FineTurbo_User_manual User Manual FINETurbo

2013-12-19

: Ensight Usermanual-Fineturbo UserManual-FINETurbo Numeca Misc

Open the PDF directly: View PDF PDF.
Page Count: 351 [warning: Documents this large are best viewed by clicking the View PDF Link!]

NUMERICAL MECHANICS APPLICATIONS
User Manual
FINE™/Turbo v8.10
Flow Integrated Environment
- November 2012 -
NUMERICAL MECHANICS APPLICATIONS
User Manual
FINE™/Turbo v8.10
Documentation v8.10c
NUMECA International
Chaussée de la Hulpe, 189
1170 Brussels
Belgium
Tel: +32 2 647.83.11
Fax: +32 2 647.93.98
Web: http://www.numeca.com
Contents
FINE™/Turbo iii
CHAPTER 1: Getting Started 1-1
1-1 Overview 1-1
1-2 Introduction 1-1
Components 1-1
Multi-Tasking 1-2
Project Management 1-2
1-3 How To Use This Manual 1-4
Outline 1-4
Conventions 1-4
1-4 First Time Use 1-5
Basic Installation 1-5
Expert Graphics Options 1-5
1-5 How to start the FINE™/Turbo Interface 1-6
1-6 Required Licenses 1-7
Standard FINE™/Turbo License 1-7
Additional Licenses 1-7
CHAPTER 2: Graphical User Interface 2-1
2-1 Overview 2-1
2-2 Project Selection 2-2
Create New Project 2-2
Open Existing Project 2-4
Grid Units & Project Configuration 2-4
2-3 Main Menu Bar 2-6
File Menu 2-6
Mesh Menu 2-9
Solver Menu 2-11
Modules Menu 2-12
2-4 Icon Bar 2-12
File Buttons 2-12
Grid Selection Bar 2-13
Solver Buttons 2-14
Module Buttons 2-14
User Mode 2-14
2-5 Computation Management 2-14
2-6 Graphical Area Management 2-15
Configuration Management 2-15
Parameters Management 2-16
View Area 2-16
Mesh Information 2-18
Parameters Area 2-18
Graphics Area 2-19
Viewing Buttons 2-19
2-7 Profile Management 2-22
Contents
iv FINE™/Turbo
CHAPTER 3: Fluid Model 3-1
3-1 Overview 3-1
3-2 The Fluid Model in the FINE™/Turbo GUI 3-2
Properties of Fluid Used in the Project 3-2
List of Fluids 3-2
Add Fluid 3-3
Delete Fluid from List 3-9
Edit Fluid 3-9
Show Fluid Properties 3-10
Filters 3-10
Import Fluid Database 3-10
Expert Parameters 3-10
CHAPTER 4: Flow Model 4-1
4-1 Overview 4-1
4-2 Mathematical Model 4-2
Euler 4-2
Laminar Navier-Stokes 4-2
Turbulent Navier-Stokes 4-2
Expert Parameters for Turbulence Modelling 4-4
Best Practice for Turbulence Modelling 4-9
Laminar-Transition Model 4-19
Gravity Forces 4-21
Low Speed Flow (Preconditioning) 4-22
4-3 Characteristic & Reference Values 4-22
Reynolds Number Related Information 4-22
Reference Values 4-23
CHAPTER 5: Boundary Conditions 5-1
5-1 Overview 5-1
5-2 Boundary Conditions in the FINE™/Turbo GUI 5-1
Inlet Condition 5-4
Outlet Condition 5-7
Periodic Condition 5-11
Solid Wall Boundary Condition 5-12
External Condition (Far-field) 5-16
5-3 Expert Parameters 5-17
Imposing Velocity Angles of Relative Flow 5-17
Inlet Mass Flow Boundary Condition 5-17
Outlet Mass Flow Boundary Condition 5-17
Outlet Averaged Mach Number Boundary Condition 5-18
Control of backflows 5-18
Torque and Force 5-18
Euler or Navier-Stokes Wall for Viscous Flow 5-18
Pressure Condition at Solid Wall 5-19
5-4 Best Practice for Imposing Boundary Conditions 5-19
Contents
FINE™/Turbo v
Compressible Flows 5-19
Incompressible or Low Speed Flow 5-20
Special Parameters (for Turbomachinery) 5-20
CHAPTER 6: Numerical Scheme 6-1
6-1 Overview 6-1
6-2 Numerical Model 6-1
Introduction 6-1
Numerical Model in the FINE™/Turbo GUI 6-2
Expert Parameters 6-5
6-3 Time Configuration 6-10
Interface for Unsteady Computation 6-10
Expert Parameters for Unsteady Computations 6-13
Best Practice on Time Accurate Computations 6-14
CHAPTER 7:Physical Models 7-1
7-1 Overview 7-1
7-2 Fluid-Particle Interaction 7-1
Introduction 7-1
Fluid-Particle Interaction in the FINE™/Turbo GUI 7-3
Specific Output 7-7
Expert Parameters 7-8
7-3 Fluid-Structure 7-9
Thermal 7-9
Mechanical 7-13
7-4 Passive Tracers 7-23
Boundary Conditions 7-23
Initial Solution 7-23
Outputs 7-24
7-5 Porous Media Model 7-24
Porous Media Model in the FINE™/Turbo GUI 7-24
Experts Parameters 7-24
7-6 Cavitation Model 7-25
Cavitation Model in the FINE™/Turbo GUI 7-25
Experts Parameters 7-25
CHAPTER 8:Dedicated Turbomachinery Models 8-1
8-1 Overview 8-1
8-2 Rotating Blocks 8-1
8-3 Rotor/Stator Interaction 8-4
Rotor/Stator Interfaces in the FINE™/Turbo GUI 8-4
How to Set-up a Simulation with Rotor/Stator Interfaces? 8-6
8-4 Harmonic Method 8-19
Introduction 8-19
Interface & Best Practice for Harmonic Computations 8-20
Expert Parameters 8-27
Contents
vi FINE™/Turbo
8-5 Clocking 8-30
Introduction 8-30
Interface Settings 8-31
8-6 Cooling/Bleed 8-33
Introduction 8-33
Cooling/Bleed Model in the FINE™/Turbo GUI 8-34
Expert Parameters 8-54
Cooling/Bleed Data File: ’.cooling-holes’ 8-54
8-7 Rigid Motion 8-59
8-8 Aeroacoustics 8-59
Aeroacoustics in the FINE™/Turbo GUI 8-60
Expert Parameters for Aeroacoustics 8-62
8-9 Laminar-Transition Model 8-63
Introduction 8-63
Transition Model in the FINE™/Turbo GUI 8-63
Expert Parameters 8-65
8-10 Performance Curve 8-66
Introduction 8-66
Performance Curve in the FINE™/Turbo GUI 8-66
8-11 SubProject Management 8-69
Introduction 8-69
Set-up of SubProjects in FINE™/Turbo 8-70
CHAPTER 9: Initial Solution 9-1
9-1 Overview 9-1
9-2 Block Dependent Initial Solution 9-1
How to Define a Block Dependent Initial Solution 9-2
Examples for the use of Block Dependent Initial Solution 9-2
9-3 Initial Solution Defined by Constant Values 9-3
9-4 Initial Solution from File 9-3
General Restart Procedure 9-3
Restart in Unsteady Computations 9-5
Expert Parameters for an Initial Solution from File 9-5
9-5 Initial Solution for Turbomachinery 9-5
Methodology 9-6
Grouping & Parameters 9-7
Expert Parameters 9-8
9-6 Throughflow-oriented Initial Solution 9-8
CHAPTER 10:Output 10-1
10-1 Overview 10-1
10-2 Output in FINE™/Turbo 10-2
Computed Variables 10-2
Surface Averaged Variables 10-8
Azimuthal Averaged Variables 10-10
Template manager 10-11
ANSYS 10-13
Contents
FINE™/Turbo vii
Global Performance Output 10-19
Plot3D Formatted Output 10-22
10-3 Expert Parameters 10-22
Azimuthal Averaged Variables 10-22
Global Performance Output 10-23
Solid Data Output 10-24
CHAPTER 11:Task Manager 11-1
11-1 Overview 11-1
