cover the same pitch distance (have the same periodicity). If the periodicity of the rotor and the stator is not the same this can be solved in three different ways: • modelling a higher number of blade passages on each side to find a common periodicity, • scaling the geometry (with the scaling being as close to 1 as possible). The common way to scale the geometry is to modify the number of blades during the mesh generation process. The time frequencies are resolved with an error that is proportional to the scaling coefficient. • using the phase lagged approach explained in section 5-4.4. Apart from this constraint on the periodicity, there is no constraint on the patches and mesh nodes configurations. 5-4.3.2 Settings in FINE™ 1. 2. Domain Scaling Method is an unsteady simulation technique so the Time Configuration in the Flow Model page should be set to Unsteady. By default, in the Rotating Machinery page under Rotor-Stator thumbnail, the Domain Scaling approach is selected. However the user has to specify for each of these patches the ID and the upstream/downstream location as described in section 5.4.1.3 at step 2. Therefore, the boundary condition type must be set to "ROT" in IGG™ for all grid patches belonging to a rotor/stator interface. The initialization process can be performed in two ways: 3. • A steady state initialization is performed in a separate computation with steady Time Configuration. It is suggested to model all rotor/stator interfaces in this case using frozen rotor approach. The unsteady domain scaling computation is using the result of this steady computation as initial solution. See Chapter 10 for more information on how to start a computation from an initial solution file. • The steady state initialization is automatically performed before starting the time accurate computation (that means within the same computation), switching to unsteady Time Configuration in the Flow Model page and selecting in the interface an appropriate Number of Steady Iterations in the Steady Initialization parameters on the Control Variables page. 4. 5. 6. The Number Of Angular Positions is defined in the Control Variables page. The Number Of Time Steps is defined in the Control Variables page. The Outputs Files available in the Control Variables page are: FINE™ 5-11 Rotating Machinery How to Set-up a Simulation with Rotor/Stator Interfaces? • Output For Visualization/At end only and Multiple Files: multiple set of output files saved for restart of the unsteady computation and visualization in CFView™ only available at the end of the computation. • Output For Visualization/At end only and One Output File: one set of output files saved for restart of the unsteady computation and visualization in CFView™ only available at the end of the computation. • Output For Visualization/Intermediate and Multiple Files: multiple set of output files saved for restart of the unsteady computation and visualization in CFView™ during the computation. • Output For Visualization/Intermediate and One Output File: one set of output files saved for restart of the unsteady computation and visualization in CFView™ during the computation. IRSNEW =1 to activate the full non-matching interpolation algorithm at the rotor/stator interface. This is in general recommended since it requires less memory and significantly reduces the pre-processing time. It also offers the advantage that conservation of mass, momentum and energy is guaranteed. Note: When a sliding mesh simulation with IRSNEW=1 is started from a mixing plane simulation with IRSNEW=0 it is not possible to use the *.fnmb file of the mixing plane simulation to read in the initialization of the sliding mesh simulation. It is necessary to compute the full non-matching connections again. 5-4.3.3 Illustrative Example For the example case of the flow around a cube where the flow is entering the domain at the bottom of Figure 5.4.3-9. The upstream portion of the domain is the 'rotor' with a cube fixed on it. The second part is a 'stator'. With domain scaling approach, one can observe a strong vortex shed into the stator passage, leading to a correct physical simulation of the unsteady phenomenon (at the expense of much higher CPU time compared to mixing plane approach). FIGURE 5.4.3-9 Flow around a cube: Domain Scaling method 5-12 FINE™ How to Set-up a Simulation with Rotor/Stator Interfaces? Rotating Machinery 5-4.3.4 Expert Parameters The following expert parameters can be used with an unsteady computation using domain scaling method: IRSNEW = 0 (default): old interpolation method at the rotor/stator interface IRSNEW = 1: full non-matching interpolation at the rotor/stator interface. This is in general recommended since less memory is required. Parameters for Saving/Reading of Pre-Processing Data: When IRSNEW = 0 (default approach): ISIDAT = 1 (default): pre-processing performed and results saved in the file with extension ".burs". ISIDAT = 2: pre-processing not performed, results read in the file with extension ".burs". When IRSNEW = 1 (new approach): IFNMFI =1 (default): pre-processing performed and results saved in .fnmb file. IFNMFI =2: pre-processing not performed and results read from .fnmb file. In both cases the pre-processing needs to be restarted if either the Number Of Angular Positions or the number of grid levels is changed. ICYOUT =1 is used in combination with Multiple Files option to avoid overwritting of the output files at each blade passage. 5-4.4 Phase Lagged Method The Phase Lagged Method is an unsteady simulation technique for rotor/stator interfaces. The effect of displacement due to rotation is taken into account. At each time step, the rotor is set at its correct position and equations are solved for that particular time step for the whole computation domain. The final solution is therefore a succession of instantanious solutions for each increment of the rotor position. This method is allowing the user to reduce the CPU time needed for computing an unsteady simulation of a turbomachinery stage (rotor-stator interaction). This capability has been implemented as an additional functionality into the release FINE™/Turbo. 5-4.4.1 Constraints on the Mesh The only constraints is that the boundary condition type must be set to "ROT" in IGG™ for all grid patches belonging to a rotor/stator interface. It is recommended to have an overlapping in the circumferential direction between the channel(s) of the rotor and the channel(s) of the stator. 5-4.4.2 Settings in FINE™ 1. 2. Phase Lagged Method is an unsteady simulation technique so the Time Configuration in the Flow Model page should be set to Unsteady. At the top of the Rotating Machinery page, the Phase Lagged option has to be activated and under RotorStator thumbnail, the Phase Lagged approach is selected automatically. However the user has to specify for each of these patches the ID and the upstream/downstream location as described in section 5.4.1.3 at step 2. Therefore, the boundary condition type must be set to "ROT" in IGG™ for all grid patches belonging to a rotor/stator interface. The initialization process can be performed in two ways: 3. FINE™ 5-13 Rotating Machinery How to Set-up a Simulation with Rotor/Stator Interfaces? • A steady state initialization is performed in a separate computation with steady Time Configuration. It is suggested to model all rotor/stator interfaces in this case using frozen rotor approach. The unsteady domain scaling computation is using the result of this steady computation as initial solution. See Chapter 10 for more information on how to start a computation from an initial solution file. • The steady state initialization is automatically performed before starting the time accurate computation (that means within the same computation), switching to unsteady Time Configuration in the Flow Model page and selecting in the interface an appropriate Number of Steady Iterations in the Steady Initialization parameters on the Control Variables page. 4. The Number Of Angular Positions defined in the Control Variables page is the number of time step per full revolution (2π) of the rotor. In theory, the number of time step per full rotation has to be a multiple of the number of blades in the rotor (Nbrotor) and number of blades in the stator (Nbstator). Number Of Angular Positions = i x Nbrotor x Nbstator The two periods of blade passing frequencies are respectively (ixNbrotorx∆t) and (ixNbstatorx∆t). Since the number of time step per passage is usually imposed around 40, the value of i should be adjusted so that (ixNbrotor) and (ixNbstator) are both close to this number. By experience, if the number of time step per passage is lower than 30 the solution starts to be deteriorated. 5. The Number Of Time Steps in the Control Variable page is defined as: Number Of Time Steps = j x (Number Of Angular Positions)/min(Nbrotor,Nbstator) During the calculation, it is recommended to repeat the longer period at least 15 to 20 times (j evolves from 15 to 20). By experience, usually after 20 times (j=20), the flow becomes periodic. There are thus no need to make many full rotation and sometimes even one full rotation. 6. The Outputs Files available in the Control Variables page are: • Output For Visualization/At end only and Multiple Files: multiple set of output files saved for restart of the unsteady computation and visualization in CFView™ only available at the end of the computation. • Output For Visualization/At end only and One Output File: one set of output files saved for restart of the unsteady computation and visualization in CFView™ only available at the end of the computation. • Output For Visualization/Intermediate and Multiple Files: multiple set of output files saved for restart of the unsteady computation and visualization in CFView™ during the computation. • Output For Visualization/Intermediate and One Output File: one set of output files saved for restart of the unsteady computation and visualization in CFView™ during the computation. By default, the Phase Lagged method used to compute the viscous fluxes at the rotor/ stator interface from dummy cells values set from other side inner cells instead from same side inner cells by extrapolation (more detail in section 5-5.4.3). 5-14 FINE™ Theoretical Background on Rotor/Stator Interfaces Rotating Machinery 5-4.4.3 Illustrative Example Results obtained from Phase Lagged calculations usually look similar to unsteady ones when the expert parameter IRSVFL=1. Old Viscous Fluxes Detection at R/S interface IRSVFL = 0 New Viscous Fluxes Detection at R/S interface IRSVFL = 1 FIGURE 5.4.4-10 Aachen Turbine: Domain Scaling method: IRSVFL=0 vs IRSVFL=1 5-4.4.4 Expert Parameters The following expert parameters can be used with an unsteady computation using phase lagged method: ICYOUT =1 is used in combination with Multiple Files option to avoid overwritting of the output files at each blade passage. RELPHL =0.5 0.5 if necessary, under-relaxation factor can be applied on Periodic and R/S boundary conditions by reducing the two values of the expert parameter for respectively the periodic and the R/S boundary conditions. NPLOUT =0 (by default) enables to visualize multiple non periodic passage output in CFView™ by loading the corresponding ’.cfv’ file. 5-5 Theoretical Background on Rotor/Stator Interfaces 5-5.1 Introduction The relative motion between successive blade rows together with boundary layers, wakes, shocks and tip leakage jets are the major sources of unsteadiness that may affect a turbomachinery flow locally or as it travels through the next rows. All these interactions are strongly coupled, increasing in magnitude as the gap between successive blade rows is decreased, and affecting consequently the performance of the machine. FINE™ 5-15 Rotating Machinery Theoretical Background on Rotor/Stator Interfaces Solving for such flows requires an unsteady and viscous flow solver with the capability to manage enormous data storage. One way to optimize the computer memory requirement is to resolve the steady flowfield on a truncated computational domain. This requires a pitchwise averaging process to be performed at the so-called rotor/stator interfaces. This particular boundary condition is available under the FINE™/Turbo environment as the mixing plane approach. The rotor-stator interaction is done by exchanging circumferentially averaged flow quantities. Physically, this means that the blade wake or separation occurring in the blade passage are mixed circumferentially before entering the downstream component. As a result, the velocity components and pressure is uniform in the circumferential direction at the rotor/stator interface. This physical approximation tends to become more acceptable as rotational speed is increased. This mixing plane technique is by far the most used rotor/stator modeling in industry approach. See section 5-5.2 and section 5-5.3 for more detail on the mixing plane approach. The second step allowing for a higher level of accuracy consists of considering an unsteady rotor/ stator interaction. Various techniques allowing to treat configurations with an arbitrary number of blades in the rotor and the stator have been proposed by many authors (Giles, 1990, Lemeur, 1992, Erdos et al, 1977, He, 1997), each of them having their own advantages and disadvantages, each of them affecting differently the memory requirement, solution time and the most important parameter, the accuracy of the computed flow solution. But none of these techniques allows to resolve on a truncated computational domain all time frequencies present in the turbomachinery configuration, except if the pitch distance is the same in the successive rotors and stators. In fact, each of them are affecting the computed time frequencies and Fourier modes that are propagating the flow information inside the gap region. The Domain Scaling Method is another type of unsteady rotor/stator interface treatment (Rai, 1989), that has been selected and implemented in the EURANUS flow solver. This technique is based on the constraint that the pitch distance must be identical on both sides of the interface. If the numbers of blades in the rotor and the stator are different, this implies either to increase the number of passages modelled or to scale the geometry. The Domain Scaling Method presents the advantage that it allows to resolve all time frequencies with an error that is proportional to the scaling coefficient. The accuracy of the computed unsteady flow solution may then be improved at the expense of more data storage and larger solution time if more blade passages are considered. Finally, the Phase Lagged Method is the last type of unsteady rotor/stator interface treatment that has been selected and implemented in the EURANUS flow solver. This technique is removing the Domain Scaling constraint that the pitch distance must be identical on both sides of the interface. The Phase Lagged Method presents the advantage that it allows to resolve all time frequencies with an error that is proportional to the scaling coefficient. The accuracy of the computed unsteady flow solution may then be improved at the expense of more data storage and larger solution time if more blade passages are considered. 5-5.2 Default Mixing Plane Approach 5-5.2.1 Geometrical and Topological Constraints The rotor-stator interfaces are defined by stripes. A stripe is the element along which the required averaging in tangential direction is carried out. It is composed of a number of boundary patches which must cover the same range in the spanwise direction. The upstream and the downstream sides are distinguished. Each boundary condition must belong either to the upstream or to the downstream side. These two sides communicate through the exchange of pitch-averaged variables. The meshes do not need to match in the spanwise direction, but the azimuthal mesh lines on the boundaries must be circular arcs. 5-16 FINE™ Theoretical Background on Rotor/Stator Interfaces Rotating Machinery 5-5.2.2 Communication Process On both sides, the flow state is extrapolated from the inner cells onto the interface. It is then interpolated onto meshes that share the same spanwise grid point distribution on both sides. The pitchwise averaging is carried out on those meshes and the mixing process, depending on the boundary condition type, is applied. This mixing process combines the variable on one side of the interface with the pitchwise averaged variables of the other side. Once the mixing process is completed, the flow state is interpolated back onto the initial mesh interface and the dummy cells are set to impose the calculated variables on the interface. The extrapolation of the flow state from the inner cells onto the interface can be done using different techniques. These are the same as those used by the outlet boundary conditions exposed in section 8-5. Before the mixing process, the averaged variables can be underrelaxed to stabilize the calculation. The relaxation factor is user input (RQSTDY), the default value being 1, which means that no under-relaxation is performed in the default configuration of the solver. The possibility is given to the user to update the rotor-stator boundary conditions every NQSTDY iterations. If the parameter NQSTDY is set to zero (default), the update is done at every Runge-Kutta step. 5-5.2.3 Different Available Boundary Conditions The rotor/stator interface included in the EURANUS flow solver exchange the mass, momentum, and energy fluxes instead of the classical primitive variables. The advantage of a flux-based approach is that a more strict global conservation through the interface is ensured. Two kinds of boundary conditions are currently available and are described in this paragraph: • The local conservative coupling (with flux decoding), • The conservative coupling by pitchwise rows (no flux decoding). a) Local Conservative Coupling (With Flux Decoding): On each mesh point of both sides of the interface, a test is done to detect whether the interface can be considered as a sub- or supersonic in- or outlet. Then a transfer of the fluxes and pressure from the other side is performed depending on the result of the test. • If the side is considered as a supersonic inlet, all the averaged fluxes from the other side are taken with the averaged pressure. • If the side is considered as a subsonic inlet, the averaged fluxes are taken from the other side. The local pressure is kept. • If the side is considered as a subsonic outlet, only the pressure is transferred from the other side. The local fluxes are kept. • If the side is considered as a supersonic outlet, nothing is taken from the other side. Once the transfer is completed, a decoding of the fluxes with pressure is carried out on each side with the formulas which depend on the type of fluid. Compressible flows For compressible flows, the density, velocity vector and pressure are derived from Q ρ, Q v, Q E , respectively the flux of mass, the flux of momentum plus the pressure force and the flux of energy. The other variables such as k or ε are also derived from their fluxes. They are referred to, in the following as X an QX. The fluxes are constructed from the primitive variables using: FINE™ 5-17 Rotating Machinery Theoretical Background on Rotor/Stator Interfaces Qρ = ρ ( V ⋅ S ) Q v = ρV ( V ⋅ S ) Q E = ρ ( CpT + V ⁄ 2 ) ( V ⋅ S ) Q X = ρX ( V ⋅ S ) where ρ is the density, V the absolute velocity vector, T the temperature, Cp the heat capacity and S the surface vector of the cell face. After application of the mixing process the primitive variables are calculated from the fluxes using: Qv ⋅ S p s = --------------------- ± 2 S (γ + 1) Qv – ps S v = ------------------Qρ Qρ ρ = --------v⋅S QX X = -----Qρ where γ is the specific heat ratio. Incompressible flows For incompressible flows, the velocity vector and pressure are derived from Q ρ, Q v , respectively the flux of mass and the flux of momentum plus the pressure force (See Eq. 5-1). The other variables like k or ε are also derived from their fluxes. They are referred to, in the following, as X and QX. As far as the energy equation is concerned, the temperature is also derived from its flux like the other X variables. ( Qv ⋅ S – Qρ ⁄ ρ ) p s = -------------------------------------2 S ( Qv – ps S ) V = -----------------------Qρ QX X = -----Qρ (5-3) 2 2 . (5-1) b) Conservative Coupling by Pitchwise Rows (No Flux Decoding): The local conservative coupling approach presents two weaknesses: • The decoding of the fluxes might in some case lead to a blow up of the process, especially at transonic flow conditions, because of the presence of a square root in Eq. 5-2, whose positivity is not always guaranteed. • The local approach may lead to opposite decisions on the flow direction for the corresponding mesh points of both sides of the interface, which as a consequence decreases the accuracy on the global conservation. 5-18 ⎠ ⎟ ⎞ Qv ⋅ S --------------------2 S (γ + 1) 2 · 2 ( γ – 1 ) ( Q v – ( 2Q ρ Q E ) ) + ---------------------------------------------------------2 S (γ + 1) ⎝ ⎜ ⎛ (5-2) FINE™ Theoretical Background on Rotor/Stator Interfaces Rotating Machinery Therefore a new boundary conditions has been developed, in which the decision on the direction of the flow is taken only once per pitchwise row, and which avoids the fluxes decoding. This new boundary condition has shown to be more robust in most cases and guarantees a strict global conservation. As mentioned in section 5-3 the only type of application for which a local approach would better suit is the impeller-volute interaction. 5-5.3 Full Non-matching Technique for Mixing Planes 5-5.3.1 Concept The major purpose of the development of the new mixing plane module was the elimination of the geometrical constraints imposed by the previous module. The new module uses the concept of image. An image of the real mesh patches is built on both sides of the interface, the left and right images respecting the above constraints and being in addition matching in the spanwise direction. The only remaining constraints are the followings: • the hub and the shroud lines are assumed to be located on a circular arc, and each extremity of the hub and shroud lines should coincide with one corner of one of the patches. • all patches constituting a rotor/stator interface should form a filled closed surface with no gap • the rotor/stator patches should be fully included in the rotor/stator interface: contrary to the full non matching algorithm, which includes an automatic detection of the connection zone, and in which the patches can then be partially connected, the rotor/stator module assumes that the patches are fully connected. FIGURE 5.5.3-11 Creation of the image mesh One image mesh is constructed on both sides of the interface. It respects the following constraints: FINE™ 5-19 Rotating Machinery Theoretical Background on Rotor/Stator Interfaces • The image is a "concatenation" of all the patches constituting the left or right side of the interface. • The pitchwise mesh lines lie on circular arcs. • The left and right images have the same spanwise distribution of the nodes. • The mesh density of the image is similar to the one of the initial patch. The creation of the image mesh is illustrated by Figure 5.5.3-11, showing the creation of the image of a butterfly configuration. With the previous version of the mixing plane module such a configuration would have required the creation of an intermediate block with one face connected to the butterfly and the opposite face respecting the constraints of rotor/stator patches. 5-5.3.2 Implementation of Mixing Plane Approach with Full Nonmatching Technique The communication algorithm between rotors and stators is organised in several steps: 1. 2. Extrapolation of the flow solution from the inner cells to the boundary: the cylindrical velocity components are extrapolated. Sending of the flow solution from the initial mesh to the image (on both sides): an interpolation tree is built between the image and the initial mesh, by applying the full non matching connecting algorithm. Application of the mixing plane algorithm between the left and right images, with construction of flux variables to be imposed on the left and right side. Sending of the fluxes from the image to the initial meshes: this is again performed with the aid of the full non matching algorithm, which allows for an exactly conservative distribution of the calculated fluxes throughout the cells. The transformation of the flux variables to the primitive ones is not required, as the fluxes are directly added to the residuals of the finite volume scheme, without the use of the dummy cells. 3. 4. The mixing plane algorithm implementation is similar to the one of the previous module. Only the conservative coupling by pitchwise rows has been implemented. The algorithm is organised under the following steps: 1. Calculation of the flux variables on both sides F 1 = ρV n ∆S F 2 = ρV r V n ∆S F 3 = ρV θ V n ∆S F 4 = ρV z V n ∆S F 5 = ρHV n ∆S 2. 3. For all spanwise positions perform a pitchwise averaging of the flux and of the primitive variables. For all spanwise positions determine the upstream and downstream side according to the flow direction, and build the mixing plane fluxes. 5-20 FINE™ Theoretical Background on Rotor/Stator Interfaces Rotating Machinery The local fluxes on the upstream side are taken from the upstream, with a contribution of the averaged downstream static pressure.: F1 F2 F3 ups ups = F1 ups down = F2 + p = F3 ups ups ups n r ∆S ups ups F4 = F4 + p = F5 ups down n z ∆S F5 ups On the downstream side the local fluxes are taken as the averaged fluxes on the upstream side with a contribution of the local static pressure: F1 F2 F3 down down = F1 ups down = F2 + p = F3 ups ups ups n r ∆S down down F4 = F4 + p = F5 ups down n z ∆S F5 down 5-5.4 Domain Scaling Method The Domain Scaling Method considers in the computational domain respectively K1 and K2 blade passages with the following condition to be satisfied: K1 P1 = K2 P 2 . (5-4) where the indices 1 & 2 refer to the upstream and downstream sides of the interface, and P1 & P2 are the pitches of the two connected blade rows. If the numbers of blades in respectively the rotor and the stator are not equal, the user should make the choice between: • modelling a higher number of blade passages (or even the entire machine if a common multiple can not be found). If for instance the numbers of blades are 16 & 24, the numbers of passages to model are respectively 3 & 2. This permits to avoid the introduction of an error due to the geometry scaling, at the cost of an increased memory requirement. • scaling the geometry. The easiest way to proceed in order to obtain the required scaling is to generate a mesh with a blade number different from the real one. The ratio between the modified and the real blade numbers should be as close as possible to 1.0. In some cases the most appropriate treatment may be a combination of the 2 above approaches. If for instance the numbers of blades are 18 & 24, one could scale the stator by changing the number of blades from 18 to 16, and then choose to model 2 & 3 passages. The scaling factor is then 1.125, instead of 1.33 in case only one blade passage is modelled. The major advantage of having the same pitch distance on both sides of the interface is that it permits to avoid considering any time periodicity in the boundary condition treatment. The boundary conditions to be imposed along the periodic boundaries inside the gap region are given by FINE™ 5-21 Rotating Machinery Theoretical Background on Rotor/Stator Interfaces U i ( r, θ i , z, t ) = U i ( r, θ i ± p, z, t ) R R R R i = 1, 2 , (5-5) where p = K 1 P 1 is the pitch distance on both sides of the interface. The “+” sign is to be used when imposing boundary conditions on the lower periodic segment (minimum azimuthal coordinates) and the “-” sign is to be used for the higher periodic segment (maximum azimuthal coordinates). Along the rotor/stator interface, the boundary condition is defined as Ui R(i) ( r, θ i R(i) , z, t ) = U 3 – i ( r, θ i R(i) R(i) – mp, z, t ) R(i ) m∈Z i = 1, 2 , (5-6) where the parameter m is selected such that the point θ i – mp is part of the computational domain of row 3-i to allow for the interpolation across the interface. Since only the spatial periodicity is accounted for in the connecting boundary condition, the periodic surfaces become simple nonmatching rotating boundaries, while the interface is a non-matching connecting boundary. The solution procedure is then as follows, for each physical time t: • Rotate the grid in function of the physical time step and of the rotation speed of each row. • Resolve the flowfield at the given physical time t. The boundary conditions to be imposed along the periodic segments are defined by equation Eq. 5-5. The boundary condition to be imposed along the interface boundary is defined by equation Eq. 5-6. • Save the flow solution for future post-processing. This method does not impose any time periodicity in the boundary condition treatment and thus, allows to capture all time frequencies of the various unsteady interactions, but occurring on a modified geometry due to the grid scaling. The effect of the grid scaling on the accuracy of the computed flow solution is of great importance when comparing computational results with the experimental data, as another one-stage configuration has been truly resolved. These effects may be summarized as: • a shift in the spectrum of time frequencies for the blade row that has not been scaled. • the modification in both blade rows of the Fourier modes that are propagating the flow information. The unsteady governing flow equations are resolved in the relative system of each row. Thus, no grid rotation needs to be performed at each physical time step and only the interpolation data structure needs to be modified in function of the relative position of each component. For example, a downstream rotor will see an upstream stator moving in the opposite direction of its own rotation velocity, while the upstream stator will see the rotor moving in the direction of the rotor rotation velocity. Finally, the previous implementation lets the rotor do the full rotation. The problem in this method is that the rotor and the stator are in front of each other for a little fraction of time. During this time, no time shift is necessary at the R/S interface which acts then as a pure connection. The modification proposed aims at increasing the time during which the R/S interface acts as a connection. To perform this, only the periods during which the rotor and the stator are in front of each other, are repeated. But, since the length of the periods are different in the 2 blades rows, the solution has to be stored and reset in the row with the smallest period. Example: if row 1 has the highest number of blades and therefore is submitted to the larger period, this last period T1 is repeated over and over, while a fractional number of periods will be simulated in row 2. The solution is thus stored at the end of the last completed period in row 2, to be reused at the beginning of each T1. This method increases a lot the speed of exchange between the two blade rows. It increases also the robustness of the computation. 5-22 FINE™ Theoretical Background on Rotor/Stator Interfaces Rotating Machinery 5-5.4.1 Full Non-matching Approach (IRSNEW=1) It is highly recommended to activate the FNMB approach when using the domain scaling method as it presents several advantages: • smaller pre-processing CPU time, • smaller memory requirement, • strict conservation of mass, momentum and energy. The implementation is practically identical to the one that is adopted in the steady state frozen rotor approach. The FNMB connecting algorithm is used in order to exchange the flow variables and fluxes between the left and right image. The difference in the case of unsteady calculations is that the boundary condition patches linked to the rotor side need to be positioned according to the current time step. This implementation is organised in nearly the same way as the mixing plane approach, except from the fact that the mixing plane technique applied between the two image must be replaced by an additional full non-matching connection. The global organisation is the following: 1. 2. 3. 4. Extrapolate the inner flow solution to boundary condition patches (on both sides), Interpolate the flow solution from initial patches to the image (on both sides), Full non-matching connection between the two images (with appropriate rotation of the rotorlinked image), Transfer of the calculated fluxes to the initial boundary condition patches. 5-5.4.2 Sliding Grid Interpolation Approach (IRSNEW=0) The sliding grid interpolation approach is still available (IRSNEW=0), mainly for backward compatibility reasons. This connection algorithm is based on a high order interpolation of the flow variables. Although well validated the approach does not strictly guarantee conservation. Another drawback is that different interpolation data structures are built for all relative stator/rotor positions, with as a consequence a very long pre-processing time. 5-5.4.3 Improved Rotor/Stator Viscous Fluxes (IRSVFL=1) The previous implementation of the R/S interface only ensured the continuity of the inviscid fluxes. The viscous fluxes were computed at the interface from the value in the dummy cells which were extrapolated from the inner cells. This new implementation simply interpolates the value from the other side inner cells to the dummy cells, reproducing the correct behaviour of a connection (Figure 5.5.4-12). FIGURE 5.5.4-12 Rotor/stator interface improvement: viscous fluxes continuity FINE™ 5-23 Rotating Machinery Theoretical Background on Rotor/Stator Interfaces X’ and X” are respectively extrapolated on R/S interface from X3 and X4. Then X2’ is interpolated from X’ and X”. Finally, X2” is defined in the dummy cell by extrapolating X2 (result coming from the stator) and X2’ (result coming from the rotor). This last method, automatically activated when dealing with phase-lagged simulation, can be activated for non phase-lagged simulation through the expert parameter IRSVFL (by default set at 0) that has to be set at 1. 5-5.4.4 Frozen Rotor The frozen rotor technique consists of a simple connecting boundary condition, ignoring the rotation of the rotor. The implementation is identical to the one adopted in the full non-matching domain scaling approach (section 5-5.4.1), except from the fact that no rotation of the rotor-linked image is performed, allowing the creation of a steady-state solution. 5-5.4.5 References Erdos J.I., Alzner E. & McNally W. (1977), Numerical Solution of Periodic Transonic Flow Through a Fan Stage, AIAA Journal, Vol. 15, No. 11, pp. 1559-1568 Giles M.B. (1990), Stator/Rotor Interaction in a Transonic Turbine, Journal of Propulsion, pp. 621627 He L. (1997), Computational Study of Rotating-Stall Inception in Axial Compressors, Journal of Propulsion & Power, Vol. 13, No. 1, pp. 31-38 Lemeur A. (1992), Calculs 3D stationnaire et instationnaire dans un étage de turbine transonique, AGARD Report CP-510 Rai M.M. (1989), Three-Dimensional Navier-Stokes Simulations of Turbine Rotor-Stator Interaction; Part I - Methodology and Part II - Results, Journal of Propulsion, Vol. 5, No. 3, pp. 305-319 Van Leer B. (1985), Upwind-Difference Methods for Aerodynamic Flows Governed by the Euler Equation, Lectures in Applied Mathematics, Vol. 23, Part 2, AMS, Providence, pp. 327-336 5-24 FINE™ CHAPTER 6: Throughflow Model 6-1 Overview The Throughflow module is intended for the design and the analysis of turbomachinery flows. This kind of simulation is based on the two-dimensional steady state axisymmetric Euler equations with a specific model for blade rows. It is fully integrated in EURANUS, the three-dimensional EulerNavier-Stokes flow solver. As a consequence: • Options that apply to comparable 3D calculations also apply to throughflow calculations: the physical fluid model, the boundary conditions, the spatial and time discretization, the convergence acceleration techniques and the output, including data for visualization. • The code accepts any number of blade rows. • Throughflow blocks can be combined with 3D blocks in a single computation. • Any improvement introduced in the 3D solver also applies to the througflow blocks. The throughflow simulation should be used only with the perfect gas model currently available through the FINE™ interface. The throughflow simulation can be activated directly from the FINE™ interface by clicking on the Throughflow Blocks thumbnail in the Configuration/Rotating Machinery page. This thumbnail is only accessible when the Mathematical Model is set to Euler on the Flow Model page. In the next section the Throughflow Blocks option in the FINE™ interface is described including all related parameters. Finally, section 6-5 provides its theoretical background. FINE™ 6-1 Throughflow Model Throughflow Blocks in the FINE™ Interface 6-2 Throughflow Blocks in the FINE™ Interface When selecting this thumbnail the page as displayed in Figure 6.2.0-1 is appearing. Two sections are displayed: Global parameters and Block dependent parameters. The global parameters affect all throughflow blocks, while the block dependent parameters can be tuned independently for each throughflow block. FIGURE 6.2.0-1Throughflow Blocks in Rotating Machinery page 6-2.1 Global Parameters The Global parameter for the throughflow method only concern the time discretization of the blade force equation (see section 6-5.1). The relaxation factor determines the amplitude of the blade force updates and can be interpreted as a CFL number whose value can be different from the one that is adopted for the other equations. The default value is 1. The optimal value usually varies between 0.5 and 5. Higher values result in faster convergence, but can lead to divergence if the stability limit is exceeded. 6-2.2 Block Dependent Parameters The Block dependent parameters section is subdivided into two areas. The left area is dedicated to the block selection. The right area allows to specify the throughflow parameters for the selected block(s). The Apply to Selection button assigns to the selected block(s) the values of the parameters specified in the right area. One or several blocks may be selected in the left area by simply clicking on them. Clicking on a block unselects the currently selected block(s). Clicking on several blocks while simultaneously pressing the <Ctrl> key allows to select a group of blocks. 6-2.2.1 Block Type: Throughflow or 3D Two toggle buttons are provided to specify the block type: 3D or Throughflow. The 3D choice disables the throughflow method for the selected block(s). This is the default. It is also the required setting for 3D blocks coupled with throughflow blocks in a single computation. Each throughflow block contains exactly one blade row, with a mesh configuration that corresponds to the one prescribed in section 6-2.3. 6-2 FINE™ Throughflow Blocks in the FINE™ Interface Throughflow Model Two different types of throughflow blocks are available. The throughflow module is fully active by selecting either the Compressor or Turbine options. The difference between the two lies in the definition of the loss coefficient: for a turbine the pressure used as reference is taken at the trailing edge and for a compressor at the leading edge. 6-2.2.2 Analysis or Design Mode Two main working modes are available: • Classical Analysis: the blade geometry is known, and the user specifies the relative flow angle distribution along the trailing edge. The leading edge flow angle distribution results from the calculation and the user specifies the type of streamwise distribution to be used between the leading and trailing edges. • Design: the user specifies the relative tangential velocity distribution along the trailing edge, and the throughflow module is used to compute the flow angles and hence to define the blade geometry. The leading edge tangential velocity distribution results from the calculation and the user specifies the type of streamwise distribution to be used between the leading and trailing edges. Two additional analysis modes are provided to the user, more appropriate than the classical one in some cases: • Hybrid Analysis mode: similar to the classical analysis mode, but the user specifies the streamwise distribution of the tangential velocity instead of the flow angle, which has shown to provide more accurate results especially at transonic conditions. • analysis mode with Throat Control: this mode permits to impose the throat section instead of the tangential thickness, which is more appropriate in case of high relative flow angles with respect to the axial direction (high turning turbine blades for instance). In this working mode the user has to specify the flow angle distributions along both leading and trailing edges. In all working modes the user has to specify: • the blockage distribution (tangential thickness of the blades) or the throat section. • the relative flow angle (analysis) or relative tangential velocity (design) at the trailing edge • the value of the loss coefficient along the trailing edge. Depending on the chosen analysis or design mode the appropriate parameters are available under the three thumbnails described in the next paragraphs. 6-2.2.3 Number of Blades When the block type throughflow is selected, the number of blades needs to be specified for each throughflow block presenting a grid recommended periodicity of 360 (α = 1o), with a mesh configuration that corresponds to the one prescribed in section 6-2.3. 6-2.2.4 Blade Geometry When clicking on the Blade geometry thumbnail the parameters as shown in Figure 6.2.2-2 appear. In the case the analysis mode with Throat Control is selected different parameters will appear as shown in Figure 6.2.2-3 and described at the end of this paragraph. FINE™ 6-3 Throughflow Model Throughflow Blocks in the FINE™ Interface FIGURE 6.2.2-2Blade Geometry Parameters in Design, Classical or Hybrid Analysis mode In all modes except the analysis mode with Throat Control the geometry can be defined by: • 2D input file: the file defining the blade geometry should contain the (Z,R,θcl,θss,θps) coordinates of the blade camber line, suction and pressure sides throughout the meridional domain covered by the blade. For each (Z,R) meridional position the circumferential coordinate θ is given at the camber line, the suction and pressure sides. For the format of a 2D input file see section 6-3. • 1D input parameters where the user specifies: — the streamwise location of the maximum thickness at hub and shroud (a linear evolution is assumed from hub to shroud), — a file containing the spanwise distribution of maximum tangential thickness, — the normalised streamwise distribution of blade thickness: This distribution can be computed using a power function whose exponent has also to be specified or loaded from a 1D input file with the format as specified in section 6-3. For most configurations a power function with an exponent of 2 leads to a correct modelling of the blade generating a quadratic thickness evolution. The thickness function is set to zero at the leading and trailing edges and presents a maximum at the prescribed position of maximum thickness. An additional blockage can be introduced to take the endwall boundary layers (Endwall boundary layer and wake blockage factors) into account. The two real parameters refer to the inlet and outlet values of the endwalls blockage. A linear variation is assumed between the inlet and the outlet. 6-4 FINE™ Throughflow Blocks in the FINE™ Interface Throughflow Model FIGURE 6.2.2-3Blade geometry parameters in Throat control Analysis mode In case the analysis mode with Throat Control is selected the user specifies the streamwise evolution of the effective blockage, which results from the tangential blockage and the flow angle beff= b cosβ, with b the tangential blockage and β the relative flow angle at the trailing edge. The user specifies: — the streamwise location of the throat at hub and shroud. If a negative value is entered, it is assumed that there is no throat and a linear evolution of the effective blockage from the leading to the trailing edge will be adopted. — a file containing the spanwise distribution of the throat section. The throat is by definition the section in which the effective blockage is minimum. In transonic turbines it determines the mass flow. — the normalised streamwised distribution of effective blockage: This distribution can be computed using a power function whose exponent has also to be specified, or loaded from an input file. The streamwise distribution of effective blockage results from the values specified by the user at the leading and trailing edges and at the throat (if a throat is given). 6-2.2.5 Flow Angle/Tangential Velocity When clicking on the Flow angle/Tangential velocity thumbnail the parameters related to the direction of the velocity at the trailing edge become available: In Analysis mode the user should always provide the spanwise distribution of the flow angle β at the trailing edge. In Design mode the tangential velocity Wθ (design) at the trailing edge is required instead of the flow angle. A normalized streamwise distribution is also required. It is either read from a file or specified through a power function whose exponent is given by the user. A zero value at the shroud implies that the shroud value is equal to the hub one. The leading edge value being a result of the calcula- FINE™ 6-5 Throughflow Model Throughflow Blocks in the FINE™ Interface tion, the streamwise distribution of the flow angle or of the tangential velocity is iteratively computed according to the calculated value at the leading edge and the value defined at the trailing edge. The default value of the exponent is 1, which generates linear evolutions from leading to trailing edge. Two definitions of the flow angle are available, respectively based on the axial and meridional directions. The choice between these definitions is made through the expert parameter ITHVZM: Wθ=Wz.tan β(ITHVZM=0, default) Wθ=Vm.tan β(ITHVZM=1). In case of radial configurations the parameter ITHVZM should be set to 1. In the case of the analysis mode with throat control one additional input is required: the spanwise distribution of the leading edge flow angle has to be provided in a file. This is required in order to define the value of the effective blockage at the leading edge. 6-2.2.6 Loss Coefficient When clicking on the Loss coefficient thumbnail the distribution of the loss coefficient can be defined through: • The spanwise distribution along the trailing edge as specified in a file. • The normalized streamwise distribution as imposed through an external file or by using a power function. The value 1 (recommended value) for the exponent of the power function means that a linear function with a shift towards front is used. The leading edge value of the loss coefficient is assumed to be 0. 6-2.3 Mesh for Throughflow Blocks Figure 6.2.3-4 shows a configuration with two blade rows. Each throughflow block contains a single blade row. The mesh has only one cell in the pitchwise direction. The cell opening angle, α in Figure 6.2.3-4, has no influence theoretically but excessive values should be avoided (α > 10o or α < 0.01o). A value of 1o is recommended. All blocks, must have the same cell opening angle. The mesh indices I, J, and K are oriented as shown in Figure 6.2.3-4. The hub and shroud surfaces correspond to the I=1 and I=Imax grid surfaces respectively, whereas the I=Cst grid surfaces correspond to the successive streamwise positions. Rotors are computed in the relative frame of reference. The leading trailing edges positions are described by spanwise mesh lines (I=Cst). The blade region is identified through the patch-decomposition of the periodic faces (See section 6-2.4.1). If multigrid is to be used, the inlet region, blade row, and outlet region must each have a suitable number of cells in the I-J-directions. Please note that according to Figure 6.2.3-4 the K=1 surface must be defined along the (Y=0) plane. 6-6 FINE™ Throughflow Blocks in the FINE™ Interface Throughflow Model FIGURE 6.2.3-4 The throughflow mesh 6-2.4 Boundary Conditions for Throughflow Blocks Compared with 3D turbomachine cases, throughflow calculations require the same boundary conditions. All the necessary boundary conditions can be set through the general dialog box Patch Selector through the menu Grid/Boundary Conditions... in IGG™. Table 6-1 lists the four types of boundaries and the pertaining boundary conditions. TABLE 6-1 Boundary Conditions Boundary condition number BC 2 BC 16, BC 17 BC 124, BC 125, BC 27, BC 23, BC 22 BC 1, BC 44 Type of Boundary Periodic Boundaries (K-faces) Hub and Shroud Walls (I-faces) Inlets and Exits (J-faces) Connecting Boundaries (J-faces) 6-2.4.1 Periodic Boundaries The axisymmetric periodic boundaries require a rotational periodicity condition. Except for the patch decomposition, they are set exactly as periodic boundaries of a 3D or axisymmetric nonthroughflow block. As described in section 6-2.3 the block is composed of an inlet region, a blade passage, and an outlet region. Instead of specifying one boundary condition for the entire K-face, the latter must be artificially divided in three boundary patches, labelled P1, P2, and P3 in Figure 6.2.3-4 and designating respectively the inlet, the blade, and the outlet region. Both patches P1 and P3 must have at least one cell in the J-direction. The decomposition needs to be performed in IGG™. • The block is composed by the blade passage only. One boundary patch covers the entire Kface, leading and trailing edge coincide with respectively inlet and exit of the domain. FINE™ 6-7 Throughflow Model Throughflow Blocks in the FINE™ Interface 6-2.4.2 Hub and Shroud Walls The present throughflow model assumes an inviscid fluid. Euler wall boundary conditions have to be applied to the hub and to the shroud walls (I-faces). 6-2.4.3 Inlet and Exit All rotor inlet and outlet boundary conditions as described in Chapter 8 can be applied at inlet and outlet (J-faces). 6-2.4.4 Connecting Boundaries Under the framework of throughflow calculations, rotor/stator interfaces are replaced by simple connections between the throughflow blocks. Connection between throughflow blocks must be matching. Throughflow blocks can also be connected to 3D blocks. This implies the use of a quasi-steady interface (rotor-stator interface). 6-2.5 Initial Solution for Throughflow Blocks Especially for the throughflow module the initial flow solution has an important influence on the speed and robustness of the resolution algorithm. Exactly as in FINE™/Turbo for 3D applications, a turbomachinery-oriented initial solution algorithm has been implemented, generating automatically an initial solution based on the inlet/outlet boundary conditions and on a user-specified value for the inlet static pressure. The initial solution constructed with this algorithm respects the basic laws of rothalpy and mass conservations. In order to activate this algorithm, the user should select on the Initial Solution page the for turbomachinery option. The user then has to enter a value for the inlet static pressure and a radius if radial equilibrium is selected. The rotor/stator interfaces do not appear in the Initial Solution page because they are identified as simple connections. The static pressure level at the successive rotor/stator interfaces can however be specified through the expert parameter PRSCON. The values to be entered are p1, R1, p2, R2,...,pi,Ri, where i is the index of the rotor/stator interface, p the static pressure in Pascal [Pa] and R the radius in meters [m]. If the expert parameter is not modified by the user, a linear pressure evolution is assumed from inlet to outlet. In order to impose a constant pressure at the rotor/stator interface, the corresponding radius has to be set at zero. 6-2.6 Output for Throughflow Blocks The output for throughflow simulations can be selected on the Output/Computed Variables page under the Throughflow thumbnail. The following quantities can be stored: -• Blockage: tangential blockage factor b = 1 – d , s ∇b • Grad(B)/B-1st component: radial component of the ------- vector, b ⎠ ⎞ ⎝ ⎛ 6-8 FINE™ File Formats for Throughflow Blocks Throughflow Model ∇b • Grad(B)/B-3rd component: axial component of the ------- vector, b • Lean vector (tangential vector along the blade in the spanwise direction), • Shape function for β = atan ( W θ ⁄ Wm ) or Wθ , • Loss coefficient ψ , • Blade force vector fB , • Friction force vector f F , • Unit stream vector (USV), • Flow angle atan ( W θ ⁄ ( Wm ⋅ USV ) ) , • Effective streamtube thickness, • Blade force magnitude: magnitude of blade force f B , • Friction force magnitude: magnitude of friction force f F , • W_theta target: target relative tangential velocity Wtθarg et , • Beta target: target relative flow angle β t arg et = atan ( Wtθarg et ⁄ W m ) . · 6-3 File Formats for Throughflow Blocks The names of all throughflow input files are specified by the user in the above described interactive windows (Figure 6.2.2-2). The aim of this section is to present the structure of these files. A short description of a specific throughflow output file generated by the interface is also provided. One can distinguish two types of files: the two-dimensional and the one-dimensional files. The file format for each is described in the next paragraphs. 6-3.1 One-dimensional Throughflow Input File The one-dimensional files consist of two parts: 1. A header line containing four integer (the number of data points and 3 integer switches). 2. The data, organised in 2 columns. The 4 integers contained in the header line define: — the number of data points. — the type of coordinate along which the data is given. The available coordinates are the Xcoordinate (1), the Z-coordinate (3), the radius (4) and the meridional coordinate (6). — if the coordinate should be normalized (1) or not (0). The normalized data describes a distribution between the leading and the trailing edge, or between the hub and the shroud. FINE™ 6-9 Throughflow Model File Formats for Throughflow Blocks — if for a streamwise distribution, the leading and/or trailing edge values should be extended to the upstream/downstream ends of the block. Values of 1 and 3 extend the upstream region, whereas values of 2 and 4 extend the downstream regions. This switch is used to achieve a blockage factor below 1. upstream and/or downstream of the blade passages. The angles are in degrees, the length in meters, except for the blade thickness, which is in millimetres. Some examples of the geometrical files are given hereafter: • Spanwise distribution of the maximum blade thickness: 14 4 1 0 .1181262 .1282913 .138422 .1484767 .1583352 .1680261 .1778827 .1877939 .197697 .2076666 .217709 .2277728 .2378241 .2477884 8.20958 8.22191 8.16546 8.03777 7.85892 7.58743 7.26814 6.86779 6.45259 6.11613 5.78311 5.65696 5.84635 6.27821 • Spanwise distribution of the trailing edge flow angle: 11 4 1 0 .0 .1060092 .2095564 .3126917 .4146 .5148696 .6134925 .7112999 .8084939 .9048644 1.0 10.10562 -5.70642 -16.2939 -27.0153 -35.7384 -41.7166 -46.4628 -50.3735 -54.3548 -57.9392 -59.542 • Spanwise distribution of trailing edge loss coefficient: 11 4 1 0 1.0 .9048644 .8084939 .7112999 .6134925 .5148696 .4146 .3126917 .2095564 .1060092 .0 3.78416E-02 3.78416E-02 3.28353E-02 3.74248E-02 1.96157E-02 3.18909E-02 3.61507E-02 3.23982E-02 5.45700E-02 9.97951E-02 9.97951E-02 6-10 FINE™ File Formats for Throughflow Blocks Throughflow Model 6-3.2 Two-dimensional Throughflow Input File The two-dimensional input file, only available for the blade geometry definition, consists of two parts: 1. A header line containing the number of points in the two dimensions of the structured data surface and three switches. 2. The data organised in 5 columns (the coordinates should be R,Z,θcl,θss,θps where θcl,θss,θps are respectively the angle at the camber line, suction side and pressure side of the blade) and evolves from hub to shroud and from the leading to the trailing edge. The three additional switches define: — the type of coordinates: should be 4. — the type of structure: should be 3. — the number of variables: should be 5. All lengths in the data files should be in meters, and the angles in radians. Following is an example of the two-dimensional input file: 57435 9.37745E-02 .1934945 ... **(5*7 points: 5 points in spanwise and 7 points in streamwise)** -8.87817E-03 6.47041E-02 7.40556E-02 5.53526E-02 8.93166E-03 5.71797E-02 5.99261E-02 5.44332E-02 6-3.3 Output File Absolute (V) and Relative (W) velocities components along R,T,M ALPHA = arctg(VT/VZ) BETA = arctg(WT/VZ) GAMMA = arctg(VR/VZ) Mach Number Meridional Mach Number Static Pressure, Static Temperature, Density Absolute Total Pressure Rothalpy Total Pressure Relative Total Pressure Absolute Total Temperature Rothalpy Total Temperature Relative Total Temperature Isentropic Efficiency Polytropic Efficiency Mass Flow Total Area FIGURE 6.3.3-5 Throughflow Output File ".gtf" FINE™ 6-11 Throughflow Model Expert Parameters Related to Throughflow Blocks In addition of files which can be read by CFView™, a summary file is created when the throughflow module is activated. It has the extension ".gtf" and gives the average inlet and outlet results for each block in SI units. 6-4 Expert Parameters Related to Throughflow Blocks 6-4.1 Under-relaxation Process Two types of under-relaxations have been introduced, allowing for an increased robustness of the algorithm during the initiation of the resolution procedure. This under-relaxation process is controlled through 2 sets of expert parameters (accessed on the Computation steering/Control variables page in expert mode), THNINI (2 integer parameters) and THFREL (2 real - float parameters). • the first THNINI and THFREL parameters permit to impose that during the first THNINI(1) iterations, the blade force update factor is not the one specified in the "Throughflow blocks" menu (section 6-2.1), but a (lower) value given by THFREL(1). This under-relaxation process can be important for transonic cases especially. The default values for THNINI and THFREL are respectively 10 and 0.1 • the second THNINI and THFREL parameters permit to under-relax the imposed value of trailing edge velocity or flow angle during the first THNINI(2) iterations. The under-relaxation factor multiplying by the imposed value varies linearly between THFREL(1) and 1.0 during the first THNINI(2) iterations. The default values for THNINI and THFREL are respectively 10 and 0.85. 6-4.2 Others. = 1: Wθ=Vm.tan β • ITHVZM = 0 (default): Wθ=Wz.tan β Definition of the flow angle. The selection of ITHVZM to 1 is crucial for a correct treatment of radial machines. • PRCON to define the pressure for the initial solution at rotor/stator interfaces. If this parameter is not modified a linear pressure distribution from inlet to outlet is assumed. 6-12 FINE™ Theoretical Background on Throughflow Method Throughflow Model 6-5 Theoretical Background on Throughflow Method 6-5.1 The Time Dependent Approach The dominant aspect of an Euler throughflow method is the modelling of the turning and the associated distributed blade force. Most authors so far have adopted a spatial discretization approach, in which the blade force is determined from the tangential projection of the momentum equation in conjunction with the imposed flow direction (analysis) or swirl (design), leaving four differential equations to be solved. In the present approach the blade force is treated as an additional time dependent unknown. The full 5-equations Euler system is then solved, with an additional equation for the blade force. This is the so-called time dependent approach, which has proven to be more robust than the space discretization, especially at transonic and supersonic flow conditions. The other advantage is that the fact that the throughflow solver is based on the same time marching algorithm as the 3D one makes hybrid 3D-throughflow calculations possible. 6-5.2 Basic Equations and Assumptions The basic equations describing axisymmetric throughflow are obtained through averaging in the θdirection of the three-dimensional Euler conservation laws for mass, momentum, and energy, yielding, in concise notation and after introduction of the distributed loss model, ρ 0 = ∇b ρQ + p ------ + ρ ( f B + f F ) b ρQ (6-1) ∂ 1 ---+ -- ∇ ⋅ b ( ρW ⊗ W + pI ) ∂t ρW b ρE bρWH bρW This is a system of 5 PDE for 5 unknowns (the dependent variables, e.g., the primitive variables in cylindrical coordinates, ρ, Wr, Wθ, Wz, p) in two spatial dimensions (r and z). Apart from the absence in the differential operators of derivatives with respect to the tangential direction, the system differs from the three-dimensional Euler equations in three ways: • The presence of the blockage factor b in the fluxes. ∇b • Source terms p ------- and fB representing the inviscid action of the blades. b • A source term f F grouping all the effects of viscosity and heat conduction. The system is solved in Cartesian coordinates using explicit Runge-Kutta integration in time and either central or upwind spatial discretization. 6-5.3 The Tangential Blockage Factor The tangential blockage factor, b, also called the stream tube thickness parameter, represents the contraction of the flow path that arises from the tangential thickness of the blades, d. With the pitch, s, depending on the radius, r, and the number of blades, z, the tangential blockage factor is defined as: FINE™ 6-13 Throughflow Model Theoretical Background on Throughflow Method d b = 1 – -s where 2πr s = -------z (6-2) Thus, b = 1 outside blade rows and 0 < b ≤ 1 inside blade rows (including the hypothetical case of blades with zero thickness). The blockage factor is an external input to the computation. 