11-2 Getting Started 11-1
PVM Daemons 11-1
Multiple FINE™/Turbo Sessions 11-2
Machine Connections 11-2
Remote Copy Features on UNIX/LINUX 11-4
Remote Copy Features on Windows 11-4
11-3 The Task Manager Interface 11-5
Hosts Definition 11-5
Tasks Definition 11-6
11-4 Parallel Computations 11-17
Introduction 11-17
Management of Inter-Block Communication 11-19
How to Run a Parallel Computation 11-19
Use an External OpenMPI Library on LINUX/UNIX 11-20
Troubleshooting 11-21
Limitations 11-22
11-5 Task Management in Batch 11-22
Launch IGG™ in Batch 11-22
Launch AutoGrid™ in Batch 11-23
Launch FINE™ in Batch 11-24
Launch the flow solver in Sequential Mode in Batch 11-30
Launch the flow solver in Parallel Mode in Batch 11-31
Launch CFView™ in Batch 11-43
11-6 Limitations 11-45
CHAPTER 12:Computation Steering & Monitoring 12-1
12-1 Overview 12-1
12-2 Control Variables 12-1
Control Variables in the FINE™/Turbo GUI 12-1
Expert Parameters 12-2
12-3 Convergence History 12-3
Convergence History in the FINE™/Turbo GUI 12-3
Expert Parameters 12-10
12-4 MonitorTurbo 12-10
Introduction 12-10
The MonitorTurbo GUI 12-11
12-5 Best Practice for Computation Monitoring 12-14
Introduction 12-14
Contents
viii FINE™/Turbo
Convergence History 12-14
MonitorTurbo 12-16
Analysis of Residuals 12-16
APPENDIX A:File Formats A-1
A-1 Overview A-1
A-2 Files Produced by IGG™ A-1
The Identification File: ’project.igg’ A-2
The Binary File: ’project.cgns’ A-2
The Geometry File: ’project.geom’ A-2
The Boundary Condition File: ’project.bcs’ A-2
The Configuration File: ’project.config’ A-2
A-3 Files Produced by the FINE™/Turbo GUI A-2
The Project File: ’project.iec’ A-2
The Computation File: ’project_computation.run’ A-3
A-4 Files Produced by the FINE™/Turbo solver A-3
The Binary Solution File: ’project_computation.cgns’ A-3
The Global Solution File: ’project_computation.mf’ A-7
The Global Solution File: ’project_computation.xmf’ A-7
The Residual File: ’project_computation.res’ A-8
The LOG File: ’project_computation.log’ A-9
The STD file: ’project_computation.std’ A-10
The Wall File: ’project_computation.wall’ A-10
The AQSI File: ’project_computation.aqsi’ A-10
The ADF File: ’project.adf’ A-10
The Plot3D Files A-10
The Meridional File: ’project_computation.me.cfv’ A-11
A-5 Files Used as Data Profile A-11
Boundary Conditions Data A-12
Fluid Properties A-14
Solid Properties A-14
A-6 Resource Files A-15
Boundary Conditions Resource File: ’euranus_bc.def’ A-15
Fluids Database File: ’euranus.flb’ A-15
Units Systems Resource File: ’euranus.uni’ A-15
APPENDIX B:List of Expert Parameters B-1
B-1 Overview B-1
B-2 List of Integer Expert Parameters B-1
B-3 List of Float Expert Parameters B-3
APPENDIX C:Characteristics of Thermodynamic Tables C-1
C-1 Overview C-1
C-2 Main Characteristics for Water (Steam) C-1
C-3 Main Characteristics for R134a C-2
Contents
FINE™/Turbo ix
APPENDIX D:TabGen D-1
D-1 Overview D-1
D-2 Graphical User Interface D-2
Start Program D-2
Main Window D-4
D-3 Launch TabGen in Batch Mode D-9
Contents
xFINE™/Turbo
FINE™/Turbo 1-1
CHAPTER 1: Getting Started
1-1 Overview
Welcome to the FINE™/Turbo User Manual, a presentation of NUMECA’s Flow INtegrated Envi-
ronment for computations on structured meshes. This chapter presents the basic concepts of
FINE™/Turbo and shows how to get started with the program by describing:
•what FINE™/Turbo does and how it operates,
•how to use this guide,
•how to start the FINE™/turbo interface.
1-2 Introduction
1-2.1 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 FINE™/turbo solver, 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™/Turbo, allowing the achievement of complete simulations of 3D
internal and external flows from the grid generation to the visualization, without any file manipula-
tion, through the concept of project. Moreover, multi-tasking capabilities are incorporated, allowing
the simultaneous treatment of multiple projects.
Getting Started Introduction
1-2 FINE™/Turbo
1-2.2 Multi-Tasking
FINE™/Turbo has the particularity of integrating the concept of multi-tasking. This means that the
user can manage a complete project in the FINE™/Turbo interface; making the grid using IGG™,
running the computation with the FINE™/Turbo solver 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 computa-
tions in background has been implemented. See Chapter 11 for more detail on how to manage mul-
tiple tasks through the interface or in background.
1-2.3 Project Management
To manage complete flow analyses, FINE™/Turbo 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™/Turbo:
•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 con-
ditions is also done during this process. The five files that contain the information about the
mesh have the extensions ".igg", ".geom", ".bcs", ".config" and ".cgns".
•The project file: The project file is created by FINE™/Turbo. It has the extension ".iec" and
contains the input parameters needed for the flow computations.
•The result files: FINE™/Turbo 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™,
—a ".cgns" file that contains the solution and that is used for restarting the solver,
—a ".res" file used by the Monitor to visualize the residual history (see Chapter 12),
—two files used to visualize the convergence history in the Steering with extensions ".steer-
ing" and ".steering.binary" (see Chapter 12).
—two files with extensions ".mf" and ".wall" that contain global solution parameters.
—a ".xmf" file that stores the information contained in the ".mf" file in XML format.
—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 11).
•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 direc-
tory 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 2-
Introduction Getting Started
FINE™/Turbo 1-3
3.1.4) or to create a new project (see section 2-3.1.1) for those computations.
The special characters, such as ü, ë and ê et al., are not allowed in the path name.
Off line files on Windows operation system are not supported.
The length of the path name should be less than 256.
FIGURE 1.2.3-1 Example of file management for a FINE™/Turbo project
Both the absolute and relative path names are used in ".iec" and ".run" files for the mesh and initial
solution files. When moving the project from one location to another location in the local machine
or between different machines (the same or different OS), the use of the relative pathnames allows
the user to:
•open the graphical user interface and (re)start calculation without the need to (re)link the mesh
and pathnames,
•open a solution file within CFView™ without the need to open the graphical user interface,
•start calculations in batch mode without the need to open the graphical user interface and
(re)link the mesh and pathnames.
The limitations on the use of relative pathnames are as follows:
•All files (mesh and computations) related to a given project must be located in hard-coded sub-
directories (e.g. _mesh).
•Keywords related to relative path in ".iec" and ".run" files are only vaild if the concerned files
are at the same level of the project file ".iec" or in subdirectories.
•Both the project and the directory in which it is included must have the same name. They can’t
be renamed.
•When duplicating or moving the project, the user must be able to copy either the entire project
(mesh files and computations with existing solutions), or a partial project (mesh files and com-
putations, restricted to ".run" files)
Getting Started How To Use This Manual
1-4 FINE™/Turbo
•Relative path is not compatible with FINE™/Design3D.
1-3 How To Use This Manual
1-3.1 Outline
This manual consists of five distinct parts:
•Chapters 1 and 2: introduction and description of the interface,
•Chapters 3 to 10: computation definition,
•Chapter 11: task management,
•Chapter 12: monitoring capabilities,
•Appendix A: used file formats,
•Appendix B: list of supported non-interfaced expert parameters,
•Appendix C: characteristics of steam tables.
At first time use of FINE™/Turbo it is recommended to read this first chapter carefully and cer-
tainly section 1-4 to section 1-6. Chapter 2 gives a general overview of the FINE™/Turbo interface
and the way to manage a project. For every computation the input parameters can be defined as
described in the Chapters 3 to 10. Chapter 11 gives an overview of how to run computations using
the Task Manager or using a script. Chapter 12 finally describes the available tools to monitor the
progress on a computation.
In Chapters 3 to 10, the expert user finds a section describing advanced options that are available in
expert user mode. Additionally Appendix B provides a list with all supported expert parameters on
the page Computation Steering/Control Variables in expert user mode. For each parameter a ref-
erence 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 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.
First Time Use Getting Started
FINE™/Turbo 1-5
A light bulb in the margin indicates a section with a description of expert parameters.
1-4 First Time Use
1-4.1 Basic Installation
When using FINE™/Turbo for the first time it is important to verify that FINE™/Turbo is properly
installed according to the installation note. The installation note provided with the installation soft-
ware 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™/Turbo 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™/Turbo and the desired compo-
nent 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™/Turbo 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 user manual.
1-4.2 Expert Graphics Options
a) Graphics Driver
The graphics area of the FINE™/Turbo interface uses by default an OPENGL driver that takes
advantage of the available graphics card. When the activation of OPENGL is causing problems,
FINE™/Turbo uses an X11 driver (on UNIX) or MSW driver (for Windows) instead.
It is possible to explicitly change the driver used by FINE™/Turbo 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.
Getting Started How to start the FINE™/Turbo Interface
1-6 FINE™/Turbo
The selection will take effect at the next session.
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 the FINE™/Turbo Interface
In order to run FINE™/Turbo, the following command should be executed:
On UNIX and LINUX platforms type: fine -print <Enter>
When multiple versions of FINE™/Turbo are installed the installation note should be
consulted for advice on how to start FINE™/Turbo in a multi-version environment.
On Windows click on the FINE™/Turbo icon in Start/Programs/NUMECA software/fine#.
Alternatively FINE™/Turbo 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.
Required Licenses Getting Started
FINE™/Turbo 1-7
1-6 Required Licenses
1-6.1 Standard FINE™/Turbo License
The standard license for FINE™/Turbo allows for the use of all basic features of FINE™/Turbo
including:
•IGG™ (see separate IGG™ manual),
•AutoGrid™ (see separate AutoGrid™ manuals),
•CFView™ (see separate CFView™ manual),
•Task Manager (see Chapter 11),
•Monitor (see Chapter 12).
1-6.2 Additional Licenses
Within FINE™/Turbo the following features are available that require a separate license:
•parallel computations (see Chapter 11),
•treatment of unsteady rotor-stator interfaces (see Chapter 8),
•harmonic method (see Chapter 8),
•transition (see Chapter 4 and Chapter 8),
•fluid-particle interaction (see Chapter 7),
•passive tracers (see Chapter 7),
•conjugate heat transfer (see Chapter 7),
•thermodynamic tables (see Chapter 3),
•cooling/bleed flow (see Chapter 8),
•ANSYS outputs (see Chapter 10),
•SubProject module (see Chapter 8),
•porous media (see Chapter 7),
•cavitation module (see Chapter 7).
•MpCCI Coupling (Chapter 7)
•Modal Coupling (Chapter 7)
•Mesh Deformation (Chapter 7)
•Aeroacoustics (Chapter 8)
•CPU Booster (Chapter 6)
Next to FINE™/Turbo other products are available that require a separate license:
•FINE™/Design 3D (3D inverse design, see separate user manual).
Getting Started Required Licenses
1-8 FINE™/Turbo
FINE™/Turbo 2-1
CHAPTER 2: Graphical User
Interface
2-1 Overview
When launching FINE™/Turbo 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™/Turbo 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™/Turbo 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.
To define a profile through the FINE™/Turbo interface a Profile Manager is included. The Profile
Manager is described in more detail in section 2-7.
FIGURE 2.1.0-1 Default FINE™/Turbo Interface
Graphical User Interface Project Selection
2-2 FINE™/Turbo
FIGURE 2.1.0-2 Complete overview of the FINE™/Turbo interface
2-2 Project Selection
When the FINE™/Turbo 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 Create New Project
To create a new project when launching the FINE™/Turbo interface:
1. click on the Create a New Project... icon ( ) in the Project Selection dialog box. A File
Chooser will appear, which allows to select a name and location for the new project.
The layout of the File Chooser depends on the used operating system but a typical layout is shown
in Figure 2.2.1-3. 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.
Main menu bar Icon bar
Computations
Parameters
button
Graphics area Parameters area
Mesh information
View
button
button
Grid Configuration (under license)
Project Selection Graphical User Interface
FINE™/Turbo 2-3
FIGURE 2.2.1-3 Typical layout of a File Chooser window
2. 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.
3. 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™/Turbo will automatically create a project file with this extension).
4. Click on OK (on UNIX) or Save (on Windows) to accept the selected name and location of the
new project.
A new directory is automatically created with the chosen name as illustrated in figure below indi-
cated 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 2.2.1-4 - (2)). Inside the project directory FINE™/Turbo creates automatically a subdirec-
tory "_mesh" (Figure 2.2.1-4 - (3)).
FIGURE 2.2.1-4 Directories managed through FINE™/Turbo
5. A Grid File Selection window (Figure 2.2.1-5) appears to assign a grid to the new project. There
are three possibilities:
•To open an existing grid click on Open Grid File (Figure 2.2.1-5 - 1.1). 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
(Figure 2.2.1-5 - 1.2). Set the parameters in this window as described in section 2-2.3 and click
OK to accept.