6-5.4 The Blade Force By definition, the inviscid action of the blades consists in a distributed force normal to the blade surfaces, i.e., suction and pressure surface. In our implementation the blade force is split into two components: • the first main component is proportional to the suction-to-pressure side difference, and is oriented in the direction normal to the mean camber surface. The tangential component of this force is the additional unknown considered in the time dependent approach, for which an additional equation will be solved together with the 5 Euler equations. • the second component is due to the deviation of the suction and pressure side normals from the normal to the mean camber surface. It is computed according to p ------ , and is therefore deter∇b b mined entirely by the tangential blockage factor, b, which is external input as seen in the preceding section, and by the static pressure, which is a result of the computation. As mentioned in section 6-5.2, the blade force is treated as an additional unknown with the present approach. Starting from some initial value in each cell, the blade force is modified locally, until the current converged solution exactly matches the externally imposed target, for instance the flow angle β (analysis) or the tangential velocity Wθ (design). The correction is proportional to the difference between the actual and a required tangential velocity: ( ρF Bθ ) k+1 = ( ρF Bθ ) + κ ( W θ – W θ ) k t (6-3) where the constant κ is user input. The target tangential velocity Wθt is either direct external input (design mode) or locally calculated from the prescribed relative flow angle β and the current meridional velocity (analysis mode: Wθ=Vmtanβ). The vector of the blade force, fB , is perpendicular to the mean camber surface, which is internally defined by the flow angle and the lean angle. Currently, a zero lean angle is assumed. Robust analysis mode In the case of the analysis mode another formulation of the above equation is adopted, based on the magnitude of the blade force instead of its tangential component: ( ρFB ) k+1 ·· ˜ k F = ( ρF B ) – κ W n ---˜ W ⎠ ⎞ ⎝ ⎛ (6-4) where FB is the magnitude of the blade force and n is the normal vector whose direction results from the imposed relative flow angle distribution. In case the angle is measured with respect to the axial direction (ITHVZM=0): n r = 0.0 n θ = – sin β n z = cos β (6-5) 6-14 FINE™ Theoretical Background on Throughflow Method Throughflow Model 6-5.4.1 The Friction Force The distributed loss model retains, from all the effects of heat conduction and viscous stresses, the contribution to the entropy production. The dissipative action of the viscous stresses is expressed through a distributed friction force, f F . It acts in the direction opposite to the velocity vector and for a perfect gas its amplitude is proportional to the loss coefficient derivative in the streamwise direction: p W ρf F = – ------------ p ref ∂ m ψ -------pt rot W (6-6) This formulation ensures that a loss coefficient of zero will give exactly a zero friction force. The imposed loss coefficient is defined as: LE ptrot – ptrot ψ = ------------------------------p ref (6-7) where ptrot is the total pressure associated with rothalpy defined as: γ ---------Tt rot γ – 1 ptrot = p -----------T ⎠ ⎞ ⎝ ⎛ where 2 2 W – ( ωr ) Tt rot = T + ---------------------------2c p (6-8) where W is the relative velocity magnitude and pref is a reference dynamic pressure taken at the leading edge (for compressors) or trailing edge (for turbines) on each streamwise mesh line. FINE™ 6-15 Throughflow Model Theoretical Background on Throughflow Method 6-16 FINE™ CHAPTER 7: Optional Models 7-1 Overview FINE™ contains the following three optional models: • Fluid-Particle Interaction to model solid particles in the flow. • Conjugate Heat Transfer to model the heat transfer between the fluid and solid walls. • Cooling/Bleed to model cooling holes or bleed. • Transition Model to model the flow transition. Each of these models requires a special license feature. If the model is not accessible due to a missing license it is displayed in gray under Optional Models. Contact NUMECA sales or support team for more information about the possibility to obtain a license. 7-2 7-2.1 Fluid-Particle Interaction Introduction Particle-laden flows cover a large class of two-phase flows, such as droplets or solid particles in a gas or liquid flow, or bubbles in liquids. One phase is assumed to be continuous and occupies the majority of the flow. It is called the "carrier" phase. Another phase, whose volume fraction is relatively small (usually less than 10-2), exists as a number of separate elements or particles. It is called the "dispersed" phase. 7-2.1.1 Lagrangian Approach A Lagrangian approach is used here, whereby the trajectories of individual groups of particles are calculated as transported by the velocity field of the carrier phase, including the effect of drag and other forces. The calculations of the carrier flow and of the particles can be fully coupled, the fully coupling approach implying that the calculation of the particles trajectories is followed by a second flow calculation, taking into account the presence of the particles in the flow (the interphase forces are introduced as source terms in the flow calculation). The sequence consisting of a flow calcula- FINE™ 7-1 Optional Models Fluid-Particle Interaction tion and of the particle traces tracking can be repeated several times until no changes are observed in the results (usually 3 to 10 times). In the present Lagrangian model, the motion of the particles is only influenced by their own inertia and by the flow, i.e. the local aerodynamic or hydrodynamic forces. Interactions between the particles are currently not considered. This implies the hypothesis of a dilute flow. On the contrary in a dense flow, particle motion is governed by their direct interaction, which implies more complex models, such as the Eulerian ones, in which both phases are modelled as continuous phases. Particle-laden flows are found in many industrial applications such as cyclone separators, pneumatic transport of powder, droplet and coal combustion system, spray drying and cooling or sandblasting. In all cases, the flow consists of a continuous phase - also named carrier flow - and a dispersed phase in the form of solid particles, liquid droplets or gas bubbles. In general, the motions of the carrier flow and of the dispersed phase are interdependent. In the lagrangian approach, the physical particle cloud is represented by a finite number of computational particles. The continuous phase (fluid) is treated as a continuum using a boundary-controlled method whereas the dispersed phase (particles) is treated as a number of separate particles. The particles are successively tracked as a single probe particle through the flow field using a Lagrangian formulation. In the case of laminar flows, each particle will follow a unique deterministic trajectory. In the case of turbulent flows however, particles will have their own random path due to interactions with the fluctuating turbulent velocity field. This feature is taken into account in EURANUS through a stochastic treatment. This approach consists of employing a sampling technique based on a Gaussian probability density function to introduce the random nature of the turbulent velocity field. The particle diffusion due to turbulence can therefore be modelled without introducing artificial diffusion properties of the cloud. According to the distribution and contents of the particles, an averaging procedure provides phase coupling source terms to be added into the Eulerian carrier phase conservation equations. The twoway coupling can be achieved through global iterations. 7-2.1.2 The Algorithm The hypothesis of a dilute mixture permits to have a very simple sequential calculation of the trajectories of the different particles injected through the inlet sections. The algorithm considers successively the different inlet patches. The user specifies the number of trajectories per cell. The origins can be located at a given point chosen by the user, or equally distributed throughout the cell. The algorithm proceeds cell by cell, the time step being calculated so that several time steps are performed in each mesh cell. The procedure starts at a cell of an inlet boundary and stops when a boundary is reached. Each time step consists of: • the calculation of the force on the particle. • the integration to find the new velocity and position. • the determination of the cell in which the particle is located. 7-2.1.3 Overview In this chapter an overview is given of the fluid particle interaction module incorporated in NUMECA’s FINE™ environment: 7-2 FINE™ Fluid-Particle Interaction Optional Models • section 7-2.2 describes the main functionalities of the module and the way to proceed in the FINE™ interface. • section 7-2.3 gives the format of the files associated with the module. • section 7-2.6 summarizes the main theoretical features of the Lagrangian model. 7-2.2 Fluid-Particle Interaction in the FINE™ Interface To access the parameters related to Fluid-Particle Interaction select the corresponding page under the Optional Models. In the parameters section click on Fluid-particle calculation to activate this model (see Figure 7.2.2-1). The user enters not only the main features of the numerical simulations but also the characteristics (i.e. processes to be taken into account) of the interphase force between the fluid and the particles. The top window allows to choose the degree of influence of the particles on the flow. The calculation of the carrier flow and of the particles can be fully (2-way) or weakly (1-way) coupled: • in the 1-way coupling approach the flow calculation (ignoring the influence of the particles on the flow field) is followed by a calculation of the trajectories of particles. In this case, there is no influence of the particles on the flow. • in the 2-way coupling approach the calculation of the trajectories of particles is followed by a second flow calculation, taking into account the presence of the particles in the flow (the interphase forces are introduced as source terms in the flow calculation). The sequence can be repeated several times (by entering the Number of global iterations) until no changes are observed in the results (usually 3 to 10 times). Concerning the simulation itself, the user can choose the Global Strategy: • Start from scratch: to start the flow calculations and then pursue with the particle tracking simulation. In this particular case, the criterion for the carrier flow calculations convergence is the one set on the Control variables page (-6 by default). • Start from converged flow solution: to proceed directly with the Lagrangian coupling from a previous converged flow calculation. FIGURE 7.2.2-1 Parameters page of the lagrangian fluid-particle interaction model. The usual way to proceed is: 1. 2. perform a pure flow study without activating the Fluid-Particle Interaction model in a computation. while this computation is active in the list of Computations on the top left of the interface create a new project by clicking on the New button. FINE™ 7-3 Optional Models Fluid-Particle Interaction 3. in this new computation activate the Lagrangian Fluid-particle calculation and perform a computation with Lagrangian coupling.The particles encounter several forces: the friction force, i.e. the resultant of the pressure and viscous stress in the carrier phase over the particle surface, as well as potential inertia and gravity forces. The user is free to introduce the gravity force through the vectorial components of the acceleration of gravity on the Flow Model page. An inertial force due to the rotation of the system of reference can also be included. If some of the blocks are rotating this button should systematically be activated. In this case the reference rotation velocity is the one specified on the Rotating Machinery page. 7-2.2.1 The Boundary Conditions All boundary conditions available for the carrier flow solver are also accepted by the particle tracking algorithm. The only boundary conditions requiring user’s input are: • inlet boundary • solid boundary The boundary conditions are imposed by selecting a patch on which to fix the condition. The user has to confirm the entered values by clicking on the Apply to selection button (Figure 7.2.2-2). In the list of patches it is not possible to group patches but multiple patches can be selected at the same time to apply the same boundary conditions to all of them. To select multiple patches hold the <Ctrl> key while selecting them. a) Inlet Boundary The user can enter a number of classes of particles, each class representing a different type of particles. For each class the inlet boundary conditions have to be specified. The displayed boundary conditions are the one for the class specified in the bar as indicated (a) in Figure 7.2.2-2. To select another class use the scroll buttons on both sides of this bar. The purpose of this is to be able to simulate the presence of different types of particles in the same patch. (a) FIGURE 7.2.2-2 Inlet boundary conditions for the fluid-particle interaction model 7-4 FINE™ Fluid-Particle Interaction Optional Models Note however that multiple classes are of interest for fully couples calculations only, by allowing the flow calculation to account for the presence of different particle types. In the case of a weak coupling strategy it is recommended to create one computation per particle class, because only one particle class can be visualized in CFView™. The Expert parameter (in Expert Mode on the Control Variables page) CLASID permits to specify which particle class must be included in the CFView™ output. The inlet boundary conditions are the following: • spatial distribution of the injection points: uniform over the chosen patch or located at a chosen point of coordinates (x,y,z). • inlet velocity of the particles (absolute or relative frame of reference). The velocity is always considered in the same relative frame of reference as the one of the block in which the inlet particle is located. The relative velocities here defined as the difference between the particle and the flow velocity (a zero relative velocity is therefore very commonly used) whereas the absolute velocity boundary conditions is used when the velocity of the particle is well known and different from the velocity of the flow. Note that only the Cartesian coordinate system is available. • density and mean diameter of the particles. • particle concentration (number of particles/m3). • number of particles per cell should be seen as the number of trajectories per cell. The use of multiple trajectories per cell permits to ensure a more uniform covering of the inlet (and hence of the computational domain) by the particles. This is only of interest in the case of fully coupled calculations where it is important to ensure that the source terms are correctly evaluated in all mesh cells. The use of multiple trajectories does not modify the number of particles entering the domain. Each trajectory must be seen as an ensemble of particles. It is also very often referred to as a computational particle. In the case of full coupling, the number of particles per cell should be statistically large enough to provide accurate averaging of the dispersed phase parameters. Therefore it is recommended in this case to have a high number of particles per cell. This increases the computational time required for the particle tracking process, but gives rise to a smoother distribution of the particles in the domain. In the case of a weak (1-way) coupling, only one particle per cell is usually enough to provide a sufficiently detailed description of the particles distribution in the field. b) Solid Wall Boundary Condition The solid wall boundary condition requires an additional input data, which is the reflection ratio. If the ratio is zero, all the particles remain stuck on the wall, whereas if it is 1.0, all particles are reflected, without any loss of mass or energy. The user can choose the reflection ratio by clicking on the corresponding button while moving the mouse (Figure 7.2.2-3). Two reflection modes are available and can be selected by the expert parameter IBOUND: • In the default mode (IBOUND = 1) the particle loses a fraction of its mass and hence of its kinetic energy at each wall hit. After several wall hits, the size of the particles becomes very small, and the tracking stops (once the diameter has reached a given ratio of the initial one, specified by the expert parameter DIAMR). • In the other mode (IBOUND = 2) the velocity of the particle is reduced, with an unchanged mass. The particle is stopped as soon as the velocity becomes too small (also specified by the parameter DIAMR). FINE™ 7-5 Optional Models Fluid-Particle Interaction FIGURE 7.2.2-3 Solid boundary conditions for the fluid-particle interaction model 7-2.3 Outputs ⎠ ⎟ ⎞ The following quantities are calculated by the solver (see Figure 7.2.3-4): • the number concentration of volume Ω, ∑ Ni i • the mass concentration ρ ipart i is the density of the particle of class i and volume Ω ipart , ⎠ ⎟ ⎞ • the volumetric concentration • the Vx = ⎝ ⎜ ⎛ ∑ Ni Ωipart i ⁄ Ω (volume of particles per cell volume), components of ⎠ ⎟ ⎞ the mass ∑ Vxi ρipart Ωipart Ni ⁄ ∑ ρipart Ωipart Ni , i i ⎠ ⎟ ⎞ • the weighted mass and weighted absolute or relative velocity vectors number, • the components of the interphase force F = The solver automatically writes an output file containing the particle traces that is read by the CFView™ post processing software. 7-6 ⎝ ⎜ ⎛ ⎠ ⎟ ⎞ ⎝ ⎜ ⎛ ⎝ ⎜ ⎛ ⎝ ⎜ ⎛ ⁄ Ω where Ni is the number of particles of class i in the cell ∑ ρipart Ni Ωipart ⁄Ω (mass of particles per cell volume) where weighted absolute velocity vector ∑ Fi N i i ⁄Ω . FINE™ Fluid-Particle Interaction Optional Models FIGURE 7.2.3-4 Outputs of the fluid-particle interaction model 7-2.4 Specific Output of the Fluid-Particle Interaction Model This section describes the specific outputs generated by the Lagrangian module. 7-2.4.1 Field Quantities The solver automatically includes in the CFView™ output (’.cgns’) of the project the field quantities that have been specified by the user under the Outputs thumbnail in the Fluid-Particle Interaction page. These quantities can be scalars or vectors, and are the following: • Vectors Mass-weighted relative velocity (1) Number-weighted relative velocity (2) Mass-weighted absolute velocity (3) Number-weighted absolute velocity (4) Interphase force vector (5) • Scalars Number concentration (51) Mass of particles per cell volume (52) Volume of particles per cell volume (53) Presence (1) or absence (0) of particles in cells (54) Vx: x-component of mass-weighted velocity vector (55) Vy: y-component of mass-weighted velocity vector (56) Vz: z-component of mass-weighted velocity vector (57) Fx: x-component of interphase force (58) Fy: y-component of interphase force (59) Fz: z-component of interphase force (60) 7-2.4.2 Particles Traces (’.tr’) The solver also creates an specific lagrangian output file (’.tr’), containing the trajectories of the all the particles. This file is automatically transmitted to CFView™, which allows for the visualization of the trajectories. FINE™ 7-7 Optional Models Fluid-Particle Interaction 7-2.4.3 Summary File (’.tr.sum’) In addition to the previous outputs, a summary file ’.tr.sum’ is automatically written by the solver (in the same directory as the CFView™ project), giving for each injection patch the particles numbers and mass flows through the inlet/outlet boundaries, and the number of particles that remain stuck on the walls. 7-2.5 Expert Parameters for Fluid-Particle Interaction Other parameters appear in the Expert Mode of the Fluid-Particle Interaction page under the Parameters thumbnail: • The maximum residence time (TMAX in corresponding ’.run’ file), which is the time limitation for particle residence in the flow. It may be used either to prevent particle stopping or to avoid an infinite loop, having for instance a particle captured in a separation bubble. After the time has expired, the particle disappears. • The governing equations for particles in a carrier flow consist of a set of non-linear ordinary equations. Two methods are provided to integrate this equations with respect to time (that can be selected in expert mode): — The Runge-Kutta scheme, in which the transfer to the next time level is fulfilled through a finite number of intermediate steps. A two-stage and a four-stage option (NRKS in corresponding ’.run’ file) are available. This scheme is limited to big particles. — The exponential scheme that lies on a semi-analytical method. This scheme is particularly suitable for small particles. • The Drag force is in general the only considered part of the interphase force. It corresponds to the force on a particle moving in a still fluid at constant velocity (or using the particle reference system, a fixed particle in a uniform laminar flow). At extremely low Reynolds numbers (Rep << 1 i.e. at low relative velocities), it is expressed through the Stokes formula. For higher Reynolds numbers, an optional standard curve fit may be chosen (section 7-2.6.1). The choice between the two types of forces can be made in expert mode. Other parameters have a standard value, which may be modified only on rare occasions. They are accessible in the Expert Mode of the Computation Steering/Control Variables page: CLASID: selection of class for CFView™ output LMAX: the maximum number of segments along a trajectory may be used to avoid an infinite loop in the case of an oscillatory movement for instance. DDIMAX: tolerance factor to establish that a particle has left a cell (default=1.E-4). I2DLAG: simplification for 2D problems (0 if 3D, 1 if 2D). DIAMR: diameter ratio under which the particle tracking process stops (default value: 0.1). CELT: coefficient for eddy life time (for turbulent flows only): 0.28. KOUTPT: enables to write the ASCII ’.tr.out’ file containing the output of the trajectories (default value: 0). Contact support at [email protected] to have more details on this file. 7-8 FINE™ Fluid-Particle Interaction Optional Models 7-2.6 Theory In a Lagrangian approach the particle cloud is modelled by a finite number of computational particles, representing a group of real physical particles with similar properties. The particles are tracked separately, each as a single probe particle, through the flow field. 7-2.6.1 Calculation of the Trajectories - Integration Method The calculation of the trajectories is based on the Newton law: ∆V F = ma = m -----∆t (7-1) where a is the acceleration vector of the particle of velocity V and F is the sum of the friction force between the fluid and the particle and the eventual inertia and gravity forces: F = Fd + F inertia + Fgravity (7-2) The gravity force is defined by the user on the Flow Model page: Fgravity = mg It is assumed that the mesh blocks for which a rotation of the reference system is introduced in the carrier flow equations (when rotation of the reference system is selected under the Parameters thumbnail of the Fluid-Particle interaction page) are also considered as rotating ones for the particles calculation. The inertia force due to the rotation of the reference system contains the two terms related to the inertia and Coriolis effects: F inertia = – m [ ω × ( ω × r ) + 2ω × V ] (7-3) Fd is the drag force between the flow and the particles, calculated according to the Stokes law: D Fd = – ---- ( V – U ) Fs (7-4) where D is the diameter of the particles, U is the velocity of the fluid and Fs depends on the viscosity of the fluid and on the Reynolds number Re p based on D: F s = 1 ⁄ ( 3πµC ) (7-5) where: ρ ( V – U )D C = 1 (simple Stokes law for Re p ≡ -------------------------- « 1 ) µ or C = 1 + 0.179Re p + 0.013Re p (standard curve approximation). 0.5 Up to now, no model is incorporated in which the mass and the volume of the particle would change (for instance by combustion or evaporation). FINE™ 7-9 Optional Models Fluid-Particle Interaction 7-2.6.2 Integration Time Step - Relaxation Time The calculation of the trajectories is obtained by integrating the Newton law in time, using either a 2- or 4-steps Runge-Kutta or an exponential scheme. At each time step the force vector is re-calculated to obtain a new value for the velocity vector, whereas the velocity vector is used to calculate the new position of the particle. This sequence is repeated until a boundary is reached. In order to have an appropriate integration method to calculate the trajectories, the integration time step must be properly chosen. The time step used by the algorithm is the minimum between the time required to traverse the mesh cell (which depends on the particle velocity and on the cell size) and the relaxation time, which is the time required by the particle to lose its initial slip velocity: τ drag = ( ρD ) ⁄ ( 18µC ) 2 (7-6) For a stationary reference system (no inertia force) and in the case of no gravity, the relaxation time is the time required by the particle to reach the flow velocity U, whereas in the presence of an inertia and/or a gravity force, the velocity reached by the particle after the relaxation time is not U, but U + g . τdrag. In some cases (for instance with very small particles) the relaxation time is very small, which leads to a large number of time steps per mesh cell, and hence to a larger CPU time for the particle tracking algorithm. A faster convergence may then be reached by using the so-called exponential scheme for the time integration step. 7-2.6.3 Full Coupling Between the Carrier and Particle Flows In case of a full coupling between the carrier and particles flows, the particles traces calculation is followed by a coupled carrier flow calculation including the effect of the presence of the particles. This is achieved by the introduction of source terms in the momentum equations, these source terms being calculated according to the interphase force vector: ∆V F interphase = m ------ – Finertia – F gravity ∆t (7-7) 7-2.6.4 Interaction with Turbulence While moving through a turbulent flow, each particle faces a sequence of random turbulent eddies that result in a lack of accuracy in particle velocity and position. This process is taken into account using a stochastic treatment. The k-ε turbulence model is assumed for the carrier flow simulation. The instantaneous fluid velocity is represented as the sum of the local mean velocity (available from the computed carrier flow field) and a random fluctuation: U = U + U' (7-8) The fluctuation U' is randomly sampled from the normal Gaussian distribution with the probability-density-function f: u' 1 f ( u' ) = ----------------- exp – --------- and 2 2 2u' 2πu' ⎠ ⎟ ⎞ ⎝ ⎜ ⎛ 2 u' U' = –∞ ∫ f ( u' ) du' (7-9) The individual components of the velocity fluctuation are assumed to be non-correlated. The mean square deviation is evaluated from the turbulent kinetic energy: 7-10 FINE™ Conjugate Heat Transfer Optional Models 2 2 u' = -- k 3 (7-10) It is accepted that this sample velocity fluctuation remains unchanged within the turbulent eddy during its life time. The eddy life time Te and size Le are calculated according to: ⎠ ⎞ ⎝ ⎛ k Te = C lt ε -and Le = Te 2 k 3 1⁄2 (7-11) Where C lt is an empirical coefficient with a default value of 0.28. The calculated fluctuation gives the instantaneous flow velocity, which is used while tracking the particle. As soon as the life time has expired or the particle has left the eddy, a new fluctuation is chosen as described before, assuming no correlation with the previous sample. Note that turbulence is therefore taken into account only for the different linear and non linear k-ε models. In the particular case of the Baldwin-Lomax model, turbulence does not have a direct influence on the particles trajectories. 7-2.7 References Chang, K. C., Wang, M. R., Wu, W. J., Liu, Y. C., Theoretical and Experimental Study on TwoPhase Structure of Planar Mixing Layer, AIAA Journal, Vol. 31, No 1, pp 68-74, 1993. 7-3 7-3.1 Conjugate Heat Transfer Introduction The conjugate heat transfer model allows the simulation of the thermal coupling between a fluid flow and the surrounding solid bodies, i.e. the simultaneous calculation of the flow and of the temperature distribution within the solid bodies. The current version of the model has been validated for steady state applications. It assumes that some of the blocks of the multiblock mesh are "solid", whereas the other ones are "fluid". The connections between the solid and fluid blocks become "thermal connections" along which the fluidsolid coupling is performed. First section 7-3.2 explains how to set up a project involving the Conjugate Heat Transfer model under the FINE™ user environment. In section 7-3.3 a theoretical description is provided, presenting the approach used to solve the conduction problem and describing the adopted solid-fluid coupling strategy. 7-3.2 Conjugate Heat Transfer in the FINE™ Interface The Conjugate Heat Transfer model can be directly activated from the FINE™ interface under Optional Models. When opening the Conjugate Heat Transfer page it looks like Figure 7.3.2-5. All blocks in the mesh are listed on the left of the page and all of them are by default set as "fluid". FINE™ 7-11 Optional Models Conjugate Heat Transfer FIGURE 7.3.2-5 Conjugate Heat Transfer page The only action required from the user to set up a computation involving the Conjugate Heat Transfer model can be decomposed in three steps: 1. 2. 3. Determine the Solid and Fluid Blocks. Set the Global Parameters. Define the thermal connections. Those steps are described in the following paragraphs in more detail. 7-3.2.1 Step 1: Determine the Solid and Fluid Blocks The use of the Conjugate Heat Transfer model requires the generation of a multi-block mesh, the "solid" and "fluid" parts of the domain being discretised with separate blocks. Once the mesh is generated, the first step consists in pointing the "fluid" and the "solid" blocks via the FINE™ user interface. In the default configuration of the solver all blocks are of "fluid" type, so that the Conjugate Heat Transfer page does not need to be entered for a classical flow calculation. The transfer of some of the blocks from "fluid" to "solid" is performed by selecting those blocks on the left part of the window and by pressing the button Solid. For each solid block the thermal conductivity has to be specified (in W/m/K). 7-3.2.2 Step 2: Setting the Global Parameters The only global parameter is the CFL number used for the time integration of the conduction equation. It can be different from the one used for the fluid. The default value is 1.0. 7-3.2.3 Step 3: Setting the Thermal Connections Once some blocks of the multi-block mesh are pointed as "solid" blocks, the connections between solid and fluid blocks become "thermal connections". These connections are solid wall boundary conditions with a particular thermal condition, along which the imposed temperature profile is iteratively recalculated in order to ensure a correct coupling. These patches appear in the list of patches under the thumbnail Solid on the Boundary Conditions page. Although the thermal aspect is fully controlled by the coupling procedure, the kinematic boundary condition must be specified by the user (rotation speed). 7-3.2.4 Type of Connections Between Solid and Fluid Blocks Two types of thermal connections are allowed: • matching connections (one patch on each side), 7-12 FINE™ Conjugate Heat Transfer Optional Models • full non-matching connections (one patch or one group of patches on each side). The connection algorithm is implemented in a general way, allowing on both sides a grouping of solid and fluid patches. This is useful for instance in order to facilitate the coupling of a turbine block with holes with the external flow. One single connection can be built, with on the inner side a group of patches including the blade surface and the outer face of the holes. 7-3.3 Theory This section describes the Conjugated Heat Transfer model implemented within EURANUS: • the technique used to solve the conduction in the solid bodies, • the thermal coupling strategy. 7-3.3.1 Simulation of Conduction in EURANUS It has been shown in the previous chapters that the EURANUS flow solver is based on a cell centred finite volume approach, associated with a entered or upwind space discretization scheme together with an explicit Runge-Kutta time integration method. The same type of approach can be used to simulate the conduction in solid bodies. The only term remaining in the finite volume equilibrium results from the heat conduction. The discretised form of the remaining part of the energy equation applied to the control volumes can be written as: ∆T ρC p ------ Vol = Σ k∇T n∆S ∆τ ⎠ ⎞ ⎝ ⎛ (7-12) where Vol is the volume of the control volume, n∆S is the normal vector to the faces of the control volume and k,ρ and Cp are respectively the conductivity, density and specific heat of the solid body. This equation is applied to calculate the change of temperature T at a given time step resulting from the equilibrium of the conduction fluxes through the faces of the control volume. One can notice that the absence of any advective contribution in the equilibrium permits to avoid the use of artificial dissipation (case of a centred scheme). It also imposes to adopt a pure diffusive approach for the calculation of the time step. For a 2D problem the time step is calculated according to: ρC p ∆τ Vol -------- = --------- ---------------------------------------Vol k 2 2 · Si + Sj + 2Si Sj (7-13) One can notice that once the 2 above equations are put together the heat capacity Cp is eliminated from the equation, and is hence not required as input data. Exactly as for the flow solver the adopted time integration approach is a 4- or 5-step Runge-Kutta scheme whose efficiency is largely enhanced by the use of an implicit residual technique and of a multigrid strategy. This finite volume approach can be used for both steady and unsteady conduction problems. Its efficiency has been compared for steady state applications to the classical Gauss-Seidel and PSOR schemes often employed for the resolution of pure elliptic equations. The results have shown that the use of a time marching approach together with multigrid is much more efficient. 7-3.3.2 Thermal Coupling Between the Solid and Fluid Blocks The fluid-solid interfaces constitute a new type of boundary condition, referred to as "thermal FINE™ 7-13 Optional Models Conjugate Heat Transfer connections", along which the heatflux and temperature are imposed to be equal. The calculation is performed simultaneously on the fluid and solid blocks. The thermal coupling is applied each time the boundary conditions are applied. Note that no particular procedure is required in order to initiate the calculation. The full multigrid strategy is very efficient in order to rapidly establish an overall temperature distribution in the domain. On both solid and fluid sides, the thermal boundary condition imposes a temperature profile. This profile is iteratively recalculated in order to ensure equality of the heatfluxes calculated on both sides: hf(Tw-Tf)=-hs(Tw-Ts), (7-14) where hf and hs are the heat transfer coefficients and Tf and Ts are the inner temperatures. The heat transfer coefficients are calculated in a simple way, assuming a sufficient orthogonality of the mesh: k h = ----- , ∆y (7-15) where k is the local conductivity and ∆y is the distance between the inner cell centre (where the temperature of Tf and Ts is taken) and the wall. 7-3.3.3 Full Non-matching Thermal Connections The Full Non-matching algorithm already used for the fluid-fluid connections can be used in the Conjugate Heat Transfer (CHT) module. It is based on the same coupling procedure, including the calculation of the interface temperature and heatflux. In case the patches are not fully connected, as for instance in Figure 7.3.3-6, the remaining patch is assumed to be adiabatic. The thermal coupling equation is applied successively to all elements resulting from the FNMB decomposition algorithm. This procedure gives as a result a separate value of the interface temperature and of the heatflux for all elements. The interface temperature on the left and right patch cells is then calculated as a weighted averaging of the temperatures of the elements concerned by the cell. If the cell is not fully connected an additional contribution is added, the non connected part of the cell being assumed to be adiabatic: Tw = i elmts ∑ T n w n + T inner W i with i elmts ∑ wn + Wi = 1 . i (7-16) In the generic case of Figure 7.3.2-5: • the cell 1 is not connected and the above equation is applied with Wi=1, • the cell 2 is partially connected and 0<Wi<1, • the cell 3 is fully connected and Wi=0. The heatflux density is calculated as the summation of the contribution of the elements: ϕw = ϕn Sn ⁄ S ⎠ ⎟ ⎞ ⎝ ⎜ ⎛ i elmts ∑ i i (7-17) Note that the heatflux density is saved instead of the heatflux so that the thermal connection boundary condition is compatible with the boundary condition imposing the heatflux density. In the routine imposing the heatflux into the residual the heatflux density is re-multiplied by the cell surface. It should be mentioned that hybrid connections are allowed, this means that each side of the interface can be composed of fluid and solid patches. 7-14 FINE™ Cooling/Bleed Optional Models FIGURE 7.3.3-6 Generic example of FNMB/CHT connection 7-4 7-4.1 Cooling/Bleed Introduction The Cooling/Bleed model allows both the simulation of cooling flows injected through solid walls into the flow or bleed flows where mass flow leaves the main flow through solid wall. The adopted technique makes use of additional sources of mass, momentum and energy located at given points or along given lines of the solid walls and does not require the meshing of the cooling flow injection channels. The objective of this model is not to describe the details of the cooling flow itself but rather to consider its effect on the main flow. In the next sections the following information is given on the Cooling/Bleed model: • section 7-4.4 provides a theoretical description of the approach used to solve the cooling flow problem. • section 7-4.3 gives a summary of the available expert parameters related to cooling or bleed flow. • section 7-4.2 describes how to set up a project involving the Cooling/Bleed model under the FINE™ user environment. FINE™ 7-15 Optional Models Cooling/Bleed 7-4.2 Cooling/Bleed Model in the FINE™ Interface The Cooling/Bleed model can be directly activated from the FINE™ interface by opening the Cooling/Bleed page under Optional Models. The layout of the page is shown in Figure 7.4.2-7. a) b) c) FIGURE 7.4.2-7 Cooling/Bleed page in FINE™ The list box on the top of the page (a) displays all the injectors (Cooling or Bleed) imported or added by the user. The buttons below the list enable to add, edit, remove or import (more details on data file in section 7-4.5) injectors (b). Clicking with the left mouse button over a selected injector will display its corresponding parameters in the lower part of the page (c). Clicking with the right mouse button over a selected injector will display a popup menu enabling to add/edit/remove the injector. 7-4.2.1 Injector Sector Wizard When adding an injector (Add Injector), for each injection the following parameters need to be specified through a wizard: • injector name, • injector role: Cooling or Bleed, • injector solid patches location, • definition of the geometry, • position of the injector, • flow parameters. On the first page of this wizard the user can enter the name, the role, the solid patches, the geometry definition and the type of positioning of the injector. 7-16 FINE™ Cooling/Bleed Optional Models FIGURE 7.4.2-8 Injection Sector Wizard a) Injection Sector Name The name should be entered by moving the mouse to the text box for the Injector Name and to type the name on the keyboard. By default a name is proposed like injector_1. It is strongly recommended to use only standard english letters, arabic numerals and underscore "_" symbol when naming an injection sector. Non-standard characters may not be recognized or may be misinterpreted when using the project on other computers. b) Injection Sector Role The role of the injector should be entered: Cooling if the flow is injected through solid walls into the main flow or Bleed if part of the mass flow leaves the main flow through solid walls. c) Injection Sector Geometry Three types of injection sectors can be defined through the interface: point, line or slot. • the point type corresponds to a single cooling hole. • the line type stands for a series of cooling holes regularly distributed along a line with the same geometrical and flow properties. • a hub or shroud slot is a continuous line of holes placed at constant radius and axial position (typically used on the hub or shroud surface of a turbomachine). Slots are only defined along axisymmetric surfaces. In case a slot (or a line) should traverse several patches (as for instance in a HOH mesh configuration) all the patches should be selected and one single slot should be created. d) Injection Sector Positioning Four modes are available to place the holes: FINE™ 7-17 Optional Models Cooling/Bleed • Relative mode: this mode is used for blade walls and is valid for AutoGrid meshes only. In this case, the spanwise and streamwise positions of the hole (or of the 2 extremities in the case of a line of holes) are specified. • Space Cartesian mode: the user specifies the (X,Y,Z) Cartesian coordinates of the hole or of the 2 extremities for a line. For a slot the user enters the radius and the Z-coordinate of one point of the slot. • Space Cylindrical mode: the user specifies the (R,θ,Z) cylindrical coordinates of the hole or of the 2 extremities for a line. For a slot the user enters the radius and the Z-coordinate of one point of the slot. • Grid mode: the user specifies the (I,J,K) indices of the hole or of the 2 extremities of a line of holes. The injection sectors of type "Slot" can not be presented in relative coordinates. The combination of injector geometry and positioning can be summarized as follow: TABLE 7-1 Injector sector geometry/positioning combination and restriction To cancel the modifications to the injector definition and close the wizard click on the Cancel button. Once the injector sector role, type and mode are correctly set, click on Next>> to go to the next page of the wizard. On this page, depending of the role, type and mode of injector, the flow parameters and geometry/positioning parameters have to be defined in the second page of the wizard. When defining a cooling or bleed using the Cartesian or cylindrical coordinates no procedure are implemented to check if the specified direction is correct. e) Injection Sector Geometry/Positioning Parameters As presented in Table 7-1, 11 combinations are available. As the transformation from cylindrical to Cartesian coordinates is obvious, only 8 combinations will be described in more details. e.1) Relative positioning for a single hole The user specifies the diameter of the hole in case of a single hole. Each hole is circular. The diameter of the hole is specified by the user but a hole is included in one cell only even when the diameter exceeds the cell width. 7-18 FINE™ Cooling/Bleed Optional Models As for the old algorithm, the holes are located by means of a spanwise and a streamwise relative position. The algorithm can be applied to H, I or O-meshes generated by AutoGrid. For O-mesh the blade surface is divided in two different sub-patches (one for the pressure side and one for the suction side). Therefore, the user has to select on which side of the blade (Side1/Side2) the injection will be located. A button has been added in the interface in order to select the side. This button is active only for O-meshes. FIGURE 7.4.2-9 Geometry Parameters for relative positioning of a hole Only the version of AutoGrid provided with FINE™ 6.1-1 (and latter versions) can be used to generate the mesh and this relative positioning is only available for blade surfaces. The location is defined as a fraction of the arc length from hub to shroud and from the leading edge to the trailing edge. Spanwise and streamwise coordinates are computed for each cell vertex. The closest point found in this relative coordinate frame is the one that is concerned by the injection. An option has been set-up in order to use the axial chord (Axial Coordinates button) instead of the arc length (only available for axial machines). The relative positioning does not accept meshes with a blunt at the leading edge FIGURE 7.4.2-10 . Relative positioning of a hole at 70% spanwise and 50% streamwise. Finally, when a cooling injection sector has been selected, three ways to impose the injection direction are proposed through the interface: Cartesian, cylindrical or grid indices. FINE™ 7-19 Optional Models Cooling/Bleed When Grid Indices is selected, the injection direction is provided by the user through 2 angles expressed in degrees (depending of the units selected in the menu File/Preferences). Each angle is measured with respect to the local normal and one of the 2 grid line directions tangent to the wall. In case of an I J K = ct surface, the angles are measured with respect to the ( J, K ) ( K, I ) ( I, J ) grid lines respectively. Figure 7.4.2-11 illustrates the definition of angle βk for an I = cst surface. I=constant surface V J K βk n βk is the angle of the velocity projection in the (K,n) plane with respect to the normal n to the surface. Angle definition in the cooling flow page of the FINE™ interface FIGURE 7.4.2-11 Each angle is defined as: ⎠ ⎞ Vi, j, k β i, j, k = atan -----------Vn ⎝ ⎛ (7-18) For example, in order to make the velocity direction oriented along the normal, the two angles should be set equal to 0. A 90 degrees angle is not allowed as it will induce a velocity vector tangent to the corresponding grid line direction, with null mass flow. For holes located on the blade walls and when the mesh is generated with Numeca’s AutoGrid software, the K- and J- lines are the two tangent directions along the blade wall, respectively oriented in the streamwise and spanwise directions. e.2) Relative positioning for a line of holes The user specifies the diameter of the hole in case of a line of holes. Furthermore, the number of holes has to be specified and will be uniformly distributed on the line. Each hole is circular. The diameter of the hole is specified by the user but a hole is included in one cell only even when the diameter exceeds the cell width. As for the old algorithm, the line of holes is defined by two points (holes) that are located by means of a spanwise and a streamwise relative position. The algorithm can be applied to H, I or O-meshes generated by AutoGrid. For O-mesh the blade surface is divided in two different sub-patches (one for the pressure side and one for the suction side). Therefore, the user has to select on which side of the blade (Side1/Side2) the injection will be located. A button has been added in the interface in order to select the side. This button is active only for O-meshes. 7-20 FINE™ Cooling/Bleed Optional Models For each point of the line the algorithm works as for the single hole positioning. FIGURE 7.4.2-12 Geometry Parameters for relative positioning of a line of holes Only the version of AutoGrid provided with FINE™ 6.1-1 (and latter versions) can be used to generate the mesh and this relative positioning is only available for blade surfaces. The location is defined as a fraction of the arc length from hub to shroud and from the leading edge to the trailing edge. Spanwise and streamwise coordinates are computed for each cell vertex. The closest point found in this relative coordinate frame is the one that is concerned by the injection. An option has been set-up in order to use the axial chord (Axial Coordinates button) instead of the arc length (only available for axial machines). The relative positioning does not accept meshes with a blunt at the leading edge Finally, three ways to impose the injection direction are proposed through the interface: Cartesian, cylindrical or grid indices. When Grid Indices is selected, refer to the end of section e.1) for more details. e.3) Cartesian positioning for a single hole The user specifies the diameter of the hole in case of a single hole. Each hole is circular. The diameter of the hole is specified by the user but a hole is included in one cell only even when the diameter exceeds the cell width. As for the old algorithm, the holes are located by means of the (X,Y,Z) Cartesian coordinates. For a single hole, the cell that is concerned by the injection is the closest cell face centre to the defined point. In case of repetition, the point is automatically transferred to the meshed patch FINE™ 7-21 Optional Models Cooling/Bleed Furthermore, in order to ease the capture of the right coordinates, the button Get Coordinates enables the user to interactively select the point in the mesh view after opening the mesh through the menu Mesh/View On/Off or Mesh/Tearoff graphics (only available on UNIX). FIGURE 7.4.2-13 Geometry Parameters for space Cartesian positioning of a hole Finally, three ways to impose the injection direction are proposed through the interface: Cartesian, cylindrical or grid indices. When Grid Indices is selected, refer to the end of section e.1) for more details. e.4) Cartesian positioning for a line of holes The user specifies the diameter of the hole in case of a line of holes. Furthermore, the number of holes has to be specified. Each hole is circular. The diameter of the hole is specified by the user but a hole is included in one cell only even when the diameter exceeds the cell width. As for the old algorithm, the line of holes is defined by two points (holes) that are located by means of the (X,Y,Z) Cartesian coordinates. For the two points defining the line, the cells that are concerned by the injection are the closest cell face centre to the defined point. In case of repetition, the point is automatically transferred to the meshed patch FIGURE 7.4.2-14 Geometry Parameters for space Cartesian positioning of a line of holes 7-22 FINE™ Cooling/Bleed Optional Models Furthermore, in order to ease the capture of the right coordinates, the button Get Coordinates enables the user to interactively select the point in the mesh view after opening the mesh through the menu Mesh/View On/Off or Mesh/Tearoff graphics (only available on UNIX). A line is drawn from those two points (this line do not necessarily follow the surface of the patch, see Figure 7.4.2-15). The segment is then uniformly divided into N-1 sub-segments (where N is the number of holes on this line). Each N-2 limits of the sub-segment is then projected on the patch (the closest cell face centre is found). Those are the cells where the injection will be applied. They are not necessarily uniformly distributed on the patch. points defined by user points at cell face centre where injection will be applied View from the top FIGURE 7.4.2-15 Construction View at Constant Radius of a line of holes on a turbine hub For a mesh with an important clustering, or for an important number of points in the line, several projected points could end on the same cell. This is taken into account in the algorithm. The mass flow injected is then multiplied by the relevant factor. Therefore, one should be aware that the number of cells that are highlighted in the interface should not strictly match the number of hole in the line. within Parametric Space without Parametric Space FIGURE 7.4.2-16 Definition of a line of holes without or within the parametric space FINE™ 7-23 Optional Models Cooling/Bleed On the contrary for a mesh with a relatively poor spatial discretisation, the location of the cell face centres where the injection will be applied will not be strictly on a line. A limitation of this algorithm is that the line does not necessarily follow the patch surface. Therefore, defining a line of holes at the hub of a gap (upper surface of a rotor blade) could produce the problem presented on the left side of Figure 7.4.2-16. The same problem can arise generally on a convex surface. In order to solve this problem, it has been decided to allow the user to define a line of holes following a parametric surface defined by the grid lines by activating Parametric Space. Therefore, a line of hole on a convex surface could be more easily defined (right side of Figure 7.4.2-16). One limitation of this option is that a line of hole cannot cross a connection. For instance defining a line of holes (in the parametric space) close to the trailing edge of a O mesh will produce the result sketched bellow. POSSIBLE FIGURE 7.4.2-17 Definition of a line of holes in the parametric space. For turbomachinery configuration with periodic conditions, points could be located either on the meshed passage or on one of its repetitions. Therefore, the injections should automatically be transferred to the meshed patch. Two methods are available. FINE™ 6.1 FINE™ 6.2 Meshed Patches Repetition Meshed Patches Repetition FIGURE 7.4.2-18 Two methods to respect repetition for a line of 3 holes. 7-24 FINE™ Cooling/Bleed Optional Models • In FINE™ 6.1, the method was transferring only the extremities of the line of holes to the meshed patch. • In FINE™ 6.2, the method is rotating only the final position of the injections in order to be located on the meshed patch. As illustrated in Figure 7.4.2-18, those two options could lead to rather different results. In case of multi-patch selection the algorithm described above is applied independently for each patch. Therefore, a direct definition of a line of hole crossing several patches is not possible. In this case it is recommended to define as many line as necessary (see figure bellow). In order to overcome this problem the multi-patch selection has been restricted to the slots defined by Cartesian or cylindrical coordinates. FINE™ 6.1 FINE™ 6.2 FIGURE 7.4.2-19 Example of definition of a line of 5 holes with multi-patch selection. Finally, three ways to impose the injection direction are proposed through the interface: Cartesian, cylindrical or grid indices. When Grid Indices is selected, refer to the end of section e.1) for more details. e.5) Cartesian positioning for a slot The user specifies the width of the slot. has to be specified. The multi-patch selection has been restricted to the slots defined by Cartesian or cylindrical coordinates. FIGURE 7.4.2-20 Geometry Parameters for space Cartesian positioning of a slot FINE™ 7-25 Optional Models Cooling/Bleed For the positioning of the slot, the radius and z values are asked to the user. The closest cell face of the patch to this point is found. The radius and axial position of this cell face centre become the slot position in the (r,z) plane. It should be noted that this slot position is not identical to the initial user input. For most axial machines the radius can be easily identify by calculating the closest point on the patch. In this case only the axial position of the slot is required in the interface. For radial machines, or for axial machines with complex vein geometry, the two components of the original point are required (Figure 7.4.2-21). Axial Machine Radial Machine FIGURE 7.4.2-21 Examples of slot positioning The algorithm that defines the cell faces that are concerned by this slot is the following one. For each cell face of the patch, the two extremities in the (r,z) plane of this polygon (A,B and A’,B’) are identified (i.e., the two vertices with the maximum distance in this plane). They define the limits of the cell face in the (r,z) plane. If those two points are called A,B for cell 1 and A’,B’ for cell 2, and S is the slot location specified by the user in the (r,z) plane through FINE™, as presented on Figure 7.4.2-22, S is only included in the domain of cell 1 limited by A,B in the (r,z) plane, therefore, the cell 1 is the only cell concerned by the slot S. FIGURE 7.4.2-22 Identification of the cells concerned by the slot S in the (r,z) plane. δ is the distance between A and B. 7-26 FINE™ Cooling/Bleed Optional Models On the contrary, S is not inside the domain defined by A',B'. Thus, the cell 2 will not be concerned by the slot. For O-meshes with small cells close to leading or trailing edges, this algorithm could leads to missing cells. This problem is due to a (r,z) position specified by the user in FINE™ for the slot that is not precise enough. not precise enough value exact value points are missing points are represented FIGURE 7.4.2-23 Definition of a slot for a O-mesh Furthermore, in order to ease the capture of the right coordinates, the button Get Coordinates enables the user to interactively select the point in the mesh view after opening the mesh through the menu Mesh/View On/Off or Mesh/Tearoff graphics (only available on UNIX). Finally, three ways to impose the injection direction are proposed through the interface: Cartesian, cylindrical or grid indices. When Grid Indices is selected, refer to the end of section e.1) for more details. e.6) Grid positioning for a single hole The user specifies the diameter of the hole in case of a single hole. Each hole is circular. The diameter of the hole is specified by the user but a hole is included in one cell only even when the diameter exceeds the cell width. The grid positioning used in EURANUS depends on the grid indices of the centre of the cell faces. It is different from the grid indices used in IGG™ and in CFView™. The grid indices are directly used by the flow solver in order to introduce the flow of mass, momentum and energy at this cell face. FINE™ 7-27 Optional Models Cooling/Bleed FIGURE 7.4.2-24 Geometry Parameters for Grid positioning of a hole Finally, three ways to impose the injection direction are proposed through the interface: Cartesian, cylindrical or grid indices. When Grid Indices is selected, refer to the end of section e.1) for more details. e.7) Grid positioning for a line of holes The user specifies the diameter of the hole in case of a line of holes. Furthermore, the number of holes has to be specified. Each hole is circular. The diameter of the hole is specified by the user but a hole is included in one cell only even when the diameter exceeds the cell width. From the two cell face centres defined in the interface, two geometrical points are defined by their (x,y,z) coordinates. Then, a line is constructed in the same way as for the Cartesian positioning (section e.4). In this case there is no problem of repetition because the two extremities of the line are located on the meshed patch. Furthermore, concerning the Parametric Space option, refer to section e.4) on page 7-24 for more details. FIGURE 7.4.2-25 Geometry Parameters for Grid positioning of a line of holes Finally, three ways to impose the injection direction are proposed through the interface: Cartesian, cylindrical or grid indices. When Grid Indices is selected, refer to the end of section e.1) for more details. 7-28 FINE™ Cooling/Bleed Optional Models e.8) Grid positioning for a slot The user specifies the width of the slot. has to be specified. From the grid indices a geometrical point is defined. Then the slot is defined in the same way as for the Cartesian positioning (section e.5). FIGURE 7.4.2-26 Geometry Parameters for Grid positioning of a slot Finally, three ways to impose the injection direction are proposed through the interface: Cartesian, cylindrical or grid indices. When Grid Indices is selected, refer to the end of section e.1) for more details. f) Flow Parameters The user has to specify the Mass flow: the specified mass flow is actually the total mass flow through all the blades and through all the holes in the case of a line of holes. Thus the mass flow through one hole is the specified mass flow divided by the number of blades and the number of holes. The mass flow is often responsible for initialization troubles as it might be too high. The FINE™ interface allows a tuning of the specified mass flow through an expert parameter. This is described in section 7-4.3. For cooling flow the mass flow specified in FINE™ will be considered as positive and as negative for bleed flow. FIGURE 7.4.2-27 Flow Parameters for Bleed FIGURE 7.4.2-28 Flow Parameters for Cooling FINE™ 7-29 Optional Models Cooling/Bleed Furthermore, the Arrows scaling factor parameter enables the user to control the shape of the arrows representing the injection direction after opening the mesh through the menu Mesh/View On/Off or Mesh/Tearoff graphics (only available on UNIX). For cooling additional parameters have to be defined: • static or total temperature. • turbulent kinetic energy and dissipation or turbulent intensity when the k-ε model is used. • kinematic turbulent viscosity when the Spalart-Allmaras model is used. 7-4.2.2 Injector Sector Visualization When adding an injection sector into FINE™, the location (cell face are highlighted) and the direction of the injection can be visualized. In order to be able to visualize, the user has to load the mesh through the menu Mesh/View On/Off. FIGURE 7.4.2-29 Injection Sector Visualization within FINE™ The parameters area will then be overlapped by the graphic window, and the small control button on the upper - left corner of the graphic window can be used to resize the graphics area in order to visualize simultaneously the parameters and the mesh (see section 2-10). Mesh/Tearoff graphics is only available on UNIX and enables to open the mesh in a new window. 7-30 FINE™ Cooling/Bleed Optional Models Furthermore, new outputs have been added into FINE™ on the Outputs/Computed Variables page under the thumbnail Solid data in order to enable the visualisation in CFView™ of the injected flow and the injection direction. FIGURE 7.4.2-30 Injector Sector Outputs for CFView™ 7-4.3 Expert Parameters a) COOLRT In the old algorithm (COOLFL=0), in case some difficulties appear at the beginning of the simulation, the mass flow can be reduced with the expert parameter COOLRT. The value of COOLRT (less than 1) corresponds to a constant factor applied to the imposed mass flow. This parameter has an influence on the initialization as the specified mass flow is sometimes too large. The user should definitely tune this parameter in case of problems. b) ZMNMX In the old algorithm (COOLFL=0) for the relative mode, the injector position in streamwise direction can be provided with 0 and 1 defined in two different ways: ZMNMX = 0 (default): the leading and trailing edges are the grid edges, i.e the points where the periodic lines of the mesh meet the blade walls = 1: the points located at respectively the minimum and maximum axial positions. c) COOLFL There is a possibility to specify the cooling/bleed flow data through an external input file with the extension ’.cooling-holes’. This file can be useful in case the flow calculation is integrated into an automatic procedure. For more details on the format of the file, refer to section 7-4.5. COOLFL = 0: the old algorithm of the cooling/bleed model will be used (model used in FINE™ 6.1 and previous releases). The backward is ensured through this parameter set at 0. = 1: the old algorithm of the cooling/bleed model will be used (model used in FINE™ 6.1 and previous releases) based on an external file with the extension ’.cooling-holes’ located in the corresponding computation subfolder will be read and the data specified through the FINE™ interface will be ignored. = 2 (default): the new algorithm of the cooling/bleed model will be used. FINE™ 7-31 Optional Models Cooling/Bleed d) MAXNBS The maximum allowed number of injection sectors is controlled through the expert parameter MAXNBS (the default value is 50). If the input file contains a higher number of sectors the parameter should be modified. 7-4.4 Theory If COOLFL=0, the model consists in the addition of local source terms to all the flow equations (mass, momentum, energy and k-e equations when a 2-equations turbulence model is used). These terms are added as fluxes through the solid boundary cells where a cooling hole has been placed by the user. Fluxes are computed as: • Mass: • Momentum • Energy • k,ε-equations: F F mass = ρV n S x, y, z momentum energy = ρVx, y, z V n S + p∗ n x, y, z S F = V n ( ρE + p∗ )S k, ε F = ρV n ( k, ε )S where ρ is the density, Vn is the velocity component normal to the solid wall and S is the cooling hole surface.The increased static pressure is computed as: 2 p∗ = p + -- ρk 3 and the total energy E* is: V2 E∗ = e + -- + k 2 (7-20) (7-19) The density required to calculate the velocity components is obtained from the computed pressure field along the walls and from the imposed static or total temperature. Note that for the momentum equations only the velocity term is added as a source term. The pressure term already exists even in the absence of holes. If COOLFL=2, the cooling injection/bleed are treated as additionnal inlet or outlet boundary condition. Finally, the turbulent kinetic energy and dissipation can either be directly imposed by the user or be calculated from the turbulent intensity. In that case, the turbulent kinetic energy is obtained as: k = 1.5 ( Tu ⋅ V ) 2 (7-21) where V is the velocity magnitude and Tu is the turbulent intensity. The turbulent dissipation is obtained from the relation: Cµ k ε = ------------------0.1D where D is the diameter of the hole and Cµ = 0.09. It should be noted that the velocity remains equal to zero at the walls even in the cooling flow region. Thus the boundary condition on the velocity is left unchanged and the 0.75 1.5 (7-22) 7-32 FINE™ Cooling/Bleed Optional Models effect of the cooling flow will be observed in the surrounding cells. However, the temperature field will be affected on the wall itself. 7-4.5 Cooling/Bleed Data File: ’.cooling-holes’ A parser is used to find the data in this file, using keywords to locate the position of the data in the file. The advantage of this technique is that the data do not have to be positioned at a given line in the file, but only have to be followed by the appropriate keyword (the keywords can be written with capitals or not). The user specifies in the file a series of 'injection sectors'. An injection sector is either — a single cooling hole — a series of distributed cooling holes along a line (all holes having the same geometrical and flow properties) — a hub or shroud slot (continuous line of holes along a constant radius and axial position line) Each injection sector should respectively start and end with the keywords INJECTION SECTOR END DATA Each injection sector should contain all the appropriate data. If one data is missing, the flow solver will stop and a message will appear on the screen. 7-4.5.1 Specification of an injection sector a) Type of injection sector The user should start by defining if the sector is a single injection hole (1), a line of holes (2) or a slot (3): b) Boundary patch The user should specify the block and face number, as well as the boundary patch on which the holes are located. The face number can be 1 (I=1), 2 (J=1), 3 (K=1), 4 (K=KM), 5 (J=JM), 6 (I=IM) The patch number is only required if several solid patches are present on the face (for instance on a hub or shroud wall). c) Position of the holes and slot Three modes are available to locate the holes: c.1) Relative Positioning - for blade walls (can not be used for slots) • spanwise position(s) of the hole or of the 2 extremities of the line of holes (between 0 at the hub and 1 at the shroud) • streamwise position(s) of the hole or of the 2 extremities of the line of holes (between 0 at the leading edge and 1 at the trailing edge). The leading and trailing edges can either be the grid edges, i.e. the points where the periodic lines of the mesh meet the blade walls (parameter ZMNMX=0), or the points located at respectively the minimum and maximum axial positions (parameter ZMNMX=1, valid for axial flow machines). The choice between the two possibilities is made through the expert parameter ZMNMX, whose default value is 0. Note that this "blade wall" positioning option is only valid for H- or I-type meshes, the FINE™ 7-33 Optional Models Cooling/Bleed pressure and suction surfaces being assumed to be located on two opposite faces of the mesh. c.2) space Cartesian (X,Y,Z) positioning data • in case of a hole or of a line of holes the user specifies the Cartesian coordinates of the hole or of the 2 extremities. • in case of slot the user specifies the radius and the Z-coordinate of one point of the slot. A searching procedure is applied to find the closest solid wall cell to the specified point(s). The point is periodically repeated around the machine axis so that the specified point does not need to be located in the blade passage used for the computation. c.3) Grid positioning data The user specifies the grid indices of the hole, of one point of the slot or of the 2 extremities of the line of holes. Depending on the face number, only 2 indices have to be provided (for instance, along the I=1 face, only the J and K indices are required). d) Size of the holes or Width of the slot The user specifies in addition either the diameter of the holes in case of a single hole or a line of holes, or the width of the slot (in meters). e) Flow properties • the mass flow through the hole(s): the specified mass flow is the total mass flow through all the blades. In case of a line of holes, the specified mass flow is the overall mass flow through all the holes. Therefore the mass flow through one hole is the specified mass flow divided by the number of blades and by the number of holes. Mass flow has to be negative for Bleed flow. • the static or total temperature (if both are present only the static temperature will be read). • he turbulent kinetic energy and dissipation, or the turbulent intensity (if the k-ε model is used). The kinematic turbulent viscosity (if Spalart-Allmaras model is used) cannot be specified through an external file ’cooling-holes’. f) Velocity direction Finally, when a cooling injection sector has been selected, three ways to impose the injection direction are proposed through the interface: Cartesian, cylindrical or grid indices. When the injection direction is provided by the user through grid indices, 2 angles have to be expressed in degrees. Each angle is measured with respect to the local normal and one of the 2 grid line directions tangent to the wall. The user specifies 2 of the following 3 angles (in degrees), depending on the face on which the hole is located: • Angle with respect to I-grid line • Angle with respect to J-grid line • Angle with respect to K-grid line β i , j , k = arctg ( Vi , j , k Vn ) Note that the two angles should be equal to 0 degree to make the velocity direction oriented in the normal direction to the blade wall, whereas a 90 degrees angle induces the velocity vector to be tangent to the corresponding grid line direction. In the case of holes located on the blade walls, and if the mesh has been generated with the AutoGrid software, the K- and J-lines are the two tangent directions along the blade wall, respectively oriented in the streamwise and spanwise directions. The K-angle is the streamwise angle, whereas the J-angle is the spanwise angle. 7-34 FINE™ Cooling/Bleed Optional Models 7-4.5.2 Summary of all required input data a) Global Data Keyword type number of holes diameter width block face patch mode Single hole (1), line(2) or slot(3) Number of holes (if line) Diameter (single hole or line) Width (slot) Block Number Face Number Patch Number (only if several patches) Input Mode (1-relative, 2-Cartesian(X,Y,Z), 3-Grid(I,J,K)) b) Positioning Positioning - Single Injection Hole if mode 1 Streamwise position of the hole Spanwise position of the hole Positioning - Single Injection Hole if mode 2 X-coordinate of the hole Y-coordinate of the hole Z-coordinate of the hole Positioning - Single Injection Hole if mode 3 I-index of the hole J-index of the hole K-index of the hole Positioning - Line of Injection Holes if mode 1 Streamwise position of first point Spanwise position of first point Streamwise position of second point Spanwise position of second point Positioning - Line of Injection Holes if mode 2 X-coordinate of first point Y-coordinate of first point Z-coordinate of first point X-coordinate of second point Y-coordinate of second point Z-coordinate of second point Positioning - Line of Injection Holes if mode 3 I-index of first point J-index of first point K-index of first point I-index of second point J-index of second point K-index of second point Keyword Streamwise position Spanwise position X-coordinate Y-coordinate Z-coordinate I-index J-index K-index streamwise position of first point spanwise position of first point streamwise position of second point spanwise position of second point X-coordinate of first point Y-coordinate of first point Z-coordinate of first point X-coordinate of second point Y-coordinate of second point Z-coordinate of second point I-index of first point J-index of first point K-index of first point I-index of second point J-index of second point K-index of second point FINE™ 7-35 Optional Models Cooling/Bleed Positioning - Slot - mode 2 Radius of one point of slot Z-coordinate of one point of slot Positioning - Slot - mode 3 I-index of one point of slot J-index of one point of slot K-index of one point of slot radius Z-coordinate I-index J-index K-index c) Flow Properties Keyword mass flow static temperature total temperature width turbulent dissipation turbulent intensity Mass Flow (negative if bleed flow) Static Temperature (only for cooling flow) Total Temperature (only for cooling flow) Turbulent Kinetic Energy (only for cooling flow and k-ε model) Turbulent Dissipation (only for cooling flow and k-ε model) Turbulent Intensity (only for cooling flow and k-ε model) d) Flow Direction (only for cooling flow) Flow Direction - Cartesian mode Angle with respect to x-direction(degrees) Angle with respect to y-direction(degrees) Angle with respect to z-direction(degrees) Flow Direction - Cylindrical mode Angle with respect to r-direction(degrees) Angle with respect to theta-direction(degrees) Angle with respect to z-direction(degrees) Flow Direction - Grid mode Angle with respect to K-grid line(degrees) Angle with respect to J-grid line(degrees) Angle with respect to I-grid line(degrees) Keyword x-angle y-angle z-angle r-angle theta-angle z-angle K-angle J-angle I-angle 7-4.5.3 Examples Example 1 - Bleed Flow through a Slot define in Grid (I,J,K) mode 7-36 FINE™ Transition Model Optional Models Example 2 - Bleed Flow through a Slot define in Cartesian (X,Y,Z) mode Example 3 - Cooling Flow through a Hole define in Cartesian (X,Y,Z) mode 7-5 7-5.1 Transition Model Transition Model Introduction The boundary layer which develops on the surface of a solid body starts as a laminar layer but becomes turbulent over a relatively short distance known as the transition region. This LaminarTurbulent transition is a complex and not yet fully understood phenomenon. Among the numerous parameters that affect the transition one can list: the free stream turbulence intensity, the pressure gradient, the Reynolds number, and the surface curvature. Furthermore, predicting the onset of turbulence is a critical component of many engineering flows. It can have a tremendous impact on the overall drag, heat transfer, and performances especially for low-Reynolds number applications. However, most of the turbulent models fail to predict the transition location. Therefore, it is proposed to include a transition model in the original Spalart-Allmaras turbulence model in order to take into account the transition onset at a certain chord distance on a blade pressure and suction sides. The transition location (transition line in 3D) should be imposed either through a FINE™ 7-37 Optional Models Transition Model user input or via a separate guess. It should be pointed out that these transition terms should only be active when the transition module is used. When it is not used, the fully turbulent version of the Spalart-Allmaras turbulence model remains unchanged. In the next sections the following information is given on the Transition Model: • section 7-4.4 provides a theoretical description of the approach used to solve the transition region. • section 7-4.3 gives a summary of the available expert parameters related to the Transition model. • section 7-4.2 describes how to set up a project involving the Transition Model under the FINE™ user environment. 7-5.2 Transition Model in the FINE™ Interface The transition model can be directly activated from the FINE™ interface by opening the Transition Model page under Optional Models. The layout of the page is shown in Figure 7.4.2-7. FIGURE 7.5.2-31 Transition Model page in FINE™ A list of all the blades appears in the left box and the remaining area is divided into two boxes for suction and pressure side, respectively. Four choices are possible: — — — — Fully Turbulent Fully Laminar Forced Transition Abu-Ghannam and Shaw (AGS) Model Furthermore, for Forced Transition, the user has to specify the position of the transition lines on each side of each blade. It is based on the relative stream-wise position and it is defined as a line on the blade pressure and/or suction sides from hub to shroud. The user specifies two anchor points through which a straight line will be built by the solver. It should be noted that only blades are transitional while end walls are fully turbulent. The transition model is only available for the one-equation Spalart-Allmaras model using AutoGrid mesh and is applied to blade boundaries and work in both steady and 7-38 FINE™ Transition Model Optional Models unsteady modes. The transition model is not adapted to external cases. R/S interfaces should be correctly oriented (from upstream to downstream) and solid wall of the blades should be adiabatic. For the Abu-Ghannam and Shaw model: only one "downstream" R/S upstream of each blade is allowed. Furthermore, there are no restrictions on the number of inlets. Finally, a new output has been added into FINE™ on the Outputs/Computed Variables page under the thumbnail Solid data in order to enable the visualisation in CFView™ of Intermittency (more details on this quantity in section 7-5.4). 7-5.3 Expert Parameters INITRA (integer): control the number of multigrid iterations (default = 100) performed in fully turbulent after the coarse grid initialization process. Thereafter, the blade pressure side and suction side are identified and the transition line is defined. The computation pursue for the remaining iterations in transitional mode. The transition line derived from the Abu-Ghannam and Shaw model is computed at each iteration. . Fully Turbulent MultiGrid Initialization Full MultiGrid Coarse Grid Initialization INITRA Transition Model MultiGrid For starting or restarting a computation in transitional mode from a previous solution (fully turbulent or in transitional mode) the expert parameter INITRA should be set to 0 (otherwise iterations will be performed in fully turbulent mode). INTERI (integer): control the type of intermittency distribution (0:binary or 1: from Dhawan and Narasimah) (default = 0). INTERL (integer): control the type of location used for forced transition (0: base on arc length or 1: based on axial chord) (default = 0). FTURBT (real): control the proportion close to the trailing edge that is fully turbulent (default = 0.95). FINE™ 7-39 Optional Models Transition Model FTRAST (real): prevents the transition to start in an area defined from the leading edge of the mesh. The value set is a percentage of the chord upstream of which the transition is not allowed (by default 0.05: 5%). ITRWKI (integer): switches on the wake induced transition model. When activated (ITRWKI set to 1), the free stream turbulence intensity (defined at the inlet or at the rotor/stator interface) and the turbulence intensity from the boundary layer edge are used to define the transition region. When this parameter is not checked, only the free stream turbulence intensity is used. 7-5.4 Theory The Transition Model consists of introducing a so-called intermittency, Γ, defined as the fraction of time during which the flow over any point on a surface is turbulent. It should be zero in the laminar boundary layer and one in fully developed turbulent boundary layer. The intermittency function is defined on each point of the blade surface and at each iteration. It is extended to the computational domain by a simple orthogonal extension (i.e., each point of the computational domain has the same intermittency than the closest point on the blade surface). The intermittency is used to multiply the turbulence production term. For the Spalart-Allmaras turbulence model this gives: ~ ~ S = ΓS (7-23) ˜ where S is the production term in the Spalart-Allmaras in Eq. 4-52. Free-stream wakes (with only a weak production term) will not be affected by the intermittency. A laminar boundary layer will be preserved upstream of the transition location and turbulence could freely develop thereafter. The transition location imposed by the user through the Forced Transition option and by the AGS Model is only appearing if it has been defined in a turbulent boundary layer. 7-5.4.1 Fully Turbulent When the Fully Turbulent model is selected, the intermittency, Γ is set at 1 on the whole blade suction and/or pressure sides (fully developed turbulent boundary layer). 7-5.4.2 Fully Laminar When the Fully Laminar model is selected, the intermittency, Γ is set at 0 on the whole blade suction and/or pressure sides (laminar boundary layer). 7-5.4.3 Forced Transition The first step is to have a description of the blades in EURANUS to be able to position the transition line. Therefore AutoGrid has been adapted to output the position of the leading and trailing edges and the topological patches composing the blade surfaces. This last information is read by FINE™ and transmitted to the solver EURANUS. A dialog box has been created to allow the positioning the transition line on the blade surfaces (Figure 7.5.4-32). 7-40 FINE™ Transition Model Optional Models In Forced Transition mode, each transition line is positioned through a point on the hub and a point on the shroud. By default, these points are defined by a percentage of the arc length (Appendix 7.5.4-32). However, a special treatment is also available where the transition points are defined by a percentage of the axial chord (only available for axial machines). This option can be activated via the expert parameter INTERL that should be set to 1 (default value = 0). The intermittency, Γ, is then computed on each point of the blade surface (it is set to 0 upstream of the transition line and tends towards 1 downstream). Each point of the computational domain has the same intermittency as the one of the closest point on the blade surface. However a special treatment is required close to the trailing edge and in tip gaps. FIGURE 7.5.4-32 Example of the calculation of a transition point on a blade suction side as a percentage of the chord length. A last aspect of the implementation is the post-processing. Spalart & Allmaras propose in their article a turbulent index to be able to distinguish turbulent zone from laminar zone. This index is implemented in EURANUS as a solid data. It is defined as: it = ~ ∂ν κ ν ω ∂n 1 (7-24) where n is the direction normal to the solid wall. It is near 0 in the laminar zone and near 1 in the turbulent zone. 7-5.4.4 Abu-Ghannam & Shaw Model (AGS) The location of transition could be computed from the flow solution by using empirical relations related to external parameters. It is here proposed to use the correlations obtained by Abu-Ghannam FINE™ 7-41 Optional Models Transition Model and Shaw [1980] and derived from experimental data from transition on a flat plate with pressure gradients. According to these authors transition starts at a momentum thickness Reynolds number: F (λθ ) ⎞ ⎛ τ⎟ Rθs = 163 + exp⎜ F (λθ ) − 6.91 ⎠ . ⎝ λθ is a dimensionless pressure gradient defined as: (7-25) λθ = θ 2 dU e ν ds (7-26) where Ue is the velocity at the edge of the boundary layer, s is the streamwise distance from the leading edge, and θ denotes the momentum thickness in the laminar region. τ is the free stream turbulence level (in %). The function F(λθ ) depends on the sign of the pressure gradient: F (λθ ) = 6.91 + 12.75λθ + 63.64(λθ ) 2 for adverse pressure gradient (λθ < 0), (7-27) F (λθ ) = 6.91 + 2.48λθ − 12.27(λθ ) 2 for a favourable pressure gradient (λθ > 0). (7-28) Therefore, according to these relations, transition is promoted in adverse pressure gradient whereas it is retarded in favourable pressure gradient. The range of application of the AGS correlation is 0.1 > λθ > -0.1, and for a free stream turbulent level ranging from 0.3 to 10%. 7-5.4.5 Expert Parameters Either using the Forced Transition option or the Abu-Ghannam and Shaw (AGS) Model, the streamwise evolution of intermittency should be defined. It could be either a binary field or a smoother field. In the current implementation those two options are available. It is controlled by the expert parameter INTERI. With its default value (INTERI = 0) the intermittency is 0 before transition and 1 after the transition onset. If INTERI = 1, intermittency is defined following the relation of Dhawan and Narasimha [1958]: Γ = 1 − exp(−0.412ξ 2 ) (7-29) ξ= 1 λ Max( s − st ,0) (7-30) where st is the position of the transition onset and s is the current position on the arc from leading edge to trailing edge. λ is the characteristic extent of the transition region and is determined from the correlation: Re λ = 9 Re st 0.75 (7-31) Close to the trailing edge the intermittency is set to 1. This is necessary in order to allow a turbulent wake to be generated downstream of the blade. This special treatment is controlled by the expert parameter FTURBT that is set to 0.95 by default (i.e., only the last 5% of a blade side will have an 7-42 FINE™ Transition Model Optional Models intermittency of 1). In order to get a tri-dimensional distribution of the intermittency, the intermittency of a cell is the one of the closest cell on a solid surface (hub, shroud, and tip gap are fully turbulent and have an intermittency equal to unity). FINE™ 7-43 Optional Models Transition Model 7-44 FINE™ CHAPTER 8: Boundary Conditions 8-1 Overview During the IGG™ grid generation process, the user has to define the type of boundary condition to be imposed along all boundaries. The parameters associated with these boundary condition types can be fully defined using the Boundary Conditions page. This chapter gives a description of the boundary conditions available on the Boundary Conditions page. In section 8-2 the Boundary Conditions page is described. For expert use section 8-3 gives an overview of the available expert parameters. In section 8-4 some advice is provided on the combinations of boundary conditions to use. For more detailed information section 8-5 provides a theoretical description of each available boundary condition 8-2 Boundary Conditions in the FINE™ Interface When selecting the Boundary Conditions page the Parameters area appears as shown in Figure 8.2.0-1. Five thumbnails are available, depending on the boundary condition types defined in the mesh. There are currently five types of boundary conditions available in the NUMECA flow solver: • • • • • inlet, outlet, periodic (connection with or without rotational or translational periodicity), solid walls, external (far-field). Each of those is described in the next sections. Note that the connecting (matching (CON) and non-matching (NMB)) boundary conditions (without periodicity) do not appear in this menu, because they do not require any input from the user. Only the "periodic" conditions appear under the Periodic menu. FINE™ 8-1 Boundary Conditions Boundary Conditions in the FINE™ Interface A common particularity of the five Boundary Conditions pages is their subdivision into two areas. The left area contains always a list of the different patches that are of the boundary condition type of the selected thumbnail. A patch can be identified either by the name of the block face to which it belongs and by its number, or by the numbers of the block and face and by its local index on the face (if no name is provided in IGG™). The right area is the area where the boundary condition parameters are specified for the selected patch(es). FIGURE 8.2.0-1 Boundary Conditions page One or several patches may be selected in the left area by simply clicking on them. Clicking on a patch unselects the currently selected patch(es). It is possible to select several patches situated one after another in the list by clicking on the first one and holding the left mouse button while selecting the next. To select a group of patches that are not situated one after another in the list, the user should click on each of them while simultaneously holding the <Ctrl> key pressed. Several patches can be grouped by selecting them and clicking on the Group button. A dialog box will appear asking for a group name. The name of the group will appear in red color in the list of patches to indicate that this is a group of patches. Every change in the parameters when a group is selected applies to all patches in the group. The Ungroup button removes the group and its patches are displayed individually in the list. The Ungroup button is active only when at least one group is selected. Clicking with the left mouse button on the plus sign + left of a group name in the list will display the patches included in this group. If some of the patches have been given names in IGG™, these names will appear in 8-2 FINE™ Boundary Conditions in the FINE™ Interface Boundary Conditions FINE™. If the patches have been grouped in IGG™, by giving the same name to many patches, they will appear ungrouped in FINE™ (with block, face and patch number shown after the name) to avoid contradiction between grouping in IGG™ and FINE™. Ungroup button will toggle the IGG™ name of the selected patch(es) with the default FINE™ name (block, face and patch number). If the Graphics Area window with the mesh topology of the project is opened (Mesh/View On/Off menu), all the selected patches and/or groups will be highlighted. A click with the right mouse button over a selected patch will select all the patches and groups in the list that have the same parameters. If the user selects several patches that have different parameters, a warning dialog box will appear. When clicking on OK all parameters will be set equal to the ones of the first patch. Selecting Cancel instead will cancel the selection. (1) (2) (3) FIGURE 8.2.0-2 Two patches have been grouped into a group called HUB. The right area of all the notebook boundary condition pages is created in a generic way by means of a resource file, where all the boundary condition parameters are described altogether with their default values. Some boundary conditions are only available for an incompressible, compressible or condensable gas flow. FINE™ will automatically disable the boundary conditions that are not available, depending on the type of fluid selected on the Fluid Model page. Also the type of boundary conditions are adjusted according to the selection for Cartesian or cylindrical boundary conditions. The five pages associated to each of the five types of boundary conditions are described in detail in the following sections. FINE™ 8-3 Boundary Conditions Boundary Conditions in the FINE™ Interface 8-2.1 Inlet Condition 8-2.1.1 Available Inlet Boundary Condition Types The inlet boundary condition page is customized according to the configuration of the project (Cartesian or cylindrical) as shown in the following two figures. The user has the freedom to access both types of configurations in the boundary conditions page independently of the mesh properties. FIGURE 8.2.1-3 Subsonic inlet boundary conditions page for cylindrical problems. FIGURE 8.2.1-4 Subsonic inlet boundary conditions page for Cartesian problems. 8-4 FINE™ Boundary Conditions in the FINE™ Interface Boundary Conditions The upper part of the inlet boundary condition page allows the user to select the type of inlet condition to apply to the selected patches through a series of toggle buttons. There are two categories of inlet conditions: conditions applicable to subsonic inlets and conditions applicable to supersonic inlets. Note that to determine whether an inlet (or an outlet) boundary is subsonic or supersonic, the velocity component normal to the boundary should be considered. For each inlet condition type, the lower part of the page is adapted in order to provide input boxes only for the physical variables that are required to fully determine the boundary condition. These variables are for instance: the pressure and temperature (static or total), the velocity components, the velocity magnitude, the velocity angles (specified in radians), or the mass flow. In case of a simulation involving the k-ε turbulence model, the inlet values of the parameters k and ε are also required. A turbulent viscosity entry appears in case the Spalart-Allmaras turbulence model is used. For the inlet boundary conditions: • The velocity components are defined in the Cartesian or cylindrical coordinate system, depending on the selected type. • The pressure and the temperature values to specify can be the static or the total values. • For rotating configurations, the specified values are always the absolute quantities. Three major types of inlet boundary conditions can be identified: • velocity components and the static temperature, • total pressure, total temperature and the flow angles, • total enthalpy, dryness fraction and the flow angles (only for condensable fluid), • mass flow and the static temperature (see the next paragraph for detail on coupling with the outlet). See section 8-5.1 for more theoretical detail on those boundary conditions. 8-2.1.2 Coupling Temperature with Outlet Taverage Outlet Taverage + ∆T Inlet FIGURE 8.2.1-5 Meridional view of the "Coupling with Outlet ID" functionality When mass flow is imposed at an inlet patch, the temperature may be chosen to be coupled to an outlet patch. The coupling is performed through the static temperature. Only in that case, the average temperature Taverage is computed at the specified outlet and imposed at the inlet as Tinlet = Taverage + ∆T (see Figure 8.2.1-5). The quantity ∆T is a constant temperature difference (>=0 or <0) FINE™ 8-5 Boundary Conditions Boundary Conditions in the FINE™ Interface specified by the user. This is done in FINE™ by choosing Mass Flow Imposed as boundary condition type for the inlet and clicking on the Coupling Temperature With Outlet button. A pull-down menu allows to select which patch of the outlet must be involved in the coupling. The value to be entered in the static temperature box is ∆T. 8-2.1.3 Imposing Variables as an Interpolation Profile Each variable can be defined as constant or as an interpolation profile of the variable. The imposed boundary condition may be variable in space (one or two dimensions) and/or in time (in case of an unsteady calculation). To visualize and/or edit the profile data press the small button ( ) on the right side of the label "profile data". This button opens the Profile Manager with the existing profile. See section 2-12 for a detailed description of the Profile Manager. It offers the possibility to modify or to create a data profile interactively. Click on the OK button to set the new profile to the selected patch(es). FIGURE 8.2.1-6 The Profile Manager The button Surface data toggles 1D and 2D editing modes. It can be used to change the dimension of an existing profile. 2D profiles are displayed as a "cloud of points". Selecting a point will display the f(x,y) value in blue in the corresponding column of the Profile Manager. If a quantity is defined as a function without the definition of a valid profile a warning message will appear when saving the project or opening a new page or thumbnail. In such a case a default constant value is used in the computation. 8-2.2 Outlet Condition For a supersonic outlet all variables are extrapolated. An outlet is considered as supersonic on the basis of the normal velocity direction to the boundary. 8-6 FINE™ Boundary Conditions in the FINE™ Interface Boundary Conditions Three types of subsonic outlet boundary condition are available, as shown in Figure 8.2.2-7. These three different boundary conditions are described in the following paragraphs. An option for treatment of Backflow Control can be activated in the case of radial diffusers outlet. The purpose of this option is to control the total temperature distribution along the exit section. In case the flow partially re-enters the domain through the boundary, the total temperature of the entering flow is controlled so that the entering and outgoing flows globally have the same total temperature. . FIGURE 8.2.2-7 Outlet boundary conditions page. 8-2.2.1 Pressure Imposed There are three different methods to impose the pressure at the outlet: • Static Pressure Imposed: the static pressure is imposed on the boundary, the static temperature and the absolute velocity components are extrapolated. As described for the inlet conditions, the static pressure can be constant or defined as a data profile. • Averaged Static Pressure: if imposing an uniform static pressure at the outlet is not an appropriate approximation of the physical pressure distribution at the outlet this boundary condition may be used. In this case only an averaged value for the static pressure is imposed while the pressure profile (around this average) is extrapolated from the interior field (see section 85.2.1). • Radial Equilibrium: This boundary condition is applicable only to cylindrical problems. It is adapted for a patch in which the mesh lines in the circumferential direction have a constant radius. The outlet static pressure is then imposed on the given radius and the integration of the radial equilibrium law along the spanwise direction permits to calculate the hub-to-shroud profile of the static pressure. A constant static pressure is imposed along the circumferential direction. See section 8-5.2.1 for further details. FINE™ 8-7 Boundary Conditions Boundary Conditions in the FINE™ Interface The pressure imposed at the outlet can be constant or as a function of space and/or time. To define a profile as a function of space and/or time click on the profile button ( box. The Profile Manager will appear as described in section 8-2.1.3. ) right next to the input text 8-2.2.2 Mass Flow Imposed When imposing the mass flow at the outlet the related patches must be grouped. This permits to have several groups of patches, each of the groups constituting an outlet through which the mass flow can be controlled. Two different techniques are available to impose the mass flow: • Velocity Scaling: the pressure is extrapolated and the velocity vector is scaled to respect the mass flow. This technique is only valid for subsonic flows, and is not recommended in case of significant back flows along the exit boundary. • Pressure Adaptation: this boundary condition is identical to the ’Uniform outlet pressure’ or ’Radial equilibrium’ boundary conditions, except from the fact that the exit pressure is automatically modified during the resolution process so that after convergence, the prescribed mass flow is obtained. The pressure asked in addition to the imposed mass flow with both options is only used to create the initial solution and for the full-multigrid process, during which a uniform static pressure outlet condition is used. 8-2.2.3 Characteristic Imposed This boundary condition has been implemented to increase the robustness in the frame of a design process and is only available when using a perfect and real gas in the Fluid Model page. Figure 8.2.2-8 shows as an illustration performance curves for a centrifugal compressor. Near choking conditions the mass flow stays almost constant with a variation of the pressure. Therefore it is recommended in this region to impose the static pressure at the outlet. Near stall however, the pressure varies only slightly with varying mass flow. Therefore it is recommended in this region of the performance curve to impose the mass flow at the outlet instead of the static pressure. (static pressure) (mass flow) FIGURE 8.2.2-8 Example of performance curves for centrifugal compressor 8-8 FINE™ Boundary Conditions in the FINE™ Interface Boundary Conditions In a design process, with a variation of the geometry, it is not always known in advance where in the performance curve the computations are performed. Therefore it is not always possible to choose the appropriate boundary condition at the outlet for the complete design process. To overcome this problem this boundary condition allows to impose a relation between the mass flow and the pressure at the outlet. It is no longer needed to choose between imposing pressure when working around the chocking part and imposing mass flow when working close to the stall limit. The user has to impose a very simple characteristic line defined through 3 parameters: a target outlet mass flow and a target outlet pressure (at point 2 in Figure 8.2.2-8) and the pressure at zero mass flow (point 1 in Figure 8.2.2-8). For more detail on this boundary condition see section 8-5.2. 8-2.3 Periodic Condition One important feature of the IGG™ mesh generator concerns the automatic establishment of all connecting and periodic boundary conditions. The corresponding information is transmitted to the FINE™ interface, with the advantage that the user does not need to specify any input concerning these boundary conditions. In the present version, periodic connection is not allowed for blocks with different rotation speed on each side of an interface. Thus no frozen rotor calculation should be performed with periodic connections. Normally no user input is required on this page. The only periodic boundary condition cases for which a user input is required are those in which some of the boundary conditions have to be applied with a periodicity angle that differs from the global periodicity angle of the block. FIGURE 8.2.3-9 Periodic boundary condition page. In case some input is required this section explains how to define the periodic conditions using the PERIODIC thumbnail. The type of periodicity connection between the patches (Matching or Non Matching) can be entered. A connection is Matching if the numbers of mesh points along the connected patches are FINE™ 8-9 Boundary Conditions Boundary Conditions in the FINE™ Interface identical, and if all the corresponding points along these patches coincide. The Non Matching connection requires the use of an interpolation process to establish the connection, whereas a matching one consists of a single communication of the flow variables. Some additional characteristics need to be given to fully determine the periodic boundary condition: • For rectangular (Cartesian) problems, the user has to specify the translation vector defining the periodicity. The positive translation vector goes from the current patch to the periodicity patches. • For cylindrical problems, the user has to specify the rotation angle in degrees. The rotation angle is calculated from the connected patch to the current patch, according to the rule of the right handed system. 8-2.4 Solid Wall Boundary Condition The solid wall boundary condition page is customized essentially according to the type of calculation (inviscid or viscous). For Euler cases (i.e. inviscid), no parameter is requested for the wall boundary conditions. For Navier-Stokes cases, the box at the top of the page allows to set both velocity and thermal conditions. The type of boundary conditions determines the way the velocity and thermal conditions are defined for the solid boundary. 8-2.4.1 Cylindrical Boundary Condition a) Area Defined Rotation Speed The wall rotation velocity can be constant or area defined (see Figure 8.2.4-10). The area defined option allows to attribute a specific rotation velocity to a rectangular zone in the meridional plane independently of the grid structure. FIGURE 8.2.4-10 Solid boundary conditions page in case of a cylindrical boundary condition 8-10 FINE™ Boundary Conditions in the FINE™ Interface Boundary Conditions When the area defined option is selected, a small picture defining the parameters is displayed (the z axis is the rotation axis, the r axis is the radial axis). The rotation velocity is set to ω 1 outside the domain and to ω 2 inside the domain. The specified range must be a valid range for the used geometry. For example, for an axial machine the limits for rotation of the hub can be defined by setting the lower and higher axial limit to appropriate values. In such a case it is important to set the radial limits such that they include the full solid (hub) patch. b) Thermal Condition Three options are available for the thermal condition: constant heat flux (in W/m2), adiabatic or isothermal. The imposed heat flux or temperature can be constant on the patch or defined as a profile. Use the pull down menu to change Constant Value to for example Fct(space). Click on the profile button to launch the Profile Manager as described insection 8-2.1.3. 8-2.4.2 Cartesian Boundary Conditions The user can define a translation or a rotation velocity vector. In the latter case, the coordinates of the rotation centre are requested. The thermal conditions are similar to those for cylindrical flows. 8-2.4.3 Force and Torque Below the box, a "Compute force and torque" button is provided that permits to include the selected patches in the calculation of the global solid boundary characteristics. For a cylindrical project (as defined in Mesh/Properties) in an internal flow (the expert parameter IINT set to 1 as by default): — the axial thrust, i.e. the projection of the global force on the rotation axis, — the torque, i.e. the couple exerted by the global force, calculated at (0,0,0). These quantities are often calculated on the rotating walls. They are calculated from the pressure and the velocity fields on the walls. The axial thrust is computed as: ∑ F ⋅ nz . S (8-1) The projection of the torque along a given direction z , i.e. the couple exerted by the global force along the rotation axis: ⎠ ⎟ ⎞ ∑r × F S In all other cases the force and torque are computed as: — the lift, — the drag, — the moment calculated at (0,0,0) by default. The direction of the forces and torque as well as the location of the point for the moment can be determined with the expert parameters IDCLP, IDCDP, IDCMP and IXMP (see section 8-3). Within EURANUS v5.1-6 it is possible to calculate and to store the partial torque in the corresponding ".wall" file of the computation through the use of the expert parameter IFRCTO within FINE™ GUI. FINE™ ⎝ ⎜ ⎛ ⋅z (8-2) 8-11 Boundary Conditions Boundary Conditions in the FINE™ Interface The partial torque is the torque computed for each layer on the whole blade. When IFRCTO is set to 2 (1 or 3), the torque is defined on each J-direction (I-direction or K-direction) layer (i.e. when using AutoGrid meshes, J-direction corresponds to the spanwise direction). IFRCTO = 2 Total Torque and Force on Suction Side Partial Torque and Force on Suction Side • 56 = 56 sublayers in J-direction (spanwise) • column 1: %span corresponding to the layer • column 2: Fx on the sublayer • column 3: Fy on the sublayer • column 4: Fz on the sublayer IFRCTO = 0 Total Torque and Force on Suction Side FIGURE 8.2.4-11 File ".wall" when computing partial torque along the blade Finally, the resulting ".wall" will contain, in addition of the global torque and force on the selected blade, the partial torque for each layer along the J-direction of the blade as presented in Figure 8.2.4-11. 8-2.4.4 Properties of Solid for Turbulence In addition, if the standard k-ε model or the non-linear high-Reynolds k-ε model is used, the user has to specify the type of wall ("Smooth" or "Rough") and the following constants: the von Karman constant κ and the B constant. If the wall type is rough, the equivalent roughness height k0 and the height of the zero displacement plane d0 are also required. A description of these constants is provided in section 4-3.6.3. The application field of the ’law of the wall’ imposes restrictions on the grid. The user is strongly advised to check the conformity of this grid with these conditions (section 4-3). 8-12 FINE™ Expert Parameters for Boundary Conditions Boundary Conditions 8-2.5 External Condition (Far-field) The external boundary condition is provided to treat the far-field boundaries when dealing with external flow computations (the expert parameter IINT=0). An example is given in Figure 8.2.5-12. This type of boundary condition determines whether the flow is locally entering or leaving the flow domain and uses the theory of the Riemann invariants to act consequently on the appropriate variables (see section 8-5.4). Depending on the chosen turbulence model, five or seven input boxes are provided to specify the free-stream values of the variables to be used in the boundary condition formulation. FIGURE 8.2.5-12 External (far-field) boundary conditions page. Use an external condition rather than an inlet condition for cases for which it is not known if the flow enters or leaves the domain. Condensable gas is not compatible with external boundary condition. 8-3 8-3.1 Expert Parameters for Boundary Conditions Imposing Velocity Angles of Relative Flow In case of a stator calculation it may be convenient to impose the velocity angles of the relative flow at the exit of the upstream rotor. In case of rotors the user may also prefer to impose relative boundary conditions. This procedure is only available in case total conditions and flow angles are FINE™ 8-13 Boundary Conditions Expert Parameters for Boundary Conditions imposed. In addition to that the extrapolation of Vz must be selected. Note also that both flow angles and total conditions are then treated in the relative mode. The following parameters have to be defined: INLREL: allows to specify relative angles for the cylindrical inlet boundary conditions with total quantities imposed (default value = 0) = 1: inlet for a stator (extrapolation of the axial velocity only). The expert parameter OMGINL has also to be specified, = 2: inlet for a rotor. ANGREL (for stator only): data use with the expert parameter INLREL (default = 1 0.05 0.05): 1st real: relaxation angle (in degrees), 2nd real: distance (%) from hub where the absolute flow angle is extrapolated, 3rd real: distance (%) from shroud where the absolute flow angle is extrapolated. 8-3.2 IMASFL: Extrapolation of Mass Flow at Inlet expert parameter specially dedicated to radial inlets. The mass flow is extrapolated instead of the velocity for the cylindrical inlet boundary conditions with imposed total quantities: = 0 (default): treatment inactive, the velocity is extrapolated, = 1: option activated, extrapolation of the mass-flow. 8-3.3 RELAXP: Outlet Mass Flow Boundary Condition is the under-relaxation for the outlet boundary condition where the mass flow is imposed with the exit pressure adaptation (default value = 1.). VELSCA: is the maximum value allowed for the velocity scaling (outlet boundary condition with mass flow imposed by scaling velocity) (default value = 2.) 8-3.4 IDCDP: Torque and Force Calculation if cylindrical project (as defined in Mesh/Properties) and IINT=1: direction (x,y,z) of axial thrust, in all other cases: direction (x,y,z) of drag. IDCLP: IDCMP: IFRCTO: direction (x,y,z) for lift (not used if cylindrical project and IINT=1), direction (x,y,z) for moment, calculate and to store the partial torque in the corresponding ".wall" file. More details in section 8-2.4.3, on page 11, IXMP: coordinate (x,y,z) of the point around which the moment has to be calculated. 8-14 FINE™ Best Practice for Imposing Boundary Conditions Boundary Conditions 8-3.5 Euler or Navier-Stokes Wall for Viscous Flow If the flow type selected is laminar or turbulent Navier-Stokes, it is possible in Expert Mode to choose between an Euler wall (zero normal velocity) and a Navier-Stokes wall (no-slip condition). Further details on the numerical treatment of the walls are provided in section 8-5.3. Note that the default (’normal mode’) is a Navier-Stokes wall. 8-3.6 Pressure Condition at Solid Wall When the interface is in Expert Mode, two toggle buttons are provided to select the type of pressure condition at the wall: extrapolated or computed from the normal momentum equation. The default (active in Standard Mode) is the extrapolation of the pressure. 8-4 Best Practice for Imposing Boundary Conditions The quality of the flow simulation rests primarily on the quality of the grid and the imposed boundary conditions. In this section the most adapted boundary conditions are proposed according to the type of studied flow. In case of divergence in calculations it is strongly recommended to check by post processing of the solution (in CFView™) that appropriate boundary conditions have been imposed. 8-4.1 Compressible Flows For compressible flows it is recommended that the inlet boundary condition fixes the absolute total quantities (pressure, temperature) and the flow angles and that the outlet boundary condition fixes the static pressure (exit pressure). This exit pressure can be imposed as: • a constant value along the exit, • an average value at the exit, • the pressure at mid-span for radial equilibrium (only for an axial outlet). The static pressure at the exit of the domain is rarely constant. It is thus advised to impose the pressure as an average value or as a initialization data for radial equilibrium. Even if this value of pressure is known, for numerical reasons it is possible that the computed massflow differs from the expected one. It is thus necessary to modify the exit pressure repeatedly until obtaining the accurate mass-flow. This procedure can be numerically expensive especially if the calculations are carried out on fine grid. A solution to overcome this drawback is to impose the mass-flow at the outlet. This can be made by the way of two options: • Velocity Scaling: for low subsonic outlet (Mach number lower than 0.4) this condition fixes the mass-flow at a given control surface by scaling the vectors on this surface. This is not as robust as to impose the exit pressure and is not recommended in case significant backflow are detected along the exit. In this condition the next option is better suited. FINE™ 8-15 Boundary Conditions Theory on Boundary Conditions • Pressure Adaptation: in this case, an automatic procedure introduces a variation of the imposed exit pressure at each iteration of the calculation. The pressure is then iteratively updated in order to reach at convergence the imposed mass-flow. This is not as robust as to impose the exit pressure but is more robust than the velocity scaling option. 8-4.2 Incompressible or Low Speed Flow For compressible or low speed flows it is recommended to impose the mass-flow and the static temperature at the inlet and a static pressure at the exit. This couple of conditions inlet-outlet has a stabilizing effect on calculations and is also well adapted to provide initial solutions for multi-stage calculations. 8-4.3 Special Parameters (for Turbomachinery) In case of flow separation at the outlet of radial diffusers it is recommended to use the backflow treatment option. This option can be activated by pressing the corresponding button (Backflow Control) in the FINE™ interface on the Boundary Conditions page under the OUTLET thumbnail. When end-walls in the inlet regions are strongly varying in radius (e.g. centripetal turbines as in Figure 8.4.3-13) or in case of highly tangential inlet flow angles it is advised to use the IMASFL expert parameter (in the list of expert parameters on the Computation Steering/Control Variables page in Expert Mode). This option is adapted when the inlet boundary conditions fixes the absolute total quantities (pressure, temperature) and is only valid for non-preconditioned computations. When it is activated, the mass-flow is extrapolated instead of the velocity. Radial turbine FIGURE 8.4.3-13 Example of case with strongly varying radius in the inlet1 8-5 Theory on Boundary Conditions The boundary conditions are identified in EURANUS by a number (ITYPE) indicating the type of boundary condition and an index (OPSEL) indicating the variant of the type of boundary condition. In this section the type number and variant index of each described boundary condition is given. 1. Picture from D. Japikse, N.C. Balines, Introduction to Turbomachinery, Concept ETI Inc. and Oxford University Press, 1994. 8-16 FINE™ Theory on Boundary Conditions Boundary Conditions 8-5.1 Inlet Boundary Conditions 8-5.1.1 Cylindrical Inlet Boundary Conditions This boundary condition is activated for the values of the parameter ITYPE = 124 (subsonic) and ITYPE=23 (supersonic). a) Static Quantities Imposed (Subsonic) The complete absolute velocity vector followed by the static temperature on the boundary are specified. Several possibilities exist: • the magnitude of the velocity and the flow angles α and γ are specified (OPSEL = 1): Vθ α = atan ----Vz V γ = atan ----r Vz (8-3) • the magnitude of the velocity and other flow angles δ and ε are specified (OPSEL = 5): Vr δ = acos -----Vm Vt ε = atan -----Vm with V m the meridional velocity ( V m = 2 2 (8-4) V r + V z ). This option has been designed to allow radial inlet with zero axial velocities, • the cylindrical velocity components are specified (OPSEL = 7). The static pressure is extrapolated from the interior by Eq. 8-13, which allows to calculate all the primitive variables on the boundary. For a turbulent calculation with the Spalart-Allmaras model, the turbulent viscosity has also to be specified on the inlet boundary. When the two-equation turbulent model is selected, the boundary values of k and ε have to be specified. These conditions can also be used for incompressible flows. b) Total Quantities Imposed (Subsonic) Several variants are available based on the specification of flow angles or velocity components. b.1) Absolute flow angles from axial direction: The user specifies two flow angles (of the absolute flow) at the boundary, α and γ, which are defined by Eq. 8-3 and given in radians. The absolute total pressure and the absolute total temperature on the inlet boundary are also specified and imposed. For turbulent models with additional equations, the corresponding quantities are also specified and imposed. Three variants are available depending on the value that is extrapolated. FINE™ 8-17 Boundary Conditions Theory on Boundary Conditions • the module of the absolute velocity vector is obtained by extrapolation from the interior field, cf. Eq. 8-15. (OPSEL=2) • the axial velocity component is extrapolated (OPSEL = 3): ( Vz )0 = ( Vz )1 Note that it is assumed that the angular velocity vector is in the z-direction, ω = ω ⋅ 1z , (8-6) (8-5) which makes this direction the axial one. Also note that, as a result of Eq. 8-6 the absolute and relative axial velocity component are equal. • the mass flow is extrapolated, assuming that the meridional component of the velocity is the one contributing to the mass flow. ( Qm )0 = ( Qm )1 , with Q m = ρV m S . (8-7) (8-8) This boundary condition is specially dedicated to radial turbomachinery for which problem of mass flow conservation can arise. It is not interfaced but it can be used by selecting the previous boundary condition (absolute flow angles with extrapolation of velocity) and setting the expert parameter IMASFL to 1. the inlet patches have to be grouped in one group to use this last boundary condition (extrapolation of mass flow). b.2) Relative flow angles from axial direction For a stator calculation it may be convenient to impose the velocity angles of the relative flow at the exit of the upstream rotor. In case of rotors the user may also prefer to impose relative boundary conditions. This procedure is only available in case total conditions and flow angles are imposed. In addition to that the extrapolation of Vz must be selected. Note also that both flow angles and total conditions are then treated in the relative mode. This boundary condition is not directly available in the Boundary Conditions page of the interface. It can be used by selecting the previous boundary condition (absolute flow angles with extrapolation of the axial velocity component) and using the expert parameter INLREL. In this case, relative flow angles, relative total pressure and relative total temperature are specified in the interface instead of the absolute values. Set INLREL to 1 in the case of stators. In the case of rotors (INLREL=2) the approach is exactly the same as the one used when absolute conditions are imposed. The adopted approach consists of imposing boundary conditions, which are still defined in the absolute frame of reference, but which vary from one iteration to the other in order to respect the imposed relative value. This technique provides a robust algorithm with an under-relaxation of the evolution of absolute conditions and a special treatment of the hub and shroud boundary layers. Indeed as the hub and shroud walls are usually not rotating, the relative flow angle tends to 90 degrees in the boundary layer, which complicates the boundary condition treatment if the relative conditions are imposed. The above approach (switch to the absolute frame of reference) allows computing the absolute flow angles distribution through an extrapolation in the boundary layers. The under-relaxation factor as well as the percentage of the distance from the hub and the shroud where the angle is extrapolated are specified in the expert parameter ANGREL. The relation between the relative (β) and absolute (α) angles is the following: 8-18 FINE™ Theory on Boundary Conditions Boundary Conditions ωr tan α = tan β + ----Vz (8-9) where ω is the speed of rotation of the upstream rotor specified in the expert parameter OMGINL and r the radial position. The update of the flow angle is followed by the update of the absolute total conditions according to: ( ωr ) ωrV θ a r T 0 = T 0 – ------------- + -----------2c p cp 2 a p0 = r p0 The initial values of the absolute flow angle and total conditions are set to the value of the relative ones except with the initial solution for turbomachinery. In the initial solution for turbomachinery, Eq. 8-9 and Eq. 8-10 are used to compute the initial absolute flow angle and total conditions from the specified relative values. b.3) Velocity direction The user first specifies a direction (given under the form of a vector) that corresponds to the direction of the absolute velocity vector. Note that this vector does not have to be a unitary vector. The r,θ,z components of the direction vector are given. E.g. if the user enters the direction (0,1,1) the user imposes that the θ- and z-components of the absolute velocity vector at inlet are equal and that the radial velocity is zero. The absolute total pressure and the absolute total temperature on the inlet boundary are also specified. These values will be imposed. The module of the absolute velocity vector is extrapolated from the interior field. Using subscript 0 for the boundary, and subscript 1 for the first internal cell: V0 = V 1 where V represents the absolute velocity. (OPSEL = 4). The velocity vector on the boundary is found by scaling the velocity vector specified in the boundary condition file such that the correct module is obtained. For a turbulent calculation with the Spalart-Allmaras model, the turbulent viscosity has also to be specified on the inlet boundary. When the two-equations turbulent model is chosen, the boundary values of k and ε have to be specified. (8-11) c) Mass Flow Imposed (Subsonic) This boundary condition permits to impose the value of the mass flow through a specified control surface. The control surface is defined by grouping several patches into the same group. In addition to the mass flow the direction of the velocity vector and the static temperature are imposed (ITYPE=28). Two variants are available: • the swirl can be imposed, as well as the direction of the velocity vector in the meridional plane (Vr/Vm,Vθ,Vz/Vm) (OPSEL 1). • the direction of the absolute velocity vector can be imposed (Vr /|V|, Vθ/|V|, Vz/|V|) (OPSEL 2). FINE™ ⎠ ⎟ ⎞ T0 ---r T0 a γ ⁄ (γ – 1) . (8-10) ⎝ ⎜ ⎛ 8-19 Boundary Conditions Theory on Boundary Conditions Two possibilities exist for the treatment of the static temperature: • it can be imposed at a given fixed value, • a relation can be imposed between the inlet static temperature and the averaged temperature along a specified outlet. In this case the user specifies the patch name (or group name) of the connected outlet and the difference of temperature between the inlet and outlet temperatures. The difference of temperature is specified instead of the static temperature. If the specified value is zero, the temperature at the inlet will be equal to the average outlet temperature, whereas if the specified values is for instance 20, the temperature will be equal to the outlet temperature + 20. For turbulent models with additional equations, the corresponding quantities are also specified and imposed on the inlet boundary. d) Imposing the Complete Flow Conditions (Compressible, Supersonic) d.1) Total quantities Instead of specifying static pressure, static temperature and the three absolute velocity components, one can also specify absolute total pressure, absolute total temperature, absolute Mach number and two flow angles α, β defined as (ITYPE = 23, OPSEL = 1): Vθ α = atan ----Vr Vz β = acos ----V with the angles given in radians. For a turbulent calculation with two-equation model the boundary values of k and ε also have to be specified. With the Spalart-Allmaras model, the turbulent viscosity has to be specified along the boundary. d.2) Static quantities The flow at inlet is completely specified, by giving the static pressure, static temperature and the three absolute cylindrical velocity components (ITYPE = 23, OPSEL = 2). For turbulent models with additional equations, the corresponding quantities are also specified and imposed on the inlet boundary. , (8-12) e) Total Enthalpy & Dryness Fraction Imposed (Subsonic - Condensable Gas) In cases where the inlet thermodynamic state is located on the saturation curve or inside the biphasic zone, traditional boundary conditions based on total temperature and total pressure are not sufficient, as pressure and temperature become interdependent. An additional information is required, which is the dryness fraction. The boundary condition proposed under FINE™ GUI is based on the absolute total enthalpy and the dryness fraction. The velocity direction is also specified, either by means of two flow angles (from axial direction) or of velocity direction vectors. It should be mentioned that the use of this boundary condition requires the presence of the saturation table (’PSA.atab’) of the fluid in the corresponding subfolder. The boundary condition is based on the dryness fraction (X), whose value is bounded between 0 and 1. The inlet thermodynamic must be either saturated or be located inside 8-20 FINE™ Theory on Boundary Conditions Boundary Conditions the biphasic zone. The validity of the condensable fluid model is limited to gases with small fraction of liquid (X > 0.9) or reversely to liquids with small fraction of gas (X < 0.1). The implementation of the boundary condition is based on extrapolation of the static pressure, which permits to evaluate the saturated liquid and gas values of the density and enthalpy. The dryness fraction permits to deduce the values of the local static enthalpy and density. The other boundary conditions are then used to calculate the velocity vector. 