(1) project directory
(2)
(3)
automatically created
"_mesh" directory
(4) computation directory
Graphical User Interface Project Selection
2-4 FINE™/Turbo
•If the grid to be used in the project is not yet created use Create Grid File to start IGG™
(Figure 2.2.1-5 - 2.1). Create a mesh in IGG™ or AutoGrid™ (Modules/AutoGrid4 - Mod-
ules/AutoGrid5) and save the mesh in the directory "_mesh" of the new project. Click on
Modules/Fine Turbo and confirm "yes" to return to the FINE™/Turbo project. Select the cre-
ated mesh with the pull down menu (Figure 2.2.1-5 - 2.2) 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.
FIGURE 2.2.1-5 Grid File Selection window.
•When using the AutoBlade™ or FINE™/Design 3D modules it is not necessary to select a
grid. In that case close the Grid File Selection window (Figure 2.2.1-5 - 3) and select Mod-
ules/AutoBlade or Modules/Design 3D menu to use these modules.
2-2.2 Open 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.
2-2.3 Grid Units & 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 centimeters.
1.1
1.2
2.1
2.2 3
Project Selection Graphical User Interface
FINE™/Turbo 2-5
•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.
 If a 2D project is created by selecting Cartesian and 2 Dimensions, the mesh must have
K direction and Z direction perpendicular to the surface.
 Some options in FINE™/Turbo are linked to the used mesh configuration. For example,
the Cartesian mesh is not compatible with some TURBO features (Rotating Blocks, Azi-
muthal averaged output, ...). The user should select an appropriate coordinate system
according to the applications.
•Use Grid Configuration: This option is only available with a special license feature (Sub-
Projects). The user can choose whether or not to use the automatic grouping based on the grid
configuration file (.config). More information on the automatic grouping can be found in
Chapter 8. This choice can only be made when loading the mesh for the first time, it cannot be
changed afterwards.
FIGURE 2.2.3-6 Grid Units & Project Configuration window
 The mesh properties are always accessible after linking the mesh to the project through
the menu Mesh/Properties...
Graphical User Interface Main Menu Bar
2-6 FINE™/Turbo
2-3 Main Menu Bar
2-3.1 File Menu
2-3.1.1 New Project
The menu item File/New allows to create a new FINE™/Turbo project. When clicking on File/New
a File Chooser window appears. Browse in the Directory list to the directory in which to create a
new project directory (in the example of Figure 2.2.1-4 the directory "/home" 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 (Figure 2.2.1-4) created with the cho-
sen 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™/Turbo 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. 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 computa-
tion.
After the new project is created a Grid File Selection window (Figure 2.2.1-5) 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 win-
dow 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 be used in the project was not yet created use Create Grid File to start IGG™.
Create a mesh in IGG™ or AutoGrid™ (Modules/AutoGrid4 - Modules/AutoGrid5) and
save the mesh in the directory "_mesh" of the new project. Click on Modules/Fine Turbo and
confirm "yes" to return to the FINE™/Turbo project. Select the created mesh with the pull
down menu in the icon bar. A window will appear to define Grid Units and Project Configura-
tion. Set the parameters in this window as described in section 2-2.3 and click OK to accept.
 If the name of an already existing project is specified, this project file will be overwrit-
ten. 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 2-4.2.
2-3.1.2 Open Project
There are two ways to open an existing project file:
a) Use File/Open Menu
1. Click on File/Open.
2. A File Chooser window appears.
3. 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.
Main Menu Bar Graphical User Interface
FINE™/Turbo 2-7
4. Select the project file.
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) Select File From the List of Files in 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™/Turbo 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 and can be saved when FINE™/Turbo 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 (highlighted in blue in the Computations list). This menu is mainly use-
ful when the Task Manager is used (see Chapter 11 for a detailed description of the Task Manager).
 Together with the ".run" file, a ".batch" (UNIX) or ".bat" (Windows) file is saved. This
file can be used to launch the computation in batch mode, without the need of opening
Graphical User Interface Main Menu Bar
2-8 FINE™/Turbo
the interface. More information on how to use this ".batch" file can be found in
Chapter 11.
 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 com-
putation through the main menu (Solver/Start...).
2-3.1.6 Preferences
When clicking on File/Preferences... the Preferences window appears and 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 inde-
pendently 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 2.3.1-7). 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
are stored into the project file ".iec" in the same units as they appear in the interface (e.g. the rota-
tion speed is in [RPM]), but in the ".run" file, which is used by the flow solver, the numerical values
are always stored in SI units (e.g the rotation speed is in [rad/s]). The results can be visualized with
the flow visualization system CFView™ in the units specified in FINE™/Turbo.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 our local support
office for more information.
FIGURE 2.3.1-7 Project Units in the Preferences Window
(1)
(2) (3)
Main Menu Bar Graphical User Interface
FINE™/Turbo 2-9
b) Global Layout
In this section, the user may specify project independent preferences for the layout of the interface.
More specifically the user may activate or deactivate the balloon help (Show 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 ses-
sion of FINE™/Turbo. When FINE™/Turbo is closed and launched again the balloon help will
always be active by default.
Furthermore, the section allows the user to control the Number of curves that can be plotted in the
Convergence History page of the Task Manager. By default the parameter is set to 10 meaning that
only 9 curves can be plotted in the steering (more details in Chapter 12).
c) Solver Preferences
In this section, the user may select the calculation accuracy for the flow solver. Single and double
precision modes of the FINE™/Turbo solver are available. For most cases, the single precision
solver (much less demanding in memory consumption) will be sufficiently accurate and should be
considered as the default option. However, some special cases, such as very long thin pipe and con-
jugate heat transfer problems, may benefit from the double precision solver.
One of the most important criteriums to choose the double precision solver is the maximum dimen-
sion of the domain and its positioning in the 3D field. If the ratio is bigger than roughly
1e-6, the double precision solver should be considered. Where is the local cell size and is
the local coordinate value.
After selecting single or double precision solver, the value will be used as default value for new
projects.
2-3.1.7 Quit
Select the File/Quit menu item to quit the FINE™/Turbo integrated environment after confirmation
from the user. The active project will be saved automatically by default (Save Active Project acti-
vated).
Note that this action will not stop the running calculations. A FINE TaskManager window will
remain open for each running computation. Closing the FINE TaskManager window(s) will kill the
running calculation(s) after confirmation from the user.
2-3.2 Mesh Menu
2-3.2.1 View On/Off
This toggle menu is used to visualize the grid in FINE™/Turbo GUI. 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-
Δxx
local
⁄
Δx
xlocal
Graphical User Interface Main Menu Bar
2-10 FINE™/Turbo
6.6). 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™/Turbo interface:
• the View subpad (see section 2-6.3 for more details),
•the mesh information area (see section 2-6.4 for more details),
•the graphics area will appear in the FINE™/Turbo interface (see section 2-6.6 for more
details),
•the Viewing buttons will appear on the bottom of the graphics area. Their function is described
in section 2-6.7).
The graphics area and the Viewing buttons will disappear when the mesh is hidden (Mesh/View
On/Off). All the tools will disappear when the mesh is unloaded (Mesh/Unload).
2-3.2.2 Repetition
This menu opens the following dialog box to control the repetition of the blocks when the mesh is
visualized:
For each block, the number of repetition desired can be set in the Nb Repet entry. The repetition of
all blocks can be displayed or hidden respectively by pressing the Show or Hide button.
2-3.2.3 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™/Turbo window.
 This feature is only available on UNIX systems.
2-3.2.4 Unload
Mesh/Unload clears the mesh from the memory of the computer.
2-3.2.5 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 Con-
figuration window allows 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.
Main Menu Bar Graphical User Interface
FINE™/Turbo 2-11
•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.
FIGURE 2.3.2-8 Mesh Properties dialog box
2-3.3 Solver Menu
This menu gives access to the FINE™/Turbo solver, which is a powerful 3D code dedicated to
Navier-Stokes or Euler computations. The FINE™/Turbo solver uses the computational parameters
and boundary conditions set through the FINE™/Turbo GUI and can be fully controlled both from
the FINE™/Turbo Solver Menu and from the Task Manager (see Chapter 11).
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 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 pro-
duced by a previous calculations on that computation will be overwritten with the new result val-
ues. It also implies that the initial solution will be created from the values set in the Initial Solution
page.
 To restart a computation from an existing solution the solver should be also started using
the Solver/Start... menu. On the Initial Solution page the initial solution has to be spec-
ified from an existing file (".run"). Chapter 9 describes the several available ways to
define an initial solution.
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 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 files and CFView™ files) exactly as if the computation
was finished. This operation may take from few seconds to few minutes depending on the
Graphical User Interface Icon Bar
2-12 FINE™/Turbo
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.
•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.
2-3.4 Modules Menu
Clicking on the menu item Modules shows a pull down menu with the available modules. The first
four items are related to geometry and mesh definition:
•IGG™ is the interactive geometry modeller and grid generator,
•AutoGrid™ 4 & AutoGrid™ 5 are the automated grid generators for turbomachinery.
•AutoBlade™ is the parametric blade modeller,
Furthermore a design module is available:
•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 11.
To start the flow visualization from FINE™/Turbo, click on the Modules/CFView ... 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 inter-
mediate results of a computation, wait until the flow solver has written output. For more informa-
tion about the flow visualization system, please refer to the CFView™ User Manual.
Finally, the Harmo2Time module launches a reconstruction tool that will generate unsteady flow
simulation results from existing harmonic flow simulation results, for more details, see Chapter 8-4.
2-4 Icon Bar
The icon bar contains several buttons that provide a shortcut 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 four buttons on the left of the icon bar are shortcuts for items of the File menu:
The New Project icon is a shortcut for the menu item File/New.
The Open Project icon is a shortcut for the menu item File/Open.
Icon Bar Graphical User Interface
FINE™/Turbo 2-13
The Save Project icon is a shortcut for the menu item File/Save.
The Save RUN Files icon is a shortcut for the menu item File/Save Run Files.
2-4.2 Grid Selection Bar
By clicking on the icon 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 at least
the files with extensions ".igg", ".geom", ".bcs" and ".cgns" need to be available in the
same directory with the same name as for the chosen mesh.
If a mesh has already been linked to the current project and another mesh is opened, FINE™/Turbo
will check the topological data in the project and compare it against the data in the mesh file. If the
topological data is not equal, a new dialog box (Figure 2.4.2-9) will open. This dialog box informs
the user that a merge of the topologies is necessary and will also show at which item the first differ-
ence was detected.
The three following possibilities are available:
•Merge Mesh Definition will merge the project and mesh data. For example, if a new block has
been added to the mesh. 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 allowing 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™, where it can be modified.
FIGURE 2.4.2-9 Merge Topology dialog box
The merge process may also occur when opening an existing project, or when switching between
IGG™ and FINE™/Turbo, because the check of the topology is performed each time when a
project is read.
Graphical User Interface Computation Management
2-14 FINE™/Turbo
In case the mesh file no longer exists, or is 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 is selected and its topology is 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 details on this window.
2-4.3 Solver Buttons
Three buttons allow to start, suspend and kill the active computation:
The Start Flow Solver icon is a shortcut for the menu item Solver/Start....
The Suspend Flow Solver icon is a shortcut for the menu item Solver/Suspend....
The Kill Flow Solver icon is a shortcut for the menu item Solver/Kill....
2-4.4 Module Buttons
Two buttons allow to start the pre- and post-processor:
The Start IGG icon is a shortcut for the menu item Modules/IGG.
The Start CFView icon is a shortcut 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 Computation Management
When selecting the Computations subpanel at the top left of the interface a list of all the computa-
tions in the project is shown. The active computation is highlighted in blue 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 modifica-
tions are applied.
 When selecting multiple computations, the parameters of the active page in the "parame-
ters area" are copied from the first selected computation to all other computations.
Graphical Area Management Graphical User Interface
FINE™/Turbo 2-15
With the buttons New Computation and Remove computations can be created or removed. When
clicking on New Computation the active computation (highlighted in blue) 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 Computation. 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>. These options are also available when click-right on the
active computation.
Two buttons Create Performance Curve and Edit Performance Curve are dedicated to the creation
and management of the performance curve for turbomachinary. More details can be found in
Chapter 8-10.
FIGURE 2.5.0-10 Computations subpanel
2-6 Graphical Area Management
2-6.1 Configuration Management
When creating a mesh within AutoGrid™ or IGG™, the multiblock data structure can become very
complex. A database, named Grid Configuration, is created automatically at the end of the mesh
generation, saved together with the project into a file ".config" (more details can be found in the
IGG™ or AutoGrid™ User Manuals).
To access the grid configuration menu in FINE™/Turbo, the Use Grid Configuration option has to
be activated when linking the mesh for the first time, see section 2-2.3. This option is only available
through a special license feature (SubProjects).
FIGURE 2.6.1-11 Use Grid Configuration
Right-Click
Graphical User Interface Graphical Area Management
2-16 FINE™/Turbo
The grid configuration describes (as presented in the figure below) the mesh structure of the project
as a tree through which the user can access the domain structure. The structure is defined as a set of
fluid and solid domains interconnected together through domain interfaces. Each domain contains a
set of subdomains and a set of interfaces. Each domain interface contains a type of boundary condi-
tion, a type of free boundary condition and the possible connected domain reference.
FIGURE 2.6.1-12 Grid Configuration control
This data structure is very useful. It can be used to reduce the time needed to analyse and visualize
the mesh of a project, to setup the boundary conditions within FINE™/Turbo and to create sub-
projects starting from the main project (see Chapter 8 for more details).
2-6.2 Parameters Management
The Parameters subpanel on the left, below the Computations subpanel, is presenting a directory
structure allowing the user to go through the available pages of the project definition. The "parame-
ters 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.
FIGURE 2.6.2-13 Parameters subpanel
2-6.3 View Area
When the mesh is loaded with Mesh/View On/Off, a subpanel is shown in the list on the left: the
View subpanel. By default the View subpanel 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
Graphical Area Management Graphical User Interface
FINE™/Turbo 2-17
and/or block groups of the mesh and allow to create new groups. This possibility is only useful in
the FINE™/Turbo GUI 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).
FIGURE 2.6.3-14 View subpanel
The third page provides visualization commands on the grid. It consists of two rows: a row of but-
tons and a row of icons.
The row of buttons is used to determine the viewing scope, that is the grid scope on which the view-
ing commands provided by the icons of the second row will apply. There are five modes determin-
ing 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 in yellow. Simply click-left 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.
Graphical User Interface Graphical Area Management
2-18 FINE™/Turbo
 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.
2-6.4 Mesh Information
When the mesh is loaded also the Mesh Information area is shown containing the following infor-
mation for the selected section of the mesh:
FIGURE 2.6.4-15 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.