8-5.1.2 Cartesian Inlet Boundary Conditions This boundary condition is activated for the values of the parameter ITYPE = 24 (subsonic) or ITYPE=23 (supersonic). a) Static Quantities Imposed with Extrapolation of the Static Pressure (Subsonic) The complete absolute velocity vector followed by the static temperature on the boundary are specified (OPSEL = 1). For turbulent models with additional equations, the corresponding quantities are specified also. The static pressure is extrapolated from the interior. Using subscript 0 for the boundary, and subscript 1 for the first internal cell one has: p0 = p 1 , which allows to calculate all the primitive variables on the boundary. These conditions can also be used for incompressible flows. (8-13) b) Total Quantities Imposed (Subsonic) The user first specifies a direction (given under the form of a vector) that corresponds to the direction of the absolute velocity vector. Note that this vector does not have to be a unitary vector. The x,y,z components of the direction vector are given. E.g., entering the direction (0,1,1) imposes that the y- and z-component of the absolute velocity vector at inlet should be equal. In other words, the flow comes in at an angle of 45 degrees between z- and y-direction, whereas the angle between zand x-direction is 0 degrees. The absolute total pressure and the absolute total temperature on the inlet boundary are also specified. These values will be imposed.Two variants are available depending on the value that is extrapolated: • the absolute Mach number is extrapolated from the interior field (OPSEL = 2, only available for compressible fluid): M0 = M1 , (8-14) • the module of the absolute velocity vector is extrapolated from the interior field. V0 = V1 where V represents the absolute velocity. (OPSEL = 3). For both variants, the velocity vector on the boundary is found by scaling the velocity vector specified in the boundary condition file such that the correct module is obtained. (8-15) FINE™ 8-21 Boundary Conditions Theory on Boundary Conditions For a turbulent calculation with the Spalart-Allmaras model, the turbulent viscosity has also to be specified on the inlet boundary. For a turbulent calculation with a two-equation model, the boundary values of k and ε have to be specified. c) Mass flow, Direction of Absolute Velocity Vector and Static Temperature Imposed (Subsonic) This boundary condition permits to impose the value of the mass flow through a specified control surface. The control surface is defined by grouping several patches into the same group. In addition to the mass flow, the direction of the velocity vector and the static temperature are imposed (ITYPE=28). • the direction of the absolute velocity vector is imposed in the Cartesian coordinate system (Vx/ |V|,Vy/|V|,Vz/|V|) (OPSEL 3). Two possibilities exist for the treatment of the static temperature: • it can be imposed at a given fixed value, • a relation can be imposed between the inlet static temperature and the averaged temperature along a specified outlet. In this case the user specifies the patch name (or group name) of the connected outlet and the difference of temperature between the inlet and outlet temperatures. The difference of temperature is specified instead of the static temperature. If the specified value is zero, the temperature at the inlet will be equal to the average outlet temperature, whereas if the specified values is for instance 20, the temperature will be equal to the outlet temperature + 20. For turbulent models with additional equations, the corresponding quantities are also specified and imposed on the inlet boundary. d) Imposing the Complete Flow Conditions (Supersonic) The flow at inlet is completely specified, by giving the static pressure, static temperature and the three absolute Cartesian velocity components (ITYPE = 23, OPSEL = 0). This boundary condition is only available for a compressible fluid. For a turbulent calculation with the Spalart-Allmaras model, the turbulent viscosity has also to be specified on the inlet boundary. When the two-equation turbulent model is selected, the boundary values of k and ε have to be specified. 8-5.2 Outlet Boundary Conditions 8-5.2.1 Outlet Boundary Conditions for Subsonic Flow a) Static Pressure Imposed ITYPE = 25; OPSEL = 10. The static pressure at the outlet boundary is specified. The remaining dependent variables on the outlet boundary are obtained from the interior field through extrapolation. The default extrapolation is a zero order extrapolation of the static temperature and the absolute velocity. Several options are available: • order of extrapolation: zero or first order (in expert user mode), • backflow treatment (see section 8-5.2.3): active or not. 8-22 FINE™ Theory on Boundary Conditions Boundary Conditions The purpose of the treatment of backflow is to control the total temperature distribution along the exit boundary. In case the flow partially re-enters the domain through the exit boundary, the total temperature of the entering flow is controlled so that the entering and outgoing flow globally have the same total temperature. b) Averaged Static Pressure Imposed ITYPE = 27; OPSEL = 40 In some cases, an uniform pressure can not be imposed on the whole outlet area. This boundary condition allows imposing an averaged static pressure. The remaining dependent variables on the outlet boundary are obtained from the interior field through extrapolation. The pressure profile is obtained by extrapolation from the interior field and it is translated to ensure that the computed averaged pressure on the outlet area is the target averaged pressure specified by the user. This translated profile is then the imposed pressure profile. The options described in the previous paragraph (section a) are still available. The outlet patches have to be grouped in one group to use this boundary condition. c) Static Pressure Imposed with Radial Equilibrium ITYPE = 125 This boundary condition is only valid on surfaces with mesh lines at constant radius. The static pressure in the outlet section is assumed to be uniform in the tangential direction and to vary in radial direction according to: v θ ∂p = ρ ⋅ ------ . ∂r r 2 (8-16) The user specifies the static pressure at a specific radius, followed by that radius and the radial direction. The radial direction is specified by using the block orientation (I-direction, J-direction or K-direction). The pressure distribution in the outlet section is then found by integrating Eq. 8-16 with pitchwise averaged values of Vθ and r. The other variables are extrapolated following the system of options exposed above. See “Static Pressure Imposed” on page 22. The treatment of backflow is not implemented for this boundary condition. d) Mass Flow Imposed ITYPE = 27 The outlet patches have to be grouped in one group to use this boundary condition. d.1) Velocity Scaling OPSEL = 20 This condition can be used for low speed subsonic outlet (Mach Number < 0.3). It fixes the mass flow at a given control surface by scaling the velocity vectors on this surface. The other variables are extrapolated following the system of options exposed above. FINE™ 8-23 Boundary Conditions Theory on Boundary Conditions The scaling of the velocity vector is not totally free. The value of the scaling factor is constrained between VELSCA and 1/VELSCA, where VELSCA is an expert parameter available in the Control variables page in the expert mode. Given that the pressure is also extrapolated with this condition, it is imperative that the inlet boundary condition fixes the pressure through the total pressure. Fixing the mass flow is not as robust as to impose the pressure and this is particularly sensitive with full-multigrid. A pressure is thus requested as input and is imposed during the full-multigrid process. Consequently, the mass flow computed at outlet is not exactly the target mass flow during the computation on the coarse grids. This option is not recommended in case significant backflow is detected along the exit. The next option (exit pressure adaptation) is then better recommended. d.2) Pressure Adaptation OPSEL = 30 This boundary conditions is an adaptation of the "uniform static pressure imposed" and "static pressure imposed with radial equilibrium" boundary conditions. The only difference is that an automatic procedure is included that introduces a variation of the imposed exit pressure at each iteration of the calculation. The pressure is iteratively updatet in order to reach at convergence the imposed mass flow. The successive pressure modifications are calculated according to: new old p = p · r gas T ref actual imposed + RELAXP --------------------- ( Q –Q ) , 2 L ref (8-17) where Lref and Tref are the characteristic length and reference temperature specified in the Flow Model page. rgas (RGAS) and RELAXP are expert parameters defined in the Control Variables page. The expert parameter RELAXP introduces an under-relaxation of the successive modifications of the exit pressure. The default value is 1. The value of the exit pressure provided by the user is the initial one. In case the radial equilibrium is used, the initial value of the exit pressure is imposed at midspan. Contrary to the previous option fixing the mass flow through velocity scaling, it is only after convergence of the procedure that the mass flow reaches the imposed value. e) Characteristic Imposed ITYPE = 29 This boundary condition has been implemented to increase the robustness in the frame of a design process. Indeed it is not always suitable to impose the pressure at the exit because it can drive the machine to stall when the geometry change affects its characteristic line. The proposed solution is to impose a relation between the mass flow and the pressure at the outlet. It is no longer needed to choose between imposing pressure when working around the chocking part and imposing mass flow when working close to the stall limit. The user has to impose a line defined through 3 parameters: a target outlet mass flow ( Qt ), a target outlet pressure ( p Qt ) and the pressure at zero mass flow ( p Q0 ). See section 8-2.2 for a schematic representation of this boundary condition. The implementation follows three principles: 8-24 FINE™ Theory on Boundary Conditions Boundary Conditions • The relation between mass flow and pressure is imposed from a function of the type: F ( Q, p ) = 0 , with ( p Qt – p Q0 ) 2 F = p – p Q0 – -------------------------- Q . 2 Qt (8-19) (8-18) (8-20) A linearisation of the relation is applied to obtain: ∂F ∂F F + ------ δQ + ----- δp = 0 , ∂p ∂Q (8-21) where the δ are the variations of the mass flow and averaged exit pressure and where F and its derivatives are computed from the old values of p and Q. • The local outgoing characteristic variables are extrapolated. • the relation between p 1 and p 0 is imposed as follows: p 0 = p 1 + ∆p , (8-22) with ∆p is constant over the whole outlet and with the subscripts 0 and 1 corresponding respectively to the value in the first outer cell and in the first inner cell. Combining these three principles and expressing Q and p in function of ∆p at the outlet, Eq. 8-21 can be written as a polynome of second order in ∆p. The suitable root is chosen so that the imposed pressure always respects the relation defined between the mass flow and the pressure during the computation. 8-5.2.2 Outlet Boundary Conditions for Supersonic Flow ITYPE = 22 This condition is to be used in case of supersonic outflow and is only valid for compressible fluids. The dependent variables at the outlet are extrapolated from the interior through first-order extrapolation. If no preconditioning is used, there is some checking on negative or small pressures: if the static pressure is less than 1E-15 after extrapolation, it is put to 1E-15. 8-5.2.3 Treatment of Backflow at Outlet (Radial Diffuser) The option for the treatment of backflow can be activated by pressing the corresponding button in the FINE™ interface. This option has been initially implemented in order to ensure a proper treatment of radial diffusers outlets in case of flow separations. The treatment is based on the hypothesis that the absolute total temperature should be constant throughout the outlet section. If the flow is re-entering the numerical domain through a part of the outlet section, a hybrid boundary condition is applied in that region: • the static pressure is imposed, • the velocity vector is extrapolated, FINE™ 8-25 Boundary Conditions Theory on Boundary Conditions • the absolute total temperature is imposed at a value equal to the averaged total temperature along the outlet (the averaging is performed throughout the region where the flow leaves the domain. This treatment permits to avoid the introduction of an uncontrolled total temperature level in the regions where the flow re-enters the domain, and in this way to better respect the physics of the flow. Limitations: • only for compressible fluid, • it is applied separately on each outlet patch when an uniform static pressure is imposed (it is applied to a group of patches if ITYPE=27, i.e. averaged static pressure and mass flow imposed). • not available for the outlet boundary conditions where static pressure is imposed with radial equilibrium. 8-5.3 Solid Wall Boundary Conditions 8-5.3.1 Euler Walls ITYPE = 15, ITYPE = 16 (default). For Euler walls the velocity has to be tangential to the wall. To obtain the velocity vector on the wall, the velocity vector is first extrapolated from the interior with zero or first order extrapolation according to the selected option in the FINE™ interface: w∗ w = w 1 3 1 w∗ w = -- w 1 – -- w 2 2 2 with subscripts w,1,2 denoting respectively the wall, the first and the second inner cell. The tangential part of the extrapolated velocity vector is: w ** w (8-23) = w∗ w – ( w∗ w ⋅ n )n , (8-24) with n the normal to the wall. The velocity vector on the wall is finally found by a scaling process such that its module equals: ww = w1 . 3 1 w w = -- ⋅ w 1 – -- ⋅ w 2 2 2 (8-25) The wall density and pressure are obtained through extrapolation from the interior with zero order: ρw = ρ1 pw = p1 8-26 FINE™ Theory on Boundary Conditions Boundary Conditions or first order: 3 1 ρ w = -- ρ 1 – -- ρ 2 2 2 pw 3 1 = -- p 1 – -- p 2 2 2 . (8-26) Alternatively the pressure can be solved from the normal momentum equation (ITYPE=15): n ⋅ ∇p = ρv ⋅ v ⋅ ∇ n , which is written in a local curvilinear system as: ∂n ∂n ∂p ∂p ∂p ρv wall ( v wall ⋅ S i ) ----- + ( v wall ⋅ S k ) ----- = S i ⋅ n ----- + S j ⋅ n ------ + S k ⋅ n ----∂ξ ∂ζ ∂ξ ∂η ∂ζ , (8-28) ⎠ ⎞ ⎝ ⎛ (8-27) where ξ, η, ζ represent the coordinate directions, and where it is assumed that the j-direction and η is the direction away from the wall (which is not necessarily perpendicular to the wall). ∂p Eq. 8-28 is then solved for ------ , whereas zero-order extrapolation is used for the density. ∂η 8-5.3.2 Navier-Stokes Walls a) Adiabatic Walls The velocity vector on the wall vanishes. ITYPE = 11 or 13 are used for Cartesian boundary condition, 111 or 113 for cylindrical. If condition 111 or 113 is used, the angular velocity of the wall (in the absolute frame of reference) has to be specified. The velocity relative to the wall should be zero, leading to: w = – ( u s – uw ) , with subscripts s, w referring to respectively the system and the wall. A relation for the pressure is obtained by projection of the momentum equation onto the wall normal direction n . Written in the absolute frame of reference: n ⋅ ∇p = – ρ n V ⋅ ∇ V + n ⋅ ∇ ⋅ τ . ⎠ ⎞ ⎝ ⎛ ⎠ ⎞ ⎝ ⎛ (8-29) (8-30) The normal pressure gradient can be written as a function of pressure derivatives along the coordinate lines: 1 ∂p ∂p ∂p n ⋅ ∇p = ----------- S j ⋅ S i + S j ⋅ S j + S j ⋅ S k ∂ζ ∂η ∂ζ Sj Ω , (8-31) where ξ, η, ζ represent the coordinate in the i, j and k directions, and where it is assumed that the jdirection is directed away from the wall (not necessarily perpendicular to the wall). S i, j, k are the surface vectors of the corresponding cell faces. Combining Eq. 8-30 and Eq. 8-31 and considering that the velocity vanishes on the wall, yields: FINE™ 8-27 Boundary Conditions Theory on Boundary Conditions = COR 1 COR2 COR3 Two implementations of the adiabatic Navier-Stokes wall are available. In the simplest one (ITYPE=13 or 113), only the terms COR1 and COR2 of the equation above are taken into account in the evaluation of the pressure derivative. This corresponds to assume that the normal pressure gradient equals zero. Taking into account that the velocity, appearing in the term COR2, is the velocity on the wall, this term can be simplified to: Ωρ 2 COR2 = -------- ⋅ S j r ⋅ ω w 2 Sj Note that COR2 vanishes for a stator wall. In the more complicated implementation (ITYPE=11 or 111) the complete normal momentum equation is considered in the evaluation of the pressure derivative, i.e. the term COR3 is also accounted for. Applying Gauss' theorem this term can be rewritten as: n n COR3 = ----- Ω ∇ ⋅ τ = ----S S ⎠ ⎞ ⎝ ⎛ Once ∂p/∂η is determined, the pressure on the wall is obtained as (assuming the direction points inside the interior field, and with indices w,1 representing the wall and the first inner cell): 1 ∂p p w = p 1 – -- ------ . 2 ∂η (8-35) The temperature on the wall is obtained by expressing that the normal temperature gradient vanishes, or in terms of the derivatives along the coordinate lines, cf. Eq. 8-31: ∂T 1 ∂T ∂T = – -------- S j ⋅ S i + S j ⋅ S k 2 ∂η ∂ξ ∂ξ Sj . (8-36) The wall temperature is then found using a similar equation as Eq. 8-35. The density follows from pressure and temperature through the appropriate relation, depending on the type of gas. b) Isothermal Walls The implementation of this boundary condition is very similar to the adiabatic Navier-Stokes wall. The only difference is in the determination of the wall temperature, which is fixed to the specified temperature in the current boundary condition. Again two versions are available, depending on whether all the terms in the normal momentum equation are taken into account when determining the wall pressure (ITYPE 12 ≡ 11; 14 ≡ 13; 112 ≡ 111; 114 ≡ 113). For the cylindrical isothermal walls, #112 and #114, the angular velocity of the wall has to be specified. For all versions (#12,#112,#14,#114) the wall temperature is specified. The pressure is determined as in the adiabatic condition and the density follows from pressure and temperature through the appropriate relation, depending on the type of gas. 8-28 ⎠ ⎞ ⎝ ⎛ ∫ Sj n ∇ ⋅ τ dΩ = ----- τdS ≈ ------τ i ⋅ Si . 2 S faces S ∫ ° ∑ ⎠ ⎞ ∂p 1 Ω ∂p ∂p Ωρ = – -------- S j ⋅ S i + S j ⋅ S k – ------- ⋅ n V ⋅ ∇ V + ------ n ∇ ⋅ τ 2 ∂η ∂ξ ∂ξ S Sj Sj j ⎝ ⎛ ⎠ ⎞ ⎝ ⎛ (8-32) (8-33) (8-34) FINE™ Theory on Boundary Conditions Boundary Conditions c) Wall with Imposed Heat Flux The implementation of this boundary condition is very similar to the previous ones. For this condition (ITYPE = 10 or 110) the temperature is determined from the imposed heat flux (W/m2). The pressure is determined as in the adiabatic condition and the density follows from pressure and temperature through the appropriate relation, depending on the type of gas. 8-5.4 Far-field Boundary Condition ITYPE = 21 uses Riemann invariants that are defined as: 2c ± R n = Vn ± ---------- , γ–1 + (8-37) where R n are the Riemann variables associated with the direction n and c is the local speed of sound. For subsonic inflow, R n corresponds to a positive, incoming characteristic. R n is then obtained from the free stream values: 2c ∞ + R n = V ∞ ⋅ n + ---------- , γ–1 where V ∞ is the free stream velocity, c ∞ the free stream speed of sound. R n , on the other hand, corresponds to an outgoing characteristic and has to be estimated from inside the computational domain by an appropriate extrapolation: 2c i R n = V i ⋅ n – ---------- , γ–1 + + (8-38) (8-39) where subscript i refers to values from the interior. Linear extrapolation of the variables to the external boundary will be used to obtain a sufficiently accurate solution: 3 1 q i = -- q 1 – -- q 2 , 2 2 where subscript 1 and 2 refer to the first two inner points. The normal velocity and the local speed of sound can now be obtained on the boundary by adding and subtracting both Riemann variables R n and R n : Rn + Rn + - γ–1 V w ⋅ n = ----------------- , c wall = ( R n – R n ) ---------- . 2 4 + + - (8-40) (8-41) The entropy on the wall is set to the free stream entropy. All the flow variables can then be obtained. Corresponding formulas hold for a subsonic outflow with the difference that R n entropy are obtained from interior values. + and the wall FINE™ 8-29 Boundary Conditions Theory on Boundary Conditions For supersonic flows, both Riemann variables and the entropy are obtained from free stream values for inflow, interior values for outflow. For preconditioning computation, the same principle is used with modified invariants defined as: 2 2 pg β β ± 2 R n = v n – ----------- v n 1 – ---- – α − v n 1 – ---- – α + 2 2 2 2ρβ c c 2 vn - 2 + 4 1 – ------ β , 2 c ⎠ ⎟ ⎞ ⎝ ⎜ ⎛ 2 where p g = p – p ref β = β∗ U ref 2 2 . The free stream variables of static pressure, static temperature and the three velocity components are specified by the user in the boundary condition file. For a turbulent calculation with a two-equation model, the k and ε values on the boundary are set to their free stream values (inflow) or extrapolated from the interior (outflow). 8-30 ⎠ ⎟ ⎞ ⎝ ⎜ ⎛ ⎠ ⎟ ⎞ ⎝ ⎜ ⎛ (8-42) (8-43) FINE™ CHAPTER 9: Numerical Model 9-1 Overview To define numerical parameters of the computation, the Numerical Model page allows to define several aspects of the computation: • the CFL number, • the multigrid parameters, • preconditioning parameters (if applicable). These parameters are described in the next section. FIGURE 9.1.0-1 Numerical model interface In expert user mode (Expert Mode) additional parameters are available as shown in Figure 9.1.0-2: additional multigrid parameters and unsteady parameters. These interfaced expert parameters are described in section 9-3. Also the non-interfaced expert parameters are described in this section. More theoretical information on the available parameters related to the numerical model (spatial and temporal discretizations) is provided in section 9-4. FINE™ 9-1 Numerical Model Numerical Model in FINE™ FIGURE 9.1.0-2 Numerical Model page in expert mode 9-2 9-2.1 Numerical Model in FINE™ CFL Number This box allows to tune the CFL (Courant-Friedrich-Levy) number to be employed in the computation. This number globally scales the time-step sizes used for the time-marching scheme of the flow solver. A higher value of the CFL number results in a faster convergence, but will lead to divergence if the stability limit is exceeded. 9-2.2 Multigrid parameters In the left part of the Numerical Model page, three boxes are visible. The first one is an information box, named ’Grid levels: current/coarsest’. It indicates for each of the i, j and k directions the currently selected grid level and the number of the coarsest grid level available in the corresponding direction. The second box of the Numerical Model page is an input box that allows to define for each of the i, j and k directions the ’Current grid level’. • The coarsest grid level depends on the number of times the grid can be coarsened, along each of the (i,j,k) directions. For example, if the grid has 17*33*33 points in the i, j, k directions, it has respectively 16*32*32 cells. The i direction (16 cells) can thus be divided 4 times by 2, while the others can be divided 5 times by 2. The following grid levels are then available: 000 17*33*33 (18,513 points) 111 9*17*17 (2,601 points) 222 5*9*9 (405 points) 333 3*5*5 (75 points) 444 2*3*3 (18 points) 455 2*2*2 (8 points) 9-2 FINE™ Expert Parameters for the Numerical Model Numerical Model The coarsest grid level available is then 4 along i and 5 along j and k. • The current grid level is the finest grid level (for each of the i, j and k directions) on which the computation will take place. The selected levels should be in the range between 0 and the coarsest grid level available for each of the i, j and k directions. Referring to the example given just above, the user can do a first run on level 3 3 3 to validate the computational parameters and then switch to level 1 1 1 or 0 0 0 for a finer solution. It gives a high flexibility to the system since with one grid, the user can run simulations on several sub-meshes. All combinations between the i, j and k grid levels, in the specified range, are possible such as 2 3 1 or 0 3 2...etc. Press <Enter> after each modification to validate the new specified levels. The use of multigrid is highly recommended in order to ensure fast convergence of the flow solver. The mesh used to discretise the space can have multiple grid levels in each direction of the computational domain i, j and k. These levels are numbered from 0 (finest grid) to N (coarsest grid). The grid level (N) available in one direction (I, J, or K) is the smallest grid among all patches on that particular direction (I, J, or K). The third box, named ’Number of Grid(s)’, permits to significantly accelerate the convergence to steady state if several grid levels are available: the flow calculation is performed simultaneously on all the grid levels. This technique is referred to as the multigrid strategy. This number should be chosen as high as possible, and deduced from the information displayed on the available grid level and the grid level on which the computation will be performed (’Current Grid Level’). Finally, the toggle button ’Coarse Grid Initialization’ enables, before calculating the flow on the mesh contained in the IGG™ files, to perform a preliminary flow calculations on a coarser mesh automatically created by the flow solver by coarsening the initial one. This provides a rapid estimation of the flow. This technique is referred to Full Multigrid. 9-2.3 Preconditioning Parameters This box allows to define the preconditioning numerical parameters. These parameters are only available when an incompressible fluid is selected on the Fluid Model page or when the Low Speed Flow (M<0.3) option is selected on the Flow Model page. Preconditioning is described in detail in section 4-3.8. Especially section 4-3.8.5 provides more information on the value to choose for β*, the reference velocity and the option to use Local velocity scaling. 9-3 9-3.1 Expert Parameters for the Numerical Model Interfaced Expert Parameters 9-3.1.1 Multigrid Strategy If the button ’Coarse Grid Initialization’ is activated, the computation starts on the coarsest grid level and includes a finer grid level each time one of the two following criteria is satisfied: FINE™ 9-3 Numerical Model Expert Parameters for the Numerical Model • The maximum number of cycles to be performed on each grid level is reached. This parameter is specified through the input box in the Full MultiGrid Parameters area as the Maximum number of cycles per grid level. • The residual on the current grid level has dropped a certain order of magnitude as indicated by the Convergence criteria on each grid level in the Full MultiGrid Parameters area. • An additional input box permits to select the number of sweeps to be performed on the coarse grid levels through the input box ’Number of sweeps on successive grid levels’. The amount of sweeps is the amount of times the Runge-Kutta operator respectively the chosen relaxation operator is applied (see section 9-4.4 for more detail). In the default configuration of the solver called ’Linear progression’, the number of sweeps on each level equals the level number (2 sweeps on second level,...). It has been observed in many cases that the convergence rate may be significantly improved by performing a higher number of sweeps on the coarsest levels. Recommended sets of values are proposed in the Sweeps area through the parameter Scheme definition: for instance (1,2,16) in case of 3 grid levels. However, it is should be noted that more sweeps have as a consequence more time required for an iteration. 9-3.1.2 Spatial Discretization Two types of spatial discretization are available: • central scheme (default) and • upwind scheme. Furthermore, if an upwind discretization is chosen, an input box appears in a ‘Spatial discretization parameters’ area to specify the order of accuracy of the desired upwind scheme: first or second order. See section 9-4 for more detail on those different schemes. Condensable fluid option is not compatible with the use of upwind schemes for space discretization. 9-3.1.3 Temporal Discretization The temporal discretization scheme used for the computation is an explicit multi-stage Runge-Kutta scheme. In the interface, the time stepping technique should be selected between Local time stepping (default) and Global time stepping. See section 9-4 for more detailed information on the temporal discretization. In general the default scheme is recommended. If the computation is an unsteady computation, unsteady parameters box appears. Please refer to chapter section 4-2.1 for a description of those unsteady parameters. 9-4 FINE™ Expert Parameters for the Numerical Model Numerical Model 9-3.2 Non-interfaced Expert Parameters Additional parameters related to the numerical model are available in the list on the Control Variables page in Expert Mode. 9-3.2.1 Multigrid IPROLO: Indicates the order of the prolongation within the multigrid approach: = 0: is piecewise constant prolongation, = 1 (default): is linear prolongation (no damping if -1), = 2 linear prolongation except at boundaries(-2). When used with a preconditioned formulation, this damping option is somewhat useless and can be damaging. FINETM sets it therefore to off when the preconditioning is involved. IRESTR: Gives the order of the restriction operator of the multigrid. = 0 (default): corresponds to linear restriction, = 1: to quadratic restriction. MGRSTR: Applies only for multigrid and fixes the type of multigrid cycle. MGRSTR=1: V-cycle; MGRSTR=2: W-cycle; MGRSTR=3: F-cycle; MGRSTR=4: V-cycle in sawtooth; MGRSTR=5: W-cycle in sawtooth; MGRSTR=6: F-cycle in sawtooth. Default MGRSTR=1. MGSIMP: Applies only for multigrid. If MGSIMP>1 a simplification will be used on coarser levels. If MGSIMP=1 a more dissipative scheme is used on coarser meshes, i.e. first-order upwind (if IUPWIN=1) or central scheme with increased 4th order dissipation on solid walls (if IUPWIN=0). If MGSIMP=2, in addition to the simplification for MGSIMP=1, viscous and source terms (of turbulence) are neglected on coarser levels. No simplification for MGSIMP=0. Default MGSIMP=1 RSMPAR: Residual smoothing parameter σ*/σ. A value less or equal to zero means no residual smoothing. SMCOR: Only used in case of multigrid. SMCOR has the same meaning as RSMPAR but applies to the interpolated multigrid corrections instead of the residuals. SMCOR indicates whether interpolated corrections should be smoothed or not. The default value for SMCOR is 0. 9-3.2.2 Spatial Discretization IFACE: = 1(default): Cell face gradients are used for the viscous fluxes, = 0: cell corner gradients. IWAVVI: Only used if IFACE=0. If IWAVVI=0 the cell face gradients are obtained by arithmetic averaging of the cell corner gradients. If IWAVVI=1 a weighted averaging is used instead, taking the cell volumes into account. a) Central Discretization CDIDTE: Constant used in the exponential damping factor that is used in the numerical dissipation for k and ε, both if central or upwind schemes are used. The default value for CDIDTE is 100 FINE™ 9-5 Numerical Model Expert Parameters for the Numerical Model EXPMAR: Exponent in the multi-dimensional scaling model of Martinelli of the dissipation used in central schemes (see section 9-4.1.3). Default EXPMAR=0.5 i.e. multidimensional scaling not used. Define whether the second order artificial dissipation switch should be based on both pressure and temperature gradients (parameter IARTV2=1) or on pressure gradients only (IARTV2=0). In the default configuration, only pressure gradients are taken into account. Both pressure and temperature gradients (IARTV2=1) can only be taken into account for compressible cases. Coefficient κ(2) for 2nd order dissipation in the central scheme (default VIS2=1.0). Used only for k-ε turbulence model. Coefficient κ(2) for 2nd order dissipation in the central scheme, as applied to the k and ε equations. Default VIS2KE=1.0 This parameter switches off all second order dissipation for incompressible fluids (when set to the default: VIS2SW=1). Second order dissipation is intended for stabilization of the shocks but there are no shocks in incompressible flows. Therefore the default is to switch off all second order dissipation for incompressible fluids. Sometimes it may be stabilizing to use some second order dissipation. In that case set this parameter to zero. Coefficient κ(4) for 4th order dissipation in the central scheme. Default VIS4=0.1 Used only for k-ε turbulence model. Coefficient κ(4) for 4th order dissipation in the central scheme, as applied to the k and ε equations. Default VIS4KE=0.1 Eliminates 2nd order dissipation fluxes along the physical boundaries (central scheme). Default VISNUL=1. If VISNUL=0, the procedure is not applied. IARTV2: VIS2: VIS2KE: VIS2SW: VIS4: VIS4KE: VISNUL: b) Upwind Discretization ENTRFX: Entropy coefficients, see Eq. 9-2, on page 9-8 and Eq. 9-3, on page 9-8. The first value is the entropy coefficient applied to the linear field, the second value is applied to the non-linear field. ENTRFX<1. means a constant value, ENTRFX>1. means scaled with the spectral radius through a factor ENTRFX-1. Vector of two values, that indicate which effective ratio is to be used, see Eq. 927, on page 9-13. The first value applies to the linear field, the second to the non-linear field. IRATIO is only active for second-order upwind schemes. IROEAV:1 indicates that Roe averages are to be used to calculate cell face data. See Eq. 9-14, on page 9-10. If IROEAV=0, arithmetic averaging will be used. IRATIO: 9-3.2.3 Time Discretization IBOTH: used in combination with ISWV. The latter parameter indicates whether the dissipation terms are recalculated or not in the different Runge-Kutta stages. IBOTH=0 means that the dissipation term only contains the physical, viscous dissipation; IBOTH=1 means that it also contains the artificial/upwind dissipation. The default value = 2 means that the dissipation term contains only the artificial dissipation. The physical dissipation is computed once per time step. IRKCO: Runge-Kutta coefficients. One for each stage, the first one for the first stage, the second one for the 2nd stage and so on. The default values that are used when nothing is set in IRKCO are: 9-6 FINE™ Theory Numerical Model 1st order upwind - Van Leer: 4stage .0833 .2069 5stage .0533 .1263 2nd order upwind - Van Leer: 4stage .1084 .2602 5stage .0695 .1602 central scheme - Jameson: 4stage .25 .3333 5 stage .25 .1666 both central and upwind - Eliasson: 4stage .125 .306 5stage .0814 .191 .4265 .2375 .5052 .2898 .5 .375 .587 .342 1. .4414 1. .5060 1. .5 1. .574 1. 1. 1. 1. NSTAGE: number of stages for the explicit Runge-Kutta scheme. In practice, 4 or 5 stage schemes are mostly used. IRSMCH: specifies the type of residual/correction smoothing. = 1: standard version, Eq. 9-58, = 2 (default in incompressible cases): Radespiel & Rossow, Eq. 9-59, = 3 (default in compressible cases): Zhu, time step dependent coefficients, see Eq. 9-61, = 4: Swanson & Turkel viscous, = 5: Vatsa, Eq. 9-63. On meshes without high aspect ratio. governs the recalculation of the dissipative residual in the different Runge-Kutta stages. A value α between 0 and 1 is allowed. Zero means no recalculation of dissipative residual (latest available value will be used); 1 means recalculation. For intermediate values, a weighted averaging of the latest dissipation residual and of the preceding one is applied with the weight α and (1-α) respectively. E.g. for a 5-stage scheme: ISWV = 1 0 1 0 1, means that the dissipative residual is calculated in 1st,3rd and 5th stage only. ISWV is used in combination with IBOTH. ISWV: RSMPAR: residual smoothing parameter σ*/σ. A value less or equal to zero means no residual smoothing. Default value 2. 9-4 9-4.1 Theory Spatial Discretization The discretization in space is based on a cell entered control volume approach. The general Navier Stokes equation Eq. 9-1 is discretised as: ∫ Ω∂ t ∂U dΩ + faces ∑ F ∆S + ∑ F ∆S = ∫ Q dΩ , I V faces Ω (9-1) where F I ∆S , F V ∆S are respectively the inviscid and viscous fluxes. FINE™ 9-7 Numerical Model Theory 9-4.1.1 Viscous Fluxes The viscous fluxes are determined in a purely central way. As they contain gradients, gradients must be evaluated on the cell faces. This is done by applying Gauss' theorem: 1 1 ∇Φ = --- ∇Φ dΩ = --- ΦdS . Ω Ω ∫ ∫ ° (9-2) Two options exist: If the expert parameter IFACE=0, the gradients are first calculated in cell corners. This is done by applying Eq. 9-2 using as control volume, the volume that has the cell centres that surround the cell corner of interest as corner points, as depicted in Figure 9.4.1-3 (a) below for two dimensions. The cell face gradient is then obtained by averaging the gradients in the 4 corners of the cell face. Arithmetic averaging (input variable IWAVVI=0) or a more accurate weighted averaging may be chosen (IWAVVI=1). cell centre (a) FIGURE 9.4.1-3 : cell corner cell face i+1/2 (b) cell face j+1/2 (c) Different control volumes used to calculate gradients in cell corners or cell faces. If IFACE=1 (Default), gradients are calculated directly on cell faces. Figure 9.4.1-3 (b) and (c) illustrate the control volumes used to find the gradient on respectively the cell face i+1/2 and j+1/2. The option IFACE=1 is more robust and therefore preferred (default), although it is more expensive as the total number of cell faces is approximately 3 times the number of cell corners. 9-4.1.2 Inviscid Fluxes The inviscid fluxes appearing in Eq. 9-1 are upwind based numerical fluxes, and therefore noted with a * superscript. The inviscid numerical flux is expressed as, Hirsch (1990): ( Fn ) * i+1⁄2 1 = -- { ( Fn ) i + ( Fn ) i + 1 } – d i + 1 ⁄ 2 . 2 (9-3) The first term in the right-hand-side of Eq. 9-3 corresponds to a purely central evaluation of the flux. The term d i + 1 ⁄ 2 represents a numerical dissipation term, that may be an artificial dissipation, used in combination with central schemes, or the dissipation associated with upwind schemes. In Eq. 9-3 an arithmetic averaging technique is used. Alternatively, instead of averaging the fluxes in Eq. 9-3, a flux can be used, based on the averaged unknowns, i.e. 9-8 FINE™ Theory Numerical Model i+1/2 Theoretically, the formulation Eq. 9-3 is to be preferred, but, in combination with the central scheme, the formulation of Eq. 9-4 (default) is sometimes more robust, especially for high speed flows. Both central schemes and upwind schemes are available within EURANUS. Currently, the arithmetic averaging given by Eq. 9-4 is the only available option. 9-4.1.3 Central Scheme In the former case, a Jameson type dissipation is used with 2nd and 4th order derivatives of the conservative variables, Jameson (1981): di + 1 ⁄ 2 = ε (2 ) i + 1 ⁄ 2 δU i + 1 ⁄ 2 + εi δ Ui + 1 . The scalar coefficients ε are given by: ε (2 ) i+1⁄2 (4) 1 (2) * = -- κ λ max ( ν i – 1, ν i, ν i + 1, ν i + 2 ) 2 ⎠ ⎞ i+1⁄2 The coefficients κ , κ ters. (2) (4 ) are user input, respectively VIS2,VIS4 in the non-interfaced parame(4) The cell entered values of ε in Eq. 9-5 are obtained by arithmetic averaging of the cell face val- ues of Eq. 9-6. The variables v i are sensors to activate the second-difference dissipation in regions of strong gradients, such as shocks, and to deactivate it elsewhere. They are based on pressure and temperature variations (depending on the value for the expert parameter IARTVZ) and are defined as: ⎭ ⎬ ⎫ p i + 1 – 2p i + p i – 1 T i + 1 – 2T i + T i – 1 v i = max ----------------------------------------- , -----------------------------------------p i + 1 + 2p i + p i – 1 T i + 1 + 2T i + T i – 1 ⎩ ⎨ ⎧ for all equations except the k and ε equations. For liquids, only a pressure switch is used. For the k and ε equations, v i is based on the pressure, on the turbulent kinetic energy and on the dissipation rate: ⎭ ⎬ ⎫ p i + 1 – 2p i + p i – 1 k i + 1 – 2k i + k i – 1 ε i + 1 – 2ε i + ε i – 1 v i = max ----------------------------------------- , ---------------------------------------- , ---------------------------------------p i + 1 + 2p i + p i – 1 k i + 1 + 2k i + k i – 1 ε i + 1 + 2ε i + ε i – 1 * λ in Eq. 9-6 is a measure of the inviscid fluxes and is commonly chosen as the spectral radius multiplied with the cell face area: λ = λ * * i+1⁄2 = ( v∆S + c∆S ) i + 1 ⁄ 2 . On high aspect ratio meshes, the resulting dissipation in the streamwise direction may become very low. Increasing it may improve the robustness and the convergence rate. According to Martinelli (1987), the spectral radii in the other directions are also accounted for. Instead of Eq. 9-9 one uses: FINE™ ⎝ ⎛ ε 1 (4 ) * (2 ) = max 0, -- κ λ -ε i + 1 ⁄ 2 2 ⎠ ⎞ ⎝ ⎛ ( Fn ) * Ui + Ui + 1 = Fn ----------------------- – d i + 1 ⁄ 2 . 2 (9-4) ( 4) 3 (9-5) . (9-6) (9-7) ⎩ ⎨ ⎧ . (9-8) (9-9) 9-9 Numerical Model Theory λ = max { λ * * i + 1 ⁄ 2, (λ * i + 1 ⁄ 2) 1–σ (λ * j + 1 ⁄ 2) σ ,(λ * i + 1 ⁄ 2) 1–σ (λ * k + 1 ⁄ 2) σ } (9-10) The spectral radii in the other directions are defined similar as in Eq. 9-9, e.g. for the j-direction: λ * j+1⁄2 = ( v i + 1 ⁄ 2 ∆S j + 1 ⁄ 2 + c i + 1 ⁄ 2 ∆S j + 1 ⁄ 2 ) (9-11) The cell face normal ∆S j + 1 ⁄ 2 is obtained by averaging the normals on the 4 cell faces in the jdirection, belonging to the 2 cells that share the i+1/2 cell face. The parameter σ is user input (EXPMAR). The default value is 0.5, i.e. Eq. 9-9 is used. In the current version of EURANUS, the Martinelli approach is not yet implemented for the turbulence equations. Note that if the k – ε turbulence model is chosen, the resulting equations for k and ε are solved with the central scheme. Separate coefficients κ , κ for the artificial dissipation can be chosen, respectively VIS2KE and VIS4KE in the non-interfaced expert parameters. Both the 2nd and 4th order dissipation are damped by multiplying them with the following exponential function: ⎠ ⎟ ⎞ ⎝ ⎜ ⎛ ⎠ ⎠ ⎞ ⎞ (2) (4 ) y 1 – exp – ---C ⎝ ⎝ ⎛ ⎛ + 2 V exp – ----3 S 2 . (9-12) The constant C corresponds to the input variable CDIDTE. The above expression means that the damping is applied in the region where y+<CDIDTE, the default is CDIDTE=100; V is the cell volume and S the cell face area. 9-4.1.4 Upwind Schemes In the upwind case, the dissipation term is: 1 l d i + 1 ⁄ 2 = -- R i + 1 ⁄ 2 diag ( α i + 1 ⁄ 2 )δ i + 1 ⁄ 2 W , 2 tive variables U or the primitive variables V through δW = R δU = L δV . The matrices R and R l –1 –1 –1 (9-13) where δW represents the variation of the characteristic variables which is related to the conserva- (9-14) contain respectively the right and left eigenvectors of the Jacobian matrix. l diag ( α i + 1 ⁄ 2 ) in Eq. 9-13 represents a diagonal matrix with α i + 1 ⁄ 2 the element in row and column l. They are to be evaluated on the cell faces, and therefore require the knowledge of the primitive variables on the cell face. These can be obtained either by arithmetic averaging of the primitive variables in the cell centres left and right of the cell face (input variable IROEAV=0) or by a Roe-type of averaging (IROEAV=1). In the latter case the following formulas are used: 9-10 FINE™ Theory Numerical Model ρi + 1 ⁄ 2 = ρi ρi + 1 vi ρ i + vi + 1 ρi + 1 v i + 1 ⁄ 2 = --------------------------------------------ρi + ρi + 1 Hi ρi + Hi + 1 ρi + 1 H i + 1 ⁄ 2 = -----------------------------------------------ρi + ρi + 1 c 2 i+1⁄2 2 = (γ – 1) H i+1⁄2 – v i+1⁄2 (9-15) Theoretically the Roe averages have to be used. However, in practice, arithmetic averages can be used in most applications without any repercussion on accuracy or convergence. Arithmetic averaging has the advantage that it is computationally less expensive. Different upwind schemes result, depending on the expression for α. In EURANUS a TVD version of the Flux Difference Splitting scheme (FDS TVD), Roe (1981), and Symmetric TVD (STVD), Yee (1987), are available. For both schemes α can be expressed as: α i + 1 ⁄ 2 = λi + 1 ⁄ 2 [ 1 – Qi + 1 ⁄ 2 ] ensuring monotonicity. Both the FDS TVD and STVD scheme do not have a built-in entropy criterion, which would guarantee that the 2nd law of thermodynamics is satisfied. These schemes therefore may allow unphysical solutions, such as expansion shocks. In order to avoid unphysical solutions an entropy fix is used. The eigenvalue λ i + 1 ⁄ 2 in Eq. 9-16 is replaced by λ i + 1 ⁄ 2 : λ i+1⁄2 + δ λ i + 1 ⁄ 2 = ----------------------------- if λ i + 1 ⁄ 2 ≤ δ 2δ . = λ i + 1 ⁄ 2 if λ i + 1 ⁄ 2 > δ ) 2 2 (9-16) where λ i + 1 ⁄ 2 represents the eigenvalues of the Jacobian matrix and Q i + 1 ⁄ 2 is a limiter function, ) (9-17) Eq. 9-17 limits the minimum value of λ i + 1 ⁄ 2 to δ . In subsonic and transonic cases a small constant value (<1.) for the entropy fix δ suffices (choose the input variable ENTRFX < 1.). For flow simulations in high speed regime, it is advised to scale the entropy fix with the spectral radius, by choosing the input variable ENTRFX > 1, e.g. ENTRFX=1.05 or 1.1. The scaling factor is then ENTRFX-1., i.e.: δ = ( ENTRFX – 1. ) λ * i+1⁄2 . (9-18) The latter choice also increases the robustness, at the expense of a slightly increased dissipation. Two values for ENTRFX are to be specified. The first one applies to the linear field (the characteristic variables that propagate with speed un ), the second value to the non-linear field (the characteristic variables that propagate with speed un ± c ). For first-order upwind schemes, the limiter vanishes and both FDS TVD and STVD reduce to the same first-order accurate upwind scheme. FINE™ 9-11 Numerical Model Theory For second-order upwind schemes, the limiter is activated. The limiter Q i + 1 ⁄ 2 acts on ratios r i + 1 ⁄ 2 of variations of the characteristic variables, defined as: δi – 1 ⁄ 2W + δi + 3 ⁄ 2W r i + 1 ⁄ 2 = -------------------- , r i + 1 ⁄ 2 = -------------------δi + 1 ⁄ 2W δi + 1 ⁄ 2W (9-19) For the FDS TVD scheme, Q is function of only one of the ratios, according to the sign of the eigenvalue: Q = Q ( ri + 1 ⁄ 2 ) Q = + Q ( ri + 1 ⁄ 2 ) - λi + 1 ⁄ 2 > 0 λi + 1 ⁄ 2 < 0 (9-20) The following limiters are available: Q ( r ) = minmod ( 1, r ) , r+r Q ( r ) = ------------2 1+r = 0 r<0 (9-23) 2 (9-21) r>0 (9-22) r+ r Q ( r ) = ------------- , 1+r Q ( r ) = max [ 0, min (1,2r), min (2,r) ] , (9-24) which represent respectively the Min Mod limiter (LIMITE=1), the Van Albada limiter (LIMITE=2), the Van Leer limiter (LIMITE=3) and the Super Bee limiter (LIMITE=4). The function minmod chooses the value with the minimum module. In the STVD scheme, the check on the eigenvalue sign is avoided by choosing Q as a function of the two ratios r and r + Q = Q ( r i + 1 ⁄ 2, r i + 1 ⁄ 2 ) . - + (9-25) Since the 'classical' limiters such as Van Leer, Van Albada, Min Mod, Super Bee are defined as a function of one ratio, Eq. 9-25 would exclude these limiters in a STVD context. A new family of non-separable limiters, containing also smooth limiters, is proposed within EURANUS, Lacor et al. (1993). The classical limiter functions are applied to a so-called effective ratio r , which is an average of r and r : Q ( r , r ) = Q ( r* ) . + + * (9-26) The same functions Q as given in Eq. 9-21 to Eq. 9-24 can be chosen, where the ratio r is replaced by the effective ratio r* (the same limiters as for the FDS scheme are used). The following possible choices for the effective ratio are proposed: 9-12 FINE™ Theory Numerical Model r (r ) + r (r ) 2r r + + + + min (r ,r ) ≤ -------------------------------------- ≤ --------------- ≤ r r ≤ .5 ( r + r ) ≤ max (r ,r ) . 2 2 + + r +r (r ) + (r ) It can be shown that these new limiters guarantee monotonicity provided that: r* ≥ 0 , which is easily achieved by switching the limiter off for negative r* . + - 2 - + 2 + - (9-27) (9-28) The effective ratios in Eq. 9-27 are given in order of increasing magnitude. It can be shown that the lower r* , the more diffusive the resulting limiter is. The choice of effective ratio is governed by the input parameter IRATIO. IRATIO=1 corresponds to the smallest value in the list of Eq. 9-27, IRATIO=2 to the 2nd smallest value, and so forth, with IRATIO=6 corresponding to the maximum value. For both the FDS and the STVD scheme, different limiters can be applied to the linear field (the characteristic variables that propagate with speed un ) and to the non-linear field (the characteristic variables that propagate with speed un ± c ). In addition, for the STVD scheme, a different specific ratio can be chosen for both fields. To this end, the input variables LIMITE (corresponding to the type of limiter selected in the Numerical Model page) and IRATIO are vectors of length two. The first component determines the choice of limiter, respectively the effective ratio for the linear field, the second component for the non-linear field. In general, robustness is increased by applying a more diffusive limiter. By applying this limiter only to the non-linear field, and a compressive one to the linear field, a good compromise between robustness and accuracy can be obtained. The upwind dissipation can also be reformulated to let the limiter act on ratios of variations of the primitive variables. Combining Eq. 9-9 to Eq. 9-11 the limiter function can be moved outside the diagonal matrix and put in front of the primitive variable variation: 1 1 –1 d i + 1 ⁄ 2 = -- R i + 1 ⁄ 2 diag ( λ i + 1 ⁄ 2 )L i + 1 ⁄ 2 [ 1 – Q i + 1 ⁄ 2 ]δ i + 1 ⁄ 2 V . 2 (9-29) The limiter function is the same as before and acts on ratios as in Eq. 9-19 or Eq. 9-27 where the characteristic variable variations are replaced by primitive variable variations. Eq. 9-29 can be simplified to 1 d i + 1 ⁄ 2 = -- An i + 1 ⁄ 2 ( 1 – Q i + 1 ⁄ 2 )δ i + 1 ⁄ 2 V . 2 ∂V (9-30) ∂ ( Fn ) The Jacobian matrix in Eq. 9-30 is the Jacobian with respect to the primitive variables -------------- : An = RΛL –1 . (9-31) 9-4.2 Multigrid Strategy EURANUS uses multigrid for efficiency and fast convergence. The input variable given by the user (Numerical Model page: Number of Grid(s)) denotes the number of grid levels to be used. The coarser grids are automatically created within EURANUS by dropping nodes in each direction. If in FINE™ 9-13 Numerical Model Theory a certain direction, the grid can not be coarsened any more (because of an odd number of cells) before reaching the desired number of grid levels, EURANUS will create the missing grids by coarsening only in the remaining directions. Finest level : 000 Coarse level : 111 Coarse level : 2 2 2 Coarsest level : 3 3 3 MG Cycle FIGURE 9.4.2-4 Scheme of the multigrid strategy The multigrid method is based on the Full Approximation Storage (FAS) approach. V (input parameter MGRSTR=1), W (MGRSTR=2) and F-cycle (MGRSTR=3) can be chosen by the user, or if preferred their sawtooth variant (MGRSTR =4,5,6 for respectively V,W,F sawtooth). In the sawtooth variant no smoothing (i.e. Runge-Kutta solver or implicit solver) will be applied in the coarseto-fine part of the cycle. As a result, the solution is only prolonged when passing from coarse to fine. FIGURE 9.4.2-5 Scheme of the multigrid method Consider a set of meshes denoted with an index l = 1,...,L with L being the finest level. The NavierStokes problem on the finest level can be written as: ∂U --------- + N L ( U L ) = 0 , ∂t L L (9-32) where N L ( U ) is the spatial discretization of the Navier-Stokes operator on the finest mesh L . The problem is then approximated on coarser levels l as: ∂U -------- + N l ( U l ) = F l , ∂t with F l the forcing function, defined recursively as: F l = N l ( Il + 1 U l l+1 l l+1 ) + ˆl + 1 [ Fl + 1 – Nl + 1 ( U ) ] , I l (9-33) (9-34) 9-14 FINE™ Theory Numerical Model l l where I l + 1 and ˆ l + 1 represent restriction operators of respectively the unknowns and the residuI als. If the input variable IRESTR=0, they are defined as: ˆl Rl + 1 = Il + 1 l+1 l Il + 1 U where R l+1 ∑R , ∑Ω U = -------------------------------- , ∑Ω l+1 l+1 l+1 l+1 l+1 (9-35) (9-36) is defined as: R l+1 = Fl + 1 – Nl + 1 ( U ) (9-37) and Ω represents the cell volume. The summation in Eq. 9-35 and Eq. 9-36 is over the 8 fine cells contained within a coarse cell. If IRESTR=1 a more complicated quadratic restriction is used both for the residuals and the unknowns. After temporal discretization, Eq. 9-33 becomes: S∆U + N l ( U l (0 ) l l(0) ) = Fl . (9-38) U is the current solution on mesh l, around which the equations have been linearized (in an implicit method) and which has to be smoothed. One has: U ∆U is an update of U l l (0 ) l (0 ) = Il + 1 U l l+1 (9-39) and is to be calculated. S is the smoother. It is the operator that corresponds to the chosen time integration method. In EURANUS, an explicit multi-stage Runge-Kutta time-marching scheme has been implemented, see below. The linear problem Eq. 9-38 can be solved for ∆U . The updated solution U will be smoothed (provided S is a good smoother) and can be restricted to the next coarser level, according to Eq. 939 with l replaced by l-1. Note that the number of smoothing sweeps (i.e. the number of times the Runge-Kutta operator respectively the chosen relaxation operator is applied) can be chosen by the user for each grid level (Numerical Model page in Expert Mode: Scheme definition and Number of sweep on successive grid levels) as described in section 9-3.1.1. Once the solution on the coarsest mesh is smoothed, the coarse-to-fine sweep of the multigrid cycle is initiated. The current solutions on finer grids are updated with the solution on the next coarser level: Ul= Ul + Ill-1 (Ul-1 - Il-1 Ul) l l l l (9-40) The operator Il-1 is a prolongation operator, which may be of zero- (i.e. piecewise constant, input parameter IPROLO=0) or first-order (IPROLO=1). FINE™ 9-15 Numerical Model Theory In the basic V,W,F cycle (MGRSTR = 1,2,3 respectively) the new solution on the finer mesh is smoothed before proceeding to the next finer level, by solving Eq. 9-35, with U = U . The number of sweeps of the smoothing operator is user input (Numerical Model page in Expert Mode: Scheme definition and Number of sweep on successive grid levels). In the sawtooth type cycles (MGRSTR=4,5,6) the system of equations is not solved in the coarseto-fine part of the multigrid cycle. The user also has the possibility to smooth the corrections after prolongation (2nd term in the righthand-side of Eq. 9-40) before adding them to the current finer grid solution, by applying the residual smoothing operator to the corrections. This is governed by the input parameter SMCOR which has the same definition as RSMPAR, see below, and allows to calculate the smoothing parameter, according to the chosen type of residual smoothing (parameter IRSMCH), see below. In EURANUS, the computing cost of a multigrid cycle is significantly reduced by using simplifying assumptions on coarser (i. e. all levels but the finest) grids (input parameter MGSIMP). If MGSIMP=1, a first-order accurate upwind scheme is used on coarser levels (if Upwind spatial discretization scheme is selected in the Numerical Model page in Expert Mode), else a more diffusive central scheme is used on coarser levels (if Central spatial discretization scheme is selected in the Numerical Model page in Expert Mode). If MGSIMP=2 in addition to the changes for MGSIMP=1 also viscous terms as well as source terms (of turbulence and chemistry) are omitted on coarser levels. l ( 0) l 9-4.3 Full Multigrid Strategy In order to create a good initial solution, Full Multigrid is also available. The structure of Full Multigrid can be well explained through Figure 9.4.3-6. One starts an iteration method, such as a multi-stage Runge-Kutta explicit scheme, on the coarsest grid. The solution on that level will not be interpolated to the next finer grid until it converges to a certain accuracy level. Then the solution on the finer grid is taken as the initial solution for further iterations run on that grid level. The process is recursively used until the finest grid is reached. The initial solution on the finest grid is called the solution obtained by a Full Multigrid method. Finest level : 000 Coarse level : 111 Coarse level : 2 2 2 Coarsest level : 3 3 3 FMG Cycle Prolongation of solution Prolongation of correction of the full multigrid strategy FIGURE 9.4.3-6 Scheme It should be mentioned that there are two different kinds of prolongation in Full Multigrid. One is the same as that used in the standard multigrid cycle, the other is the prolongation of solutions, which replaces corrections in a standard multigrid prolongation. The latter could be different from the former. Normally a zero-order prolongation is often used for the solution interpolation in a full multigrid cycle. Based upon numerical experiments, it has been found out that it is very important to check the convergence level of solutions on the coarser grid before switching to the next finer grid. The reason 9-16 FINE™ Theory Numerical Model for this is that if solutions do not converge on the coarser grid, it may cause divergence on the next finer grid. In addition, an initial solution on coarse grids is less sensitive to multigrid convergence than on the finest grid. A large cell size makes solutions converge easily and fast. Hence it takes much less computational time and risk of blowing up to get reasonable solutions on the finest grid, when compared to the start directly on the finest grid. A full multigrid method can therefore improve the robustness and efficiency of numerical iterations methods. 9-4.4 Time Discretization: Multistage Runge-Kutta An explicit q-stage Runge-Kutta scheme for the equation dU = F(U) dT can be written: u = u + α 1 ∆tF ( u ) u = u + α 2 ∆tF ( u ) … u = u + ∆tF ( u u n+1 q n q–1 2 n 1 1 n n (9-41) (9-42) ) = u q The coefficients α i determine the stability area and the order of accuracy of the Runge-Kutta scheme. They can be chosen in such a way that they suit the problem to be solved. For inviscid calculations the local (i.e. for each cell) inviscid time step is calculated as: ⎠ ⎞ ∆t ---Ω I CFL = ------------------------------------------------------------------------------------------------- . wS i + wS j + wS k + c [ S i + S j + S k ] CFL is the user specified CFL number (variable CFL on the Numerical Model page). The vectors S are cell normals at the cell centre (obtained by averaging the normals on the cell faces) in respectively i,j and k-direction. The module corresponds to the cell face area. For viscous calculations one also calculates a local viscous time step in each cell. If a viscous CFL number (expert parameter CFLVIS by default set at -1) is specified by the user in the Control Variables page, i.e. the input variable CFLVIS > 0, the following formula is used for the viscous time step: ⎠ ⎞ ∆t ---Ω ν with µ the local laminar viscosity (laminar simulation) or the sum of local laminar and turbulent viscosity (turbulent simulation). The actual local time step is then the minimum of both time steps: FINE™ ⎝ ⎛ ⎝ ⎛ (9-43) CFLVISΩρ = ------------------------------------------------------------------------------------------------------------------------ , 2 2 2 8µ { S i + S j + S k + 2 [ S i S j + S i S k + S k S j ] } (9-44) 9-17 Numerical Model Theory If the input variable CFLVIS < 0 (Default) the viscous CFL number, CFLVIS, is replaced by the inviscid CFL number, CFL in Eq. 9-44. The actual local time step is then obtained by weighting the inviscid and viscous time step according to a harmonic mean formula: ∆t ∆t ---- ---Ω I Ω ν ∆t ---- = ------------------------------Ω ∆t ∆t ---- + ---Ω I Ω ν ⎠ ⎞ ⎠ ⎞ ⎝ ⎛ ⎝ ⎠ ⎛ ⎞ ⎠ ⎞ ⎝ ⎛ ⎝ ⎛ ⎠ ⎞ If local time stepping is used i.e. each cell in the computation domain has its own time step given by Eq. 9-43, for inviscid calculations and Eq. 9-45 or Eq. 9-46 (depending on CFLVIS) for viscous calculations. If global time stepping is used, i.e. in all cells the same time step is used, which is, for stability reasons, the minimum of the local time steps. This option is only to be used for unsteady simulations when the dual time stepping approach (default) is not selected. For steady simulations, it is recommended always to choose local stepping, as it will increase the convergence rate. In practice, 4 or 5 stage Runge-Kutta schemes are mostly used. In EURANUS the following coefficients are default for 4 and 5 stage schemes: For central schemes α 1 = .125; α 2 = .306 ; α 3 = .587 ; α4 = 1. α 1 = .0814 ; α 2 = .191 ; α3 = .342 ; α4 = .574 ; α5 = 1. For first-order upwind schemes: α 1 = .0833 ; α 2 = .2069 ; α 3 = .4265 ; α4 = 1. α 1 = .0533 ; α 2 = .1263 ; α 3 = .2375 ; α4 = .4414 ; α 5 = 1. For second-order upwind schemes: α 1 = .1084 ; α 2 = .2602 ; α 3 = .5052 ; α 4 = 1. α 1 = .0695 ; α 2 = .1602 ; α 3 = .2898 ; α4 = .5060 ; α5 = 1. (9-49) (9-48) The user has the possibility to provide the Runge-Kutta coefficients through the expert parameter IRKCO. The first element of IRKCO corresponds to the first coefficient, the 2nd element to the second, and so forth. A maximum of 10 coefficients (i.e. a 10-stage scheme) is foreseen. If all elements of IRKCO are zero the default values are used as listed in section 9-3.2.3. In Jameson (1985) the dissipative terms are calculated only once or a few times in a q-stage RungeKutta scheme. This approach reduces the computational cost substantially. The disadvantage is that the dissipative terms need to be stored separately. For the laminar NavierStokes equations with 5 equations, 5 extra arrays are required to store the dissipative residuals from the artificial dissipation. The residual F ( U ) is split into a convective and a dissipative part: F(U)=Q(U)-D(U) (9-50) The artificial (central or upwind) dissipation terms, cf. Eq. 9-2, are accounted for either in the convective part (parameter IBOTH = 0) or in the dissipative part (parameter IBOTH = 1). 9-18 ⎭ ⎬ ⎠ ⎫ ⎞ ν ⎝ ⎠ ⎛ ⎞ ⎩ ⎝⎨ ⎛⎧ ∆t ---- = min Ω ⎠ ⎞ ∆t ∆t ---- , ---Ω I Ω . ⎝ ⎛ ⎝ ⎛ (9-45) (9-46) (9-47) FINE™ Theory Numerical Model The expression for F in Eq. 9-42 at any stage m is then F m= F(Um ) = Q(Um ) – D(U r) (9-51) where m is the current stage and r is the latest stage at which the dissipative residuals have been evaluated. The recalculation of the dissipative residuals is governed by the (vector) variable ISWV. For a mstage Runge-Kutta scheme the m first elements of this vector are used, the first element corresponding to the 1st stage, the 2nd element to the 2nd stage and so on. If the element of ISWV is 0 it means that the dissipative residual should not be calculated at the corresponding stage, and the latest available dissipative residuals will be used; if it is 1, D will be calculated. Note that for consistency reasons, the first value of ISWV should always be one. For upwind schemes, in order to run at high CFL numbers, it is advised to recalculate the upwind dissipation at every stage. The best strategy is to chose IBOTH=0 (upwind dissipation put in convective residuals, and hence calculated at each stage). ISWV monitors then only the recalculation of the physical dissipation (i.e. Navier-Stokes terms) and a calculation on the first stage only is usually enough (ISWV=1 0...0). Central schemes are usually less sensitive to the recalculation of the artificial dissipation, so that IBOTH=1 can be used. The recalculation of artificial dissipation is then also governed by ISWV. However only one calculation (ISWV=1 0...0) may not be enough; a better choice is for instance recalculation once every 2 stages, e.g. ISWV= 1 0 1 0 1 for 5-stage Runge-Kutta. For IBOTH=2 (Default), the same strategy as for IBOTH=1 is used but in addition the physical viscous terms are evaluated only once per iteration. For non-equilibrium real gas calculations (ITYGAS=4 in corresponding ’.run’ file) the input variable ISWS governs the recalculation of the source terms of the species equations. Apart from the source terms, ISWS also governs the recalculation of the diagonal terms of the Jacobians of the source terms (which are used in the point implicit procedure). From Eq. 9-42 it can be seen that, after the update in the last stage, the residual is normally not recalculated any more. Strictly spoken however, within a multigrid approach, one should use in the calculation of the forcing function for the coarser level, Eq. 9-34, the residual corresponding to the latest solution. For single grid computations, re-calculation is never done. Within multigrid, the Runge-Kutta operator can be applied more than once on each grid level, to ensure a better smoothing. The parameter "Number of sweeps on successive grid levels" give the number of times the Runge-Kutta operator has to be applied to each grid level during the fine-tocoarse - respectively the coarse-to-fine - part of the multigrid cycle. They can take different values on each grid level. Within the explicit Runge-Kutta approach, the source terms of the two-equation turbulence models and of the chemistry equations (non-equilibrium real gas) are treated in a point implicit way. For the k-ε equations the Jacobian of the negative part of the source term is diagonalized by assuming that the turbulent viscosity is approximately constant. This leads to the following relations between ρk and ρε : ρk = µ t ρε ---------Cµfµ 2 . (9-52) ( ρk ) ρε = C µ f µ -----------µt FINE™ 9-19 Numerical Model Theory For instance, for the Chien model, this results in the following diagonal terms of the Jacobian, including the compressibility corrections of Sarkar and of Nichols, cf. Eq. 4-75, on page 4-37, Eq. 4-77, on page 4-37: ∂S k Cµ C p1 ( γ – 1 )Mk µ 1 2 = – 2 ----- ρk 1 + -- αM t – 2 ------- – 2 -------------------------------- P k , 2 2 ∂ ( ρk ) 2 µt ρka ρy ∂S ε C µ ρε 3 µ – 0.5y+ = – -- C ε 2 f 2 ------------ – 2 ---- e . 