2-6.5 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 dis-
played.
Toggles face grid.
Toggles shading.
Icon Command
Active block, face, edge and segment indices
Number of blocks, faces, edges and segments
for the active topology
Graphical Area Management Graphical User Interface
FINE™/Turbo 2-19
2-6.6 Graphics Area
button to resize
Graphics area
FIGURE 2.6.6-16 Resizing of 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 Grid page, in the View subpanel on the left, and the viewing buttons can be
used to influence the visualization of the mesh. The View subpanel is described in section 2-6.3 and
the viewing buttons area are described below.
2-6.7 Viewing Buttons
The viewing buttons are used to perform viewing manipulations on the active view, such as scroll-
ing, 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.
2-6.7.1 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 changes direction at each click.
Graphical User Interface Graphical Area Management
2-20 FINE™/Turbo
2-6.7.2 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 2-6.3.
2-6.7.3 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.
2-6.7.4 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 or use the mouse wheel
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.
The 3D viewing tool is also accessible with the <F1> key.
2-6.7.5 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 counter-
clockwise rotation will be performed, proportional to the mouse displacement. Release the
button when finished.
Graphical Area Management Graphical User Interface
FINE™/Turbo 2-21
•Middle: press and drag the middle mouse button to the left or to the right. A continuous rota-
tion will be performed, clockwise or counter-clockwise. Release the button when finished.
2-6.7.6 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.
2-6.7.7 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. Move the mouse to the active view.
2. Press and drag the left mouse button to select the rectangular region.
3. Release the button to perform the zoom operation.
These operations can be repeated several times to perform more zooming.
Press <q> or click the right mouse button to quit the option.
The region zoom is also accessible with the <F2> key.
2-6.7.8 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).
2-6.7.9 Original Button
The original button is used to fit the content of the view and to change back to the default orienta-
tion of the camera.
2-6.7.10 Cutting 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 trans-
parent). It is highly advised to deactivate the plane transparency when using X11 driver to
increase the execution speed.
Graphical User Interface Profile Management
2-22 FINE™/Turbo
2-7 Profile Management
When a law is defined by a profile clicking on the button right next to the pull down menu will
invoke a Profile Manager window.
FIGURE 2.7.0-17 Profile Manager for boundary conditions parameters
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 option Surface data allows the user to impose a 2D profile. The formats of the profile files are
explained in Appendix A where all file formats used by FINE™/Turbo and the flow solver are
detailed.
If the mouse cursor is placed over a point in the graph window, this point is highlighted and the cor-
responding 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™/Turbo window.
 When imposing profiles, a zero extrapolation is applied for point located outside the
defined range of the profile. E.g. if the density profile is given for a pressure between 10
bar and 100 bar, the density at 1 bar will be the one imposed at 10 bar.
FINE™/Turbo 3-1
CHAPTER 3: Fluid Model
3-1 Overview
Every FINE™/Turbo project selects a fluid and its properties, defined by:
1. Using the fluid defined in the project file of which the properties are shown on the fluid selec-
tion page (see section 3-2.1), or
2. 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
3. creating a new fluid (see section 3-2.3).
In the next section the interface is described in detail, including advises for use of the fluid defini-
tions. The theoretical background for the different fluid models is described in the theoretical man-
ual.
Fluid Model The Fluid Model in the FINE™/Turbo GUI
3-2 FINE™/Turbo
3-2 The Fluid Model in the FINE™/Turbo GUI
FIGURE 3.2.0-1 Fluid Selection page
3-2.1 Properties of Fluid Used in the Project
Every FINE™/Turbo 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 default fluid is a perfect gas,
pre-defined by FINE™/Turbo. 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 details on each of these types, please see Chapter 2 in the theoretical manual. For the first
three fluid types, the properties can be defined through the interface as described in section 3-2.3.
To add a condensable fluid to the list of fluids proposed by default, please use TabGen to generate
the appropriate tables.
To modify the properties of the fluid used, a fluid can 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. For each fluid the
fluid type and the permissions are defined.
list of properties
list of pre-defined fluids
filters
The Fluid Model in the FINE™/Turbo GUI Fluid Model
FINE™/Turbo 3-3
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 only have Read Only
permissions.
If the user selects a fluid from the list, the selection will be highlighted and the properties are dis-
played 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.
FIGURE 3.2.3-2 Fluid Wizard
Once the fluid name and type are correctly set, click on Next>> to go to the next page of the wiz-
ard. 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 dia-
log 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
law is defined by a formula, the Formula Editor can be opened by clicking on the button ( ) right
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™/Turbo interface. As a consequence, this information will not be available to
Fluid Model The Fluid Model in the FINE™/Turbo GUI
3-4 FINE™/Turbo
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 is allowed.
•The constant specific heat ratio ( ) characteristic of the fluid.
•The heat conductivity which may be constant, defined by a polynomial or a profile in tempera-
ture or specified through a constant Prandtl number.
•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 pol-
ynomial 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 but-
ton ( ) right next to the pull down menu.
FIGURE 3.2.3-3 Sutherland Law Parameters
The default law uses the dynamic viscosity but the user can specify the kinematic viscosity if
required.
3-2.3.2 Definition of a Real Gas
A real gas is defined by laws for the dependence of and/or gamma with the temperature and/or
gas constant r.
By default when adding a new fluid, the recommended specific heat law consists on imposing
with the temperature and the gas constant r.
The user can either define a profile, using the Profile Manager, or impose a polynomial approxima-
tion using the Formula Editor. In this last case, the polynomials take the following form:
(3-1)
(3-2)
where the coefficients are chosen by the user
and set in the dialog box for and g respectively. In the definition of real gas properties, lower and
upper bounds of temperature variations [Tmin-Tmax] allowed in the domain must be provided.
cp
cpcv
⁄
cp
cp
cpT() A0T3– A1T2– A2T1– A3A+4T1A5T2A6T3
+++ ++=
γT() B0T3– B1T2– B2T1– B3B+4T1B5T2B6T3
+++ ++=
A0A1A2A3A4A5A6B0B1B2B3B4B5and B6
,,,,,,,,,,,,
cp
The Fluid Model in the FINE™/Turbo GUI Fluid Model
FINE™/Turbo 3-5
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.
FIGURE 3.2.3-4 New Fluid Definition - Real Gas
For the default definition of a real gas, the user has to specify:
•The gas constant r and the specific heat at constant pressure , which depend on the tempera-
ture through a polynomial or a profile. In both cases, the user has to specify the temperature
range over which the specific heat is defined. Furthermore there are alternative modelling meth-
ods for a real gas that consists on:
—involving a compressibility factor and two laws defining the dependence of and gamma
with the temperature.
—constant r model with gamma dependent on the temperature and calculated from r and
gamma.
 For the pre-defined fluids, the value of is defined as a function of the temperature
through a profile. These profiles have been computed for a constant pressure 100,000Pa.
•The heat conductivity, which can be constant, defined by a polynomial or a profile in tempera-
ture or specified through a constant Prandtl number.
•The viscosity law, which can be constant, dependent on temperature or specified by the Suther-
land law. In case the viscosity depends on the temperature the user can specify the law through a
polynomial or as profile. 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 default law uses the dynamic viscosity but the user can specify the kinematic
viscosity if required, see Figure 3.2.3-3.
cp
cp
cp
cp
Fluid Model The Fluid Model in the FINE™/Turbo GUI
3-6 FINE™/Turbo
Compared to a perfect gas computation ( and g 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 a preliminary run with averaged physical properties. However, convergence difficulties
may arise during the convergence process (say the first 100-200 iterations) if either the allowed
temperature range is too large or if the properties are expected to vary significantly in the allowed
temperature range. At these occasions, it is often useful to make an equivalent perfect gas computa-
tion, with average properties, in order to remove any temperature dependency and ease the conver-
gence process.
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 is allowed.
•The heat conductivity, which can be constant, defined by a polynomial or a profile in tempera-
ture or specified through a constant Prandtl number.
•The viscosity law, which can be constant, dependent on temperature or specified by the Suther-
land law. In case the viscosity depends on the temperature the user can specify the law through a
polynomial or as profile. 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 default law concerned the dynamic viscosity but the user can specify the kine-
matic if required, see Figure 3.2.3-3.
•The density law, which can be pressure dependent (using a polynomial law or as a profile
through the Profile Manager) or following the 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
momentum equation and the energy equation in order to model the gravitational effect (i.e. nat-
ural 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. 4-19).
3-2.3.4 Definition of a Condensable Fluid
The aim of the condensable fluid module is modelling the real thermodynamic properties of the
fluid by means of interpolation of the variables from dedicated tables.
 A generation tool TabGen for the condensable tables is provided in FINE™/Turbo. The
details can be found in Appendix D.
The module can be used for a single-phase fluid of which the properties are too complex to be
treated with a perfect or real gas model. It can also be used in order to treat thermodynamic condi-
tions 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. However
the hypothesis of an equilibrium mixture is not valid if the dryness (wetness) fraction exceeds 20%.
cp
cp
The Fluid Model in the FINE™/Turbo GUI Fluid Model
FINE™/Turbo 3-7
The module can not be used above these fractions, as it completely ignores evaporation-condensa-
tion phenomena.
The approach that has been adopted in the FINE™/Turbo solver consists of using a series of ther-
modynamic 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 an input, but presents the advan-
tage that no iterative inversion of the tables is done in the solver, with as a consequence a very small
additional CPU time.
By default, two sets of thermodynamic tables are provided in the standard FINE™/Turbo package:
Refrigerant R134a and Water-Steam tables. The other thermodynamic tables can be generated
using TabGen by the user or provided by NUMECA, upon request.
In order to use a condensable gas as a fluid model, the user has to copy the provided tables in a user-
defined subdirectory called "/tables_fluidname/". The location of this subdirectory is platform
dependent:
•On Unix/Linux systems:
"/NUMECA_INSTALLATION_DIRECTORY/fine#/COMMON/thermodynamic_tables/"
•On Windows systems:
"/NUMECA_INSTALLATION_DIRECTORY/Fine#/bin/thermodynamic_tables/"
The subdirectory has to be created before launching FINE™/Turbo. When the subdirectory is exist-
ing, the condensable gas is recognized by FINE™/Turbo and the fluid will appear in the list with
respectively Fluid Name and Fluid Type as "Condensable__fluidname" and "Condensable Fluid".
 The condensable fluid option is not compatible with the use of cooling/bleed module
and/or upwind schemes for space discretization.
a) Selection of the Viscosity, Conductivity, and Specific Heat
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).
Since the complete integration of the condensable fluid module in the user interface is not yet fin-
ished, 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. create a perfect gas,
2. enter the desired properties for the viscosity and conductivity,
3. save the corresponding computation,
4. 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.
Fluid Model The Fluid Model in the FINE™/Turbo GUI
3-8 FINE™/Turbo
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 3.2.3-5 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 temperature range, in which the polynomial function is
defined. Press <Enter> after each entry to validate the input. Values outside of the specified temper-
ature range, will be considered constant and equal to the minimum or maximum value (as shown in
the graph in Figure 3.2.3-5).
 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 ( ) next to the pull down menu will start
the Profile Manager.
The Profile Manager is used to interactively define and edit profiles for both fluid and boundary
condition parameters. To input a profile, the user has to enter the corresponding coordinates in the
two columns on the left. The graph is updated after each coordinate entry (after pressing the
<Enter> key).
The button Import can be used to import a profile, which is already existing as a data file on the
disk. The Export button is used to store the current data in the profile manager as a data file (for
example to share profiles between different projects and users). The format of the profile files is
explained in detail in Appendix A.
If the mouse cursor is placed over a point in the graph window, this point is highlighted and the cor-
responding coordinates on the left will be also highlighted, giving the user the possibility to verify
the profile.
The Fluid Model in the FINE™/Turbo GUI Fluid Model
FINE™/Turbo 3-9
The button OK will store the profile values into the fluid definition.
FIGURE 3.2.3-6 Profile Manager for fluid parameters
 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.
 Only uniform distributions should be entered in the Profile Manager. Non-uniform distri-
butions will be converted to a uniform distribution by the FINE™/Turbo solver.
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 available fluids.
 Information linked to fluid removal is stored in the fluid database only when closing the
FINE™/Turbo interface. As a consequence, this information will not be available to
other users until this operation is 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
When the user has the write permission for a fluid, the properties of the selected fluid can be modi-
fied 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™/Turbo interface. As a consequence, this information will not be available to
other users until this operation is completed. A message will however warn users that the
fluid properties have been modified by the owner.
Fluid Model The Fluid Model in the FINE™/Turbo GUI
3-10 FINE™/Turbo
3-2.6 Show Fluid Properties
When the user does not have the write permission (Read Only) for a fluid the Show Fluid Proper-
ties... button opens the wizard with the properties of the fluid. In this case it is not possible to mod-
ify any of the properties in the wizard but the user has access to visualize the 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 out of
the complete 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 data-
base is stored locally and user defined fluids are accessible with full permissions to all
Windows users.
 The filters are used only to browse the fluid list and not to change the current fluid asso-
ciated to the active computation except if selected in the list by left-click on it.
3-2.8 Import Fluid 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™/Turbo is automatically checking if the fluid is existing or not in the fluid data-
base. 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). If the fluid is not existing in the fluid database, no fluid will be
selected but the fluid parameters defined in the project will be kept.
3-2.9 Expert Parameters
In this section, the expert parameters which can be used in the definition of the fluid type can be
found. This is only a summary to know directly the expert parameters related to the definition of a
fluid.
All expert parameters related to fluid definition are available in Expert Mode in the Control Vari-
ables page. For these expert parameters the default values only have to be changed in case the user
has specific wishes concerning the fluid modelling.
PRT(real): Allows to define the turbulent Prandtl number (default value = 1.0).
CLIPCG(integer): The thermodynamic tables are generated in a given range of thermodynamic
variables. When the thermodynamic variables are not in the given range, the
expert parmeter CLIPCG can be used to control the computing method of the
dependent thermodynamic variable.
0 (default): the dependent thermodynamic variable is extrapolated from the
interior field.
1: a clipping value will be used for the dependent thermodynamic variable.
FINE™/Turbo 4-1
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 char-
acteristics 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
•the characteristic scales defining the Reynolds number of the flow,
•the reference values of the temperature and pressure in the flow.
This chapter is organised in the following way:
•section 4-2 describes the interface and best practice for the definition of the mathematical
model and especially the available turbulence models,
•section 4-3 provides details on the Reynolds number related information and reference values.