2 2 ∂ ( ρε ) µt y Note that in the equations above the damping function f µ is not taken into account. - 9-4.5 Implicit residual smoothing Implicit residual smoothing can be used in combination with Runge-Kutta to speed up the convergence to steady state. One stage in the explicit Runge-Kutta scheme Eq. 9-41 might be written: u m+1 = u + α m ∆tF ( u ) = u + α m R ( u ) n The residual R may then be smoothed first, before applying the update of Eq. 9-55. The smoothing ˜ may be obtained by applying a central type operator leading to a smoothed residual R : 2 2 2 ˜ ( I – ε i ∆ i ) ( I – ε j ∆ j ) ( I – ε k ∆ k )R = R with the operator ∆ i 2 2˜ ˜ ˜ ˜ ∆ i R = R i – 1 – 2R i + R i + 1 and similar for the operators in the directions j and k. ε is a smoothing parameter on which the stability criterion is: 1 ε > -4 * σ ----σ where σ , σ are the CFL numbers of the smoothed and unsmoothed Runge-Kutta scheme respectively. The result of the residual smoothing is thus that one can run at higher CFL numbers: choose σ /σ > 1 and by an adapted choice of ε, according to Eq. 9-58, the scheme remains stable. Though theoretically Eq. 9-58 guarantees stability for any value of σ /σ , in practice this is not the case. A good practical value is σ /σ =2. The parameter σ /σ is user input (RSMPAR). Different types of residual smoothing, corresponding to different definitions of ε are available. Each one corresponds to a different value of the input parameter IRSMCH. For IRSMCH = 1 the definition of Eq. 9-58 is used, with the restriction that ε should be positive. For higher values of IRSMCH, the definition of ε also takes the mesh aspect ratio into account. For IRSMCH = 2 one uses, after Radespiel & Rossow: * * * * 9-20 ⎠ ⎞ ⎝ ⎛ (9-53) (9-54) m n m (9-55) (9-56) (9-57) * 2 –1 , (9-58) FINE™ Theory Numerical Model 1 ε i = -4 σ* 1 + max ( ( λ j * ⁄ λ i * ), ( λ k * ⁄ λ i * ) ) ------ -------------------------------------------------------------------------------------σ 1 + max ( λj * ⁄ λ i *, λ k * ⁄ λ i * ) 2 –1 , (9-59) with the spectral radius (scaled with the cell face area), e.g.: λ i * = [ ( un + c ) ⋅ S ] i . (9-60) A similar definition as Eq. 9-59 holds for ε in the directions j and k. For IRSMCH = 3, after Swanson & Turkel, one has: 1 ε i = -4 σ* 1 ------ ------------------------------------------------------------------------------------------σ 1 + 0.0625 ⋅ ( ( λ j * ⁄ λ i * ) + ( λ k * ⁄ λi * ) ) 2 –1 (9-61) IRSMCH=4 is also after Swanson & Turkel but for viscous flows. First Eq. 9-61 is applied. Denoting the obtained value as ε*, the final value is: 10 ⋅ λ d 1 ε i = max [ε*,-- ------------------------------------ ] 4 λ i * + λj * + λ k * Finally, for IRSMCH = 5, one has, after Martinelli & Vatsa: 1 ε i = -4 σ* 1 + ( λ j * ⁄ λ i * ) + ( λ k * ⁄ λ i * ) ------ ------------------------------------------------------------------------1 + λ j * ⁄ λi * + λ k * ⁄ λ i * σ 2 . (9-62) –1 . (9-63) FINE™ 9-21 Numerical Model Theory 9-22 FINE™ CHAPTER 10:Initial Solution 10-1 Overview FINE™ provides the possibility to start a computation from an initial solution. The following initial solution types are available: • constant values, • from file, • for turbomachinery, • from throughflow. Each of these types is described in the next sections. FINE™ allows to define a different initial solution type for each block or group of blocks. Such a block dependent initial solution provides more flexibility in the restart of previously computed solutions. The next section describes how to set up a block dependent solution. 10-2 Block Dependent Initial Solution This procedure permits to initiate the calculation of some of the blocks with the results of a previous calculation, whereas the other blocks are started from a uniform flow. Another possibility is to initiate one new calculation with the results of several previous calculations. This is for instance the case if a multistage turbomachinery calculation is preceded by the calculation of the separate stages. The flow solver can start from files resulting from calculations performed on different grid levels. Only the grid levels that are used in the multigrid cycle are considered here. For instance, a computation of a three-stage turbine can start from three solutions for each stage, each one on a different grid level. Furthermore, the full multigrid cycle is automatically removed when at least one file is provided on the finest grid level. FINE™ 10-1 Initial Solution Block Dependent Initial Solution 10-2.1 How to Define a Block Dependent Initial Solution The Initial Solution page is divided in two parts. On the left, a tree displays the structure of the groups of blocks. On the right, four buttons allow the user to choose the type of initial solution: constant values, turbomachinery oriented, restart from a solution file or restart from a throughflow file. At the bottom two buttons allow to modify the group(s). It is possible to create new groups of blocks in the same way as for the groups of patches on the boundary conditions page (see section 81). Different initial solutions can be assigned to these groups of blocks. By default, all the blocks are grouped in one group named "MESH" and constant values are selected. In the constant values page, the toggle button Cylindrical is set on. FIGURE 10.2.1-1Default settings of the initial solution page 10-2.2 Examples for the use of Block Dependent Initial Solution The block dependent initial solution is helpful in many industrial cases. The following are two scenarios in which this capability is very useful: 1. A solution has been calculated for a turbine including 10 stages. A new stage is added. Now the turbine has 11 stages. The designer does not want to begin a computation from scratch for the turbine with 11 stages. He can take advantage of the solution that has been found for the 10 first stages. The new computation will contain one group with the 10 stages and one group with the last stage. The first group will be assigned to a from file initial solution and the second group can be assigned to another type of initial solution. 10-2 FINE™ Initial Solution Defined by Constant Values Initial Solution 2. A turbine includes 10 stages. Even with the turbomachinery-oriented initial solution, the code does not succeed to converge properly. The designer could split the turbine in several parts and calculate the solution for each of these parts. Then a global project is created. In the Initial Solution page, a from file initial solution is assigned to each part of the project. The computation will have a far better chance to succeed. 10-3 Initial Solution Defined by Constant Values When selecting on the Initial Solutions page constant values the user can modify the physical values used as initial solution on the page as shown in Figure 10.2.1-1. The physical values are uniformly used as initial solution all over the selected group of blocks, except on the boundaries. The variables for which initial values need to be specified are the static pressure, the static temperature, the velocity components and the turbulence-based variables k and ε, if a two-equation turbulence model is used. Note that the velocity components specified by the user are the Cartesian (cylindrical) ones for a Cartesian (cylindrical) case. The lower part of the page allows for a further control of the initial field. First, for both Cartesian and cylindrical projects, the velocity direction can be fitted along the I, J or K mesh lines. The reverse option determines whether the velocity vectors will point in the I (J or K) increasing or decreasing direction. By default, no specific velocity direction is set and the input box is set to “None”. For the cylindrical projects only, an option for the fitting method can be chosen. The first option fits Vm, the meridional velocity (defined as Vm = V r + V z ), and uses Vθ to set the azimuthal absolute 2 2 velocity. The second option fits W, the relative velocity, to the mesh lines. Furthermore, for the cylindrical projects only, it is also possible to act on the initial pressure field. To this end, two options are available: constant pressure field (default) and a radial equilibrium pressure gradient. In a rotational machinery for instance, a radial equilibrium pressure gradient is often closer to the physics than a constant field. The radial equilibrium factor allows to adjust the influence of the pressure gradient (its default value is 1.0). FINE™ 10-3 Initial Solution Initial Solution from File 10-4 Initial Solution from File 10-4.1 General Restart Procedure FIGURE 10.4.1-1Restarting from a file To continue on the result of a previous computation the user must simply select the solution. Clicking on the Open browser button will open a File Chooser window to select the ’.run’ (or ’.cgns’) file of a computation. To restart from a solution the computation definition file with extension ’.run’ is not sufficient. It is required that the solution file with extension ’.cgns’ is present, which contains all the saved and requested quantities. The toggle button Reset convergence history can be selected. When selecting this button the ’.res’ file, which contains all the residuals from the previous computation, will be erased. The new residuals will be calculated with respect to the first iteration of the new computation. If the from file solution is already very close to the exact solution, the normalized residuals will decrease slowly. It is just because the starting state is already a good approximation of the solution. When all the blocks are grouped in only one group, the user is able to unselect the button Reset convergence history. In this case, the new residuals are appended to the ’.res’ file and are calculated with respect to the first iteration of the old computation. If only one group of blocks exists the button to Reset convergence history can be set on or off. If several groups of blocks exist, the button is disabled and automatically the convergence history is reset. There is a limitation in the current version of the FINE™ interface: if the user wants to keep the convergence history, the ’.run’ file MUST belong to the active computation. The following steps 1. Compute a solution. 10-4 FINE™ Initial Solution from File Initial Solution 2. 3. Create a new computation. In this new computation, select a from file initial solution. are not compatible with the Reset convergence history option. Whatever the user selects, the toggle button Reset convergence history will be set ON automatically. If, for some reason, the user still wants to keep the convergence history in a new computation, the only workaround is to copy all the files from the old computation directory to the new computation directory and to rename them with the name of the new computation. Then the File Chooser will point to a ’.run’ file belonging to the active computation and the convergence history will not be reset. The initialization of the flow computation from a solution file is currently limited to CGNS files. As the initial pressure and temperature fields are block dependent, discontinuities in these quantities can be present at block connections and the flow solver could have difficulties to converge in that case. Therefore boundary conditions should be carefully checked in order to avoid any important discontinuity at block connections. The flow solver can start from files resulting from calculations performed on different grid levels. Only the grid levels that are used in the multigrid cycle are considered here. For instance, a computation of a three-stage turbine on 0/0/0 with 3 grid levels can start from three solutions for each stage, each one on a different grid level (0/0/0, 1/1/1, and 2/2/2). Furthermore, the full multigrid cycle is automatically removed by the flow solver when at least one file is provided on the finest grid level. 10-4.2 Restart in Unsteady Computations To allow a second order restart for unsteady computations it is necessary to set in the Computation Steering/Control Variables page Multiple Files in the Output Files. This parameter allows to have multiple output files: for each saved time step also the solution of the previous time step is saved. To perform a second order restart for an unsteady computation select in the Initial Solution page from file. Using the File Chooser select the solution file with extension ’.cgns’ at a certain step (’_ti.cgns’). EURANUS will automatically find the solution of the previous time step if present (’_ti-1.cgns’). If EURANUS can not find the solution of the previous time step a message will appear in the Task Manager to indicate that a first order restart will be performed. 10-4.3 Expert Parameters for an Initial Solution from File There is no current limitation to start a k-ε computation from a Baldwin-Lomax solution. In this case, the turbulent quantities are estimated from the friction velocity if the expert parameter INIKE is set to 2 (default value) or from the turbulent viscosity field µt if INIKE = 1. In the latter case, the turbulent viscosity is initialized or read from file depending on the value of the expert parameter IMTFIL (default value IMTFIL = 0 to initialized µt or IMTFIL = 2 to read µt from file). FINE™ 10-5 Initial Solution Initial Solution for Turbomachinery 10-5 Initial Solution for Turbomachinery This type of initial solution respects the inlet and outlet boundary conditions and assumes a constant rothalpy along the axisymmetric grid surfaces typical of the turbomachinery oriented meshes (e.g., created by AutoGrid). In addition, the velocity field is automatically aligned with the blade passages. When using the turbomachinery-oriented initial solution, make sure that the INLET boundary condition is set in cylindrical mode and not in Cartesian mode. This last mode is not compatible with the turbomachinery initial solution in the present version. FIGURE 10.5.0-1Example of Turbomachinery-oriented initial solution The turbomachinery-oriented page displays two major panels: one for the inlet patches and one for the Rotor/Stator interfaces (see Figure 10.5.0-1). On the left of each panel, a tree shows the names of the patches. If no patch name has been given in IGG™, the default name will be a concatenation of the name of the block, the index of the face and the index of the patch. The Inlet Patches grouping displayed in this initial solution page is identical to the Inlet Patches grouping created under the INLET thumbnail of the Boundary Conditions page. Similarly, the Rotor/stator interface grouping displayed in the initial solution page is based on the ID given in the Rotor-Stator thumbnail of the Configuration/Rotating Machinery page. There is no way to modify the groups of patches in the Initial Solution page. If the user wants to edit the groups of patches, the user must go back to the Boundary Conditions and the Rotating Machinery pages. An input dialog box is provided per group of patches in order to select the type of static pressure specification: constant distribution or radial equilibrium. One or two input boxes are provided per group of patches in order to define the static pressure value to be used and, if radial equilibrium is chosen, the radius on which this radial equilibrium will be based. Provided that a k-ε turbulence model is selected, a third panel is displayed that requires the initial values for the turbulent kinetic energy (k) and the turbulent dissipation rate (epsilon). For advice on the initial values to choose for k and epsilon see section 4-3.5.4. Make sure that there is an inlet patch among the blocks for which a Turbomachinery initial solution has been chosen. If there is no inlet patch for the selected group of blocks, a warning message is displayed in the FINE™ interface asking the user either to edit the 10-6 FINE™ Throughflow-oriented Initial Solution Initial Solution group or to change the type of initial solution. 10-6 Throughflow-oriented Initial Solution This type of initial solution, of interest in turbomachinery calculations, allows to get an initial field on the basis of an axisymmetric throughflow solution. The initial solution is defined through an external file created by the user. The file contains 2D data in the format described hereafter. The solver will use data to generate an initial throughflow-oriented solution. Note that there is no direct link between the throughflow module integrated in the FINE™ interface and the format currently available. Work is in progress to make the bridge between both tools. The solver will create a virtual mesh based on the hub and shroud definitions, forcing points on the data points. Two additional stations will be created, at the inlet and outlet, respectively. The inlet data are extrapolated from the first spanwise station while the outlet data come from the last station. It is therefore recommended that the inlet and outlet boundaries of the mesh lie outside the meridional domain covered by the throughflow data. The meridional velocity is based on the mesh direction. 10-6.1 File Format The file will include three parts, that must be separated by a blank line: • solution definition, • hub definition, • shroud definition, Once it is created, the file is selected in the FINETM interface through a File Chooser click on the Open browser button in the Initial Solution/from throughflow page. 10-6.1.1 Solution Definition The first part of the file contains the values of the flow variables throughout a meridional structured mesh covering the entire machine. For each node of the meridional mesh, the (R,Z) coordinates are specified together with the pressure, temperature and velocity components. Here an axial case is taken as an example: Throughflow Axial Stator RZ 43 0.246 -0.025 150000 0 0 0 0.275 -0.025 150000 0 0 0 0.29 -0.025 150000 0 0 0 1st spanwise section close to inlet at Z=-0.025 #Comment line #Type of data (ZR or RZ are accessible) #Number of spanwise and streamwise stations 0.246 -0.0 130000 0 0 0 0.275 -0.0 130000 0 0 0 2nd spanwise section at Z=-0.0 FINE™ 10-7 Initial Solution Throughflow-oriented Initial Solution 0.29 -0.0 130000 0 0 0 0.246 0.025 100000 0 0 0 0.275 0.025 100000 0 0 0 0.29 0.025 100000 0 0 0 3rd spanwise section at Z=0.025 0.246 0.05 90000 0 0 0 0.275 0.05 90000 0 0 0 0.29 0.05 90000 0 0 0 4th spanwise section close to outlet at Z=0.05 There are 4 spanwise stations in this example (Z=-0.025, Z=0.0, Z=0.025 and Z=0.05), each with 3 points in spanwise direction (R direction). The point order in a streamwise and spanwise station goes respectively from hub to shroud and from inlet to outlet. Each data line is made of the two (R,Z) coordinates (in m), the static pressure (in Pa), the static temperature (in K), the meridional velocity and the tangential velocity (in m/s). 10-6.1.2 Hub Definition The hub definition uses the same format as for AutoGrid. The first line must be HUB. The second line specifies the type of coordinate (ZR or RZ) and the third line the number of hub points. The next lines correspond to the hub coordinates. Taking again the example of the case above: HUB RZ 2 0.245 -0.02 0.245 0.051 #Type of data (ZR or RZ are accessible) #Number of points on hub #Point coordinates (in m) The hub is described in increasing Z coordinate from -0.02 to 0.051. The first column contains the R coordinate for each of the two points on the hub. 10-6.1.3 Shroud Definition The shroud definition is similar to the hub definition, except for the first line that will be replaced by SHROUD and the points coordinates. SHROUD RZ 2 0.3 -0.02 0.3 0.051 #Type of data (ZR or RZ are accessible) #Number of points on hub #Point coordinates (in m) 10-8 FINE™ Throughflow-oriented Initial Solution Initial Solution Meridional Average View SHROUD BLADE 3D View 1st spanwise section 2nd spanwise section 3rd spanwise section 4th spanwise section INLET HUB OUTLET FIGURE 10.6.1-4 Throughflow-oriented Initial Solution FINE™ 10-9 Initial Solution Throughflow-oriented Initial Solution 10-10 FINE™ CHAPTER 11:Output 11-1 Overview With the EURANUS flow solver in the FINE™ environment the user has the possibility to specify the content of the output generated by the solver. The output does not only contain the flow variables for which the equations are solved (density, pressure, velocity components), but also other variables such as the temperature, the total conditions, the Mach number, customized velocity projections, etc... Furthermore CFView™ allows to calculate derived quantities, which permits to limit the memory size of the output and to avoid re-launching the flow solver in case one quantity of interest is not available. With this functionality the user can find the compromise between an acceptable memory size for the output and the ease of having all flow quantities of interest immediately available for visualization. In the next sections the way to control the output from the EURANUS flow solver is described in more detail: • field quantities: calculated at all the mesh nodes (see section 11-2.1), • solid data: calculated along the solid wall boundaries (see section 11-2.1.5), • customized averaged data: — the evolution of some averaged quantities can be provided along the streamwise direction as described in section 11-2.2, — for turbomachinery applications, a pitchwise averaged output can be created for visualization as described in section 11-2.3, • global performance output (see section 11-2.5), • additional output for the ANSYS code, a widely used finite element code for structural analysis (see section 11-2.4). The global performance output is written in a ASCII file with the extension ’.mf’. All other output generated by the solver is written in one single ’.cgns’ file, compatible with the CFView™ visualisation software. It is also possible to request for the output to be written in Plot3D format as described in section 11-2.6. FINE™ 11-1 Output Output in FINE™ 11-2 Output in FINE™ 11-2.1 Computed Variables Using the Outputs/Computed Variables page, the user can choose which physical variables have to be included in the output generated by the flow solver EURANUS, see Figure 11.2.1-1 to Figure 11.2.1-6. All the selected variables will then be automatically available when launching CFView™ in order to visualize the results. 11-2.1.1 Thermodynamics n FIGURE 11.2.1-1 Thermodynamics computed variables page (for cylindrical projects) Table 11-1 and Table 11-2 give the formulae used to calculate the thermodynamic quantities. Cartesian and cylindrical cases Incompressible Compressible Pstat V +k Ptot = P stat + ρ -------------2 2 Quantity Static pressure Total pressure Pstat T tot ---------T stat γ ---------γ–1 Static temperature T stat P stat T stat = -----------ρr gas 2 Total temperature V +k T tot = T stat + -------------2C p ρ T stat s = C p ln -------------------T statinlet µ V +k T tot = T stat + -------------2C p ρ ( P stat ⁄ P statinlet ) s = C v ln ----------------------------------------γ ( ρ ⁄ ρ inlet ) µ 2 Density Entropy Dynamic viscosity TABLE 11-1 Thermodynamics quantities generated by EURANUS 11-2 ⎠ ⎞ ⎝ ⎛ Ptot = Pstat FINE™ Output in FINE™ Output Incompressible Relative total pressure 2 Cylindrical cases only Compressible Ptot = P stat ⎠ ⎟ ⎞ ⎝ ⎜ ⎛ r W +k P tot = Pstat + ρ --------------2 r T tot ---------T stat r γ ---------γ–1 Relative total temperature W +k r T tot = T stat + --------------2C p Pstat W 2 + k – ω 2 r 2 I = C p T stat + ----------- + --------------------------------ρ 2 2 r W +k T tot = T stat + --------------2Cp 2 Rothalpy W + k – ω rI = C p T stat + --------------------------------2 2 2 2 ω is the angular rotation speed and r, the distance from the rotation axis TABLE 11-2 Thermodynamic quantities generated by EURANUS in cylindrical cases Furthermore five definitions of the pressure coefficient are available: CP1, CP*1, CP2, CP*2, CP3: inlet — CP1 = ------------------------------- , 2 2 ( P – Pt ) ρinlet U ref — Pt inlet – Pt CP∗ 1 = ------------------------- , Pt inlet 2( P – P 2 ( Pt ) ρ inlet W inlet inlet — CP2 = ----------------------------- , 2 inlet — CP∗ 2 = --------------------------------- , 2 – Pt ) ) ρ inlet W inlet ρU inlet — CP3 = ----------------------------- . 2 2( P – P where Xinlet corresponds to the mean value of the variable X on the inlet, and where Uref is defined as: • ω RLEN in cylindrical cases, with RLEN, the reference length given in the Flow Model page, and ω, the rotational speed (defined block per block), • UENTR (Cartesian case) to be specified in the expert parameters list of the Computational Steering/Control Variables page. When applying FINE™ to external flow situations (expert parameter IINT set to 0), only the quantity CP2 is well-defined. In external flows this pressure coefficient is defined in terms of the Reference values and Reynolds Number Related Info specified in FINE™ on the Flow Model page: 2 ( P – P ref ) CP2 = -------------------------2 ρ ref U ref . The user must then ensure that the far field or free stream quantities set on the Boundary Conditions page as well as the initial solution values (set on the Initial Solution page) are fully consistent with the reference values specified on the Flow Model page. FINE™ 11-3 Output Output in FINE™ Finally, when a condensable fluid is selected in the Fluid Model page, new quantities at the bottom of the page will appear. Those variables are defined using the thermodynamic tables defining the condensable gas (see section 3-2.3.4 for more details). When the condensable fluid option is used, 6 flow variables are stored at all mesh cell centers instead of 5 for a perfect gas or liquid. These variables are the following: density, velocity components, static pressure and total energy ( ρE = ρ e + ----- ). The static and total enthalpy can easily be ⎠ ⎞ V 2 2 derived using: ρ ⎠ ⎞ p • static enthalpy h = e + -⎝ ⎛ . 2 V • absolute total enthalpy H a = h + ----- . 2 2 -----• relative total enthalpy H r = h + W - . 2 The dryness fraction permits to evaluate the location of the local thermodynamic state with respect to the saturation curve. For each value of the pressure an interpolation from the saturation table (’PSA.atab’) permits to determine the saturated liquid (ρl) and gas (ρv) values of the density. The dryness fraction is then computed by: ( ρ – ρl )ρv • dryness fraction X = ------------------------- . ( ρv – ρl )ρ The generalised dryness fraction directly results from the above expression whereas the standard dryness fraction is bounded in the [0,1] interval. It should be mentioned that the presence of the saturation table (’PSA.atab’) is required in order to allow the calculation of the dryness fraction, although this table is not required by the solver itself (unless an inlet boundary condition based on dryness fraction is used). 11-2.1.2 Velocities FIGURE 11.2.1-2 Velocities computed variables page (for cylindrical projects) 11-4 ⎝ ⎛ ⎠ ⎞ ⎠ ⎞ ⎝ ⎛ ⎝ ⎛ FINE™ Output in FINE™ Output The velocity quantities that can be selected are described below. Both for Cartesian and cylindrical cases: • Absolute velocities: Vx, Vy, Vz, Vxyz, V. • Velocity projections: Vi, Vj, Vk, |Vi|, |Vj|, |Vk|,Vis,Vjs,Vks. · Vi = V ⋅ Si ⋅ Si with Si , surface vector of the i surface, · Vis = V – V ⋅ Si ⋅ Si . ⎠ ⎞ ⎝ ⎛ • Absolute Mach Number, only for compressible fluids: ⎠ ⎞ ⎝ ⎛ M abs = V ⁄ γP stat ------------- . ρ For cylindrical projects only: • Absolute velocities in the rotating frame:|V|, Vr, Vθ, Vm: Vr = Vx cos θ + Vy sin θ , Vθ = Vy cos θ – V x sin θ , Vm = Vr + Vz . 2 2 • Relative velocities: Wx, WY, Wxyz, W, Wθ: W= V – ω × r , Wθ = Wy cos θ – W x sin θ . • Relative velocity projections: Wi, Wj, Wk, |Wi|, |Wj|, |Wk|, Wis, Wjs, Wks · Wi = W ⋅ Si ⋅ Si with Si , surface vector and · Wis = W – W ⋅ Si ⋅ Si . ⎠ ⎞ ⎝ ⎛ • Relative Mach Number: ⎠ ⎞ ⎝ ⎛ M rel = W ⁄ γPstat ------------- . ρ 11-2.1.3 Vorticities The vorticity is calculated according to the following expression: FINE™ ⎠ ⎞ ⎠ ⎞ ⎝ ⎛ ⎝ ⎛ FIGURE 11.2.1-3 Vorticities computed variables page 11-5 Output Output in FINE™ ζ= ∇ × V , where ∇ is the gradient operator. From the above expression, ζx, ζy, ζz, ζxyz, and ζ are available. 11-2.1.4 Residuals FIGURE 11.2.1-4 Residuals computed variables page The residuals are computed in FINE™/Turbo by a flux balance (the sum of the fluxes on all the faces of each cell). The absolute value |RES| resulting from the flux balance is written as output for each cell. The residuals for the following quantities can be selected: • density ρ, • energy E, • velocity component Wx, • velocity component Wy, • velocity component Wz, • turbulent kinetic energy k for two equations turbulence models, • turbulent energy dissipation rate ε for two equations turbulence models. 11-2.1.5 Solid Data FIGURE 11.2.1-5 Solid data computed variables page The solid wall data refer to quantities that are estimated at the solid boundaries: • static pressure at walls (see section 11-2.1.1). • static temperature at walls (see section 11-2.1.1). τ • normalized tangential component C f = ---------------- of the viscous stress at walls, where τ is the vis2 cous stress, V is the reference velocity and ρ is the reference density defined in Flow Model page. ρV ⁄ 2 • heat transfer at walls in general DT q w = K ⋅ ------Dn and for k-ε extended wall function q w = ρCpu τ T τ where u τ and T τ are coming from page 4-34. 11-6 FINE™ Output in FINE™ Output • relative velocity at walls (see section 11-2.1.2). • viscous stress τ xyz at walls. • y+ (in first inner cell). 11-2.1.6 Turbulence FIGURE 11.2.1-6 Turbulence computed variables page. The following quantities can be stored: • y+ (3D field) ρy wall u w y + = --------------------- , µ • wall distance (i.e. closest distance to the wall: ywall), • turbulent Viscosity (µt/µ), • production of kinetic energy (Production), • k and ε for two equation turbulence models. 11-2.1.7 Throughflow For the output specific for Throughflow computations see Chapter 6. 11-2.2 Surface Averaged Variables This option is customised for turbomachinery applications and displays in a Cartesian plot the evolution of surface-averaged variables along the streamwise direction. The user should select blocks along the streamwise direction. A surface averaging is performed on the grid surfaces perpendicular to the streamwise direction. Computation on each block will be performed to create the plot. The Surface Averaged Variables page is modified according to the type of project as defined in the Mesh/Properties... menu. For a Cylindrical project the page looks like shown in Figure 11.2.2-7. In this case the streamwise direction (by default K) is defined on the Rotating Machinery page of the FINE™ interface. The blocks to include in the averaging can be selected from the list of blocks by left-clicking on them. Selected blocks appear highlighted. This selection acts as a toggle where clicking ones on a block name selects the block and clicking a second time deselects the block. To select multiple blocks it is sufficient to left-click on each of them. The variables available for averaging are listed on this page and a averaging method can be selected for each variable independently. The turbulent quantities k and ε only appear for selection if a twoequations turbulence model is used. FINE™ 11-7 Output Output in FINE™ FIGURE 11.2.2-7 Surface averaged variables page for a Cylindrical project Since the integration is performed on mesh surfaces, some differences could appear. For example, in a case with splitter, two curves will be generated and a sum on this curve should be performed to see the evolution of the quantity in streamwise direction of one channel. Since the surface averaging is performed on grid surfaces this option is mainly suitable for H-topology meshes. Especially computing the evolution of the mass flow in streamwise direction with HOH mesh topology is not correct. For Cartesian projects as defined in the Mesh/Properties... menu the Surface Averaged Variables page is displayed as shown in Figure 11.2.2-8. In this case the streamwise direction needs to be selected directly in this page by selecting to average on surfaces of constant index (in the example of Figure 11.2.2-8 surfaces of constant k). The blocks to include in the averaging need to be selected in the same way as for a cylindrical case as described before. Contrary to a cylindrical project, in this case no relative quantities are available. Like for a cylindrical project the surface averaged evolution of the quantities is shown for each block separately. 11-8 FINE™ Output in FINE™ Output FIGURE 11.2.2-8 Surface averaged variables page for a Cartesian projects 11-2.3 Azimuthal Averaged Variables The FINE™/Turbo environment provides the user with a specific turbomachinery output, i.e. the two-dimensional meridional view of the circumferentially-averaged results. Note that this functionality is also available in CFView™. Using the Azimuthal Averaged Variables page, the user can choose which physical variables have to be included in the pitchwise-averaged output generated by the flow solver. This page is therefore only accessible if the project is of the cylindrical type. The azimuthal averaging of the variables is calculated at the end of the computation. The results will be displayed as a 2D case in CFView™. The name of the file from which CFView™ can read which variables have been averaged in the azimuthal direction has the extension .me.cfv. The choice is left to the user to apply mass or area averaging, and to merge into one patch the averaging patches. This last option (Merging of meridional patches) simplifies the meridional view but the patches are merged in increasing order one after another, which is not suitable for all topologies. If Surface of revolution mesh (Autogrid) option is activated, a specific algorithm will be applied to enhance azimuthal averaging of the solution performed on revolution surfaces. The Parameters area is divided into five ’notebook pages’ which can be selected by clicking on one of the five corresponding thumbnails: Thermodynamics, Velocities, Vorticities, Residuals and Turbulence in the same way as for the control variables. Figure 11.2.3-9 shows an example of the corresponding information page for thermodynamics variables. Other pages are similar to those described in section 11-2.1. At the bottom of Figure 11.2.3-9 in expert mode the user can define the meridional patches for azimuthal averaging. See section 11-3.1 for more detail on this possibility. By default meridional averaging patches are set. Automatic setting of the meridional averaging patches only works if no manual action is involved (like renaming of some patches). FINE™ 11-9 Output Output in FINE™ FIGURE 11.2.3-9The thermodynamics azimuthal averaged variables page 11-2.4 ANSYS The FINE™/Turbo environment provides the user with a specific ANSYS output. The objective is to export results of the CFD computation on solid surfaces (nodes and elements) into ANSYS as a boundary condition for the finite element model. This approach is called FEM loading method for loading the CFD results on a Finite Element Model. The transferred results on the interface fluidstructure can be the pressure field for a structural analysis and the temperature field or the heat fluxes for a thermal analysis in the structure. The FEM approach needs to have the finite element mesh of ANSYS. If this mesh does not exist before the CFD computation, it is impossible to create directly a file that can be imported in ANSYS to apply the suitable boundary condition. Consequently the best way to manage the interface between FINE/TURBO and ANSYS can be a new postprocessing tool. The post-processing tool is needed with the specification of the ANSYS mesh, the common surfaces where the data must be interpolated and the type of boundary condition on each surface. The transfer will be carried out through the ANSYS file saved with the command CDWRITE ("project_ANSYS.cdb") in ANSYS. This file will be modified and read again in ANSYS to impose the CFD results as boundary conditions (see Figure 11.2.4-10). 11-10 FINE™ Output in FINE™ Output FIGURE 11.2.4-10Data transfer of CFD results into the ANSYS project 11-2.4.1 ANSYS Pre-Processing Before completing the Outputs/ANSYS pages, the user must create the file ’project_ANSYS.cdb’ with the command CDWRITE in ANSYS. Furthermore before the save in ANSYS, some operations needs to allow the identification of the common surface between the fluid model and the structural model. The ANSYS project must be completely defined with a special treatment for the surface loads that will be replaced by the interpolated CFD results. On each common surface, a coded constant value is specified. The default coded values are given in the table 11-3 for the different types of boundary condition. The value is incremented by one for each different surface so that for example the pressure imposed on the first surface is set to 1000001 and it is set to 1000002 on the second, ... Boundary Condition Code Pressure field 1000001 Temperature field 2000001 Temperature field for heat 3000001 flux by convection Heat flux 4000001 TABLE 11-3 Default code for different type of boundary condition imposed from CFD results The coded value can be modified in order to avoid confusion with physical values. Note that the surface must be relatively flat or smooth (without sharp angle) so that the six surfaces define a cube. Moreover the surface closed on itself as a cylinder or a blade must be divided into two parts. Validation tests are performed with ANSYS release v8.0. Please refer to ANSYS user manual for more details on the ’.cdb’ file format FINE™ 11-11 Output Output in FINE™ 11-2.4.2 Global Parameters The user can complete the Outputs/ANSYS pages when the file ’project_ANSYS.cdb’ has been created (refer to section 11-2.4.1 for more details). (1) (2) (3) (4) (5) FIGURE 11.2.4-11General Parameters of ANSYS outputs Firstly, the user needs to specify under the thumbnail Global Parameters in Boundary Conditions (Figure 11.2.4-11 - (1)) the coded constant value used in the file ’project_ANSYS.cdb’. The default coded values are given in the table 11-3 for the different types of boundary condition. Furthermore, the user has to specify the required units of the data for each type of boundary condition. The units will be specified next to the coded value. Then, the user needs to load the file ’project_ANSYS.cdb’ (Figure 11.2.4-11 - (2)) created in ANSYS (refer to section 11-2.4.1 for more details) in Input File. The data transfer between the CFD mesh and the structural mesh is possible if the common geometries are matching. It is possible that this condition is not fulfilled and the causes can be diverse. • the units: a first difference can come from the units of the meshes. Consequently the units used in the ANSYS mesh must be specified in ANSYS Mesh Units. The conversion Factor will be deduced automatically (Figure 11.2.4-11 - (3)). • the coordinate system: the second cause of mismatching is the use of different coordinate systems (Figure 11.2.4-11 - (3)). For example, the original geometry can be only rotated for the CFD model so that the axial direction corresponds to the Z axis. The necessary change of coordinate will be done through the specification of the position of the coordinate center of the ANSYS mesh in the coordinate system of the CFD mesh and the specification of the location of three common points in both meshes in Reference System. Note that these points cannot be located on a line or a plane including the zero point (not linearly dependent). The coordinates are specified in their respective units. 11-12 FINE™ Output in FINE™ Output The origin of the ANSYS mesh should be at (0,0,0). Finally in Output File, the user specifies the new output file ’project_CFD.cdb’ (Figure 11.2.4-11 (4)) containing the transferred CFD results on the solid boundaries coded in ANSYS (refer to section 11-2.4.1 for more details). In order to create the new output file, the user has to complete the page under the Surface Selection thumbnail before clicking on the Create Output File button (Figure 11.2.4-11 - (5)). 11-2.4.3 Surface Selection After completion of the page under Global Parameters thumbnail, the user can complete the page under Surface Selection page (refer to section 11-2.4.2 for more details) before creating the ANSYS output file. When the ANSYS input file is read in Input File, the common surfaces where data must be transferred are identified in the ANSYS mesh. The interface FINE™ lists each surface with the corresponding coded value (Figure 11.2.4-12 - (1)). For each detected surface of the structural ANSYS mesh, by clicking on Selected Surface Properties button (Figure 11.2.4-12 - (2)), a new window (Figure 11.2.4-13) allows the user to specify the solid patches from which the data will be interpolated and some interpolation parameters: interpolation type (Interp Type) and the allowed maximal distance (Max Dist). (1) (3) (4) (2) FIGURE 11.2.4-12Surface Selection of ANSYS outputs FINE™ 11-13 Output Output in FINE™ Two different interpolation types (Interp Type) are proposed: a conservative and a non-conservative. The suitable interpolation scheme is dependent on the type of boundary conditions. The spatial field of pressure or temperature can be interpolated from cell faces to nodes whereas a conservative transfer of the heat fluxes can be preferred. An allowed maximal distance (Max Dist) can be used to control the interpolation process by ensuring that it is performed in the nearest element of the selected solid CFD patches. FIGURE 11.2.4-13Add Solid Patches to ANSYS surface Then, the user specifies the solid CFD patches in the list of Solid Patches by <Ctrl> or <Shift> and left-click. To add or remove solid patches linked to the highlighted ANSYS surface, the buttons Add Selection and Remove Selected are respectively used. When the solid patches are well selected, the window has to be closed (Close) and the patches will appear in the list Selected Solid Patches and Groups (Figure 11.2.4-12 - (3)). Note that the ANSYS surface must be completely overlapped by the selected IGG solid patches in order to ensure a complete data transfer. The area of the selected IGG solid patches can be larger than the area of the ANSYS surface. Since the IGG™ solid patches defining a periodic structure can be divided (Figure 11.2.4-14), a periodic shift can be required to match the common ANSYS surface. This shift must be specified for each solid patch, highlighted in Selected Solid Patches and Groups list, in Periodicity by activating Rotation and Translation (Figure 11.2.4-12-(4)). The rotation and translation shifts are respectively specified degrees and IGG™ units mesh. FIGURE 11.2.4-14Mesh differences IGG™ vs. ANSYS 11-14 FINE™ Output in FINE™ Output Moreover one ANSYS surface can be covered by a group of solid patches and by the same group rotated (or translated). Consequently, a duplication of the periodic solid patches is possible by activating Duplicate patch(es) after applying a Rotation and Translation to the highlighted solid patch (Figure 11.2.4-12-(4)). FIGURE 11.2.4-15Duplicate Option Utility Finally, the new output file can be created by clicking on the Create Output File button (Figure 11.2.4-11 - (5)). 11-2.5 Global Performance Output The main results for global performance are summed up in a file with extension ’.mf’. Inlet and outlet averaged quantities, pressure ratios and efficiency are computed and stored in this file. The user can select which and what kind of information is stored using expert parameters as described in section 11-3.2. In this section the default contents of the global performance output is described. 11-2.5.1 Solid Boundary Characteristics This part of the file gives the characteristics of the quantities that are estimated at the solid boundaries. Those quantities are inferred from the global force F = Fpressure + Fviscous exerted by the flow at a given point. This force can be estimated from the pressure and velocity fields at each point. The calculated quantities for an internal configuration are: • Axial thrust, i.e. the projection of the global force on the rotation axis: ∑ F ⋅ nz . S • The projection of the torque along a given direction z , i.e. the couple exerted by the global force S ⎠ ⎟ ⎞ ∑r × F IDCMP, the default value of which is (0,0,1). For external flow configurations the expert parameter IINT must be set to 0 and the output file will contain the quantities as described in section 11-3.2 instead of the axial thrust and the torque FINE™ ⎝ ⎜ ⎛ ⋅ z along direction z . This direction is given through the expert parameter 11-15 Output Output in FINE™ 11-2.5.2 Global Performance EFFDEF Compressors p t2 γ -----–1 p t1 = ----------------------------T t2 ------ – 1 T t1 p2 γ -----–1 p t1 = ----------------------------T2 ------ – 1 T t1 p2 ---–1 p1 = --------------------------T2 ---- – 1 T1 ⎠ ⎞ ⎝ ⎛ ⎠ ⎞ ⎝ ⎛ γ–1 ---------γ γ–1 ---------- p t2 >p t1 ⎠ ⎞ ⎝ ⎛ Turbines p t2 <p t1 T t2 ln -----cp T t1 = ---- ⋅ ----------------R p t2 ln ----p t1 T2 ln -----cp T t1 = ---- ⋅ ----------------R p2 ----ln p t1 T2 ln ---cp T1 = ---- ⋅ ---------------R p2 ln ---p1 ⎠ ⎞ ⎠ ⎞ ⎝ ⎛ ⎝ ⎛ ⎠ ⎞ ⎠ ⎞ ⎝ ⎛ ⎝ ⎛ ⎠ ⎞ ⎠ ⎞ ⎝ ⎛ ⎝ ⎛ 1 η is η pol T t2 p t2 1 – -----ln ----T t1 p t1 η = ----------------------------R γ–1 = ---- ⋅ ----------------- is ---------cp T t2 p t2 γ ln -----1 – ----T t1 p t1 2 η is γ–1 ---------- η pol T2 p2 1 – ---------ln T t1 p t1 η = ----------------------------R γ–1 = ---- ⋅ ----------------- is ---------cp T2 p2 γ -----ln 1 – ----T t1 p t1 3 η is η pol T2 p2 1 – ---ln ---T1 p 1 η = --------------------------R is γ–1 = ---- ⋅ ------------------------cp T2 γ p2 ln ------1– T1 p 1 TABLE 11-4 Isentropic and polytropic efficiency definitions for perfect gases Global performance data, available in the ’.mf’ file, are calculated using the results at the inlet and outlet boundaries of the computational domain. The ’.mf’ file also provides global averages at each rotor/stator interface. If the project does not involve any of these boundaries or interfaces, the ’.mf’ file is empty. For turbomachinery cases, the output includes an efficiency. Several definitions are available, selected through the expert parameter EFFDEF (default: 1). For projects with a rotor, the expressions proposed in table 11-4 are used (index 1 and 2 refer to the inlet and exit sections respectively). The same definitions can be applied to the real gas in the case IRGCON=0 but with γ instead of γ. Compressors h 02 – h 01 η is = -------------------h 02 – h 01 is p t2 >p t1 Turbines h 02 – h 01 η is = -------------------is h 02 – h 01 p t2 <p t1 TABLE 11-5 Isentropic efficiency definition for real gases with ct r (IRGCON=1) is The definitions in Table 11-5 correspond to real gases with IGRCON=1. The value of h 02 is obtained from the temperature T02 by using the isentropic relation: is ∫1 2is C p ----- dT 0 = T0 11-16 ⎠ ⎞ ⎠ ⎞ ⎠ ⎞ ⎝ ⎛ ⎝ ⎛ ⎝ ⎛ ⎠ ⎞ ⎠ ⎞ ⎠ ⎞ ⎠ ⎞ ⎠ ⎞ ⎝ ⎛ ⎝ ⎛ ⎝ ⎛ ⎝ ⎛ ⎝ ⎛ ⎠ ⎞ ⎝ ⎛ η pol η pol η pol ∫1 2is r ----- dP 0 . P0 FINE™ Output in FINE™ Output EFFDEF Pumps p t2 >p t1 Turbines p t2 <p t1 1 · ∆p t m η = -----------------------------ρω ⋅ Torque · ∆pm η = -----------------------------ρω ⋅ Torque · ∆p t m η = ------------------ρCp∆T t ρω ⋅ Torque η = -----------------------------· ∆p t m ρω ⋅ Torque η = -----------------------------· ∆pm ρCp∆T η = -------------------t · ∆p t m 2 3 TABLE 11-6 Efficiency definitions for liquids (incompressible flows) Expressions involving the Torque in Table 11-6 are computed only if the user activates the option Compute force and torque in the Boundary Condition page devoted to solid surfaces. For non rotating projects (pure stator), the following expression is used to define the efficiency: p t2 – p 2 η = ----------------p t1 – p 2 . (11-1) Finally, relative and absolute flow angles are derived from the averaged velocity components: ⎠ ⎞ ⎠ ⎞ ⎝ ⎛ ⎠ ⎞ ⎠ ⎞ vθ α = arc tan -----Vm ⎝ ⎛ wθ β = arc tan -----Vm cylindrical , (11-2) 11-2.6 Plot3D Formatted Output On the Computed Variables page it is possible to select Plot3D output to be created according to the file format described in Appendix B. The user may select between a ASCII format or Fortran unformatted format. When selecting the Unformatted file (binary) option use the corresponding option in CFView™ to open the file: click on the File Format... button in the menu File/Open Plot3D Project... and select Unformatted. Do not select Binary format. In CFView™ the user needs to select also little endian or big endian formats. On PC platforms (Windows and LINUX) select binary low endian and on all other platforms select binary big endian. FINE™ ⎝ ⎛ v α = arc tan ---y vx ⎝ ⎛ wy β = arc tan ----wx cartesian . (11-3) 11-17 Output Expert Parameters for Output Selection 11-3 Expert Parameters for Output Selection 11-3.1 Azimuthal Averaged Variables In expert mode the user may specify on the bottom of the Azimuthal Averaged Variables page the ‘averaging patches’ of the 3D mesh used to define the mesh surface that will be projected onto the meridional plane in order to support the azimuthal averaged variables. A default selection is automatically presented for AutoGrid meshes. Four input boxes are provided to enter the number of patches, the index of the patch being defined, the block number and six indices to define the patch. For instance, the six indices: 1 1 1 65 1 129, define a patch of a given block corresponding to a face I = 1 and for J =1 to 65 and K=1 to 129. The same system is used to define blade patches that will simply be projected in the meridional plane to visualize the variables on the blade pressure side or suction side. The indices must be defined on the finest mesh. MERMAR: Safety margin for azimuthal averaged CFView™ solution. The mesh is shrunk with a factor of 1.- MERMAR. 1st entry = axial safety margin 2nd entry = radial safety margin The purpose of these two margins is to avoid points near the boundaries for which the azimuthal averaging can not be performed. In general the azimuthal averaging is performed by taking a point on the defined patch and to average the values for points in azimuthal direction starting from this point. If there is not a sufficient amount of points in azimuthal direction the average is not computed for that point and therefore the value for this point is not represented in CFView™. To avoid such ’blank’ points near the edges of the patches it may be necessary to take a certain margin from the edges of the patches. The default values for the safety margins are appropriate for meshes on surfaces of revolution. If the mesh is not a mesh on surfaces of revolution higher margins may be required. See section 114.3 for more detailed information on the methods available for azimuthal averaging and the use of these margins. Use of the 3rd and 4th entry is not supported. 11-3.2 Global Performance Output To influence the type of output written in the file with extension .mf the following expert parameters can be used: EFFDEF: Efficiency definition for projects with at least one rotating block: = 1: total to total, = 2: total to static, = 3: static to static. OUTTYP: Select the type of output: = 1: torque and drag, = 2: heat flux and energy, 11-18 FINE™ Expert Parameters for Output Selection Output IINT: Type of flow: = 0: internal flow, = 1: external flow. For external cases the following output is written in the global performance output file: • Drag coefficient, i.e. normalized projection of the global force in a chosen direction: ∑ F ⋅ n1 ⁄ ( 0.5ρref Uref S ref ) S 2 . • Lift coefficient, i.e. normalized projection of the global force in a chosen direction, generally perpendicular to that used for the Drag coefficient: ∑ F ⋅ n2 ⁄ ( 0.5ρref Uref S ref ) S 2 . • Momentum, i.e. normalized projection of the torque in a chosen direction (default 0, 0, 1): ⋅ n 3 ⁄ ( 0.5ρ ref U ref S ref C ref ) S ⎠ ⎟ ⎞ ⎠ ⎟ ⎞ ∑r × F 2 In the above equations, S is the surface of the selected patch(es), ρ ref and U ref are user defined reference density and velocity (see the Flow Model menu of the FINE™ interface). S ref is a surface of reference for which the default value SREF is set to 1 m2 and C ref is a length of reference for which the default value CREF is set to 1. n 1, n 2, n 3 are normalized vectors used for the Drag, Lift and Momentum coefficient and defined through the expert parameters IDCDP, IDCLP and IDCMP. Their default value is (0., 0., 1.). r is the distance from the reference point IXMP (default value: 0., 0., 0.). n z is the normalized vector directed along the rotation axis. The parameters mentioned here can be changed in the Computational steering/Control variables page in expert mode. IWRIT: Add some additional output on all block faces such as mass flow through these faces: = 0: deactivated, = 1: mass flow through rotor/stator interfaces, = 3: summarizes the mass flow through different boundary types (SOL, ROT, INL,...), = 4: mass flow through all block faces. SREF: Reference area to non-dimensionalize the lift, drag and momentum, to get respectively the lift coefficient, drag coefficient, moment coefficient. The default SREF=1. CREF: Reference chord to non-dimensionalize the calculated moment, to get the moment coefficient. IDCDP: This parameter gives the direction (i.e. 3 values) on which the body force has to be projected to give the axial thrust or the drag component. E.g. 1,0,0 means that the drag is the xcomponent of the body force. IDCLP: For flows around bodies this parameter gives the direction (i.e. 3 values) on which the body force has to be projected to give the lift component. E.g. 1,0,0 means that the lift is the xcomponent of the body force. For internal (IINT=1) cylindrical cases this parameter is not used. FINE™ ⎝⎝ ⎜⎜ ⎛⎛ . 11-19 Output Theory IDCMP: This parameter gives the direction (i.e. 3 values) on which the moment vector on the body has to be projected to give the moment. E.g. 1,0,0 means that the moment is the x-component of the moment vector. IXMP: Specifies the x,y,z coordinate of the point around which the moment has to be calculated. 11-4 Theory 11-4.1 Computed Variables The flow solution is stored in the .cgns file and will be used for the 3D CFView™ output. CFView™ requires a cell-vertex representation of the flow solution, i.e. the flow variables need to be provided at the mesh nodes. Since EURANUS considers the flow variables at cell centres, an interpolation process is performed by the flow solver in order to compute the flow variables at the mesh nodes. The required interpolation of the flow solution is done by arithmetic averaging. If u represents one of the primitive variables ρ, w x, w y, w z, p and u the interpolated value, 8 1 u = -8 ∑u , i i=1 (11-4) where the summation is over the eight surrounding original locations of the respective variable. The basic flow variables are calculated at the mesh nodes using the above procedure. Derived quantities ( v r, p t, H, s, ... ) are computed from this consistent representation of solution and geometry. By contrast, if a quantity involves the surface normals, these are first calculated on the cell faces of the original mesh and then averaged to the required location. Other exceptions are quantities involving gradients or which are provided by the code: • The Cartesian components of ∇ × W are computed in the cell corners, ∇ × V = ∇ × W + 2ω system . (11-5) • If a cylindrical component is requested, transformation to cylindrical coordinates is done at the cell corners, as is the calculation of ∇ × W . Only then are the requested component, the vector or its magnitude interpolated to the desired mesh. • Some of the variables used in the turbulence models are provided by the code in the cell corners and treated in the same way as the coordinates (wall distance, y , µ t ). If a two equation turbulence model is used, k and ε are additional variables treated in the same way as the primitive variables. The residuals too, are provided by the code in the cell centres and therefore treated in the same way as the primitive variables, with the difference that they are only defined in the interior and thus copied to the dummy cells as described above. The above described arithmetic averaging process used to construct the CFView™ solution is first order accurate, which has an important consequence if the user wants to extract quantitative global quantities: + 11-20 FINE™ Theory Output In case of high flow gradients the calculation within CFView™ of the average (surface integral) of a given quantity throughout an I, J or K=constant surface of the mesh or a cutting plane will be performed with an error with respect to the flow solution calculated by the flow solver. 11-4.2 Surface Averaged Variables The procedure generates a multi-column file with indices, coordinates and the streamwise evolution of the requested variables, averaged on mesh surfaces normal to the streamwise direction. This file can be processed for plotting versus the index, the coordinates x , r or z and the meridional distance. Mass or area averaging can be requested for each variable individually. FIGURE 11.4.2-16 Stencil for 1D averaged flow. The numbers are the relative weight of each cell in the contribution of the central cell to the surface average. The weight coefficients are computed on the cell face centres (index F ), since this is the natural location of the required surface normals, yielding: 1 · m F = -4 The surface average is then calculated as 1 q = --------------------------------------wFqF , w F cell face centres cell face centres four corners ∑ q corner . (11-6) ∑ ∑ (11-7) · where w F = m F or A F . The stencil shown in Figure 11.4.2-16 illustrates that the contributions from the cell face centre at a boundary contain some influence from the lateral dummy cells (weight 1/4). 11-4.3 Azimuthal Averaged Variables Exact azimuthal-averaging for general configurations requires a mechanism that is independent of the computational grid. First a meridional mesh must be defined to support the azimuthal-averaged solution. Secondly, the latter must be extracted from the 3D computational mesh. The 2D mesh is provided by the meridional projection of any suitable contiguous set of sub-surfaces contained in FINE™ 11-21 Output Theory the volumetric mesh. The domains and indices defining these sub-surfaces are provided in the input file. Choosing sub-surfaces of the actual 3D mesh ensures that the resolution of the meridional mesh is commensurate with the accuracy of the numerical solution. Starting from each point ( r, z ) of the meridional mesh, the solution is defined by the primitive variables ρ, w r, w θ, w z, p averaged along a circular arc passing through that point, 1 u = ------------- wu dθ w dθ ∫ ∫ (11-8) where u denotes the azimuthal-average of the generic variable u and where ρV m 1 for mass averaging (11-9) w = 2 2 Vm = v r + v z is the meridional velocity. Either mass or area averaging can be requested, but the same type of averaging will be used for all the primitive variables. The integrals in Eq. 11-8 are approximated by trapezoidal sums. Practically, the r, z -constant line along which the integration proceeds may be composed of k fragments of n ( j ) data points, j = 1, ...,k , so that Eq. 11-8 is evaluated as: k n(j) ij u ij with Σ i = 1 b ij a ij = b ij -----------------------------k n(j) Σ j = 1 Σ i = 1 b ij and 2w i θ 2 – θ 1 w i θi + 1 – θi – 1 2w i θ n – θ n – 1 i = 1 i = 2, ..., n-1 i = n ⎩ ⎪ ⎨ ⎪ ⎧ n ( j) bi = All requested variables are derived, if possible, from the azimuthal-averaged primitive variables. Those variables that can not be computed from the azimuthal-averaged primitive variables are computed first. The fact that they are computed by the same routines that are used for generating 3D CFView™ output ensures consistency. The suction and pressure side of the blades can be superimposed on the azimuthal averaged view. For meshes that do not lie on surfaces of revolution the accuracy of the averaged solution is decreased close to curved boundaries (see Figure 11.4.3-17). Although all boundary grid points lie on the same surface of revolution, the straight line segments forming the cell edges do not. The r, z -constant ray associated with point 1 will therefore miss some cell faces or pick values from the inside instead of boundary values. In the worst case it will not encounter any cell faces at all. Strong curvature and cells with high aspect ratio increase the inaccuracy. This problem has been addressed in two ways. First, meridional grid points encountering fewer than two cell faces are set to zero (a message printed to the screen indicates for how many points this 11-22 ⎩ ⎨ ⎧ for area averaging u = ∑ ∑a j = 1i = 1 , (11-10) (11-11) (11-12) FINE™ Theory Output was necessary). Secondly, the possibility is provided to shrink the meridional mesh by a small amount to avoid the outermost regions of the volumetric mesh as shown in Figure 11.4.3-18. Independent shrink factors k can be specified in the streamwise and spanwise directions using the expert parameter MERMAR. Figure 11.4.3-18 illustrates the global effect. Each mesh line is shrank individually by uniformly contracting towards its centre. The grid points thereby slide along the segments of the original line (dashed line in Figure 11.4.3-18). 2 a) 1 1 b) 2 along circular arcs at curved boundary (light lines = meridional mesh supporting the azimuthal-averaged solution, heavy lines = an arbitrary cell face of the computational mesh), situation (a) before shrinking and (b) after shrinking. FIGURE 11.4.3-17Azimuthal-averaging h kh/2 a b FIGURE 11.4.3-18: Shrinking of the meridional mesh, schematic illustration of (a) the global effect and (b) the modification applied to each mesh line (dashed line and circles = original line, solid line and squares = shrank line, C = centre point of the original line) FINE™ 11-23 Output Theory 11-4.4 Global Performance Output The surface integrals are approximated by rectangular sums: for any vector quantity Q and scalar quantity q , surface1/2 ∫ Q dS = cell faces ∑ QB SB surface1/ 2 ∫ qd S = cell faces ∑ qB SB (11-13) The index B indicates a boundary cell face centre value, obtained by averaging the coordinates ( r = x, y, z ) of the four corners: 4 1 r B = -4 ∑r i=1 i (11-14) and the solution ( U = ρ, w x, w y, w z, p ) in the first inner (index 1) and first outer cell (index 0): 1 U B = -- [ U 0 + U 1 ] . 2 (11-15) All variables except flow angles are first computed locally from this consistent representation of solution and geometry and then summed, multiplied by the appropriate weight factor · m B = ( ρWS ) B or A B = S B . Averages are calculated for the following variables: . VS w x, w y, w z, w r, w t, v x, v y, v z, v r, v t, W , V , ------, p, ρ, p t, rel, p t, abs, p t, rot, T t, rel, T t, abs, T t, rot S Static pressure is area averaged, all other variables are mass averaged. Explicitly, q representing any of the enumerated scalars (other than p ) and q its average: 1 q = --·m cell faces ∑ · mB qB 1 p = -A cell faces ∑ AB pB . (11-16) · The mass flow m is obtained from Eq. 11-13 with Q = ρW , the area A with q = 1 . The values of p t, rel, p t, abs, T t, rel, T t, abs are also computed from p, ρ and the averaged velocity components to be compared with the directly averaged values. 11-24 FINE™ CHAPTER 12:Blade to Blade Module 12-1 Overview This chapter describes the quasi-three-dimensional Blade-to-Blade Module for turbomachinery cascade analysis. The module is fully automatic and can be used (and acquired) independently from the other NUMECA tools. Furthermore, an additional module is associated with the present one, called FINE™/Design2D, which permits to redesign the blades for an improved pressure distribution on the blade surfaces and is presented in Chapter 13. The module assumes that the flow in the turbomachinery cascade remains on an axisymmetric streamsurface, whose shape and thickness can either be provided by the user, or automatically constructed by the module (using the given hub and shroud walls). The geometrical input data required from the user can be: 1. The streamsurface and the blade section on this last surface or, 2. The whole three-dimensional blade shape and the hub and shroud walls. The module comprises a fully automatic mesh generator (which is able to treat any type of meridional configuration) and a customised version of NUMECA’s turbulent Navier-Stokes flow solver. In the next section the interface is described in detail including advice for use of the Blade-to-Blade Module. The theoretical background for the mesh generator and the flow solver is described in section 12-4. Finally, the Blade-to-Blade Module requires geometrical data files and generates output, which are detailed in section 12-5. The Design 2D module can not be used with: • other turbulence models than Baldwin Lomax turbulence model, • upwind scheme, • real gas, • unsteady computations, • azimuthal averaged output. FINE™ 12-1 Blade to Blade Module Blade-to-Blade in the FINE™ Interface 12-2 Blade-to-Blade in the FINE™ Interface The Blade-to-Blade Module is proposed under the FINE™/Design 2D interface through the menu Modules/Design 2D., which permits a very rapid, easy and interactive use of the solver. All the parameters can be selected interactively through this user interface, which automatically creates the input files and permits to launch the solver. A monitoring tool, called the MonitorTurbo, can be launched to verify the convergence and results during and after the computation. It permits to observe the evolution of the convergence history, of the pressure distribution along the blade surface, and of the blade geometry. The results can be analysed with the NUMECA CFView™ post-processing software, whose connection with the Blade-to-Blade Module is automatically provided. The geometrical data are specified in ASCII input files, whereas the definition of the flow solver parameters and of the boundary conditions are specified via the interface. This section describes the creation of the solver input files using the interactive menus included in the FINE™/Design2D interface. Further details concerning the input and output files are provided in section 12-5. 12-2.1 Start New or Open existing Blade-to-Blade Computation When starting the interface a Project Selection window allows to Create a New Project or to Open an Existing Project. To create a new Blade-to-Blade project: 1. 2. 3. 4. click on the button Create a New Project. Browse to the directory in which the new project directory needs to be created and enter a name for the project. Close the Grid File Selection window since no grid file is associated to a Design 2D project. Switch to the Blade-to-Blade module through the menu Modules/Design 2D. When an existing Blade-to-Blade project should be opened click on the button Open an Existing Project in the Project Selection window and select the project in the File Chooser window. The most recently used projects can also be selected from the list of recent projects. If the selected project was saved in the Design 2D module, the FINE™ interface is automatically switched to this module showing the interface as in Figure 12.2.1-1. It is not possible to have Blade-to-Blade and three-dimensional computations in one project. A project is either a Blade-to-Blade project or a FINE™/Turbo project. The type of the project is determined by the module in which it is saved. The FINE™/Design 2D interface is the same as the FINE™/Turbo interface and contains a menu bar, an icon bar, a computations definition and a parameters area. The menu bar is the same in both modules, except for the Modules menu that allows to switch to the other available modules. The icon bar in the Design 2D module contains only the icons applicable for a 2D computation. The list of Parameters pages on the left of the interface is updated according to a 2D computation. Most of the pages are the same as in a FINE™/Turbo project. The only differences are in: • the Flow Model page: the Design 2D module can not be used in unsteady, • the Boundary Conditions page as described in section 12-2.3, • the Blade-to-blade Data pages as described in section 12-2.2, • the Initial Solution page as described in section 12-2.5. 12-2 FINE™ Blade-to-Blade in the FINE™ Interface Blade to Blade Module FIGURE 12.2.1-1 Design 2D in the FINE™ interface 12-2.2 Blade-to-Blade Data Three specific menus appear in the Blade-to-blade Data page: • Blade Geometry, see section 12-2.2.1, • Mesh Generation Parameters, • Inverse Design: parameters that are only used in 2D design but not in blade-to-blade analysis. Inverse design is described in Chapter 13. The blade geometry and the axisymmetric streamsurface (or hub and shroud walls) are specified under the form of a series of data points given in ASCII files, whose structure is described in section 12-5. All geometrical data has to be given in the same length unit (which can be chosen arbitrarily). The chosen length unit is defined under the Blade geometry thumbnail on the Blade Geometry page. 12-2.2.1 Blade Geometry Definition Three types of geometrical input data are possible: - 2D type: This first option is valid only for purely axial cases, in which the stream surface is a cylinder (constant radius). The blade geometry is then given on the cascade plane (cylinder developed to generate the cascade). - Q3D type (quasi 3-dimensional): The axisymmetric stream surface is given (including its thickness), and the blade geometry is specified on the given surface. - 3D type (from hub to shroud): The whole 3D blade geometry is given under the form of a series of blade sections (minimum 2, ordered from the hub to the shroud). The hub and the shroud walls are also specified. The stream surface can either be specified by the user (the lower and the upper axisymmetric surfaces have to be specified), or can be automatically constructed by the solver (geometrical division). In the latter case, the user only has to specify the spanwise position of the stream surface and its relative thickness. FINE™ 12-3 Blade to Blade Module Blade-to-Blade in the FINE™ Interface - 3D type (from .geomTurbo file): The whole 3D blade geometry is given under the form of a geometry turbo file containing the hub, shroud and blade definition (more details in AutoGrid User Manual). The stream surface can either be specified by the user (the lower and the upper axisymmetric surfaces have to be specified), or can be automatically constructed by the solver (geometrical division). In the latter case, the user only has to specify the spanwise position of the stream surface and its relative thickness. a) Streamsurface Data Figure 12.2.2-2 shows the Parameter area for entering Stream surface data. The following stream surface data files have to be specified, depending on the type of input data: • 2D or Q3D types: stream surface definition file name, • 3D case: hub and shroud file names or .geomTurbo file name. When the 3D type of input data is selected additional parameters have to be defined: • - Geometrical division or streamtube provided by the user. • - If geometrical division: spanwise position between 0 (hub) and 1 (shroud). • - If streamtube provided: lower and upper surfaces file names (2 lines). 2D&Q3D: 3D: FIGURE 12.2.2-2 Streamsurface parameters area In both cases the module automatically calculates the intersection of the 3D blade with the considered stream surface. 12-4 FINE™ Blade-to-Blade in the FINE™ Interface Blade to Blade Module In a 3D case with geometrical division, the streamtube height defines the thickness of the streamtube (the recommended value is 1%). In a 2D, Q3D or 3D case with streamtube provided, the blockage ratio permits to scale the streamtube thickness distribution. For all types of input data the number of points along meridional stream surfaces has to be specified. This input data is the number of points that the module will generate along the streamsurface in order to obtain an accurate calculation of the meridional coordinate (default: 300). b) Blade Geometry Data Selecting the Blade geometry thumbnail allows to define the characteristics of the blades and the files where the data is stored: • Blade geometry file names. — 2D or Q3D: suction and pressure side file names, — 3D case (from hub to shroud): number of spanwise section and for each section, suction and pressure sides file names. — 3D case (from .geomTurbo file): the whole 3D blade geometry is given under the form of a geometry turbo file (more details in AutoGrid User Manual). • Blunt leading edge: if active, indicates that the leading edge is blunt. • Blunt trailing edge: if active, indicates that the trailing edge is blunt. • Splitter blades: — If the "splitter" button is selected, the blade geometry input file names have to be given for the splitter blades. In a 3D case (from hub to shroud), the number of spanwise sections should be identical for the main and splitter blades, and is not repeated here. • Length unit: The user can define the geometrical data in any length unit, and simply has to define by means of this scale the ratio between the meters and the chosen unit length (if the input is in millimetres, the ratio must be 0.001). All the geometrical data must be given in the same unit length chosen by the user. • Number of blades or pitch distance. In a 2D input type, this input is the pitch distance (in the unit length chosen by the user), whereas in a Q3D or 3D case (from hub to shroud), it must be the number of blades (Figure 12.2.2-3). 3D FIGURE 12.2.2-3 Blade geometry information page for 3D cases (from hub to shroud) FINE™ 12-5 Blade to Blade Module Blade-to-Blade in the FINE™ Interface c) Blade Data Edition Selecting the Blade data edition thumbnail permits to edit the position of the leading and/or trailing edge among the data points provided by the user in the input files (see Figure 12.2.2-4). For both leading and trailing edges the user has to specify if the leading or trailing edge is on the suction side or pressure side, and to give also its position (starting from the initial position). Therefore a value of 1 will not modify the edge position. In a 2D or Q3D case this operation is performed on the data points provided by the user, whereas in a 3D case it is performed on the blade points resulting from the 3D interpolation process. In any case the data points can be visualised by plotting the "projectname.b2b.geoini" file using the MonitorTurbo. The way to visualise the data points in order to decide whether the position of the edges is acceptable is to launch the analysis module and to visualise the ".geoini" file. FIGURE 12.2.2-4 Blade data edition thumbnail 12-2.2.2 Mesh Generation Parameters Page The different Mesh generation parameters (as shown in Figure 12.2.2-5) do not necessarily have to be modified by the user. They have been set to default values, which have shown to be efficient in many cases. The available Mesh generation parameters are: • H(periodic)- or I(non periodic) -type mesh: The user defines if the upstream and/or the downstream region should be inclined (non periodic, which permits to improve the orthogonality of the mesh cells to the flow) or not. • Generation mode: fully automatic or semi-automatic: — In the fully automatic mode, the user only has to specify the number of points along the suction side. The number of points in the other segments are then calculated in order to ensure the smoothness of the mesh (the number of cells in each patch is always a multiple of 8, so that 4 multigrid levels are available for the solver). — In the semi-automatic mode, the user decides to specify the inclination angles of the upstream/downstream boundaries (radians), as well as the number of cells in each of the segments of the mesh. The number of input data depends on the number of segments, which can be 3 if the upstream/downstream boundaries are not inclined, 4 if one of them is inclined, and 5 if both are inclined. The number of cells in each segment should be chosen so that they are always a multiple of 8 (four multigrid levels are available for the flow solver). In a case with splitters the number of segments is 4 or 5 (if the downstream periodic boundaries are non periodic), and the numbers of cells should be specified for both blade passages. 12-6 FINE™ Blade-to-Blade in the FINE™ Interface Blade to Blade Module . FIGURE 12.2.2-5 Mesh generation parameters information page • Number of points in the pitchwise direction: The number of cells should better be a multiple of 8, so that four multigrid levels are available. • Periodic boundaries type: the user defines if the periodic lines should be straight or curved. In the default configuration the periodic lines are curved. • Five thumbnails give access to parameters to influence the mesh quality and points distribution as described in the next paragraphs. a) Inlet The inlet location of the mesh is imposed on the hub and the shroud. The position is specified in meridional coordinates (Z, R) or in spanwise coordinate (S). b) Outlet The outlet location of the mesh is imposed on the hub and the shroud. The position is specified in meridional coordinates (Z, R) or in spanwise coordinate (S). c) Clustering The clustering coefficient in streamwise direction can be imposed from 0.0 to 1.0. A value of 1.0 gives a uniform distribution, whereas a 0.0 value concentrates all the points at the edges. The second input defines if an Euler (no clustering in pitchwise direction) or a Navier-Stokes mesh (with clustering to capture the boundary layer) should be generated. For a Navier-Stokes mesh the following parameters should be specified: • Size of the first mesh cell in the pitchwise direction (in meters). • Number of constantly spaced cells in the pitchwise direction. FINE™ 12-7 Blade to Blade Module Blade-to-Blade in the FINE™ Interface • Constant or decreasing clustering from the blade edges to the inflow/outflow boundaries. d) Smoothing An elliptic smoother can be used in order to improve the quality of the mesh. In case the smoothing is selected, the user has to specify if the smoothing should be performed with or without the control of the clustering along the walls, and the number of smoothing steps (sweeps) to be performed (see Figure 12.2.2-6). FIGURE 12.2.2-6 Smoothing page of the Mesh generation parameters page e) Local Pre-smoothing A local pre-smoothing can be performed in the leading and trailing edge regions, which can be appropriate in cases of thick rounded leading and/or trailing edges (Figure 12.2.2-7). FIGURE 12.2.2-7 Local pre-smoothing page of the Mesh generation parameters page 12-2.2.3 Inverse Design Menu This menu concerns the inverse design module. The parameters included in this menu do not have to be specified when performing a flow analysis. A description on the Inverse design module is provided in Chapter 13. 12-2.3 Boundary Conditions The Boundary Conditions page allows to define the boundary conditions at the inlet and the outlet as well as the rotational speed. The Rotational speed must be given in RPM (revolutions per minute, positive if oriented in the θdirection, see Figure 12.5.1-12 on page 15) 12-2.3.1 Inlet Boundary Conditions Eight inlet boundary conditions are available: • Direction of absolute velocity (radians) + absolute total conditions (Pa, K). • Direction of relative velocity (radians) + relative total conditions (Pa, K). • Absolute Vθ velocity component (m/s) + absolute total conditions (Pa, K). • Relative Wθ velocity component (m/s) + relative total conditions (Pa, K). 12-8 FINE™ Blade-to-Blade in the FINE™ Interface Blade to Blade Module • Mass flow (kg/s) + direction of absolute velocity (radians) + static temperature (K). • Mass flow (kg/s) + direction of relative velocity (radians) + static temperature (K). • Mass flow (kg/s) + absolute Vθ velocity component (m/s) + static temperature (K). • Mass flow (kg/s) + relative Wθ velocity component (m/s) + static temperature (K). Selecting one of these options activates a submenu in which the user can set the inlet values. An example corresponding to a ’Direction of absolute velocity + absolute total conditions’ is shown in figure 12.2.3-8. FIGURE 12.2.3-8 Inlet boundary conditions information page 12-2.3.2 Outlet Boundary Conditions Three outlet boundary conditions are available at the outlet (Figure 12.2.3-9): • exit static pressure imposed (Pa), • mass flow imposed (kg/s) (+ exit static pressure required to initiate the calculation), • supersonic exit (exit static pressure required to initiate the calculation). FIGURE 12.2.3-9 Outlet boundary conditions information page Both zero and first order extrapolation techniques are available, and can be selected in the Expert mode (the default technique is the zero-order one). FINE™ 12-9 Blade to Blade Module Blade-to-Blade in the FINE™ Interface It should be mentioned that the inverse design method is more stable when the mass flow is explicitly imposed as a boundary condition. Therefore it is recommended to impose the mass flow during the analysis also. The recommended strategies are therefore the one imposing the mass flow at the inlet and the pressure at the outlet, or the one imposing the total conditions at the inlet and the mass flow at the outlet. 12-2.4 Numerical Model In general the default values for the Numerical Model parameters are appropriate. In the blade-to-blade module it is not possible to perform the calculations on a coarser mesh level as it is the case with 3D projects. 12-2.5 Initial Solution Menu A turbomachinery-oriented initial solution construction strategy is automatically used, which requires an approximation of the inlet static pressure to be provided by the user or an Initial solution file provided by the user (Figure 12.2.5-10) FIGURE 12.2.5-10 Initial solution page 12-2.6 Output Parameters This menu permits to select the different flow variables to be included in the output. The module automatically creates the outputs for a 3D and a 2D (in the m,θ plane) CFView™ project. Further comments about this menu are provided in section 12-5.2. 12-2.7 Control Variables Page On the Control Variables page the user defines if a flow analysis or an inverse design should be performed (Figure 12.2.7-11). All other parameters on this page are the same as for a FINE™/Turbo computation as described in Chapter 15. FIGURE 12.2.7-11 Run type page of the information area 12-10 FINE™ Expert Parameters Blade to Blade Module 12-2.8 Launch Blade-to-Blade Flow Analysis Once the ".run" has been correctly created through the menu File/Save Run Files, a flow analysis can be started, by pressing the Start button in the Solver menu. A restart from a previous calculation is also possible by pressing the Start button in the Solver menu and selecting an initial solution file in the page Initial Solution. As calculations on coarser grid levels are not possible, a restart can never be performed with the full-multigrid option. 12-3 Expert Parameters A series of expert parameters can be specified in Expert Mode on the Control Variables page.: ITFRZ: the number of iterations after which the turbulent viscosity field is frozen. It is recommended to use this option (ITFRZ=200 for instance) in order to eliminate the spurious residual oscillations due to the turbulent quantities fluctuations. IATFRZ: this switch is related to the previous one. It should usually be set to 1 (default value). However in the case of a restart and if the turbulent viscosity field has been frozen in the previous calculation, this switch should be to 2, so that the previous turbulent viscosity field is read from the previous calculation and kept unchanged. In the case the initial solution has been obtained with a frozen turbulent viscosity field (using the ITFRZ expert parameter), the parameter IATFRZ should be set to 2 in order to read the turbulent viscosity field from a file and to keep this field unchanged. 12-4 Theory The main characteristics of the mesh generation tool and of the blade-to-blade flow solver are provided in this section. 12-4.1 Mesh Generator The mesh generator is a fully automatic tool customised for blade-to-blade applications, generating H(periodic)- or I(non periodic)-type grids (see the AutoGrid manual) starting from a minimum amount of information from the user. Contrary to many quasi-3D methods that solve the flow equations on a 2D mesh constructed on the axisymmetric streamsurface, the mesh generated here is a 3D-mesh with only 1 cell in the spanwise direction. This approach permits to use a 3D flow solver without major adaptation. Another advantage is that the effects of the eventual streamtube thickness variations are then implicitly taken into account, and do no longer have to be introduced under the form of additional source terms in the equations. The main characteristics of the generator are the following ones: • can be applied to any type of meridional configuration (axial, radial and mixed flow machines, return channels...), • treatment of blunt leading and trailing edges, FINE™ 12-11 Blade to Blade Module Theory • splitters can be modelled, • generation of H- and I-type (H non periodic) meshes, • possibility to have an inclined mesh (non periodic) in both upstream and downstream regions, or only in the upstream or downstream region, • general mesh generation process, which allows to consider the real leading and trailing edges of the blade as the edges of the mesh, whereas in a classical H-mesh generator the edges (the points where the upstream/downstream boundaries intersect with the blade) are respectively the points located at the minimum and maximum x-position., • fully automatic tool: the only information required from the user is the number of points along the suction side and along the pitchwise direction. The number of points in the different segments of the mesh as well as the inclination angles of the upstream and downstream regions are calculated automatically. 12-4.2 Flow Solver The flow solver included in the blade-to-blade module is a customised version of the EURANUS flow solver, with restricted functionalities in order to optimize the efficiency. The module can be applied to compressible and incompressible flows. The space discretization of the governing flow equations is based on a cell-centered control volume approach. To compute the various fluxes, a central scheme has been adopted, using Jameson type dissipation with 2nd and 4th order derivatives of the conservative variables. Turbulence of the flow is accounted for by means of the Baldwin-Lomax model. The system of flow equations is solved explicitly using the 4-stage Runge-Kutta method. To accelerate the flow solver convergence, various strategies are used: • multigrid approach (V-cycle), • full multigrid strategy, to initiate the resolution process, • local time stepping, • implicit residual smoothing. A turbomachinery-oriented initial solution is automatically constructed to provide a fast and robust calculation. A particular boundary condition is applied along the upper and lower sides of the axisymmetric streamtube, in order to force the flow to follow the streamsurface. For this purpose a spanwise pressure gradient is computed according to: Vθ Vm ∂p ----- = ρ ----- cos δ – ρ ------ , r Rc ∂n 2 2 (12-1) where n is the spanwise direction, Vm and Vθ are respectively the meridional and tangential components of the absolute velocity, and δ and Rc are respectively the slope and the curvature radius of the meridional trace of the streamsurface. A procedure is applied to the numerical scheme in order to force the flow to be aligned to the streamsurface. This procedure eliminates the momentum residual in the direction normal to the streamsurface. In case of multigrid the same procedure is applied to the flow solution after restriction and prolongation of the solution. 12-12 FINE™ File Formats used by Blade-to-Blade Module Blade to Blade Module 12-5 File Formats used by Blade-to-Blade Module 12-5.1 Input Files The input files required for running a blade-to-blade study can be split into 3 categories: • The geometrical input files, defining the blade geometry. • The solver input file (.run), where the solver parameters and the fluid and flow conditions are defined. • The inverse design input files that allow to define an inverse problem. The geometrical input files have to be created by the user, and are compatible with the AutoGrid input file formats. The solver and inverse design input files are automatically created by the FINE™/Design 2D environment, the user has to set the parameters and flow conditions in the FINE™ interface. The next section describes the geometrical input files. 12-5.1.1 Geometrical Input Files The blade geometry and the axisymmetric streamsurface (or hub and shroud walls) are specified under the form of a series of data points given in ASCII files. Three types of geometrical input data are possible: • 2D type: This first option is valid only for purely axial cases, in which the streamsurface is a cylinder (constant radius). The blade geometry is then given on the cascade plane (cylinder developed to generate the cascade). • Q3D type: The axisymmetric streamsurface is given (including its thickness), and the blade geometry is specified on the given surface. • - 3D type (from hub to shroud): The whole 3D blade geometry is given under the form of a series of blade sections (minimum 2, ordered from the hub to the shroud). The hub and the shroud walls are also specified. The streamsurface can either be specified by the user (the lower and the upper axisymmetric surfaces have to be specified), or can be automatically constructed by the solver (geometrical division). In the latter case, the user only has to specify the spanwise position of the streamsurface and its relative thickness. • 3D type (from .geomTurbo file): The whole 3D blade geometry is given under the form of a geometry turbo file containing the hub, shroud and blade definition (more details in AutoGrid User Manual). The stream surface can either be specified by the user (the lower and the upper axisymmetric surfaces have to be specified), or can be automatically constructed by the solver (geometrical division). In the latter case, the user only has to specify the spanwise position of the stream surface and its relative thickness. All geometrical data has to be given in the same length unit (which can be chosen arbitrarily). a) Streamsurface Data: For the 2D and Q3D types, one ASCII file defining the surface and its thickness is required. For the 3D type (form hub to shroud), 2 files are required to define the hub and shroud walls separately and for the 3D type (from .geomTurbo), 1 file is required to define the hub, shroud and the blade. In case the user wants to specify the streamsurface, 2 additional files are required to define the lower and upper axisymmetric surfaces of the streamtube. The structure of the streamsurface data file is the following: FINE™ 12-13 Blade to Blade Module File Formats used by Blade-to-Blade Module — line 1: title of the input file — line 2: coordinate system: ZRB (for 2D and Q3D types) ZR, RZ or XYZ (for 3D type) — — — — line 3: number of data points N lines 4 to 3+N: data points in 2 or 3 columns (ordered from the inlet to the outlet) line 4+N: character line (facultative) line 5+N: Zin, Zout, Rin, Rout, specifying the inlet/outlet positions of the mesh (facultative). (X,Y,Z) are the Cartesian coordinates (Z being the axial coordinate along the axis of rotation), R is the radius, and B is the streamtube thickness. The inlet/outlet positions of the mesh can either be specified: • in the above streamsurface data file(s) (lines 4+N and 5+N) • through the FINE™ interface through the thumbnails Inlet and Outlet in the Mesh Generation Parameters page. In both cases the inlet/outlet positions along a given surface are specified by four real data, i.e. Zin, Zout, Rin, Rout. No extrapolation is allowed, which implies that these positions should be located inside the meridional curve formed by the data points. In a 2D or Q3D case, one single meridional position is required for both inlet and outlet boundaries, which are applied to the given streamsurface. These positions are either specified in the streamsurface data file or through the 4 first real data contained in the expert parameter B2BLIM. In a 3D case, two positions should be specified for the inlet/outlet positions. They are applied along the hub and shroud walls (geometrical creation of the streamtube), or along the upper/lower surfaces of the streamtube (streamtube specified by the user). These positions can be given in the 2 corresponding input files, or through the thumbnails Inlet and Outlet in the Mesh Generation Parameters page. b) Blade Geometry Data The blade geometry is specified by a series of sections (1 for 2D and Q3D cases, minimum 2 for a 3D case) or by a ".geomTurbo" file. When the blade is defined by sections, each section comprises 2 input files, respectively for the suction and the pressure sides. The structure of the blade geometry data file is the following: — line 1: title of the input file — line 2: coordinate system: ZTR, ZTHR, RTZ, RTHZ, YXZ, ZXY or XYZ — line 3: number of data points N — lines 4 to 3+N: data points in 2 or 3 columns (ordered from the leading to the trailing edge) (X,Y,Z) are the Cartesian coordinates (Z being the axial coordinate along the axis of rotation), R is the radius, TH is the circumferential position (in radians) and T is the circumferential coordinate multiplied by the radius (Rθ). 12-14 FINE™ File Formats used by Blade-to-Blade Module Blade to Blade Module θ W β>0 α<0 V z FIGURE 12.5.1-12 Coordinate RPM (<0) system and reference for flow angles and speed of rotation In a 2D case, if the ZTR coordinate system is used, the radius does not have to be specified in the blade geometry input file. The number of columns can be 2 or 3, the third column being not read by the solver (the radius is automatically set to the value given in the streamsurface data input file). The suction side is by convention located above the pressure side in the θ-direction Figure 12.5.1-12. It does not necessarily have to be the physical suction side. 12-5.2 Output Files Several output files are generated by the blade-to-blade module: 12-5.2.1 Geometry Files a) ’project_computationname.geoini’ and ’project_computationname.geo’ These files contain the blade shape in the (m,θ) plane. The ’.geoini’ file contains the initial blade shape as given in the input files (or resulting from the 3D interpolation process in a 3D case), whereas the ’.geo’ file contains the blade discretization points used in the computation. These files can be read and plotted by the NUMECA MonitorTurbo (Blade profile menu). b) ’project_computationname.merdat’, ’project_computationname.mer.ori’ and ’project_computationname.mer’ These files contain respectively the hub and shroud walls and the streamtube projection onto the meridional plane. The ’.merdat’ file contains the hub and shroud walls (3D case only), whereas the ’.mer’ and ’.mer.ori’ files contain the streamtube. These files can be read and plotted by the NUMECA MonitorTurbo (Blade profile menu). c) ’project_computationname.ps.ori’ & ’project_computationname.ss.ori’ These files contain respectively the pressure side and the suction side of the blade. FINE™ 12-15 Blade to Blade Module File Formats used by Blade-to-Blade Module d) ’project_computationname.split.ps.ori’ & ’project_computationname.split.ss.ori’ (if splitter blades) These files contain respectively the pressure side and the suction side of the splitter blade. 12-5.2.2 Quantity Files a) ’project_computationname.cgns’ This file contains the results of the calculation, i.e. the five flow variables (density, x-y-z components of the relative velocity and the static pressure) at all the mesh cell centers (including the dummy cells generated by the boundary conditions). It also contains all output variables to be displayed by CFView™. b) ’project_computationname.mf’ This file is a summary file containing the averaged flow quantities at the inlet and the outlet boundaries. c) ’project_computationname.mfedge’ This file is a summary file containing the averaged flow quantities at the leading and trailing edge planes. d) ’project_computationname.2d.cfv’ & ’project_computationname.3d.cfv’ The blade-to-blade module automatically creates all the files required by the NUMECA CFView™ post-processing tool. Two projects are created, the first one being named ’***.3d.cfv’, allowing a 3D visualization of the case, the second one being named ’***.2d.cfv’, allowing a 2D visualization in the (m,θ) plane. e) ’project_computationname.velini’ & ’project_computationname.vel’ These files contain the isentropic Mach number and the pressure coefficient distributions along the blade surfaces. The two quantities are plotted along the curvilinear abscissae measured along the blade surface (non-dimensionalized by the blade chord). The isentropic Mach number is calculated (for compressible flows only) using the inlet relative total temperature and pressure, which are not necessarily imposed (depending on the choice of the inlet boundary condition). In case the total conditions are not imposed, the values are the ones resulting from the calculation (average along the inlet boundary). γ–1 ---------γ where p is the local static pressure, and p0 is the local relative total pressure calculated assuming a constant rothalpy and a constant entropy in the field. The pressure coefficient is defined by: p – p exit Cp = ------------------ , p exit where pexit is the exit static pressure, and p is the local static pressure. (12-3) 12-16 ⎠ ⎞ Mis = 2 ---------γ–1 p0 ---p –1 , ⎠ ⎟ ⎟ ⎞ ⎝ ⎝⎜ ⎛⎜ ⎛ (12-2) FINE™ File Formats used by Blade-to-Blade Module Blade to Blade Module These files can be read and plotted by the NUMECA MonitorTurbo (Loading diagram menu). The ’.velini’ file contains the initial distributions, whereas the ’.vel’ contains the actual ones, and is iteratively updated during the resolution process. f) ’project_computationname.split.velini’ & ’project_computationname.split.vel’ (if splitter blades) These files contain the isentropic Mach number and the pressure coefficient distributions along the splitter blades. These files can be read and plotted by the NUMECA MonitorTurbo (Loading diagram menu). g) The ’project_computationname.loadini’ & ’project_computationname.load’ Provided that the parameter ISQUEL specified in the ’.run’ file is different from 0, these files are automatically generated, and contain the distributions of the suction-to-pressure side Mach number and pressure coefficient difference and average. These distributions can be superimposed to the suction and pressure side distributions. These files can be read and plotted by the NUMECA MonitorTurbo provided with the FINE™ user interface (Loading diagram menu). The ’.loadini’ file contains the initial distributions, whereas the ’.load’ contains the actual ones, and is iteratively updated during the resolution process. h) ’project_computationname.split.loadini’ & ’project_computationname.split.load’ (if splitter blades) These files contain the same results as the ’.load’ and ’.loadini’ files along the splitter blades. These files can be read and plotted by the NUMECA MonitorTurbo provided with the FINE™ user interface (Loading diagram menu). 12-5.2.3 Numerical Control Files a) ’project_computationname.log’ & project_computationname.std’ These files contain all the informations written by the solver during its execution. When the solver fails for any accidental reason, the explanation can usually be found in these files. b) ’project_computationname.res’ This file contains the evolution of the mean and maximum residuals and of the inlet and outlet mass flows. This file can be read and plotted by the NUMECA MonitorTurbo (Convergence history menu). FINE™ 12-17 Blade to Blade Module File Formats used by Blade-to-Blade Module 12-18 FINE™ CHAPTER 13:Design 2D Module 13-1 Overview This chapter describes the new quasi-three-dimensional FINE™/Design 2D Module for turbomachinery cascade inverse design. This module is associated with the FINE™/Design 2D Blade-toBlade module presented in Chapter 12. In addition to the mesh generator and the flow solver, the FINE™/Design 2D module includes one of the latest inverse methods for the redesign of the blades with improved performance. Such a method permits to redesign the blade shape for a target pressure distribution along the blade surfaces. The use of the design method requires a license for bladeto-blade simulation. The FINE™/Design 2D module can be used (and acquired) independently from the other NUMECA tools. In the near future NUMECA intends to extend the FINE™/Design 2D environment to other types of applications and to other design techniques. This first version is limited to the inverse design of turbomachinery cascades, and has therefore been integrated with the Blade-to-Blade method in the FINE™/Design 2D user environment. Both analysis and design modules are based on the assumption that the flow in the turbomachinery cascade remains on an axisymmetric streamsurface. The geometrical inputs required from the user to perform an inverse design are not different from the ones required to perform an analysis (as described in Chapter 12). For more information about the Blade-to-Blade method, see the description provided in the Chapter 12. In the next section the interface is described in detail including advice for use of the inverse design method. The theoretical background for the inverse method is described in section 13-3. Finally, the Design 2D Module requires geometrical data files and generates output as detailed in section 13-4. FINE™ 13-1 Design 2D Module Inverse Design in the FINE™ Interface 13-2 Inverse Design in the FINE™ Interface The Blade Design module is proposed under the new NUMECA FINE™/Design 2D environment presented in Chapter 12, which permits a very rapid, easy and interactive use of the solvers. All the parameters can be selected interactively by means of this user interface, which automatically creates the input files and permits to launch the analysis and inverse solvers. A graphical control software, called MonitorTurbo, is provided. It permits to observe the evolution of the convergence history, of the pressure distribution along the blade surface, and of the blade geometry (case of an inverse design). It also permits to create the target pressure distribution interactively. The results can be analysed with the NUMECA CFView™ post-processing software, whose connection with the blade-to-blade module is automatically provided. The geometrical data are specified in ASCII input files, whereas the definition of the flow solver parameters and of the boundary conditions are specified via the interface. This section describes the creation of the inverse design input files using the interactive menus provided in FINE™/Design 2D. Further details concerning the input and output files are provided in section 13-4. The next sections provide information concerning: • The starting of a new or an existing blade-to-blade project. • The creation of the solver input files required for a flow analysis. • The launching of a blade-to-blade flow analysis. 13-2.1 Start New or Open Existing Design 2D Project To start the FINE™/Design 2D module from the FINE™ interface select the menu item Modules/ Design 2D. When launching the FINE™ interface a Project Selection window allows to Create a New Project or to Open an Existing Project. To create a new Blade-to-Blade project: 1. 2. 3. 4. Click on the button Create a New Project. Browse to the directory in which the new project directory needs to be created and enter a name for the project. Close the Grid File Selection window since no grid file is associated to a Design 2D project. Switch to the Design 2D module through the menu Modules/Design 2D. When an existing Design 2D project should be opened click on the button Open an Existing Project in the Project Selection window and select the project in the File Chooser window. The most recently used projects can also be selected from the list of recent projects. If the selected project was saved in the Design 2D module, the FINE™ interface is automatically switched to this module showing the interface as in Figure 12.2.1-1. It is not possible to have Design 2D and three-dimensional computations in one project. A project is either a FINE™/Design 2D project or a FINE™/Turbo project. The type of the project is determined by the module in which it is saved. The interface in the Design 2D module is described in Chapter 12. The only difference with a blade-to-blade analysis computation is the use of the Inverse Design page. This page is described in more detail in the next sections. 13-2 FINE™ Inverse Design in the FINE™ Interface Design 2D Module 13-2.2 Creation of Inverse Design Input Files An inverse design calculation should always start from the converged flow analysis of the initial geometry. Once a converged flow solution for the blade-to-blade analysis has been obtained, the user can proceed with a modification of the blade using the inverse method. For this purpose the two input files "project_computationname.req" and "project_computationname.run" have to be prepared, in addition to the files required for the analysis ("project_computationname.run" and the geometrical input files). 13-2.2.1 Recommendations It is often useful to save the results obtained after the analysis computation. Therefore it is recommended to perform the inverse design in a new computation. With the analysis computation selected in the Computations area on the top left of the FINE™ interface click on the New button. A new computation is created with the same parameters as the initial computation. The Rename button may be used to rename the new computation. analysis inverse design FIGURE 13.2.2-2 Computations area The expert integer parameter IATFRZ is usually set to 2 during the inverse design procedure in order to freeze the computation of the turbulent viscosity. The consequence of this is to drastically reduce the computational time per inverse design iteration. 13-2.2.3 The Input File "project_computationname.req" The ’project_computationname.req’ file has exactly the same format as the ".vel" or ".load" output files automatically generated by the blade-to-blade analysis module. The most appropriate way to generate this file is to modify the ’projectname.b2b.vel’ or ’projectname.b2b.load’ file resulting from the flow analysis of the initial geometry, using the MonitorTurbo. In order to create a target with the MonitorTurbo, the following operations should be made: 1. 2. 3. 4. Start the ’MonitorTurbo’. Select the "Loading diagram" menu. Open the ’project_computationname.vel’ or ’project_computationname.load’ file. Choose between the ’Mis’ or ’Cp’ distributions (in case the inlet total conditions are not imposed as boundary conditions, the inverse problem has to be formulated in terms of Cp). The definition of Mis and Cp are provided in Eq. 13-1 and Eq. 13-2 presented in section 13-4. Activate the ’Markers’ to distinguish the discretization points. Activate the Edit a curve button. Choose the suction or the pressure side curve, by placing the cursor on the corresponding legend, and typing <s> to select. The activated curve changes color. 5. 6. 7. FINE™ 13-3 Design 2D Module Inverse Design in the FINE™ Interface 8. Modify the curve using the middle button of the mouse: a. Choose the left point where the modification will start (click on the middle button). b. Choose the right point where the modification will end (click on the middle button). c. Choose control points between the left and the right points (click on the middle button). d. Displace the control points. — Select the control point by placing the cursor on the point. — Press <Ctrl> on the keyboard, and displace the point vertically. The exact position of the point can be specified by pressing the right button of the mouse. e. Save the new curve by clicking on the Save button, and giving the name of the new curve, or cancel the modifications by clicking on the Cancel button. At any moment, a zoom of the curves can be obtained by defining a new rectangular window, using the left button of the mouse. The previous unzoomed view can be retrieved by pressing the right button of the mouse. 13-2.2.4 Input File "project_computationname.run" The "project_computationname.run" input file is created via the Inverse design page included in the FINE™/Design 2D interface (Figure 13.2.2-1). One of the three possible inverse formulations should be chosen: • Pressure and suction side distributions or classical formulation: both suction and pressure sides of the blade are modified for an imposed pressure distribution along the whole blade contour. If this formulation is used the profile closure constraint has to be activated. • Suction side distribution or mixed formulation: only the suction side is modified for a prescribed suction side pressure distribution. The profile closure conditions should also be activated, so that the pressure side follows the suction side modifications. • Blade loading or loading formulation: the camber line of the blade is modified for a prescribed loading (suction-to-pressure side pressure difference) distribution from the leading to the trailing edge. The blade thickness distribution is maintained constant and therefore the profile closure condition does not need to be used. The target of the inverse design computation may either be constructed in terms of isentropic Mach number (Mis) or pressure coefficient (Cp) (see Eq. 13-1 and Eq. 13-2 in section 13-4). The isentropic Mach number formulation is limited to compressible flows. Control of the leading and trailing edges is provided. The inverse method permits to maintain some parts of the blade unchanged, such as the leading and trailing edge regions. The number of frozen points along the suction and the pressure sides should be specified for each edge by the user. The default value is 1. However in many cases it is recommended to freeze the leading edge region where no modification is imposed. At the trailing edge it is highly recommended to freeze the regions where a flow separation appears in the analysis of the initial blade. Two relaxation factors are available: • The first relaxation factor (default value = 1.0) permits to consider an intermediate target between the one present in the ".req" file and the initial distribution present in the ".vel" file. This factor is not often used. • The second relaxation factor (default value = 0.05) permits to under-relax the geometry modifications. The range of variation of this factor is from 0.01 to 0.1. Higher values than 0.1 are not recommended for reasons of stability, whereas lower values than 0.01 usually mean that the inverse problem can not be treated. 13-4 FINE™ Inverse Design in the FINE™ Interface Design 2D Module The following geometry constraints are available: • the profile closure constraint should always be used, unless: — the blade thickness is automatically controlled ("loading" formulation). — the trailing edge of the blade is blunt, and the trailing edge thickness does not need to be maintained. • Constant stagger angle is not often used. • Constant blade chord: this constraint permits to maintain the blade chord (measured on the transformed m-θ plane). This constraint should not be used together with the constant radius option, as the two constraints are contradictory. • Constant radius: this option is recommended for radial machines, as it permits to guarantee an unchanged meridional position of the leading and trailing edges. The points are displaced along the circumferential direction. This option is not recommended for large rounded leading edges. • Reference point: the fixed reference point can be either the leading edge (by default) or the trailing edge (if the corresponding button is selected). FIGURE 13.2.2-1 Inverse design page Finally, the number of iterations performed for the inverse design calculation. 13-2.3 Initial Solution Menu An inverse design calculation should always start from the converged flow analysis of the initial geometry. Once a converged flow solution for the blade-to-blade analysis has been obtained, the user can proceed with a modification of the blade using the inverse method. (Figure 13.2.3-2) FINE™ 13-5 Design 2D Module Inverse Design in the FINE™ Interface FIGURE 13.2.3-2 Initial solution page 13-2.4 Launch or Restart Inverse Design Calculation Once the ’.req’ and ’.run’ input files have been correctly created, an inverse design can be started, by selecting the Inverse design option in the "run type" parameter included in the Control Variables page, and by pressing the Start button in the Solver menu. FIGURE 13.2.4-3 Run type page of the information area Exactly as in the case of the restart of a flow analysis the user has to specify the name of the initial solution file. It is recommended to save the results of the flow analysis under a different name, so that several inverse design calculations can be performed successively, starting from the same initial solution. An interrupted inverse design calculation can be "restarted". For this purpose the user should set the expert parameter INVMOD to 1 instead of 0. This implies that in addition to the correct flow solution file, the actual blade geometry will be read by the solver and considered as the initial one. 13-2.5 Expert Parameters 13-2.5.1 Using a Parametrised Target Distribution Using a parametrised target distribution is possible through the two expert parameters IADAPT and RADAPT, that can be accessed via the Control variables page. The expert mode must be activated in the top right corner of the interface. The integer variable IADAPT contains 6 values: • Type of parametrisation — 0: parametrised distribution is not used — 1: suction side (or loading) distribution is parametrised — 2: pressure side distribution is parametrised. 13-6 FINE™ Theory Design 2D Module • Number of iterations after which the adaptation process will start. • Index of starting (left) point of the parametrised target. The user specifies the position with respect to the leading edge (typically about 10 points). • Index of the ending (right) point of the parametrised target. The user specifies its position with respect to the trailing edge (typically about 10 points). • Turning angle is imposed value (0) or the change of swirl RVθ between inlet and outlet (1). • Imposed turning or swirl is taken from the analysis solution (0) or set by the user (1). The real variable RADAPT contains 4 values: • Reduced curvilinear position of the free parameter between 0. (left point) and 1.0 (right point (default: 0.5). • Relaxation factor governing the amplitude of successive updates of the parameter (default: 0.25) • Range of variation of the free parameter (in isentropic Mach number or pressure coefficient, depending on previous choice of the user) (default: 0.2). • User imposed value of the turning angle (in deg.) or swirl RVθ (m2/s) (used if the last integer of IADAPT is set to 1). INVMOD: set this parameter from 0 to 1 to allow the restart of an inverse design computation. 13-2.5.2 Splitter Blades Design Centrifugal compressors with splitters can be redesigned with FINE™/Design 2D. It is possible to modify either the main blades or the splitter blades. The choice is made through the expert variable INVSPL (accessed in the "Computation Steering" menu of the FINE™ interface): • INVSPL= 1: main blades are modified • INVSPL= 2: splitter blades are modified The target should be constructed from the ’project_computationname.vel’ or ’project_computationname.load’ files if the main blades are modified, or from the ’project_computationname.split.vel’ or ’project_computationname.split.load’ files if the splitter blades are modified. 13-3 Theory The purpose of an inverse method is to redesign the blade shape in order to obtain a prescribed pressure distribution along the blade surfaces. This provides a detailed control of the boundary layer behaviour, by limiting the amount of diffusion and by eliminating the eventual spurious acceleration and deceleration detected along the initial blade profile. Such a method also offers an indirect control of the secondary losses, as a control of the blade loading distribution can be obtained. The inverse design method adopted in FINE™/Design 2D consists of modifying iteratively the blade geometry, until a target pressure distribution is reached on the blade surfaces. The geometry modification algorithm is based on the permeable wall concept. Each iteration of the process is composed of 2 separate steps, respectively related to the geometry and to the flow field updates. Both viscous and inviscid problems can be treated with this approach. Three formulations of the inverse problem are possible: FINE™ 13-7 Design 2D Module File Formats used for 2D Inverse Design • the classical formulation, in which both suction and pressure sides are redesigned in order to obtain a pressure distribution prescribed along the whole blade surface. • the mixed formulation, in which the suction side is redesigned in order to obtain a pressure distribution specified along the suction side only. This formulation is for instance interesting for rotor blades on which strict mechanical constraints are imposed. In those cases the classical inverse formulation may be less efficient because the blade thickness is a result of the calculation, and it is often difficult and time consuming to find an appropriate target leading to a blade with an acceptable thickness distribution. • the loading formulation, in which the distribution of blade loading (pressure-to-suction side pressure difference) from the leading to the trailing edge is prescribed, and in which the camber line of the blade is redesigned (the blade thickness distribution being kept unchanged). This approach is interesting especially for radial machines. This is due to the fact that in radial machines, the average velocity level in the blade channel is mainly controlled by the shape of the hub and shroud endwalls, and therefore a modification of the blade shape mainly influences the loading distribution. The "loading" formulation is therefore more appropriate and efficient for radial machines. However no general rule can be set, and improvements can be reached in many cases using the second formulation. Several geometrical constraints and options have been implemented, to increase the flexibility of the method: • Control of the leading and trailing edges: several points can be kept unchanged in the leading/ trailing edge regions. • Constant blade chord. • Specification of the fixed reference point (leading or trailing edge). • Inverse problem formulated in terms of isentropic Mach number or of pressure coefficient. • Constant meridional position of leading and trailing edges (recommended for radial machines): with this option, the points are displaced along the circumferential direction, which guarantees that their meridional position is unchanged. An important advantage of the present method is the possibility to control the outlet flow angle or swirl. A major drawback of most inverse methods is the lack of control of the turning angle or work exchange in the cascade. The user does not have the guarantee that the specified target pressure distribution will lead to an unchanged turning angle. This implies that several iterations are sometimes required before finding the target leading to an acceptable design. FINE™/Design 2D offers a unique solution to that problem, allowing the control of the turning angle or of the change of swirl from inlet to outlet. A degree of freedom is introduced in the target pressure distribution, that is automatically modified in order to respect the outlet flow angle constraint. A part of the target pressure distribution is defined using a fourth order polynomial curve. The parameter defines the vertical position of a point of this polynomial curve. A smooth transition is ensured between the fixed part of the target and variable one. The parameter is iteratively and automatically adjusted in order to respect the outlet flow angle or the outlet swirl RVθ. 13-4 File Formats used for 2D Inverse Design 13-4.1 Input Files The input files required to run a blade-to-blade study can be split into 3 categories: 13-8 FINE™ File Formats used for 2D Inverse Design Design 2D Module • The geometrical input files, defining the blade geometry. • The solver input files, which define the solver parameters and the fluid and flow conditions. • The inverse design input files, which permit to define an inverse problem. The geometrical and solver input files have been described in Chapter 12. The inverse design input files can be interactively created with the FINE™ environment, and are described in this section. 13-4.1.1 Inverse Design Input Files In order to perform an inverse design problem, 2 additional input files are required: — The ’project_computationname.req’ file, which defines the target pressure distribution. This file can be interactively created using the MonitorTurbo. — The ’project_computationname.run’ file, which specifies the parameters for the inverse design (automatically written by the user interface when saving the ’.run’ file). It should be mentioned that an inverse design always starts from a converged analysis of the initial geometry. The target pressure distribution can be generated by modifying the pressure distribution resulting from the analysis of the initial geometry. 13-4.2 Output Files Several output files are generated by the blade-to-blade module, which have been described in Chapter 12. The inverse design method produces additional output files which are presented in this section. 13-4.2.1 Geometry Files a) ’project_computationname.geoini’ & ’project_computationname.geo’ These files contain the blade shape in the (m,θ) plane. The ’.geoini’ file contains the initial blade shape, whereas the ’.geo’ file contains the actual one. These files can be read and plotted with the NUMECA MonitorTurbo (Blade profile menu). In the case of an inverse design the visualization of the two files permits to compare the initial and the new geometry. b) ’project_computationname.split.geoini’ & ’projectname_computationname.split.geo’ (if splitter blades) These files contain the splitter blade shape in the (m,θ) plane. The ’.geoini’ file contains the initial blade shape, whereas the ’.geo’ file contains the actual one. These files can be read and plotted with the NUMECA MonitorTurbo (Blade profile menu). In the case of an inverse design the visualization of the two files permits to compare the initial and the new geometry. c) ’projectname_computationname.ss.ori’ ,’projectname_computationname.ps.ori’ & ’projectname_computationname.mer.ori’ These three files are automatically generated at the beginning of the solver execution, and contain respectively the suction side, the pressure side and the axisymmetric streamsurface on which the calculation is performed. These files are especially interesting in a 3D input type, with which this blade section results from the 3D interpolation procedure between the 3D blade and the streamsurface. These files have the same format as the blade geometry and streamsurface data input files. The coordinate system for the blade data is always XYZ, which makes these files compatible with IGG™ or AutoGrid. The coordinate system for the streamsurface is always ZRB (B is the streamtube thickness). FINE™ 13-9 Design 2D Module File Formats used for 2D Inverse Design The coordinates are given in the same unit length chosen by the user for the input data. d) ’project_computationname.ss.new’ & ’project_computationname.ps.new’ After an inverse design stage, these two files are automatically generated, and contain the new suction and pressure sides. These files have the same format as the blade geometry data input files. The coordinate system is always XYZ, which makes them compatible with IGG™ or AutoGrid. The coordinates are given in the same length unit chosen by the user in the input. In the default configuration of the solver the points included in these files are the mesh points along the blade walls. The number of points can be different and controlled by the user through the expert parameter NPTB2B. If this parameter is set to a value N different from 0, the number of points describing both suction and pressure sides will be N. 13-4.2.2 Quantities Files a) ’project_computationname.velini’ & ’project_computationname.vel’ These files contain the isentropic Mach number and the pressure coefficient distributions along the blade surfaces. The two quantities are plotted along the curvilinear coordinate measured along the blade surface (non-dimensionalized by the blade chord). The ’.velini’ file contains the initial distribution, whereas the ’.vel’ file contains the actual one. The isentropic Mach number is calculated using the inlet relative total temperature and pressure, which are not necessarily imposed (depending on the choice of the inlet boundary condition). In case the total conditions are not imposed, the values are the ones resulting from the calculation (average along the inlet boundary). The isentropic Mach number is defined by: γ–1 ---------γ where p is the local static pressure, and p0 is the local relative total pressure calculated assuming a constant rothalpy and a constant entropy in the field. The pressure coefficient is defined by: p – p exit Cp = -----------------p exit where pexit is the exit static pressure and p is the local static pressure. These files can be read and plotted by the NUMECA MonitorTurbo (Loading diagram menu). In the case of an inverse design the visualization of the two files permits to compare the initial and the new pressure distributions. b) ’project_computationname.loadini’ & ’projectname_computationname.load’ Provided that the parameter ISQUEL specified in the ’.run’ file is different from 0, these files are automatically generated and contain the distributions of the suction-to-pressure side Mach number and pressure coefficient difference and average. These distributions are useful when the ’loading’ 13-10 ⎠ ⎞ Mis = 2 ---------γ–1 p0 ---p –1 ⎠ ⎟ ⎟ ⎞ ⎝ ⎝⎜ ⎛⎜ ⎛ (13-1) (13-2) FINE™ File Formats used for 2D Inverse Design Design 2D Module formulation of the inverse design method is selected. The ’.loadini’ file contains the initial distribution, whereas the ’.load’ file contains the actual one. These files can be read and plotted by the NUMECA MonitorTurbo (Loading diagram menu). In the case of an inverse design the visualization of the two files permits to compare the initial and the new distributions. c) ’project_computationname.split.loadini’ & ’project_computationname.split.load’ (if splitter blades) Provided that the parameter ISQUEL specified in the ’.run’ file is different from 0, these files are automatically generated and contain the same quantities as the ’.load’ and ’.loadini’ files calculated along the splitter blades (Loading diagram menu). d) ’project_computationname.tarini’ & ’project_computationname.tar’ The inverse solver automatically generates these two output files, which contain respectively the initial and actual target pressure (or loading) distributions. These files can be read and plotted by the NUMECA MonitorTurbo (Loading diagram menu). The comparison of the .tarini and ’.velini’ (or ’.loadini’) permits to observe the inverse problem to be solved, whereas the comparison of the ’.tar’ and ’.vel’ (or ’.load’) files permits to verify the correct convergence of the inverse design. FINE™ 13-11 Design 2D Module File Formats used for 2D Inverse Design 13-12 FINE™ CHAPTER 14:The Task Manager 14-1 Overview Using the Solver menu in FINE™/Turbo computations can be started, suspended or killed. For basic task management these menu items are sufficient. The Task Manager provides more advanced features for the management of (multiple) tasks. It allows to manage tasks on different machines on a network, to define parallel computations or to delay tasks to a given date and time. Before using the Task Manager for the first time it is important to read the next section first. This section provides important information for getting started with the Task Manager. Read this section carefully to fully benefit of the capabilities of the Task Manager. From FINE™/Turbo the Task Manager can be accessed by the Modules/Task Manager menu item. The interface as shown in Figure 14.3.1-1 will appear. In section 14-3 the Task Manager interface is described in detail including a description of all capabilities. The current limitations of the Task Manager are listed in section section 14-6. To manage tasks through the use of scripts is also possible and has the benefit that it is not necessary to stay logged in on the machine on which the tasks are launched. See section 14-5 for more detail on the scripts to use to launch NUMECA software. 14-2 Getting Started 14-2.1 The PVM Daemons The Task Manager is based on the PVM library. It allows FINE™ to control processes and communication between processes on all the machines available by the user. PVM works with a virtual machine managed through a pvm daemon. In this section the way PVM daemons are working and its limitations under Windows are described. FINE 14-1 The Task Manager Getting Started 14-2.1.1 What PVM Daemons Do. If a user starts the FINE™ interface on a given computer where no PVM daemon is running, FINE™ will start the process pvmd on this machine that becomes the virtual machine server for the user. When adding a host in the Task Manager (on the Hosts definition page) a pvmd is started on the remote computer that is added to the virtual machine. If after that the user logs on the second computer and starts the FINE™ interface this second computer belongs also to the virtual machine whose server is the first pvmd started. If after that the user logs on a third computer on which no pvmd is running and starts the FINE™ interface, FINE™ will start a pvmd that becomes the server of a new virtual machine. When trying to add a host belonging the first virtual machine (containing the two first computers), he will see the a warning message that he cannot connect to the virtual machine because a pvmd is already running. If the user wants to have the three computers in the same virtual machine, one of the virtual machines must be shut down (on the Hosts definition page) and add the corresponding computers from the second one. 14-2.1.2 Limitation under Windows On windows only one pvmd can run and hence, only one single user can connect to the virtual machine. If an other user wants to use the NUMECA software on the PC as server (FINE™) or as client (EuranusTurbo), the first one needs to shut down the pvm daemons on this machine. To shut down go to the Hosts definition page and click on Shutdown. This will close the interface and removes all the pvm daemons on the machine. Remove the files pvml.<userID> and pvmd.<userID> from the directory defined by the PVM_TMP (by default C:\tmp). 14-2.2 Multiple FINE™ Sessions During a FINE™ session all the tasks defined by the user are stored in the tasks file in the NUMECA tmp directory. This directory is in the .numeca/tmp directory below the home directory. On UNIX the home directory corresponds to the HOME environment variable. This is also true on Windows if this variable is defined and, if it is not the case, it is set to the concatenation of HOMEDRIVE and HOMEPATH environment variables. When FINE™ is started more than once at the same time, a warning indicates to the user that FINE™ is already running and can enter in conflicts with the other FINE™ sessions. Indeed, the user can define tasks in both interfaces but the task definitions saved when exiting FINE™ will be overwritten by the other sessions. Therefore, it is not advised to open multiple FINE™ sessions when the Task Manager must be used. 14-2.3 Machine Connection from UNIX/LINUX Platforms The Task Manager allows the user to control processes on all the machines connected to the network. The rsh command is used by the PVM library to access the machines. Before using the Task Manager, the following actions must be done: 1. Modify the .rhosts file in the home directory by introducing all the machines which can be used by the Task Manager. i.e.: if the machines machine1 and machine2 will be used by the user’s tasks, the .rhosts file must be modified as follows: line1: machine1 <login1> line2: machine2 <login2> where machine1 and machine2 are the host names. 14-2 FINE Getting Started The Task Manager login1 and login2 are optional. They must be set if the login on remote host is different from the login on the local host. The .rhosts file needs to be ended by a blank line. The .rhosts file permission must be set to ’rw’ (chmod 600 ~/.rhosts). 2. Test the rsh command on the desired machine: an external check that the .rhosts file is set correctly is to enter the following command line: % rsh remote_host ls <Enter> where remote_host is the name of the machine to connect to. If the login on the remote host is not the same, ensure that the .rhosts file contains the line: remote_host local_login and in this case the command line is: % rsh remote_host -l local_login ls If the .rhosts is set up correctly, a listing of the files is shown on the remote host. Due to a limitation of the PVM library, FINE™ can not be connected to a machine where FINE™ has already been started. When PVM tries to establish the connection, it detects that a server FINE™ is already running and/or pvm daemons are still running and finally refuses the connection with a warning. To solve this problem, the PVM daemons must be stopped on the machine on which FINE™ must be connected: 1. 2. Log on the machine where the connection must be established. Start FINE™ and open the Task Manager through Modules/Task Manager and use the button Shutdown of the page Hosts definition. The button Shutdown can be used to switch off all the PVM daemons of all the machines connected to FINE™. This action will stop all the daemons on all the machines connected, kill all the tasks and finally exit FINE™. On UNIX: remove all the /tmp/pvmd.<userID> and /tmp/pvml.<userID> files. Under Windows these files should be removed from the directory defined by PVM_TMP (by default this directory is C:\tmp). Repeat this operation for all the machines on which the problems appear. The operations 2 and 3 can be done automatically using the script NUMECA_INSTALLATION_DIRECTORY/COMMON/cleanpvmd provided with the NUMECA software. 3. 4. 5. If PVM still has a problem to get the connection, it will print an error message either to the screen, or in the log file /tmp/pvml.<userID> (on UNIX) or in the directory defined by the environment variable PVM_TMP (by default C:\tmp) in the log file called: pvml.<userID>. Please send this log file to NUMECA support team ([email protected]). All these operations apply only to the user’s daemons and user’s files. Multiple users can use the Task Manager simultaneously. No interaction appears between PVM daemons and PVM log files of different users. The Task Manager does not allow to launch processes from a UNIX platform to a Windows platform. FINE 14-3 The Task Manager Getting Started 14-2.4 Machine Connection from Windows Platforms When a user stops the pvmd on a remote host (using Remove Host button on the Hosts definition page) and immediately try to restart it (using the Add Host... button), a message will appear stating that it is not possible to connect. This problem does not occur in general since there is no need to remove a host and add it immediately after. When it occurs the only solution is to wait until the host is available again (after 5 to 10 minutes). From time to time, when a user tries to connect on a remote host, an error message can appear very briefly: "Can not connect to RSH Port!!!" This may happen on Windows connecting to a host, disconnecting, and trying to reconnect again to the same host. It has the inconvenience to stop the interface FINE™. There is a socket release time parameter which keeps the connection for some time. 14-2.5 Remote Copy Features on UNIX/LINUX All the tasks defined by the user are associated with files used or created by the NUMECA’s software. When the files are not visible from the machine on which the task must be launched (i.e. the files are on the local disk of the host where FINE™ is running), the user can use the remote copy feature proposed in the Task Manager. All the files needed by the tasks will be transferred into a directory (specified by the user) of the remote machine and at the end all the created or modified files are transferred back to the host machine from which the task has been launched. By default, the available remote directories are "/tmp". The user can also specify any other directory, as long as it is visible from the remote host and has writing permission. This feature uses the rcp UNIX command. Before using the remote copy feature, it is advised to first check if the rcp command works correctly between the machines: — First try the rsh.exe command (see section 14-2.3). — Type the command: touch test;rcp -p -r test destination_machine:/tmp/test. If no error is returned by the system, the remote copy works between the local host and the destination_machine. Errors may appear if the .cshrc file contains an stty command. In order to be able to use the remote copy feature, remove all the stty commands from the .cshrc file. — If the login on the local host is different from the login on the remote host, type the command: touch test;rcp -p -r test remote_login@destination_machine:/tmp/test. 14-2.6 Remote Copy Features on Windows As files located on the local disk are not visible from a UNIX machine, this feature is proposed to be able to launch tasks on remote UNIX platforms. The principle is the same as the one described in the previous section: local files are copied in the remote directory specified by the user, then the task starts. When it terminates, all results files are transferred in the original directory. This feature uses rcp.exe windows command. Before using the remote copy feature, it is advised to first check if this command works properly: — First try the rsh.exe command (see section 14-2.3). — Create a file test, then type the command: rcp -b test destination_machine:/tmp/test. If no error is returned by the system, the remote copy works between the local host and the destination_machine. Errors may appear if the .cshrc file contains an stty command. In order to be able to use the remote copy feature, remove all the stty commands from the .cshrc file. — If the login on Windows is different from the login on the remote host, type the command: 14-4 FINE The Task Manager Interface The Task Manager rcp -b test destination_machine.remote_login:/tmp/test rcp.exe is provided with FINE™ and is located in the same directory as rsh.exe. 14-3 The Task Manager Interface 14-3.1 Hosts Definition On the Hosts definition page hosts in the virtual machine, the operating system of the machine and their connection status are visualized. For an explanation of the virtual machine see section 142.1.1. If the connection is not OK, it means that the corresponding computer is no more in the virtual machine. This may occur for example if the computer has been rebooted. FIGURE 14.3.1-1Hosts definition page 14-3.1.1 Add Host When the user clicks on the Add Host... button, the interface asks for a host name and a login name. The login name is optional. It is needed only if the user login on the local host and the one on the remote host are different. When the user accepts (Accept), the host name appears in the host list, with type of operating system and its connection status. At this point, the host is in the virtual machine, and is ready to receive a task. if the connection can not be established, check for more detail in section 14-2.1, sec- FINE 14-5 The Task Manager The Task Manager Interface tion 14-2.3 and section 14-2.4. 14-3.1.2 Remove Host When the user clicks on Remove Host button, the selected host is removed from the list, and is not in the virtual machine any more. This operation is not allowed when a task is running on the host to be removed, or when the selected host is the local one. 14-3.1.3 Shutdown When the user clicks on Shutdown button, all hosts in the virtual machine are removed. FINE™ exits and the virtual machine halts. All running tasks are killed. This option is useful when the user wants to change the machine on which FINE™ is running. See section 14-2.1.1 for more detail on virtual machines and when to change this. 14-3.2 Tasks Definition A task is a collection of subtask where a subtask is one of the program with its arguments (’.run’ file for EURANUS and Design3D, template ’.trb’, geometry ’geomTurbo’ and mesh ’.igg’ files for AutoGrid and macro file .py and ’.run’ file for CFView™). The different subtasks of a given task can be run simultaneously if the output of one subtask is not needed by other ones (for example: several CFView™ subtasks with different macro ’.py’ files or several EURANUS subtasks with different ’.run’ files started on different computer). If the output of one subtask is needed by other ones, it must be run sequentially. For example: AutoGrid generates the mesh that is used for starting an EURANUS computation whose output is used for starting CFView™. 14-3.2.1 Task List In this section, the user can visualize the defined tasks and their status. To create a task, just click on New Task button. The defaults task name can be modified by clicking on Rename Task button. The selected task can be removed by clicking on Remove Task button. Once a task is created and defined (see following section), it can be started or stopped just by clicking respectively on the Start, or Stop button. A task can be delayed: click on Delay button and enter the date and time for the moment the task needs to be launched in the dialog box. The delayed task can be disabled using the button Cancel. When the user validates the data, a little watch in the task list indicates that the task is scheduled: FIGURE 14.3.2-2Task List with Delay window to start a task at a later moment When exiting FINE™, all the delayed tasks are automatically started and stay in sleep mode until their starting dates are reached. When starting FINE™ again, all the task 14-6 FINE The Task Manager Interface The Task Manager manager related to the delayed tasks still in sleep mode are killed and FINE™ Task Manger gets back the control of these tasks. 14-3.2.2 Task Definition In this section the subtasks of the selected task of the Task List are listed. A subtask is defined by its type (euranusTurbo, AutoGrid, CFView™ or Design3D), their status and the host on which they are launched. To add a subtask click on the New Subtask. Select the executable name (EURANUS, AutoGrid, CFView™ or Design3D) and the host on which the process should be started in the two lists. The host name list contains the hosts that are in the virtual machine. They are set in the Host definition page. 14-3.2.3 Subtask Arguments a) Definition of Input and Output Once a subtask is created, input and/or output files must be defined in the Subtask arguments section: — The flow solver EURANUS and Design3D requires one argument file: the name of the runfile. This files is created using the menu File/Save Run Files in the FINE™/Turbo module. — The mesh generation system AutoGrid requires three files as arguments: the trb file, the geomTurbo file and as output the grid file name (see the AutoGrid manual for more details) FINE 14-7 The Task Manager The Task Manager Interface — The flow visualization system CFView™ requires two files: the run file and a macro file (see CFView™ manual for more details) The run file is automatically opened by CFView™ before starting the macro. The macro file may open other ’.run’ files to perform flow comparisons (see CFView™ manual for more information about the macro ’.py’ file). b) Simultaneous or Sequential Mode Moreover, a process can be executed simultaneously with the other subtasks (by selecting Run Simultaneously with Previous Subtask) or sequential (by selecting Run After Previous Subtask). In this last case, the process waits the previous subtask to be finished before starting. This is only available for AutoGrid, Design3D and EURANUS subtasks. Only a certain amount of tasks can be performed at the same time depending on the available licenses. The subtasks related to postprocessing with CFView™ are always executed in sequential mode. c) Remote Copy The Remote copy to button allows the user to specify that the files are not visible from the remote machine and must be transferred. This is only available for AutoGrid, Design3D and EURANUS. d) Parallel Computations. d.1) MPI system The flow solver euranusTurbo has integrated multiprocessor machine concept. The button Parallel Computation can be activated to specify that the parallel version of the flow solver can be used for this computation. The button Flow solver parallel settings gives access to the dialog box used to set up a parallel computation. When the dialog box is opened, the block list displayed all the block of the mesh. The user can defined new processes on all the available machines and defined manually or automatically the load balancing (using the Automatic Load Balancing button). The parallel processing can only be used on multiprocessor machine (shared memory mode) or on machines with the same operating systems (homogenous distributed memory mode) See section 14-4 for more detailed information on parallel computations. 14-8 FINE The Task Manager Interface The Task Manager Processes list with the load balancing of the cells Buttons used to remove or add new processes on the specified machine List of the block in the associated mesh Button used to link the selected block with a process Default block distribution d.2) SGE system Within the Task Manager provided in FINE™/Turbo v6.2-7, the parallel process can be set using the SGE (Sun Grid Engine) batch system. This last sytem includes the possibility to add a SGE type host and to define arguments needed to launch the computation within the Task Manager. Host Definition In the page Hosts definition the user needs to add host. When adding the host, automatic checks are performed: 1. 2. 3. it will detect if the "sge_qmaster" is running on the platform. If not, it means that the platform does not have SGE capabilities or the platform is not the SGE master processor. it will detect all parallel environment defined in SGE. it will detect all parallel environment that the user is allowed to use. If no parallel environment could be accessed by the user, his login should be added to the user list by the SGE administrator. When all checks are successfull, the SGE capability of the added host is activated and the user can see if the host added is a SGE paltform within the Task Manager GUI (Figure 14.3.1-1). Task Definition In the page Tasks definition, if the user select a SGE platform when launching an EURANUS task in parallel, he has the access to the MPI system or the SGE system (Figure 14.3.2-3). When the SGE system is used, the number of processor and the SGE environment have to be specified. Depending on the number of processor, an automatic load balancing is performed to update the block distribution and the process needs only to be started by the user. FINE 14-9 The Task Manager The Task Manager Interface FIGURE 14.3.2-3Tasks Definition - SGE inputs Process Management Once the process is starting, the ".run" file is modified automatically depending of the number of processor. Then a script file ".sge" is created at the same time as the ".p4pg" file when using MPI system. The name of the SGE job is limited to 8 characters and the following format is thus chosen "comp#000" where 000 stands for a any number depending of the number of SGE jobs already running under the same environment. To test if a computation is running, because there are no communication with the task manager since EURANUS has not been launched using PVM daemon, the "qstat" command with the job-ID number of the SGE job is used. To suspend the SGE job, the user could use the Suspend function of the Task Manager. It will create automatically a ".stop" file in the running computation directory that will enable EURANUS to suspend after saving the solution at the next iteration or after the full multigrid initialization. To kill the SGE job, the user could use the Stop function. The Task Manager will then use the SGE’s function "qdel" to kill the computation without saving the solution. To kill EURANUS properly, the SGE’s "execd parameters" variable should be set to "NOTIFY_KILL=TERM" and the "notify time" variable of nodes should be set to a sufficient value to allow EURANUS to exit properly. We invite the user to ask the SGE administrator to check these variables. e) Message Window When a task is started, a Task Manager process is launched to take care about the task management: process communication, automatic launching of the sequential and parallel subtasks. A message window linked to the Task Manager is opened. In this window the user can follow the evolution of the status of all the subtasks of the current task. In case of flow solver computations the iterations are also displayed in this window as shown in Figure 14.3.2-4. At the bottom of the Task Manager window a Refresh Rate can be chosen. This rate determines how frequently the Task Manager window is updated. A higher refresh rate will update the information in the window more frequently but will use more of the available CPU. 14-10 FINE Parallel Computations The Task Manager FIGURE 14.3.2-4Task Manager information window If the user quits FINE™, all the message windows will stay open and the tasks will continue. Closing a message window will immediately kill all the subtasks of the corresponding task. 14-4 Parallel Computations 14-4.1 Introduction Parallel computations can be defined through the FINE™ interface as described in section 14-3.2.3. Parallel processing relies on the distribution of independent tasks among several processors using communication protocols to transfer data from one processor to another whenever this is necessary. This induces of course an acceleration of the computation itself but it also makes possible very large computations that would not fit on a single processor. The present parallel processing relies on the block structure of the flow solver EURANUS. Each process is assigned a given number of blocks. As a consequence, the number of processors cannot exceed the number of blocks. Boundary data are exchanged between processors each time an update of the flow solution is required. The parallel version makes use of MPI (Message Passing Interface) libraries. MPI was chosen among other tools such as PVM or Open MP for its high communication performances (high bandwidth, low latencies). Although Open MP has better performance on shared memory configurations, i.e. on a given computer with single global memory and several processors, it is not designed for distributed memory configurations (several computers with their own memory). The parallel version is implemented for UNIX, LINUX and Windows platforms. FINE 14-11 The Task Manager Parallel Computations The present MPI implementation is based on a host/node approach. One host process is dedicated to input/output management. The host reads the mesh and input files, sends the data to the computation processes (the nodes), receives the computation results from the nodes and writes the output files. Figure 14.4.1-5 shows the task distribution on a 4 processors configuration. Note that the host/ node implementation will be replaced progressively as parallel MPI input/output functionalities are now available. Input data base reading Host writing Output data base Node 1 Node 2 boundary conditions Node 3 boundary conditions FIGURE 14.4.1-5Tasks in a parallel computation 14-4.2 Modules Implemented in the Parallel Version The following flow solver functionalities are already available in the parallel version: • All turbomachine boundary conditions (including Phase-lagged). These include rotor/stator interfaces, non matching boundaries and the fully conservative non matching boundary treatment (FNMB), • Turbomachinery initial solution, • Baldwin-Lomax, Spalart-Allmaras and k-ε turbulence models, • Real gases, • Preconditioning (low Mach number and incompressible fluids), • Cooling holes, • Outputs including pitchwise averaged output. No solid data nor surface averaged outputs are available yet. The lagrangian module is not available for parallel computations. 14-4.3 Management of Inter-block Communication The block structure of the solver allows to distribute blocks across processors or computers (in case of a cluster). Each processor will handle an integer number of blocks. The treatment of the boundary condition will be replaced by message passing between the processors or remote computers. Communication optimization The parallel version of the flow solver is optimized in order to minimize duplicated data as well as the number and the volume of exchanged messages. A significant improvement of the code performance was obtained by grouping small messages into larger buffers: the information contained in small messages is usually shared by a large number of blocks, leading to frequent messages of 14-12 FINE Parallel Computations The Task Manager that type. This is the case for block edges data that are exchanged several times during each iteration. Significant latency times are induced by these communication processes and message grouping highly reduces the number of such messages. Large message limitation Very large messages are usually exchanged during initialization and at the end of the computation between the nodes and the host. These also need to be avoided as they can cause important memory needs and eventually lead to system failure. Messages are split into buffers of maximum size MXBFSZ (see section 14-4.4) in order to avoid excessive MPI memory requests. 14-4.4 How to Run a Parallel Computation The setting of a parallel run using the FINE™ interface is described in section 14-3.2.3. The user selects the number of nodes, making sure it is smaller than the number of blocks. A balanced distribution of the blocks among the various processes is automatically performed by the FINE™ interface but the user can also define its own load balancing, i.e. process distribution. Memory allocation Memory allocation is performed as follows: • The integer data structure is duplicated for all processes. Since the integer data structure size is about a tenth of the real data structure, this does not lead to high memory overload when the number of processes is less than 10. • The real memory allocation is performed for each process. It should be set to the minimal amount of memory necessary to hold the data structure on the process that has most grid points. When the load is well balanced, the real memory overload is due to face and edge data structures. These data need indeed to be duplicated when two processors are involved in the same block connection. The total memory need Mtotal for a parallel computation involving n ( n ≥ 2 ) processors can be estimated as: n M total = M real ⋅ 1, 2 ⋅ ----------- + M integer ⋅ n n–1 where Mreal and Minteger are the real and integer memory needed for the same computation in sequential mode. From a practical point of view, the user does not specify the total memory needed but the integer real and real memory required per processor. This can be estimated as --------------- ⋅ 1, 2 for the real mem- M n ory and Minteger for the integer memory. In case of parallel calculation the estimated number of real memory displayed by FINE™ on the page Control Variables shall not be followed but the formula shown above shall be respected. FINE 14-13 The Task Manager Task Management Using Scripts The following table states the total memory need for a parallel computation using respectively 4 and 6 and 8 processors. The values of Mreal and Minteger are set to 10 Mb and 1 Mb respectively. The equivalent memory request on a single processor is thus 11Mb. n 4 6 8 TABLE 14-1 Mtotal (Mb) 20 20.4 21.7 Parallel overhead (Mb) 9 9.4 10.7 Parallel memory request In the present implementation, the presence of the host processor increases the global memory request. It also reduces the overall speed-up of the computation as it is mainly dedicated to I/O management and no computation is affected to it. Future versions of EURANUS will optimize this aspect by removing gradually the need of a host processor. Message size limitation During initialization and final steps, large messages are usually exchanged between the nodes and the host process. In order to avoid any system failure, messages are split into buffers of maximum size. This size is set to 100000 by default but the user can eventually tune this value through the expert parameter MXBFSZ. 14-4.5 Troubleshooting If the computation is interrupted for an unknown reason, more detailed information is provided in the ’.std’ and ’.log’ computation files. The file contains all relevant informations including MPI error messages and should be sent to the NUMECA support team. 14-4.6 Limitations • The distributed memory mode is restricted to homogeneous (i.e. with the same operating system) clusters. • The number of processors should not exceed the number of blocks. 14-5 Task Management Using Scripts This section provides all available information to launch installed NUMECA Software from a shell, without using IGG™, AutoGrid, FINE™ or CFView™ interfaces. Every time a task is started a script file is automatically created. On UNIX the name of this file has the extension .batch and under Windows the extension is .bat. Such files contain text lines with the commands to launch the software with the appropriate command arguments. To launch a task from a shell simply execute the automatically generated file by typing its name in a shell. In the next sections the available commands to launch NUMECA software are described in more detail. Please notice that the capability to launch in batch is currently not supported for EURANUS in Parallel Mode on PC. 14-14 FINE Task Management Using Scripts The Task Manager 14-5.1 Launch IGG™ Using Scripts 14-5.1.1 How to Launch IGG™ on UNIX To launch IGG™ without use of the interface the commands to perform must be written in a macro script file. To create such a file: 1. 2. 3. Create a script file *.py. For more details on the commands that can be included in such a script file see the IGG™ manual. Set permission for execution for the script by using the command: "chmod 755 *.py". Launch the macro script in a shell by typing: igg -script /user/script.py -batch -niversion 62_7 The command line to start the grid generator IGG™ contains its name, the full path name of the script "*.py" file to launch and the IGG™ release that will be used. The "-batch" option avoids the display of the IGG™ graphical user interface. "igg SCRIPT_PATH/script.py -batch -niversion <version>" 14-5.1.2 How to Launch IGG™ under Windows 1. 2. 3. Create script file "*.py". For more detailed information on the commands to include in a macro script see the IGG™ manual. Set permission for execution of the file *.py Launch the macro script *.py by typing in a shell: d:\NUMECA_SOFTWARE\fine62_7\bin\igg.exe -script d:\user\test.py -batch The command line to start the grid generator IGG™ contains its full path name and the full path name of the script "*.py" file to launch. The "-script" & "-batch" options respectively permits to launch the script and avoids to display the IGG™ graphical user interface. "IGG_PATH\igg.exe -script SCRIPT_PATH\script.py -batch" REMARKS: • The full path name of the executable (igg.exe) has to be specified. • The full path name of the script has to be specified. • If there is a segmentation fault at exit (due to an incontrollable "opengl" problem), it is possible to avoid it by adding -driver msw option: d:\NUMECA_SOFTWARE\fine62_7\bin\igg.exe -script d:\test.py -batch -driver msw 14-5.2 Launch AutoGrid using Scripts 14-5.2.1 How to Launch AutoGrid on UNIX 1. 2. Create a template and geometry files (*.trb and *.geomTurbo) using the AutoGrid interface. Start AutoGrid to create a mesh from these files by typing: igg -batch -autoGrid /user/test.trb /user/test.geomTurbo /user/test.igg -niversion 62_7 The command line to start the grid generator AutoGrid contains its name, the full path name of the template, of the geometry files, the full path name of the mesh that will be saved and the IGG™ release that will be used. The "-batch" option avoids the display of the IGG™ graphical user interface. FINE 14-15 The Task Manager Task Management Using Scripts 14-5.2.2 How to Launch AutoGrid under Windows 1. 2. Create a template and geometry files (*.trb and *.geomTurbo) using the AutoGrid interface. Start AutoGrid to create a mesh from these files by typing on one line: d:\NUMECA_SOFTWARE\fine62_7\bin\igg.exe -batch -autoGrid c:\users\template.trb c:\users\template.geomTurbo c:\users\mesh.igg The command line to start the grid generator AutoGrid contains its full path name, the full path name of the template, of the geometry files and the full path name of the mesh that will be saved. The "-batch" option avoids the display of the IGG™ graphical user interface. 14-5.3 Launch EURANUS in Sequential using Scripts 14-5.3.1 How to Launch EURANUS in Sequential on UNIX 1. Create a script file (for example, with the name ’batch.sh’). Such a script file (e.g. ’batch.sh’) must be created with permission for execution to launch a series of computations. An example of a ’batch.sh’ file for a series of computations on UNIX: #! /bin/csh euranusTurbo /users/project/project_computation_1/project_computation_1.run -niversion 62_7 euranusTurbo /users/project/project_computation_2/project_computation_2.run -niversion 62_7 The script is started in a C-shell that is obtained by having as its first line: " #! /bin/csh". The command line, to start the flow solver EURANUS, contains its name, the full path name of the ’.run’ file to launch and the FINE™ release that will be used: "euranusTurbo COMPUTATION_PATH/computation.run -niversion <version>" 2. 3. Set Permission for execution for the script file ’batch.sh’ by typing the command: "chmod 755 batch.sh". Create an input file (’.run’) for each computation. To create those files through the FINE™ interface, click on the File/Save Run Files menu in order to save the ’.run’ file of the activated computation, after opening the corresponding project. Launch the script ’batch.sh’ by typing the script file name: ’./batch.sh’. When saving the ’.run’ file of the computation (File/Save Run Files) and launching the computation (Solver/Start...) killed just afterwards (Solver/Kill...), a new script ’.bat’ on WINDOWS (’.batch’ on UNIX) is created in the corresponding computation subfolder that enables the user to launch the same computation in batch. 4. 14-5.3.2 How to Launch EURANUS in Sequential under Windows 1. Create Script File ’.bat’. An example of ’.bat’ file for a series of computations on Windows: C:\NUMECA_SOFTWARE\fine62_7\bin\euranus.exe C:\users\project\project_computation_1\project_computation_1.run -seq C:\NUMECA_SOFTWARE\fine62_7\bin\euranus.exe \\ C:\users\project\project_computation_3\project_computation_3.run -seq \\ 14-16 FINE Task Management Using Scripts The Task Manager C:\NUMECA_SOFTWARE\fine62_7\bin\euranus.exe \\ C:\users\project\project_computation_2\project_computation_2.run -seq The command line, to start the flow solver EURANUS, contains its full path name, the full path name of the ’.run’ file to launch and the sequential mode selection: INSTALLATION_DIRECTORY\fine62_7\bin\euranus.exe COMPUTATION_PATH\project_computation_1.run -seq \\ 2. 3. Set Permission for Execution ’.bat’ Create an input file (’.run’) for each computation. To create those files through the FINE™ interface, click on the File/Save Run Files menu in order to save the ’.run’ file of the activated computation, after opening the corresponding project. Launch the script ’.bat’ by typing the script file name: ’.bat’ in a shell or double click on the ’*.bat’ file from the Windows Explorer. When saving the ’.run’ file of the computation (File/Save Run Files) and launching the computation (Solver/Start...) killed just afterwards (Solver/Kill...), a new script ’.bat’ on WINDOWS (’.batch’ on UNIX) is created in the corresponding computation subfolder that enables the user to launch the same computation in batch. 4. 14-5.4 Launch EURANUS in Parallel using Scripts 14-5.4.1 How to Launch EURANUS in Parallel using MPI on UNIX 1. Create a script file ’batch.sh’ with permission for execution. An example of a ’batch.sh’ file for a parallel computation on UNIX: #! /bin/csh euranusTurbo_parallel /users/project/computation/computation.run -niversion 62_7 -p4pg / users/project/hosts.p4pg The script is started in a C-shell that is obtained by having as its first line: " #! /bin/csh". The command line, to start the flow solver EURANUS in parallel, contains the script name that enables parallel computation, the full path name of the ’.run’ file to launch, the FINE™ release and the full path name of the file ’hosts.p4pg’ containing the definition of the machines that will be used to launch the computation in parallel: "euranusTurbo_parallel COMPUTATION_PATH/computation.run -niversion <version> -p4pg HOST_PATH/hosts.p4pg" The name of the executable is different from the one for sequential computations. 2. Create Hosts Definition File ’hosts.p4pg’. A file needs to be created to define the hosts (e.g. ’hosts.p4pg’). This file specifies the machine information regarding the various processes. An example of a ’hosts.p4pg’ file: Example 1: Hostname1 4 euranusTurbo62_7(master host on Hostname1 and 4 processes on Hostname1) Hostname2 2 euranusTurbo62_7(2 processes on Hostname2) FINE 14-17 The Task Manager Task Management Using Scripts Example 2: Hostname1 0 euranusTurbo62_7 (master host on Hostname1 and no other process on Hostname1) Hostname2 2 euranusTurbo62_7 (2 processes on Hostname2) For each machine, a line must be added consisting of the machine name (the machine hostname), the number of processes to run on the machine, the name of the executable and the FINE™ release: "hostname 4 euranusTurbo<version>" If additional machines are to be used, subsequent lines are required for each one. If the number of processors is set to 0 for the first machine (first line of the ’hosts.p4pg’ file), only the master host process will run on that machine while the nodes will run on the next machines declared in the following lines. The first machine (hostname) specified in the file ’hosts.p4pg’ should be the one from which the script will be launched. The total number of processes defined in the file ’hosts.p4pg’ should be equal to the number of nodes running. 3. Set permission for execution ’batch.sh’ by using the command: "chmod 755 batch.sh" Create input files ’.run’ to launch the computation. The parallel settings of the computational file (’.run’) are managed by the Task Manager. Therefore before launching the parallel computation script, the following steps must be performed through the FINE™ interface: 4. 5. Create computational file (’.run’) by activating the corresponding computation and clicking on the File/ Save Run Files menu in the interface. To set the final parallel settings: — — — — 6. create a task in the Task Manager, define the parallel settings of EURANUS subtask (parallel computation), launch the task through the Task Manager by clicking on Start, kill the task when EURANUS flow solver starts by clicking on Stop. This operation is mandatory in order to have all the parallel settings correctly imposed in the computation file (’.run’). Launch the script ’batch.sh’ by typing the script file name: "./batch.sh". When saving the ’.run’ file of the computation (File/Save Run Files) and launching the computation in parallel as explained in step 5 through the Task Manager (Modules/Task Manager) and killed it just afterwards, a new script ’.batch’ and a file ’.p4pg’ are created in the corresponding computation subfolder that enable the user to launch the same computation in batch and in parallel. 14-5.4.2 How to Launch EURANUS in Parallel using MPI on Windows 1. Create a script file ’batch.bat’ with permission for execution. An example of a ’batch.bat’ file for a parallel computation on Windows: D:\NUMECA_SOFTWARE\Fine62_7\bin\mpirun.exe "D:\test\test_computation_1\test_computation_1.p4pg" "D:\test\test_computation_1\test_computation_1.run" / / The command line, to start the flow solver EURANUS in parallel, contains the script name that enables parallel computation, the full path name of the ’.run’ file to launch and the full path name of the file ’.p4pg’ containing the definition of the machines that will be used to launch the computation in parallel: 14-18 FINE Task Management Using Scripts The Task Manager "NUMECA_RELEASE_PATH/mpirun.exe HOST_PATH/hosts.p4pg COMPUTATION_PATH/computation.run " 2. Create Hosts Definition File ’.p4pg’. A file needs to be created to define the hosts (e.g. ’hosts.p4pg’). This file specifies the machine information regarding the various processes. An example of a ’hosts.p4pg’ file: Example 1: Hostname1 5 D:\NUMECA_SOFTWARE\Fine62_7\bin\euranus.exe (master host on Hostname1 and 4 processes on Hostname1) Hostname2 2 D:\NUMECA_SOFTWARE\Fine62_7\bin\euranus.exe(2 processes on Hostname2) Example 2: Hostname1 1 D:\NUMECA_SOFTWARE\Fine62_7\bin\euranus.exe (master host on Hostname1 and no other process on Hostname1) Hostname2 2 D:\NUMECA_SOFTWARE\Fine62_7\bin\euranus.exe (2 processes on Hostname2) For each machine, a line must be added consisting of the machine name (the machine hostname), the number of processes to run on the machine, the name of the executable and the FINE™ release: "hostname 4 NUMECA_RELEASE_PATH\bin\euranus.exe" If additional machines are to be used, subsequent lines are required for each one. If the number of processors is set to 1 for the first machine (first line of the ’.p4pg’ file), only the master host process will run on that machine while the nodes will run on the next machines declared in the following lines. The first machine (hostname) specified in the file ’.p4pg’ should be the one from which the script will be launched. The total number of processes defined in the file ’.p4pg’ should be equal to the number of nodes running. 3. Set permission for execution ’batch.bat’ Create input files ’.run’ to launch the computation. The parallel settings of the computational file (’.run’) are managed by the Task Manager. Therefore before launching the parallel computation script, the following steps must be performed through the FINE™ interface: 4. 5. Create computational file (’.run’) by activating the corresponding computation and clicking on the File/ Save Run Files menu in the interface. To set the final parallel settings: — — — — 6. create a task in the Task Manager, define the parallel settings of EURANUS subtask (parallel computation), launch the task through the Task Manager by clicking on Start, kill the task when EURANUS flow solver starts by clicking on Stop. This operation is mandatory in order to have all the parallel settings correctly imposed in the computation file (’.run’). Launch the script ’batch.bat’ by typing the script file name: "./batch.bat" in a DOS-shell. When saving the ’.run’ file of the computation (File/Save Run Files) and launching the computation in parallel as explained in step 5 through the Task Manager (Modules/Task Manager) and killed it just afterwards, a new script ’.bat’ and a file ’.p4pg’ are created in the corresponding computation subfolder that enable the user to launch the same computation in batch and in parallel. FINE 14-19 The Task Manager Task Management Using Scripts 14-5.4.3 How to Launch EURANUS in Parallel using SGE on UNIX 1. Create a script file ’batch.sge’ with permission for execution. An example of a ’batch.sge’ file for a parallel computation on UNIX: #! /bin/csh #$ -S /bin/sh #$ -o /home/sgeuser/parallel_sge/parallel_sge_computation_1/ parallel_sge_computation_1.std -j y #$ -N comput1 #$ -pe numecampi 3 #$ -notify P4_GLOBMEMSIZE=15000000 Export P4_GLOBMEMSIZE NI_VERSIONS_DIR=/usr/numeca MPIR_HOME=$NI_VERSIONS_DIR/_mpi cd /home/sgeuser/parallel_sge/parallel_sge_computation_1 $MPIR_HOME/bin/mpirun -np $NSLOTS -machinefile $TMPDIR/machines \ $NI_VERSIONS_DIR/bin/euranusTurbo62_7 \ /home/sgeuser/parallel_sge/parallel_sge_computation_1/parallel_sge_computation_1.run where: #$ -S /bin/sh requires Bourne shell to be used by SGE for job submission and hence, only the .profile file of the user is executed if exists on each computation host. There is nothing specific to Numeca software that must be written . the .profile file. #$ -o /home/sgeuser/parallel_sge/parallel_sge_computation_1/ parallel_sge_computation_1.std -j y tells SGE system that the standard output has to be redirected in the ".std" in the computation directory, the option "-j y" indicates that the standard error is redirected into the same file. #$ -N comput1 is the name of the job given to SGE and that will be seen when monitoring the job with the graphical monitoring utility qmon (Job Control button ) or with the qstat SGE command. SGE has a limitation of 8 characters for the job name. #$ -pe numecampi 3 requests 3 slots (processors) to the SGE system for executing the job using the numecampi parallel environment described in chapter 2.1. This must correspond to NTASK +1 where NTASK is the number of computation processes in the ".run" file, the "+1" being the host process that manages inputs/outputs. #$ -notify gives a delay between the send of the SIGKILL signal and SIGUSR2 signal. The delay is defined in the SGE interface. P4_GLOBMEMSIZE=15000000 Export P4_GLOBMEMSIZE NI_VERSIONS_DIR=NUMECA_RELEASE_PATH MPIR_HOME=$NI_VERSIONS_DIR/_mpi are the environment variables indicating respectively the Numeca software installation directory and the mpi directory that are used in the following command: 14-20 FINE Task Management Using Scripts The Task Manager $NSLOTS is the number of slots (processors) that have been allocated by SGE for the job, $TMPDIR is generated by SGE for providing the machines file used by the mpirun script. $NI_VERSIONS_DIR/bin/euranusTurbo is a symbolic link to the numeca_start startup script for all Numeca softwares and 62_7 is the version of the code that will be used and requires that it is installed under /NUMECA_RELEASE_PATH/fine62_7. /home/sgeuser/parallel_sge/parallel_sge_computation_1/parallel_sge_computation_1.run is the argument to the euranusTurbo executable. For sequential runs, the line "#$ -pe numecampi 3" must be removed and the final command must be: $NI_VERSIONS_DIR/bin/euranusTurbo62_7 \ /home/sgeuser/ parallel_sge/parallel_sge_computation_1/parallel_sge_computation_1.run -seq 2. Set permission for execution ’batch.sge’ by using the command: "chmod 755 batch.sge" Create input files ’.run’ to launch the computation. The parallel settings of the computational file (’.run’) are managed by the Task Manager. Therefore before launching the parallel computation script, the following steps must be performed through the FINE™ interface: 3. 4. Create computational file (’.run’) by activating the corresponding computation and clicking on the File/Save Run Files menu in the interface. To set the final parallel settings: — — — — create a task in the Task Manager, define the parallel settings of EURANUS subtask (parallel computation), launch the task through the Task Manager by clicking on Start, kill the task when EURANUS flow solver starts by clicking on Stop. This operation is mandatory in order to have all the parallel settings correctly imposed in the computation file (’.run’). 5. Launch the script ’batch.sge’ by typing the script file name: "./batch.sge". When saving the ’.run’ file of the computation (File/Save Run Files) and launching the computation in parallel as explained in step 4 through the Task Manager (Modules/ Task Manager) and killed it just afterwards, a new script ’.sge’ is created in the corresponding computation subfolder that enables the user to launch the same computation in batch and in parallel. 14-5.5 Launch CFView™ Using Scripts 14-5.5.1 How to Launch CFView™ on UNIX 1. Create a macro file ’.py’. For more details see the CFView™ for more detailed information on the format of a macro file and the commands that can be included in a macro file. 2. Launch the macro ’.py’ by typing: cfview -macro /user/test.py -batch -niversion 62_7 The command line to start CFView™ contains its name, the full path name of the macro ’.py’ file to launch and the CFView™ release that will be used. The ’-batch’ option avoids the display of the CFView™ graphical user interface. "cfview -macro MACRO_PATH/macro.py -batch -niversion <version>" 14-5.5.2 How to Launch CFView™ on PC under Windows 1. Create a macro file ’.py’. For more details see the CFView™ for more detailed information on the format of a macro file and the commands that can be included in a macro file. FINE 14-21 The Task Manager Limitations 2. Launch the macro ’.py’ by typing: d:\NUMECA_SOFTWARE\fine62_7\bin\cfview.exe -macro \user\test.py -batch The command line to start CFView™ contains its full path name and the full path name of the macro ’.py’ file to launch. The ’-batch’ option avoids the display of the CFView™ graphical user interface. 14-5.5.3 Command Line Arguments The command cfview may be followed by a set of command line arguments. Those command line arguments allow to override some system defaults (used driver, display, double-buffering and update abort options) or to specify files to be loaded immediately (project, macro, defaults settings, macro module). The supported command line arguments are: -help prints a summary of the command line arguments, -version prints the CFView™ version number, -date prints the CFView™ version date, -defaults <file name> starts CFView™ with the default settings from the specified file, -project <file name> starts CFView™ and opens immediately the specified project, -macro <file name> starts CFView™ and execute the specified macro script, -macromodule <file name> starts CFView™ and load the specified macro module, -display <display name> starts CFView™ on the specified display device, -doublebuffering on (off) activates (disables) double buffering, -updateabort on (off) activates (disable) update aborting (see the CFView™ manual for more detail on this option), -driver <driver name> starts CFView™ with the specified graphics accelerator, -reversevideo on (off) starts CFView™ with black (white) background color (see the CFView™ manual for more detail on this option), -facedisplacement <n> starts CFView™ with the specified face displacement (see the CFView™ manual for more detail on this option), -loaddata all (none, ask) when opening a project the quantities fields are loaded in the computed memory (are not loaded, a specific dialog box is raised where the user choose the field variables to be loaded). The defaults is to load all field quantities. (see the CFView™ manual for a description of the data management facility and of the associated dialog box), -batch on (off) starts CFView™ without graphical user interface. This mode can be used in combination with the -macro command line option in order to perform the execution of a macro script without user interaction, -hoops_relinquish_memory off this option disables the hoops garbage collection feature that is activated when CFView™ is idle during a long period of time. 14-6 Limitations The task manager have some limitations due to the current PVM and MPI libraries: 14-22 FINE Limitations The Task Manager • UNIX to PC connections are not allowed. • The remote copy works only if there is enough disk space on the remote machine. Currently, no check is performed to identify the available disk space and the flow solver crashes with "undifined reason". • Parallel computation with distributed memory are only available on homogenous UNIX/Windows platforms. • When a user launches FINE™ on different machines, the connection between these machines is not allowed as described in section 14-2.1.1. FINE 14-23 The Task Manager Limitations 14-24 FINE CHAPTER 15:Computation Steering and Monitoring 15-1 Overview This chapter describes the Computation Steering pages and the additional tool MonitorTurbo. First section 15-2 describes the Computation Steering/Control Variables page. Furthermore this chapter is completely dedicated to the monitoring tools available in FINE™ to monitor the global solution during and after a computation: • Computation Steering/Convergence History and Task Manager/Convergence History, see section 15-3 and • MonitorTurbo, see section 15-4. In section 15-5 advice is provided on how to use the monitoring tools in analysing the progress of a computation. 15-2 Control Variables The Computation Steering/Control Variables page allows to define some global parameters for the selected computation: • the Maximum Number Of Iterations on the finest grid level (i.e. not including the iterations performed during coarse grid initialization). • the Convergence Criteria corresponding to the (negative) number of orders of magnitude the norm of the residuals must decrease before stopping the calculation. If this criterium is not reached the calculation proceeds until the maximum number of iterations is performed. • The frequency for saving output (Save Solution Every): every x iterations the solver saves the flow solution and creates the output files to be read in CFView™(where x is the number of iterations defined in the FINE™ interface). • When the option Mimimum output is selected the solution is only saved at the last iteration. • the Memory Requirements for the computation. By default an estimation is given for the required memory. Depending on the parameters defining the computation additional memory may be needed. For example, more memory is required when full non-matching connections FINE™ 15-1 Computation Steering and Monitoring Convergence History or a k-ε turbulence model is used. Also the amount of selected output may require more memory. To allocate more memory for the computation select the button Set the requested memory. This will allow to define the amount of memory in Mb used for reals and integers. For unsteady computations the Control Variables page is updated to give access to additional parameters as described in section 4-2.1 and section 4-2.3. Furthermore this page contains in expert mode two lists of expert parameters. Only the expert parameters that are described in the manual are supported. Use of the other parameters is not recommended. For a summary of all supported expert parameters see Appendix C. 15-3 Convergence History The Computation Steering/Convergence History or Task Manager/Convergence History page allows the user to define quantities to be followed during the convergence process of the flow solver EURANUS. This pages is divided in 5 areas as shown in Figure 15.3.0-1: 1. 2. 3. 4. 5. The steering files selection (Select Computations) and the curves export (Export Curves To File...) only available in Task Manager/Convergence History page. The available variables (Available Variables). The parameters (Parameters type). The selected variables (Selected Variables). The graphics view (Convergence History). (2) (1) (3) (4) (5) FIGURE 15.3.0-1The five areas of the Convergence History page 15-2 FINE™ Convergence History Computation Steering and Monitoring When the flow solver EURANUS is invoked, a communication is automatically established with FINE™ allowing the user to follow the selected quantities. Two representations of the quantities are currently available: the convergence curves displayed in the area 5 and the quantity value at the last iteration in the area 4. All these data are stored in files with extension .steering and .steering.binary. These files are created and managed automatically by FINE™ If the communication between the flow solver and FINE™ is interrupted (i.e.: network problem), parts of the convergence curves can be lost. 15-3.1 Steering Files Selection and Curves Export Different mode exists for the selection of the current steering results stored in the steering files: 1. When a project is opened, the active computation steering files is automatically selected and appears in the Add or select computations window (a) appearing when clicking on Select Computations button. Each time a new computation is selected, the associated steering file is automatically loaded and becomes the active one. (a) (b) (c) (d) FIGURE 15.3.1-2Steering 2. 3. 4. 5. files selection area All the steering files already loaded can be selected by <Ctrl>-leftclick and <Shift>-leftclick in the list of available computations. The file can also be loaded manually using the button Add Computation (c). A file chooser prompts the user to select the file. The button Remove Computation allows the user to remove from the memory the selected computation (the file is not removed and remains available for selection). Additionally, when a task is started, the steering files of the flow solver computation called in the task are automatically loaded and become available through the list (b). The Export Curves To File... button enables the user to save in an ASCII file ’.cvh’ all the curves plotted in the Graphics View. 15-3.2 Available Quantities Selection The available quantities selected by default are linked to the type of computation. For example, when launching a turbomachinery computation, the global residual, the inlet and outlet mass flow, the efficiency, the pressure ratio, the axial thrust and the Torque are computed during the convergence process. The Available Quantities list (b) allows the user to select and add (c) new quantities to the computed list FINE™ 15-3 Computation Steering and Monitoring Convergence History . (a) (b) (c) FIGURE 15.3.2-3Available quantities selection area All the quantities can be added before or during the computation. When a quantities has been added, it appears in the selection list and becomes the selected quantity. If the flow solver is running, the value and the convergence curve of the new quantities is displayed after a few seconds. The convergence curve begins at the iteration corresponding to the moment when the new quantity has been added in the Selected Variables list. When a quantity is added for selection it appears in the selection list with a number behind the name. This number is only added to avoid to have two times the same variable name in the list. This is especially necessary when, for example, the static pressure is monitored at two different points in the domain. 15-3.3 New Quantity Parameters Definition When a new quantity has been added, it becomes available for selection in the Selected Variables list (area 4 in Figure 15.3.0-1). The user can select the way the flow solver computes the quantity through the parameter type area (area 2 in Figure 15.3.0-1). Several types of parameters can be chosen through the parameter type list box (a in Figure 15.3.3-4). The available types of parameters that can be defined to computed the selected quantities: 1. 2. global: the computed variable is averaged over all the domain. local 3d grid point: the user specify the grid point indices (I,J,K) and the block index (block id) where the quantity must be computed. (a) FIGURE 15.3.3-4Parameter type definition Care should be taken when using the steering of a parameter on a local 3d grid point. It should be carried out in the following way: - select the parameter (relative velocity u, static pressure...). - add for selection. It becomes available for the selected variables. 15-4 FINE™ Convergence History Computation Steering and Monitoring - set the block id and the I,J,K indices of the grid point on which the evolution of the selected parameter will be visualized. All the user modifications (I,J,K indices...) can also be done (and modified) during the computation run. 15-3.4 Quantity Selection Area When a quantity has been added, it becomes available for selection in the Selected Variables list. The list is divided in 3 columns as shown in Figure 15.3.4-5: the variable name (a) which can be changed using the button rename (d) , the quantity value (b) which displays the last computed value and the units (c) of the variable. The button remove (e) is used to remove the first selected variable. . (a) (d) (b) (c) (e) FIGURE 15.3.4-5Selected variables area When a quantity is not yet computed, the value indicated is undefined. Selecting a quantity will show its history in the graphics view as described in the next paragraph. To select multiple quantities click on them (with the left mouse button) in the list while holding the <Ctrl> or <Shift> key. To select quantities that are next to each other in the list simply click on the first one and keep the mouse button pressed while moving to the last variable. 15-3.5 Definition of Global Residual The residuals are computed by EURANUS as a flux balance (the sum of the fluxes on all the faces of each cell): RES = ∑ fluxes . , ⎠⎠ ⎞⎞ ⎝ ⎛ (15-1) The root mean square of the residuals is computed with the following formula: RES RMS RES = log RMS ---------------------------cellvolume and the maximum of the residuals in the same way: ⎠ ⎞ ⎝ ⎛ (15-2) RES MAXRES = log MAX ---------------------------cellvolume ⎝ ⎛ , (15-3) FINE™ 15-5 Computation Steering and Monitoring Convergence History with log the logarithm to the base ten. On the Computation Steering/Convergence History or Task Manager/Convergence History page, the global root mean square of the residuals normalized by its value at the first iteration is shown. These values are stored in the file with extension .steering.binary. Additionally the global residuals are shown in numerical values in the Task Manager window (3rd column). The RMS value listed in the Task Manager window is the global root mean square normalized by its value at the first iteration: RMSRES-(RMSRES)it=1. The maximum value (4th column) is the maximum residual at a certain iteration normalized by the RMS residual at the first iteration: MAXRES-(RMSRES)it=1. FIGURE 15.3.5-6Task Manager window 15-3.6 The Graphics View (a) (b) FIGURE 15.3.6-7Graphics view area in Computation Steering/Convergence History page 15-6 FINE™ MonitorTurbo Computation Steering and Monitoring The convergence history of the selected curves are displayed inside the graphics view. In the Computation Steering/Convergence History page, the color of the curves is different (up to 8 selected quantities). The automatic chosen curves colors are also used for the displayed value (a). Additionally, the error between the two first selected quantities is also indicated (b). This is especially important for checking the difference between the mass flow at inlet and outlet (Figure 15.3.6-7). In the Task Manager/Convergence History page, the color of the curves is the same (but with different markers) if related to the same computation and is different for each curves if related to different computations (up to 10 selected quantities). FIGURE 15.3.6-8Graphics view area in Task Manager/Convergence History page 15-4 MonitorTurbo 15-4.1 Introduction The MonitorTurbo can be launched independently from FINE™ in order to facilitate the batch mode control. It is a separate graphic control window in which the user can visually monitor: • the convergence history of one or several computations (Convergence history), • the blade loading distribution (Loading diagram available with FINE™/Design 2D only), • the blade profile (Blade profile available with FINE™/Design 2D only). The two last displays are only available under the FINE™/Design 2D environments, as described in Chapter 12 and Chapter 13. This section only describes the functionalities of the convergence history display. FINE™ 15-7 Computation Steering and Monitoring MonitorTurbo On UNIX and LINUX platforms type: monitorTurbo -print <Enter> When multiple versions of FINE™ are installed the installation note should be consulted for advice on how to start FINE™ in a multi-version environment. On Windows click on the Monitor icon in Start/Programs/NUMECA software/fine#. Alternatively FINE™ can be launched from a dos shell by typing: <NUMECA_INSTALLATION_DIRECTORY>\fine#\bin\monitor <Enter> FINE™ allows multi-process analyses. Therefore, the convergence histories of multiple (running) projects can be visualized at the same time. It is also possible to compare the convergence history associated with different computational parameters for the same project. The monitored variables are displayed as a x-y graph in the upper part of the window (a). The xaxis represents the number of multigrid cycles or work units (see section 15-4.3.3 and Section B4.3) achieved by the flow solver. The y-axis is a logarithmic axis representing the power of ten of the residual values. The user can choose the residual of any of the equations solved and some global parameters using the buttons visible in the lower right part of the graphic control window (b) as shown in Figure 15.4.1-9. The lower part of the graphic control window contains four boxes. The small box (c) located on the left side contains a Print button (which allows to save the current graph as a postscript file) and a Quit button (which allows to close the MonitorTurbo window). The three other boxes are described in the next sections. . (a) (c) (b) FIGURE 15.4.1-9The monitorTurbo window 15-8 FINE™ MonitorTurbo Computation Steering and Monitoring 15-4.2 The Residual File Box Three buttons are provided in this box to Add, Remove or Activate residual files through a file chooser. The residual files describe the iteration process of previous or current computations. They contain the history for internal flow of the axial thrust, mass flow, torque, efficiency, pressure ratio (lift, drag and momentum coefficients if external flow) and the residuals of five (seven or six if respectively the k-ε or the Spalart-Allmaras turbulence model is used) physical variables. The activation of a part of the residual files ’.res’ has the effect of deactivating the other loaded residual files. When a residual file is deactivated, its associated convergence history is not displayed. The selective activation of residual files allows thus to display only the convergence histories of some of the loaded residual files ’.res’. The input boxes File and Block, visible just below the three buttons Add, Remove and Activate, allow to select for which file and block the choice of the monitored variables performed in the Quantities to display menu should be applied. 15-4.3 Quantities to Display 15-4.3.1 Residuals Buttons are provided to select the type of residuals: rms or maximum as shown in Figure 15.4.1-9 on the right. The residuals relative to all transport equations of the problem are available: these are the continuity, the momentum, the energy, and eventually the turbulent kinetic energy k and the turbulent dissipation ε (if the turbulent computation is using a k-epsilon model, e.g. not for Baldwin Lomax), and the turbulent kinematic viscosity nu (if the Spalart-Allmaras model is used) or the blade force for a throughflow application. While the Computation Steering/Convergence history or Task Manager/Convergence History page displays only the global residual, the MonitorTurbo gives the RMS and maximum values per block. Computation of the RMSRES and MAXRES values is done according to Eq. 15-1 to Eq. 15-3. The values shown in the MonitorTurbo for the RMS are normalized by the value of RMSRES at the first iteration: RMSRES-(RMSRES)it=1. The values shown for the maximum residuals are normalized by the maximum residual at the first iteration: MAXRES-(MAXRES)it=1. Since the RMS and maximum residuals are normalized differently it may occur that the RMS value shown in the MonitorTurbo is higher than the maximum residual. 15-4.3.2 Global Quantities Several buttons are provided to visualize the additional global quantities available under the environment FINE™/Turbo: • Internal flow problems (expert parameter IINT=1): The axial thrust, the (inlet and outlet) mass flows, torque, pressure ratio, and efficiency. • External flow problems (expert parameter IINT=0): The drag, the lift and the momentum coefficients. The user has to specify the axis that has to be taken into account for these global quantities as described in section 11-3. If several computations are performed at the same time, the curves associated with the different projects are drawn in different colors. The buttons of the present box act only on the curves of the file and block selected through the File and Block menu. FINE™ 15-9 Computation Steering and Monitoring Best Practice for Computation Monitoring 15-4.3.3 Display Options The Legend button is used to display which files are currently activated. In addition, if the mass flow button is activated, the relative errors between the inlet and the outlet are indicated. The Work Unit button is provided to set the type of unit used on the horizontal axis in the MonitorTurbo window: multigrid cycles or work units. If Cycles option is chosen (Work Unit button deactivate), the abscissa will show the number of iterations, Work Unit option will adapt the values on the horizontal axis with respect to the grid levels (if 3 grid levels are used, one iteration on 222 and 111 is taking respectively 1/64s and 1/8s considering that one iteration on 000 is taking 1s. The Update now button updates the graph for the active residual file and the selected block. The Auto update button can be switched on to follow the iteration processes automatically. It is however a rather time-consuming option and this button is not active by default. 15-4.3.4 Zooming Option This option allows to interactively zoom in and out: 1. 2. 3. 4. In the drawing window, press the left mouse button to initiate a zooming operation, Then drag the mouse to the left or to the right to zoom in, the zooming window number is displayed on the screen, Click again on the left button when finished, To zoom out, click on the right button of the mouse. 15-5 Best Practice for Computation Monitoring 15-5.1 Introduction Several tools are available in the FINE™/Turbo package to follow the evolution of a calculation: • the Convergence History page available in FINE™/Turbo and in the Task Manager module, which allows to follow the evolution of a calculation easily and to compare globally the evolution of multiple computations. • Another useful tool is the MonitorTurbo to compare per equation the evolution of multiple computations and per block in the domain. • CFView™ to enter even into more detail. Each of them has its own specific features, but they are very complementary. This section describes how to use those tools to monitor a computation. For a detailed description of the use of CFView™ see the separate CFView™ user’s guide. When a computation has just been launched for the first time, and initialization steps have been properly passed, the solver writes a first solution file. In fact it is not yet a solution but only the result of the initialization. Still this first output is interesting to check if all boundaries conditions have been set correctly. Especially think to have a look at the rotating elements of the machine, the profiles of velocities at inlet and at outlet. This operation aims to detect a user mistake, which could cause a loss of time, like for example, a forgotten patch. To check this first output use CFView™. To check the rotating part of the machine, select the rotating walls (hub or shroud for rotating walls) using the menu item Geometry/Select Surfaces and select for the quantity the velocity. Using the 15-10 FINE™ Best Practice for Computation Monitoring Computation Steering and Monitoring Representation menu the velocity will be displayed on the selected patches and this will be the rotation speed everywhere. 15-5.2 Convergence History The global residual on the Convergence History page allows to see quickly whether the computation is iterating properly. The residuals should go down first on the coarser grid levels of the Full Multigrid strategy as shown in Figure 15.5.2-10. See Chapter 9 for more detail on Full Multigrid. When going to a finer grid level the global residual increases suddenly to decrease immediately after. When the computation reaches the finest grid, the curve of the global residual should normally decrease gradually. In general a fall of 3 orders with a stabilization of this curve is considered as a good convergence. But it is important to check if other global quantities like mass flow, efficiency, pressure ratio are also stabilized and to compare the differences between massflow at inlet and outlet (in general a difference of less than 5% is acceptable). FIGURE 15.5.2-10Example of convergence history for global residuals 15-5.3 MonitorTurbo The MonitorTurbo follows the same quantities as the Convergence History, but its main interest is to offer the possibility to follow the convergence block by block. Thus, one can localize problems and, if necessary, modify the mesh in the region associated to the block, or change a boundary condition. Finally, coming back to the Task Manager, it is possible to get a deeper control, locally, by adding control points (local 3d grid point). These points allow to track in important parts of the domain, the speed, the pressure and turbulent quantities, which could be a requested information sometimes. In the case of steady computations, the values associated to these points should converge to a constant value. One additional advice is to use CFView™ during the computation with intermediate and non-converged solutions. When having convergence problems for example CFView™ may be used to look for the zones were the residuals have too high values compared to other regions or an incorrect turbulence field. To know in which block(s) the residuals start to increase first in case of divergence problem, the MonitorTurbo may already give an indication. Combining the information from the FINE™ 15-11 Computation Steering and Monitoring Best Practice for Computation Monitoring MonitorTurbo and CFView™ allows to find the cause of convergence problems in the computations. 15-5.4 Analysis of Residuals In some cases it may occur that the MonitorTurbo shows high RMS and maximum values of the residuals in a certain block while CFView™ shows high residuals in a different block. This difference between the two tools is caused by the different ways of representing the residuals. In CFView™ the absolute values of the residuals resulting from the flux balance are directly plotted for each cell. In CFView™ the residuals are not scaled with the cell volumes and no normalization with values at the first iteration is applied. This explains why some high maximum residuals in scaled mode can be invisible in CFView™ because they occur in small cells. Also the fact that the residuals are computed on the cell centers in the solver and shown in CFView™ on the cell corners may lead to some, minor, interpolation differences. 15-12 FINE™ APPENDIX A:Governing Equations A-1 Overview The flow solver integrated into the FINE™ user environment is named EURANUS ("EURopean Aerodynamic NUmerical Simulator"). EURANUS is a multipurpose code for 2D and 3D flows in complex geometries, using the latest numerical developments in CFD. A structured mesh is required and complex geometries can be easily handled through a flexible multiblock meshing procedure. This appendix describes the basic governing equations solved in EURANUS. For more detailed information on the different aspects like turbulence, fluid modeling, multi grid strategy etc., see the related chapters in this manual. A-2 Reynolds-Averaged Navier-Stokes Equations A-2.1 General Navier-Stokes Equations The general Navier-Stokes equations written in a Cartesian frame can be expressed as: ∂ U + ∇F I + ∇F V = Q , ∂t where U is the vector of the conservative variables: ρ U = ρv , ρE (A-2) (A-1) F I and F V are respectively the inviscid and viscous flux vectors: FINE™ A-1 Governing Equations Reynolds-Averaged Navier-Stokes Equations ρv i ρv 1 v i + pδ 1i F li = ρv 2 v i + pδ 2i and – F vi = ρv 3 v i + pδ 3i ( ρE + p )v i where the stress and the heat flux components are given by: 0 τ i1 τ i2 τ i2 q i + v j τ ij , (A-3) ˜ ˜ ∂w ∂w τ ij = ( µ + µ t ) -------i + -------j – 2 ( ∇w )δ ij - -∂x j ∂x i 3 and q i = ( κ + κ t ) Q contains the source terms: 0 Q = ρf e , Wf ∂ ˜ T. ∂xi (A-4) (A-5) (A-6) with f e expressing the effects of external forces and W f the work performed by those external forces: W f = ρf e ⋅ v . Other source terms are possible, like gravity, depending on the chosen functionalities. A-2.2 Time Averaging of Quantities The Navier-Stokes equations are averaged in time. The density and the pressure are time averaged related to the instantenous value through: q = q + q' where where q is the time averaged value and q' the fluctuating part and q' = 0 The energy, velocity components and temperature are density weighted averages defined as: ρq ˜ q = ----ρ (A-9) (A-8) (A-7) A-2.3 Treatment of Turbulence in the Equations Except for the non-linear k-ε turbulence model, a first-order closure model based on Boussinesq's assumption, is used: – ρw i ″w j ″ = µ t ˜ ˜ ∂w i ∂w j 2 2 - ˜ + – -- ( ∇w )δ ij – -- ρkδ ij ∂ xj ∂ x i 3 3 (A-10) A-2 FINE™ Formulation in Rotating Frame for the Absolute Velocity Governing Equations with w i the xi component of the relative velocity. In this equation k is the turbulent kinetic energy and is defined as: 1 k = -- ρw i ″w i ″ ⁄ ρ . 2 (A-11) In contrast to the laminar case, both the static pressure and the total energy contain contributions from the turbulent kinetic energy k and are defined as: 2 p* = p + -- ρk , 3 ˜ ˜ 1˜ ˜ E = e + -- w i w i + k 2 (A-12) (A-13) Note that Eq. A-13 does not contain a term in the angular velocity. This term is accounted for in the source term, and assuming stationary flow, corresponds to the last term of Eq. A-15. A-2.4 Formulation in Rotating Frame for the Relative Velocity The resulting time averaged Navier-Stokes equations for the relative velocities in the rotating frame of reference become: ρ ˜ ρw 1 ˜ U = ρw 2 ˜ ρw 3 ˜ ρE ˜ ρw i ˜ ˜ p*δ 1i + ρw i w 1 ˜ ˜ F Ii = p*δ 2i + ρw i w 2 ˜ ˜ p*δ 3i + ρw i w 3 ˜ ˜ ( ρE + p* )w i – F vi = 0 τ i1 τ i2 τ i3 ˜ q i + w j τ ij (A-14) where the shorthand notation , i, in the Fvi expression, is used to denote derivatives with respect to x i . The source term vector Q contains contributions of Coriolis and centrifugal forces and is given by: 0 Q = ( – ρ ) [ 2ω × w + ( ω × ( ω × r ) ) ] ρw∇ ( 0.5ω r ) with ω the angular velocity of the relative frame of reference. 2 2 (A-15) A-3 Formulation in Rotating Frame for the Absolute Velocity Although the governing equations for rotating systems are usually formulated in the relative system and solved for the relative velocity components, the formulation retained for ship propeller applications or ventilators are often expressed in the relative frame of reference for the absolute velocity FINE™ A-3 Governing Equations Formulation in Rotating Frame for the Absolute Velocity components. This formulation is different from the one generally used to solve internal turbomachinery problems, where the equations are solved for the relative velocity. The two formulations should lead to the same flow solution. However, experience shows that the solution can be different, especially in the far field region. For propeller problems, the formulation based on relative velocities has the disadvantage that the far field relative velocity can reach high values. This induces an excess of artificial dissipation leading to a non physical rotational flow in the far field region, this dissipation being based on the computed variables. This formulation is controlled by the expert parameter IVELSY=0. This formulation is valid only if all boundary conditions are uniform in the azimuthal direction. If the flow field boundary conditions are not uniform in the azimuthal direction, the boundary conditions expressed in this formulation must be unsteady. In this case, the formulation for the relative velocity is suggested. Except for the non-linear k-ε turbulence model, first-order closure, based on Boussinesq's assumption, is used for the Reynolds stress: ˜ ˜ ∂v i ∂v j 2 2 - ˜ + – -- ( ∇v )δ ij – -- ρkδ ij 3 ∂ xi ∂ xi 3 – ρv i ″v j ″ = µ t (A-16) with v i the xi component of the absolute velocity. The flux vectors are decomposed into Cartesian components: F I = f I1 1 x + f I2 1 y + f I3 1 z F v = f v1 1 x + f v2 1 y + f v3 1 z (A-17) and ρ ˜ ρv 1 ˜ U = ρv 2 ˜ ρv 3 ˜ ρE ˜ ρw i ˜ ˜ p*δ 1i + ρw i v 1 ˜ ˜ F Ii = p*δ 2i + ρw i v 2 ˜ ˜ p*δ 3i + ρw i v 3 ˜˜ ˜ ρE w i + p*v i – F vi = 0 τ i1 τ i2 τ i3 ˜ q i + v j τ ij (A-18) where the shorthand notation , i, in the Fvi expression, is used to denote derivatives with respect to x i . The velocity w i is the xi component of the relative velocity. This formulation envolves thus both the absolute and the relative velocity components. The source term vector Q is given by: 0 Q = –ρ( ω × v ) , 0 with ω the angular velocity of the relative frame of reference. Other source terms are possible, like gravity, depending on the chosen functionalities. (A-19) A-4 FINE™ Formulation in Rotating Frame for the Absolute Velocity Governing Equations The averaged Navier-Stokes equations are obtained by the Favre averaging as described in section A-2.2. In contrast to the laminar case, both the static pressure and the total energy contain contributions from the turbulent kinetic energy k and are defined as: 2 p* = p + -- ρk , 3 ˜ ˜ 1˜ ˜ E = e + -- w i w i + k . 2 The stress and the heat flux components are given by: ˜ ˜ ∂v ∂v τ ij = ( µ + µ t ) ------i + ------j – 2 ( ∇v )δ ij - -∂x j ∂x i 3 and q i = ( κ + κ t ) ∂ ˜ T, ∂ xi (A-20) (A-21) (A-22) (A-23) FINE™ A-5 Governing Equations Formulation in Rotating Frame for the Absolute Velocity A-6 FINE™ APPENDIX B:File Formats B-1 Overview This Appendix describes the files used by FINE™ and the flow solver EURANUS. It is divided in two parts. The first one gives the file format information needed to use FINE™, while the second one describes the format of the files used and produced by EURANUS. As FINE™ is intended to handle the file treatment for the user, knowing the exact format of all the files used in a simulation process is not required. This Appendix is therefore written for advanced users. In the following description, it is assumed that all the files are related to a generic project called 'project'. The chapter is divided in five sections: • files produced by IGG™, • files produced and used by FINE™, • files produced and used by the flow solver EURANUS, • files used as data profile, • resource files used to control the layout and which contain default values and reference information. To simplify the notations, it is assumed that the related mesh has a topology of one block. B-2 Files Produced by IGG™ This section describes the files produced by the grid generator IGG™ and used by FINE™: • the identification file project.igg, • the binary file project.cgns, • the boundary conditions file project.bcs, • the geometry file project.geom. FINE™ B-1 File Formats Files Produced by FINE™ B-2.1 The Identification File: project.igg This file contains all the mesh geometric and topologic information. It is used by FINE™ to identify the mesh topology. A complete description of this file is given in the IGG™ User’s Guide. B-2.2 The Binary File: project.cgns When the mesh is created and saved in IGG™, the binary file project.cgns containing the grid point coordinates is created. Later on, the solver will store the wall distances used for the different turbulence models in the same file. B-2.3 The Geometry File: project.geom When the mesh is created and saved in IGG™, the geometry file project.geom containing the whole geometry (curves, surfaces and cartesian points) is created. B-2.4 The Boundary Condition File: project.bcs As described in Chapter 8, the settings of the boundary condition type have to be set inside IGG™ while the physical boundary condition parameters are set in FINE™. The settings of IGG™ are stored in the file project.bcs. This files is used by FINE™ to initialize the boundary condition types for each patch. They are updated each time the boundary condition type is changed inside IGG™. B-3 Files Produced by FINE™ This section describes the files produced and used by FINE™ (or used by the flow solver EURANUS launched from FINE™). Please note that FINE™ acts as a file manager between different software systems. Therefore, it is important that the read, write and execute permissions are set properly for all the files and directories used by FINE™. Manual modification of these files is not supported since it may corrupt the file or provide incorrect results. Such a modification should only be done on explicit advice of NUMECA support team ([email protected]). B-3.1 The Project File: project.iec This file contains all the information related to the project. It is used by FINE™ to save and recover all the user settings. This file is subdivided into several blocks. Each block contains data and/or other blocks. The beginning of the blocks is identified by the key word NI_BEGIN and by a name and the end of the block is identified by the key word NI_END and by the name of the block. a) File Header The file always has the following header containing the version number and the project type: NUMECA_PROJECT_FILE VERSION 5.0 PROJECT_TYPE STRUCTURED After the header, 3 new lines are used to store the name of the files linked to the project: B-2 FINE™ Files Produced by the Flow Solver EURANUS File Formats GRID_FILE /usr/_turnkey_tutorials/_rotor37/rotor37/_mesh/rotor37.igg TRB_FILE /usr/_turnkey_tutorials/_rotor37/rotor37/rotor37.trb GEOMETRY_FILE /usr/_turnkey_tutorials/_rotor37/rotor37.geomTurbo These are respectively the mesh, the template and the geometry files. The template and the geometry files are not used by FINE™/Turbo and are only there for backward compatibility reasons. b) The Computation Block The project file contains the settings of all the computations defined by the user. Each computation block is identified by the following keywords: NI_BEGIN computation ... NI_END computation The computation block contains the following subblocks: • The Solver Parameters Section block containing all the parameters of the solver EURANUS. • The Initial Solution & Boundary Condition Section block containing the initial solution and the boundary conditions. • The Blade-to-Blade Parameters Section block containing all the parameters of the blade-toblade module. • The Grid Parameters Section block containing the topology of the mesh. • The Fluid Properties Section block containing the fluid properties. B-3.2 The Computation File: project_computationName.run When the solver is started, FINE™ creates a new directory using the name of the active computation. A subproject file (’.run’ extension) containing the settings of the active computation is saved into this new directory. This file is used as input by the flow solver EURANUS and by the flow visualization system CFView™. The menu File/Save Run Files enables to save the ’.run’ file without starting the solver EURANUS. B-4 Files Produced by the Flow Solver EURANUS This section describes the files produced and used by the flow solver EURANUS. The flow solver uses most of the files described above and produces the following files: B-4.1 The cgns file: project_computationName.cgns This binary file contains the flow solution. It is used to restart the solver and also by CFView™ to visualize the flow field. The data structure is the following: 1. For block i= 1 to n: The primitive flow variables: density, velocity components, pressure. These are computed at cell centers and are used for restart. Depending on the type of computation, temperature or turbulent quantities such as k, ε or µt are also stored. FINE™ B-3 File Formats Files Produced by the Flow Solver EURANUS 2. For block i= 1 to n: The grid point coordinates and the 3D output flow variables as selected by the user through FINE™ (see Chapter 11). This data will be read by CFView™. Flow quantities are interpolated at mesh nodes by the flow solver as required by CFView™ (see section 11-4 for mathematical details). If the user selected solid data output, azimuthal averaged output or surface averaged output (see Chapter 11), the corresponding mesh coordinates and computed quantities are added to the corresponding ’.cgns’ file. B-4.2 The mf file: project_computationName.mf This ASCII file contains averaged quantities over the inlet, outlet and rotor-stator sections. It is generated only if both inlet and outlet boundary conditions are present. B-4.3 The res file: project_computationName.res This file contains the residual values for all blocks for each iteration of a computation as described in section 15-4.3.1. It is continuously updated during the computation. It is used by the MonitorTurbo to visualize the convergence history. The format of this file is the following: • line 1: Version line. • line 2: Number of blocks. • line 3: 3D or 2D. • line 4: NO-K-EPS or K-EPS or SPL-ALM. • line 5: Number of chemistry species (not used, for backward compatibility only). • line 6: STEADY or UNSTEADY. • line 7: TURBO (not used, for backward compatibility reasons only). • For iteration i=1 to itmax Iteration number, Total iteration number (for unsteady computations only), Work unit, CPU time, Physical time (for unsteady computations only), Lift, Drag, Torque, Qmax, Tmax, Mass flow in and out. For block j = 1 to n: RMS residual for the density ρ, the 3 momentum components (ρvx, ρvy, ρvz), the energy e, the turbulent variables k, ε and υ, and the same data for the maximum residual. Where: Iteration number = the number of iterations. For unsteady computations it includes the number of iterations performed in stationary mode to initialize the unsteady computation. Total iteration number = the total number of iterations including the dual-time step sub-iterations and the initial stationary iterations. Work unit: for single grid computations, one work unit is equal to one iteration, while in multigrid, the work unit corresponds to the computing effort of the multigrid run to the single grid run. For 3D cases it is computed as follow: WU = 1 + n2(1/2)3 + n3(1/2)6 +... While for 2D: WU = 1 + n2(1/2)2 + n3(1/2)4 +... where nx is the number of iteration done on the xth multigrid level B-4 FINE™ Files Produced by the Flow Solver EURANUS File Formats RMS is the root mean square of the residual, defined by Physical time = the physical time step. ΣR es - (see section 15-4.3). -------------------2 n Lift, Drag and Torque are scalar values corresponding respectively to the projection of the force vector along a lift direction (IDCLP), a drag direction (IDCDP) and a torque direction (IDCMP). These directions are controlled by the real expert parameters "IDCLP", "IDCDP", "IDCMP" in FINE™ (on the Computation Steering/Control Variables page in expert mode) as described in section 11-2.5.1 and section 11-3.2. For internal flows (expert parameter IINT=1): • Qmax = efficiency between inlet and outlet, • Tmax = total pressure ratio between inlet and outlet. For external flows (expert parameter IINT=0): • Qmax = maximum heat flux on surface = k*Grad T*n, • Tmax = maximum static temperature. Mass flow in/out = total mass flow for both inlet and outlet boundaries. When no inlet or outlet is present in the computation, the corresponding mass flow is set to zero. Finally, the ".res" file is given with the CPU time included. In case of parallel computations the wall clock time will be given instead of the CPU time. B-4.4 The log file: project_computationName.log This ASCII file contains all the information related to the current computation. It contains a summary of the computation variable as well as warnings and error messages. If the flow solver encounters a problem, the latter is described in the ’.log’ file. This file is for support purposes only. When a problem appears please send this file together with a detailed problem description to NUMECA support team at [email protected]. B-4.5 The std file: project_computationName.std This ASCII file contains all the information related to the current computation. It contains the whole content of the Task Manager window as well as warnings and error messages. If the flow solver encounters a problem, the latter is described in the ’.std’ file. This file is for support purposes only. When a problem appears please send this file together with a detailed problem description to NUMECA support team at [email protected]. B-4.6 The wall file: project_computationName.wall This self-explained ASCII file gives information about forces and torques on the patches for which the Compute force and torque button is activated on the Boundary Conditions page in the Solid thumbnail (see section 8-2.4). FINE™ B-5 File Formats Files Produced by the Flow Solver EURANUS B-4.7 The aqsi file: project_computationName.aqsi This ASCII temporary file is created and read by the code to ensure a smooth restart in the presence of quasi-steady rotor-stator interfaces. B-4.8 The Plot3D files The Plot3D output module of EURANUS creates 4 files. • The project_computationName.g file contains the grid data. • The project_computationName.q file contains the conservative variables. • The project_computationName.f file contains additional variables. • The project_computationName.name file contains the names of the additional variables. The first 3 files can be written in ASCII or binary format, the binary format being the Fortran unformatted format. The .name file is always written in ASCII. When the "Unformatted file (binary)" FORTRAN format is selected in FINE™: the user has to make sure that the file format is also correctly defined in CFView™. When opening the Plot3D project in CFView™ through the menu File/Open Plot3D Project... , click on the File Format... button and select Unformatted. Do not select Binary as it corresponds to binary files generated by C programs. Once this is done, the user also needs to check the "binary low endian" or "binary big endian" format on the same page. On PC platforms (Windows or LINUX) make sure to use "binary low endian" format whereas "binary big endian" is mandatory on all other platforms. 1. The project_computationName.g file format: • Line1: number of blocks, • Line2: the 3 dimensions of each block, • for each block, the coordinates of the mesh points. 2. The project_computationName.q file format: • Line1: number of blocks, • Line2: the 3 dimensions of each block, • for each block: the free stream mach number, the flow angle, the Reynolds number and the time, the 5 conservative unknowns: density, the 3 momentum components and energy. 3. The project_computationName.f file format: • Line1: number of blocks, • Line2: for each block, the 3 dimensions and the number of additional variables selected by the user, • for each block: the additional flow variables. 4. The project_computationName.name file format: This file contains the names of the additional variables stored in the ’.f’ file, one name per line. If the quantity is a vector, it will be written on 3 different lines like in the following example: B-6 FINE™ Files Used as Data Profile File Formats Velocity-X Velocity-Y Velocity-Z B-4.9 The me.cfv file: project_computationName.me.cfv This ASCII file contains data required for the visualization of the meridional averaged output under CFView™. It is created whenever the user specifies variables in the Outputs/Azimuthal Averaged Variables page of the FINE™ interface. B-5 Files Used as Data Profile This section describes the files created by the user and used as input data for the boundary conditions and for the fluid model. Once these files are read by the interface, they are imported in the ’.iec’ file described in section B-3. The flow solver does not read these files, it retrieves the profiles from the computation definition file with extension ’.run’. Profiles may also be specified by entering the coordinates directly into the profile viewer, as described in section 2-12. The imported values will be interpreted in the current project units. These values would change (in the database) if the user changes the corresponding units. Therefore all values will be converted for the flow solver EURANUS in SI system units (in radians for the angles). The values for 1D profiles should be given in increasing order of the x-coordinate. For example, when entering a profile of temperature as a function of R, FINE™ checks whether the two first points are in increasing order. If this is not the case, the profile will be inverted automatically in order to ensure compatibility with the flow solver. The next time the Profile Manager ( opened, the profile will be shown in increasing order, contrary to what was initially entered. ) is For 2D profiles there is no such constraint except for profiles as a function of r-θ (see section 42.3.2). B-5.1 Boundary Conditions Data When defining the inlet (or outlet) boundary condition parameters, the user has the option of specifying one or several input files containing each a data profile. These profiles are used to compute by interpolation the corresponding physical variables at the inlet (or outlet). The file containing the profile must be created by the user and its name must possess the ’.p’ extension. The values of the physical variable stored in this file can come from any source: experiments, previous computations, etc. The format used to create this file contains: • Line 1: • Line 2: Two strings defining the name of the coordinate axes. Type of interpolation and number of points of the profile curve. The types are: 0 for data given at each cell centre 1,2,3,4 and 5 for 1D interpolation respectively along x, y, z, r and θ. 51 for 2D interpolation along x and y. 52 for 2D interpolation along x and z. FINE™ B-7 File Formats Files Used as Data Profile 53 for 2D interpolation along y and z. 54 for 2D interpolation along r and θ. 55 for 2D interpolation along r and z. 56 for 2D interpolation along θ and z. The theta angle is defined as θ = arctg (y/x). The θ profile should cover the patch geometry, so it may take negative values. For unsteady calculations with profile rotation the θ profile must be given form 0 to 2π (see section 4-2.3.2). For time dependant profiles the interpolation type is 100. • The next lines contain the coordinate(s) of each point with the associated physical value. Example 1: r pressure 45 0.5 101000 0.6 102000 0.6 103000 0.7 102000 0.8 101000 This example is related to the interpolation of the pressure along the radius. There are 5 point coordinates in the file. This is a space profile. FINE™ uses the same file formats to import space, time, and space and time profiles. Thus if there is only one profile in the file, it will be interpreted as a space profile, if a second profile exists, FINE™ will recognize it as a time profile. Following is an example of a space and time profile: Example 2: R Pt 46 .3 95600.13 .251765 98913.46 .248412 100909.6 .24445 101527.6 .240182 101740.4 .23622 101811.4 100 10 .216713 101811.4 .210922 101872.1 .205435 101872.1 .199644 101872.1 .195682 101872.1 .191414 101872.1 .187452 101872.1 .18349 101740.4 .179222 99946.98 .1 99946.98 B-8 FINE™ Files Used as Data Profile File Formats The two profiles are separated by an empty line. The interpolation type in time is specified as 100. If this file is imported with the profile viewer invoked as "fct(space)"- only the first part will be taken into account. If "fct(time)" is specified - only the second part will be read by the flow solver. Both profiles will be imported if "fct(space-time)" is specified for the variable type. If there are less coordinates supplied than the number of points specified, FINE™ will put zero for the missing coordinates. B-5.2 Fluid Properties Fluid properties like Cp or Gamma or the viscosity can be input in the solver as constant but can also be input as variables in function of the temperature. The format used is the following: • Line 1: Two strings: "T" and the name of quantity considered ("P" and "Density" for barotropic law). • Line 2: Contains two integers: — the first number is the type of interpolation: 11 for Temperature and 12 for Pressure (barotropic profiles only), — the second one defines the number of points on the profile curve. • The next lines list the data of each point: temperature and the fluid property. Example 1: T Mu 11 5 270 6e-5 275 3e-5 280 2e-5 290 1.5e-5 300 0.9e-5 It is recommended to cover the whole temperature range of the problem. The format for the Cp and Gamma profiles is slightly different because the two profiles are specified in the same file (with extension .heat_capacity). It is as shown in the example below: Example 2: T Cp 11 4 295 1004.9 298 1005.3 301 1010.8 318 1011.0 11 3 296 1.31 298 1.34 303 1.36 FINE™ B-9 File Formats Resource Files The first set of points is for the Cp profile, the second is for the Gamma profile as functions of the temperature. B-6 Resource Files All the resource files are located in the same directory, which is ~/COMMON under UNIX and ~\bin under Windows. It is not possible to start FINE™ if any of these files is missing. B-6.1 Boundary Conditions Resource File euranus_bc.def This file contains the default values for all parameters of the available boundary conditions. The same file is also used to create the graphical layout of the page Boundary Conditions in FINE™. FINE™ only reads from this file so this file is not modified while using FINE™. B-6.2 Fluids Database File euranus.flb This file contains all the data relative to the fluids created by the users in the page Configuration/ Fluid Model. This file is overwritten each time a user quits FINE™ after modifying the fluids database (add, remove, or modify a fluid). All the users should have read and write permissions for this file. It is not recommended to modify this file manually. B-6.3 Units Systems Resource File euranus.uni This file contains the conversion factors for all physical quantities used in FINE™ for all possible combinations between existing systems of units. To add a new units system the user should add the corresponding conversion factors following the existing format shown in the extract below: ... # new units can be added by respecting the format # for UNITS NAMES AND CONVERSION FACTORS # NOTE: VALUE_UNITS_NAME value should NOT begin with capital letter ! # ----------------------------------------------------------------------# ----------------------------------------------------------------------# these are the names of the systems # used to change all the quantities at the same time DEFAULT_SYSTEM SI DEFAULT_SYSTEM Default DEFAULT_SYSTEM American 1 DEFAULT_SYSTEM American 2 # ----------------------------------------------------------------------# ----------------------------------------------------------------------- B-10 FINE™ Resource Files File Formats # this is the system that will be taken as default # when creating a new project NEW_PROJECT_DEFAULT_SYSTEM Default # ----------------------------------------------------------------------- # --------------------- UNITS NAMES AND CONVERSION FACTORS --------------NI_BEGIN UNITS_RECORD NUMBER_OF_SYSTEMS 4 VALUE_UNITS_NAME length UNITS_NAME 1 [m] CONV_FACTOR 1 2 1. CONV_FACTOR 1 3 3.280839895 CONV_FACTOR 1 4 39.37007874 UNITS_NAME 2 [m] CONV_FACTOR 2 1 1. CONV_FACTOR 2 3 3.280839895 CONV_FACTOR 2 4 39.37007874 UNITS_NAME 3 [ft] CONV_FACTOR 3 1 0.3048 CONV_FACTOR 3 2 0.3048 CONV_FACTOR 3 4 12. UNITS_NAME 4 [in] CONV_FACTOR 4 1 0.0254 CONV_FACTOR 4 2 0.0254 CONV_FACTOR 4 3 0.08333333333 NI_END UNITS_RECORD NI_BEGIN UNITS_RECORD NUMBER_OF_SYSTEMS 4 VALUE_UNITS_NAME mass UNITS_NAME 1 [kg] CONV_FACTOR 1 2 1. CONV_FACTOR 1 3 0.06852176586 CONV_FACTOR 1 4 0.005710147155 UNITS_NAME 2 [kg] CONV_FACTOR 2 1 1. CONV_FACTOR 2 3 0.06852176586 CONV_FACTOR 2 4 0.005710147155 UNITS_NAME 3 [lbf s2/ft] FINE™ B-11 File Formats Resource Files CONV_FACTOR 3 1 14.59390294 CONV_FACTOR 3 2 14.59390294 CONV_FACTOR 3 4 0.08333333333 UNITS_NAME 4 [lbf s2/in] CONV_FACTOR 4 1 175.1268352 CONV_FACTOR 4 2 175.1268352 CONV_FACTOR 4 3 12. NI_END UNITS_RECORD ...... If, for example, a new system is added on the fifth position, the user should supply the factors to convert the physical quantities from all the existing systems (1, 2, 3, and 4) to the fifth, and back from the fifth to all the others as shown below: NI_BEGIN UNITS_RECORD NUMBER_OF_SYSTEMS 5 VALUE_UNITS_NAME length UNITS_NAME 1 [m] CONV_FACTOR 1 2 1. CONV_FACTOR 1 3 3.280839895 CONV_FACTOR 1 4 39.37007874 CONV_FACTOR 1 5 new_factor_value_from_1_to_5 UNITS_NAME 2 [m] CONV_FACTOR 2 1 1. CONV_FACTOR 2 3 3.280839895 CONV_FACTOR 2 4 39.37007874 CONV_FACTOR 2 5 new_factor_value_from_2_to_5 UNITS_NAME 3 [ft] CONV_FACTOR 3 1 0.3048 CONV_FACTOR 3 2 0.3048 CONV_FACTOR 3 4 12. CONV_FACTOR 3 5 new_factor_value_from_3_to_5 UNITS_NAME 4 [in] CONV_FACTOR 4 1 0.0254 CONV_FACTOR 4 2 0.0254 CONV_FACTOR 4 3 0.08333333333 CONV_FACTOR 4 5 new_factor_value_from_4_to_5 UNITS_NAME 5 [new_units_name] CONV_FACTOR 5 1 new_factor_value_from_5_to_1 CONV_FACTOR 5 2 new_factor_value_from_5_to_2 CONV_FACTOR 5 3 new_factor_value_from_5_to_3 CONV_FACTOR 5 4 new_factor_value_from_5_to_4 NI_END UNITS_RECORD B-12 FINE™ Resource Files File Formats The default units sytem can be changed by modifying the line NEW_PROJECT_DEFAULT_SYSTEM Default with the name of the desired system. The first (SI) and the second (default) systems are identical except for the rotational speed units (RPM vs. radian). FINE™ B-13 File Formats Resource Files B-14 FINE™ APPENDIX C:List of Expert Parameters C-1 Overview On the Control Variables page under Expert Mode a list of non-interfaced expert parameters is available. As stated in the interface these parameters should not be used unless explicitly stated in this manual. This chapter contains a list of all non-interfaced expert parameters that are described in this manual. For each parameter a reference is given to the corresponding section. If more information is desired on another parameters please contact NUMECA support at [email protected]. C-2 List of Integer Expert Parameters CLASID: COOLFL: EFFDEF: I2DLAG: IADAPT: IATFRZ: IBOTH: IBOUND: ICODKE: ICOPKE: ICYOUT: IFACE: IFNMB: IFNMFI: IFRCTO: IHXINL: IINT: IKELED: IKENC: IMASFL: IMTFIL: INEWKE: class of particles for CFView™ output select cooling/bleed through external file and version efficiency definition simplification of Lagrangian module parametrised target distribution mutligrid parameter for Baldwin Lomax time discretization reflection treatment of particles on solid wall activation of compressible dissipation pressure gradient velocity model solution overwritten every NOFROT timesteps spatial discretization transform PERNM boundaries in FNMB reading full non-matching data from file activate partial torque output inlet boundary condition for condensable fluid internal or external flow activation of LED scalar scheme for k-ε non-conservative approach for k-ε mass flow extrapolation at inlet instead of velocity initial solution for k-ε definition of high Reynolds k-ε model section 7-2.5 section 7-4.3 section 11-3.2 section 7-2.5 section 13-2.5 section 4-3.4 section 9-3.2 section 7.2-2 section 4-3.4 section 4-3.4 section 4-2.2 section 9-3.2 section 4-2.2 section 5-4.3.4 section 8-2.4.3 section 3-2.9 section 11-3.2 section 4-3.4 section 4-3.4 section 8-3.2 section 10-4.3 section 4-3.4 FINE™ C-1 List of Expert Parameters List of Float Expert Parameters INIKE: INVMOD: INVSPL: IOPTKE: IPROLO: IRESTR: IRGCON: IROEAV: IRSMCH: IRSNEW: IRSVFL: ISIDAT: ITFRZ: ITHVZM: ITRWKI: ITYSTO: IUPWTE: IVELSY: IWAVVI: IWRIT: IYAP: KEGRID: KOUTPT: LIPROD: LMAX: MAXNBS: MGRSTR: MGSIMP: MXBFSZ: NIBOUND: NCLASS: NPERBC: NQSTDY: NREPET: NSUBM: NTUPTC: OUTTYP: THINI: VISNUL: ZMNMX: initial solution for k-ε restart of inverse design inverse design of splitter blades optimized implementation for k-ε multigrid prolongation order multigrid restriction order real gas modelling upwind discretization residual smoothing rotor-stator interaction viscous fluxes treatment at R/S interface rotor-stator connectivity structure freezing of turbulent viscosity definition of flow angle in throughflow wake induced transition through AGS model storage of the energy upwind discretization for turbulence equations relative frame of reference spatial discretization writing of global performance data Yap’s modification for turbulent length scale switch from Baldwin-Lomax to k-epsilon model particles trajectories output linear production term maximum number of segments in Lagrangian module maximum number of injection sectors multigrid strategy multigrid strategy maximum buffer size reflection treatment of particles on solid wall maximum nuber of classes inlet/outlet signal periodicity update rotor-stator boundary condition calculation of the wall distance number of subdomains in calculation of wall distance number of patches in calculation of wall distance select type of output throughflow under-relaxation central discretization indication of injector positions in cooling/bleed section 10-4.3 section 13-2.5 section 13-2.5 section 4-3.4 section 9-3.2 section 9-3.2 section 3-2.9 section 9-3.2 section 9-3.2 section 5-4 section 5-5.4 section 5-4 section 4-3.4 section 6-4 section 7-5.3 section 3-2.9 section 4.3.4 section A-3 section 9-3.2 section 11-3.2 section 4-3.4 section 4.3.4 section 7-2.5 section 4-3.5 section 7-2.5 section 7.4-3 section 9-3.2 section 9-3.2 section 14-4.4 section 7-2.5 section 7-2.5 section 4.2-2 section 5-4 section 4-3.4 section 4-3.4 section 4-3.4 section 11-3.2 section 6-4 section 9-3.2 section 7-4.3 C-3 List of Float Expert Parameters ALF: ALPHAP: ANGREL: C3: CDIDTE: CE1: CE2: constant for compressible dissipation preconditioning parameter relative angles for the inlet boundary conditions constant for k-ε model central discretization constant for k-ε model constant for k-ε model section 4-3.4 section 4-3.8 section 8-3 section 4-3.4 section 9-3.2 section 4-3.4 section 4-3.4 C-2 FINE™ List of Float Expert Parameters List of Expert Parameters CMU: COOLRT: CP1: CREF: DDIMAX: DIAMR: EKCLIP: ENTRFX: EPCLIP: EXPMAR: FTRAST: GAMMAT: IDCDP: IDCLP: IDCMP: IRKCO: ISWV: IXMP: LTMAX: MAVREM: MAVRES: MUCLIP: NUTFRE: PRCLIP: PRT: RADAPT: RELAXP: RELPHL: RESFRZ: RGCST: RSMPAR: RTOL: SIGE: SIGK: SIGRO: SMCOR: SREF: TEDAMP: THFREL: VELSCA: VIS2: VIS2KE: VIS4: VIS4KE: constant for k-ε model section 4-3.4 reduction of mass flow in cooling holes section 7-4.3 constant for compressible dissipation section 4-3.4 reference chord for non-dimensionalizing section 11-3 tolerance factor for Lagrangian module section 7-2.5 diameter ratio for Lagrangian module section 7-2.5 clipping value for turbulent kinetic energy section 4-3.4 upwind discretization section 9-3.2 clipping value for turbulent kinetic dissipation section 4-3.4 central discretization section 9-3.2 forbid transition before FTRAST*chord with AGS model section 7-5.3 turbulence time scale section 4-3.4 direction of drag or axial thrust section 11-3.2 direction of lift section 11-3.2 direction of moment or torque section 11-3.2 Runge-Kutta coefficients section 9-3.2 Runge-Kutta dissipative residuals section 9-3.2 definition of point for moment or torque section 11-3.2 maximum turbulent length scale section 4-3.4 control of multigrid correction for k and ε section 4-3.4 update control of k and ε section 4-3.4 clipping value for Mut/Mu for k and ε and Spalart-Allmaras section 4-3.4 initial value of turbulent viscosity for Spalart Allmaras section 4-3.3 turbulence parameter section 4-3.4 turbulent Prandtl number section 4-3.4 parametrised target distribution section 13-2.5 under-relaxation for mass flow imposed at outlet section 8-3 relaxation factor for Phase-Lagged section 4.2.2 freeze turbulent viscosity field section 4-3.4 value of the gas constant section 3-2.9 residual smoothing parameter section 9-3.2 maximum angle for normals in calculation wall distance section 4-3.4 constant for k-ε model section 4-3.4 constant for k-ε model section 4-3.4 constant for k-ε model section 4-3.4 residual smoothing section 9-3.2 reference surface to non-dimensionalize coefficients section 11-3 damping for k-e model section 4-3.4 throughflow under-relaxation section 6-4 maximum value allowed for velocity scaling section 8-3 central discretization section 9-3.2 central discretization section 9-3.2 central discretization section 9-3.2 central discretization section 9-3.2 FINE™ C-3 List of Expert Parameters List of Float Expert Parameters C-4 FINE™ APPENDIX D: Characteristics of Water (steam) Tables D-1 Overview As described in section section 3-2.3.4, the Condensable Fluid module aims at the modelling of the real thermodynamic properties of a given fluid by means of interpolation of the variables from dedicated tables. The approach that has been adopted in EURANUS consists of using a series of thermodynamic tables, one table being required each time a thermodynamic variable must be deduced from two other ones. This implies the creation of many tables as input, but presents the advantage that no iterative inversion of the tables is done in the solver, with as a consequence a very small additional CPU time. Information related to • the range of variation of admissible values for thermodynamic variables • the discretization of the grid • the nature of the interpolation algorithm selected • the relative mean error (mean and maximum) on thermodynamic variables • the size of the table is discussed here below for water (steam) tables. D-2 Main Characteristics Water (steam) tables come in the form of 11 tables, described as follows: TER: PER: RPT: EPT: SHP: PHS: interpolates static temperature as a function of internal energy and density interpolates static pressure as a function of internal energy and density interpolates density as a function of static pressure and temperature interpolates internal energy as a function of pressure and static temperature interpolates entropy as a function of total enthalpy and static pressure interpolates static pressure as a function of entropy and total enthalpy FINE™ D-1 Characteristics of Water (steam) Tables Main Characteristics RHS: HSP: MER: KER: PSA: interpolates static pressure over density as a function of entropy and total enthalpy interpolates total enthalpy as a function of entropy and static pressure interpolates dynamic viscosity as a function of internal energy and density interpolates thermal conductivity as a function of internal energy and density defines the saturation line Tables TER / PER Variables Energy [J/kg] Density [kg/m3] Pressure [bars] Temperature [K] Minimum 500,000 0.001 0.0003 237 0.002 250 0.00032 -187,568 -99,726 1,500,000 0.002 -1,582 1,850,000 2,000 0.00021 -1,655 0 0.002 500,000 3] Maximum 4,000,000 1,020 26,600 1,630 24,000 1,350 1,432 4,212,000 5,500,000 4,500,000 24,000 12,733 4,500,000 10,500 46,700 50,000,000 13,000 24,000 4,000,000 500 0.00013 0.58 RPT / EPT Pressure [bars] Temperature [K] Density [kg/m3] Energy [J/Kg] Enthalpy [J/kg] SHP Enthalpy [J/kg] Pressure [bars] Entropy [J/kg/K] PHS / RHS Enthalpy [J/kg] Entropy [J/kg/K] Pressure [bars] HSP Enthalpy [J/kg] Entropy [J/kg/K] Pressure [bars] MER / KER Energy [J/Kg] Density [kg/m 0.001 0.0000085 0.015 Viscosity [Pa.s] Conductivity [W/m/K] TABLE 1. Admissible range of variations for thermodynamic variables Table 1 on page 2 lists the range of admissible variations for the thermodynamic variables, in the different tables proposed. Ranges have been extended from the default tables proposed up to FINE™ /Turbo v6.2-7, especially at low pressures (< 1000 Pa). Significant improvements, both in terms of robustness and accuracy, are expected in that area. D-2 FINE™ Main Characteristics Characteristics of Water (steam) Tables Tables PER TER RPT EPT SHP PHS RHS HSP MER KER PSA Grid 71 x 71 71 x 71 101 x 101 101 x 101 41 x 41 81 x 81 81 x 81 81 x 81 41 x 61 41 x 61 120 Interpolation bi-cubic (double precision) bi-cubic (double precision) bi-cubic (single precision) bi-cubic (single precision) bi-cubic (single precision) bi-cubic (single precision) bi-cubic (double precision) bi-cubic (single precision) bi-cubic (double precision) bi-cubic (double precision) cubic Error RMS [%] 0.02 0.014 0.0015 0.005 0.026 0.0003 0.126 2.02 - Error Maximum [%] 80.7 1.7 < 0.1 < 0.1 0.008 5.8 9.7 0.01 8.7 27.2 - Size [Mb] 3.2 3.2 3.3 3.3 0.5 2.1 4.2 2.1 1.6 1.6 0.1 TABLE 2. Main characteristics of water (steam) thermodynamic tables Both RMS (root mean square) and maximum errors should be interpreted as relative errors. RMS error does not exceed 2%, while in most tables it is ranging from 0.0001% to 0.1%. Maximum relative errors are located nearby the saturation line, where the interpolation naturally degrades despite the use of bi-cubic double precision algorithms. Tables RPT and EPT have been tuned so as to guarantee maximum accuracy in the vapor phase (< 0.1% at maximum). However, run performed in the liquid phase are consequently prohibited since they would lead to large relative errors (> 100%) in that area. A dedicated set covering RPT and EPT tables balancing maximum relative errors both on vapor and liquid phases can however be obtained upon request. Please take direct contact at [email protected] for any question on this purpose. FINE™ D-3 Characteristics of Water (steam) Tables Main Characteristics D-4 FINE™ Index INDEX A Abu-Grannam-Shaw Model 7-41 Add Fluid 3-3 ANSYS Outputs 11-10 AutoBlade 2-3, 2-10 AutoGrid 1-2, 2-3, 2-5, 2-10 Axial Thrust 8-11, 11-15 Azimuthal Averaged Output 11-9 B Background Color 1-7 Barotropic Liquid, see Fluid, Barotropic Liquid Benedict-Webb-Rubin 3-13 Blade To Blade 12-1–?? Boundary Conditions 12-8 File Formats 12-13–12-17 Flow Solver 12-12 Geometrical Data 12-3 Initial Solution 12-10, 13-5 Input Files 12-13–12-15 Inverse Design 12-8 Mesh Generator 12-6, 12-11 New Project 12-2 Numerical Model 12-10 Open Project 12-2 Output Files 12-15–12-17 Stream Surface Data 12-4 Theory 12-11 Bleed flow Data file 7-33 Flow Parameters 7-29 Outputs 7-31 Positioning 7-18 Visualization 7-30 Wizard 7-16 Block Conjugate Heat Transfer 7-12 Throughflow 6-2–6-3 Boundary Conditions 8-1 Blade To Blade 12-8 Lagrangian Module 7-4, 7-4–7-6 Rotor/Stator 5-17–5-19 Throughflow 6-7–6-8 Turbulence 4-16 Unsteady 4-2 Boussinesq 4-47 C CFD Governing equations A-1 Introduction 1-1 CFL Number 7-12, 9-2, 9-17 CFView™ 1-3–1-4, 2-10 CGNS B-3 Characteristic Values, see Reference Values Computation Definition Area 2-12 Condensable fluid Boundary conditions 8-20 Outputs 11-4 Condensable Fluid, see Fluid, Condensable Conductivity 3-3–3-5 Laminar 3-10 Turbulent 3-10 Turbulent, Condensable Fluid 3-15 Conjugate Heat Transfer 7-11–7-15 Blocks Types 7-12 Theory 7-13–7-15 Control Variables 15-1 Unsteady 4-4 Convention 1-5 Convergence History 10-4 Cooling Theory 7-32, 7-33 Cooling flow Bleed flow 7-15 Data file 7-33 Flow Parameters 7-29 Outputs 7-31 Positioning 7-18 Visualization 7-30 Wizard 7-16 Create Grid File 2-3 Project 2-2, 2-4, 12-2, 13-2 Run Files 2-6 D Delete Fluid 3-7 Design 2D 2-10, 13-1–?? Formulation 13-4, 13-7 Input Files 13-3, 13-8 Interface 13-2 Output Files 13-9 Start 13-6 Theory 13-7–13-8 Design 3D 1-2, 2-3, 2-10 FINE™ i Index INDEX Discretization Central Scheme 9-9–9-10 Limiters 9-12 Spatial 9-4, 9-7–9-13 Temporal 9-4 Time 9-17–9-21 Upwind Scheme 9-10–9-13 Drag 8-11 Drag Coefficient 11-19 Driver 1-6 Dryness Fraction 3-15 Duplicate Active Project 2-6 E Edit Fluid 3-7 Efficiency 11-16 Enthalpy 3-11, 3-15 Entropy 3-14 Euler 4-15 2D 6-1 Equations 6-13 EURANUS 1-3 EuranusTurbo Parallel Computation 14-8, 14-17 Expert Mode 2-12 Expert Parameters C-1, D-1 External Boundary Condition 8-13 F File Chooser 2-19 File Format 6-9, B-1 File Management 1-3 File Menu 2-4 File Names, Limitations 2-7 Fluid Add 3-3 Condensable 3-13–3-16 Delete 3-7 Edit 3-7 Incompressible 5-18 Interface 3-2 Liquid 3-12 List 3-2 Models 3-1–3-16 Perfect Gas 3-10 Real Gas 3-11 Fluid-Particle Interaction. See Lagrangian Module. Force 8-11 Blade 6-14 Friction 6-15 Forced Transition 7-38, 7-40 Formula Editor 3-6 Full Non-matching 5-20 Fully Laminar 7-40 Fully Turbulent 7-40 G Gauss Theorem 9-8 Global Layout 2-7 Global Performance 11-15, B-4 Graphics 1-6 Graphics Area 2-16 Gravity 3-5, 4-41 Grid Create Grid File 2-3 Grid Generation 1-2–1-4 Units 2-4, 2-8 Group Block Rotation 5-2 Boundary Conditions 8-2 Rotor/Stator 5-3 H Hand Symbol 1-5 Host Definition 14-5 Hybrid Analysis 6-3 I Icon Bar 2-10 IGG™ 1-3, 2-3, 2-5, 2-10 Incompressible Fluid Model, see Fluid Model, Incompressible Local Conservative Coupling 5-18 Initial Solution 10-1–10-8 Blade To Blade 12-10, 13-5 Block Dependent 10-1–10-3 Coarse Grid 9-3 Constant Values 10-3 File 10-4–10-5 Full Multigrid Strategy 9-16 Throughflow 6-8–6-9, 10-7–10-8 Turbomachinery 10-6–10-7 Turbulence 4-16 Unsteady 10-5 Initialization Full Multigrid Strategy 10-1 Unsteady 4-4 ii FINE™ Index INDEX Installation 1-6 Interface 1-7 General Description of FINE™ Interface 2-1–2-19 L Lagrangian Module Boundary Conditions 7-4, 7-4–7-6 Global Strategy 7-3 Interaction With Turbulence 7-10 Outputs 7-6 Particles Traces 7-7 Theory 7-9–7-11 Laminar 4-15 Layout 2-7 License 1-8 Lift 8-11 Lift Coefficient 11-19 Light Bulb 1-5 Limitations 2-7, 2-8 Limiter Lacor 9-12 Minmod 9-12 Superbee 9-12 Van Albada 9-12 Van Leer 9-12 Linearization 4-27 LIPROD 4-27 Liquid, see Fluid, Liquid Local Conservative Coupling 5-17–?? Loss Coefficient 6-6 Low Speed Flow 4-42 M Mach Number Absolute 11-5 Condensable Fluid 3-15 Isentropic 13-4, 13-10 Relative 11-5 Mathematical Model 4-15 Menu File 2-4 Menu Bar 2-4 Mesh 2-8 Modules 2-10 Solver 2-9 Merge Merge Mesh Topology 2-11 Patch For Azimuthal View 11-9 Mesh 1-2–1-4 Information 2-15 Properties 2-8 Selection 2-11 Toggles 2-14 View 2-8, 2-16–2-18 View Area 2-13 Modules 2-10 Moment 8-11 Momentum 11-19 Monitor Convergence History 15-11 Display 15-10 Quantities 15-3 Residual File Box 15-9 Solution 15-1–15-12 Steering File 15-3 Zoom 15-10 MonitorTurbo 15-7 MSW Driver 1-6 Multigrid 9-2 Full 9-16 Prolongation 9-16 Strategy 9-3, 9-13–9-17 N New Project 2-4, 12-2, 13-2 Numerical Model 9-1 Blade To Blade 12-10 O Open Project 2-3, 2-5 OPENGL Driver 1-6 Outputs 3-15, 11-1–11-24 3D Quantity 11-2–11-7, 11-20 Azimuthal Averaged 11-9, 11-18, 11-21–11-23 Lagrangian Module 7-6 mf File 11-15, 11-18 Particle Traces 7-7 Surface Averaged 11-8, 11-21 Theory 11-20–11-24 P Pair of Scissors 1-5 Parallel Computation 14-13 Parameter Button 2-13 Parameters Area 2-2 Particles 7-1 Perfect Gas, see Fluid, Perfect Gas FINE™ iii Index INDEX Performance 11-15, B-4 Periodic Boundaries 6-7, 8-9 Phase Lagged 4-3, 4-13 Plot3D 11-17, B-6 Post Processing 1-3–1-4 Prandtl Number 3-10 Preconditioning 4-42 Parameters 4-45, 9-3 Preferences 2-6 Profile Manager 2-19, 3-3–3-6 File Formats B-7 Project Configuration 2-4 Creation 2-2 Duplicate 2-6 Management 1-3 New 2-4 Open 2-3, 2-5 Save 2-6 Units 2-6 Properties Fluid 3-1 Mesh 2-8 PVM Daemons 14-1–14-5 Q Quit 2-7 R Real Gas, see Fluid, Real Gas Reference Density 3-9, 4-47 Length 4-47 Pressure 3-5, 4-45 Reference Values 4-47 Temperature 3-5, 3-9, 4-45 Velocity 4-45, 4-47 Residual 11-6, 15-5, B-4 Implicit Smoothing 9-20 Radespiel & Rossow 9-20 Swanson & Turkel 9-21 Vasta 9-21 Restart 2-10 Design 2D 13-6 Unsteady 4-5 Reynolds Number 4-47 Rotation Blocks 5-2–5-3 Rotor/Stator Domain Scaling 5-11–5-12, 5-21–5-24 FNMB Mixing Plane Coupling 5-19–5-21 Frozen Rotor 5-9–5-10, 5-24 Initial Solution 10-6 Interface 5-3–5-5 Local Conservative Coupling 5-17–5-18 Mixing Plane Coupling 5-5–5-8, 5-16–5-21 Phase Lagged 5-13 Pitchwise Rows Coupling 5-18–5-19 Steady 5-5–5-8, 5-9–5-10, 5-16–5-21, 5-24 Theory 5-15–5-24 Unsteady 5-11–5-12, 5-13, 5-21–5-24 Rough Wall 4-35 Run File 1-3, 2-6 Runge-Kutta Scheme 9-17 S Save Intermediate Solution 2-9 Project 2-6 Scripts 14-14 Second Order Restart 4-5 SI System 2-6 Smooth Wall 4-35 Solid Data 11-6 Solver Menu 2-9 Specific Heat 3-10–3-12, 3-15 Standard Mode 2-12 Start Flow Solver 2-9 Stator Rotor/Stator Interface. See Rotor/Stator. Steady Rotor/Stator 5-5–5-8, 5-9–5-10, 5-16–5-21, 5-24 Stop Flow Solver 2-9 Surface Averaged Output 11-7 Suspend Flow Solver 2-9 Sutherland 3-9 Sutherland Law 3-9 T Task Definition 14-6 Taskmanager 14-1–14-23 Add Host 14-5 Delay 14-6 Limitations 14-22 Parallel Computation 14-8 PVM 14-1–14-5 iv FINE™ Index INDEX Remove Host 14-6 Scripts 14-14–14-22 Shutdown 14-6 Subtask 14-7–14-11 Task Definition 14-6–14-11 Tear-off Graphics 2-8 Temperature Reference 3-9 Sutherland 3-9 Thermal Connections 7-12 Thermodynamic Tables 3-13 Throat Control 6-3 Throughflow Analysis Mode 6-3 Blade Geometry 6-3–6-5 Block Type 6-2 Boundary Conditions 6-7–6-8 Expert Parameters 6-12 File Format 6-9–6-11 Flow Angle/Tangential Velocity 6-5–6-6 Global Parameters 6-2 Initial Solution 6-8–6-9, 10-7–10-8 Loss Coefficient 6-6 Mesh 6-6 Model 6-1–6-15 Theory 6-13–6-15 Time Configuration 4-2 Time Step Global Time 9-4 Local Time 9-4 Physical 4-14 Torque 8-11, 11-15 Transition Model 7-37 Abu-Grannam-Shaw Model 7-41 Forced Transition 7-38, 7-40 Fully Laminar 7-40 Fully Turbulent 7-40 Turbulence Boundary Condition 4-16 Initial Solution 4-16 Linearization 4-27 Output 11-7 Turbulence Models Baldwin-Lomax 4-28 k-epsilon 4-31 Non Linear k-epsilon 4-33 Spalart-Allmaras 4-29 TVD 9-11 U Units Grid 2-4, 2-8 Project 2-6 Unload Mesh 2-8 Unsteady 4-2 Boundary Conditions 4-2, 4-6, 4-12 Control Variables 4-4 Create 4-6 Initial Solution 10-5 Initialization of 4-7 Phase Lagged 4-3 Rotor/Stator 5-11–5-12, 5-21–5-24 Rotor/Stator Phase Lagged 5-13 Second Order in Time 4-5 Turbomachinery 4-12 User Mode 2-12 V Vander Waals 3-13 Velocity Absolute 11-5 Friction 4-21 Local Scaling 4-46 Projections 11-5 Reference 4-47 Relative 11-5 Relative Projections 11-5 View Area 2-13 View Manipulation 2-16 View On/Off 2-8, 2-13 Viscosity Inviscid Flux 9-8 Laminar 3-9 Turbulent 3-10, 4-39 Viscous Flux 9-8 Vorticity 11-5 W Wall Rough 4-35 Smooth 4-35 Work Unit B-4 X X11 Driver 1-6 Z Zoom In/Out/Region 2-18 FINE™ v


Comments

Copyright © 2024 UPDOCS Inc.