The interface and best practice for unsteady computations will be described in Chapter 6,
The interface and best practice for harmonic method will be described in Chapter 8,
Flow Model Mathematical Model
4-2 FINE™/Turbo
FIGURE 4.1.0-1 Flow Model page.
4-2 Mathematical Model
4-2.1 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.
Since the Reynolds number has no meaning for Euler calculations this number is not displayed
when Euler flow is selected.
4-2.2 Laminar Navier-Stokes
When selecting Laminar Navier-Stokes equations the only effect is on the thermodynamic prop-
erty of the flow. The viscosity will be the laminar kinematic viscosity and thus does not contain any
turbulent component.
4-2.3 Turbulent Navier-Stokes
When selecting Turbulent Navier-Stokes equations, turbulence is taken into account depending on
the chosen turbulence model. In FINE™/Turbo, several turbulence models are available:
•Algebraic model (0-equation):
—Baldwin-Lomax
•1-equation model:
Mathematical Model Flow Model
FINE™/Turbo 4-3
—Spalart-Allmaras
—Spalart-Allmaras (Extended Wall Function)
—SARC, see Chapter 4-2.4.2
—SARC (Extended Wall Function), see Chapter 4-2.4.2
•2-equation models:
—k-ε (Extended wall function)
—k-ε (Standard wall function), see Chapter 4-2.4.2
—k-ε (Low Re Yang-Shih)
—k-ε (Low Re Chien)
—k-ε (Low Re Launder-Sharma)
—Shear Stress Transport (SST)
—SST (Extended wall function)
—EARSM
—EARSM (Extended wall function)
—k-ω (Wilcox)
•4-equation model:
—v2-f (code friendly)
For the Baldwin-Lomax model, algebraic formula is used to compute the turbulent data and conse-
quently no additional input is needed. For all the 1/2/4 equation(s) models, additional equation(s)
are solved and consequently suitable initial and boundary conditions must be defined in the inter-
face.
The DES (Detached Eddy Simulations) model has been implemented in FINE™/Turbo. For more
information, please contact your local support office.
In the following sections, the parameters related to the turbulence models are described.
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 varying in space and time. The user can specify the time or spatial variations
through the profile manager.
•k-ω, SST and EARSM models: the values of the turbulent quantities (k and ε) must be defined.
They might be constant or varying in space and time. The user can specify the time or spatial
variations through the profile manager. The value for ω is determined according to:
, with β*=0.09 (4-1)
•v2-f model: the values of the turbulent quantities (k and ε) must be defined. They might be
constant or varying in space and time. The user can specify the time or spatial variations
through the profile manager. The value of v2 is deduced by assuming an isotropic turbulence.
ωε
β∗k
---------
=
Flow Model Mathematical Model
4-4 FINE™/Turbo
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 a
constant or initial solution for turbomachinery is chosen.
•k-ω, SST and EARSM models: the initial values of the turbulent quantities (k and ε) are speci-
fied by the user if a constant or initial solution for turbomachinery is chosen. The value for ω is
determined according to Eq. 4-1.
•v2-f model: the initial values of the turbulent quantities (k and ε) are specified by the user if a
constant or initial solution for turbomachinery is chosen. The value of v2 is deduced assuming
an isotropic turbulence.
It is not recommended to use a previously computed solution with different turbulence
model. For k-ε models, the Chien and the Launder-Sharma models belong to the same
family (zero value of ε at the wall) while the standard and Yang-Shih model belong to a
second family (non zero value of ε at the wall). Launching a restart from a previously
computed solution is only allowed as long as the user sticks to the same family.
4-2.4 Expert Parameters for Turbulence Modelling
4-2.4.1 Interfaced Expert Parameters
In expert mode additional parameters related to turbulence modelling are available when using the
turbulence models with extended wall functions. 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).
•When selecting a rough solid wall two additional parameters have to be specified: the equiva-
lent roughness height and the zero-displacement plane (k0 and d0).
4-2.4.2 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.
Calculation of the wall distances
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.
NREPET(integer): allows to take into account the periodicity of the computed domain. 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 (default
value =1).
Mathematical Model Flow Model
FINE™/Turbo 4-5
NSUBM(integer): is the maximum number of subdomains a domain is split into. Its value is suffi-
ciently high and it must be changed only if an error message informs the user to
increase it (default value = 1000).
NTUPTC(integer): is the number of patches whose sub-patches will be searched. In a very com-
plex geometry, the value of this parameter can be increased if the calculation of
the wall distances fail (default value = 100).
The computed wall distances should be removed from the mesh first before relaunch-
ing a computation with a different value of NTUPTC. To remove the computed wall dis-
tances, you should open your mesh in IGG™ and simply save it again.
RTOL(real): maximum angle allowed between two normals of a patch (default value = 1.8).
When the value of IDISTN is 1, the value of RTOL has to be set as the default
value (1.8).
When problems occur during the wall distance calculation (wall distance not equal to
0 on the wall), it is recommended to increase the value of NTUPTC (and to reduce RTOL
if the wall distance gradient is not smooth). Please keep in mind that increasing this
value will slow down the computing of the wall distances.
IDISTN(integer): algorithm for wall distance calculation:
0 : old algorithm
1: new algorithm
2 (default): review of new algrithm (advised for 64 bits platforms)
Limiters for all of the turbulence models
MAVRES(real): denoted here . This parameter limits the variation of the turbulence variables
for each Runge-Kutta stage. Denoting the new value of or as , the fol-
lowing restrictions are imposed when MAVRES > 0:
(4-2)
(4-3)
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. 4-3 is not applied to the turbulent dissipation rate
(ε) when this tends to increase, in order to avoid excessive values of the turbu-
lent viscosity.
If MAVRES = 0, only the restriction defined in Eq. 4-2 is applied (avoiding
negative values)
If MAVRES < 0, the restriction is:
(4-4)
ζ
k
ε
qn+1
qn+1 max qn+1 EPS,ζqn
,()=
qn+1 min qn+1 2ζ–()qn
,()=
qn1+ qn
–1ζ+()qn1+ qn
–()
1qn1+ qn
–
qn
--------------------------
+



---------------------------------------------
=
Flow Model Mathematical Model
4-6 FINE™/Turbo
MAVREM(real): a similar system is applied to the multigrid corrections with the expert parame-
ter MAVREM, denoted below as :
If MAVREM > 0:
If MAVREM = 0: restriction to positive values
If MAVREM < 0:
MUCLIP(real): controls the maximum allowable value for the ratio MUT/MU in the flow field
but not on boundary conditions (default value = 5000).
KEGRID(integer): allows the use of a particular full multigrid strategy. The Baldwin-Lomax
model is used on the coarse grids during the full multigrid stage and the k, ε, v2
and f initial solution is obtained from the Baldwin-Lomax model solution. This
parameter is not used for the Spalart-Allmaras model.
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.
Baldwin-Lomax
IATFRZ(integer): control the interaction of the model with the multigrid system
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(integer): freeze the turbulent viscosity field if the fine grid iteration exceeds ITFRZ
(default value = 1000000).
RESFRZ(integer): freeze the turbulent viscosity field if the fine grid residual is lower than RES-
FRZ (default value = -12).
Spalart-Allmaras
NUTFRE(real): constant to initialize the turbulent viscosity field (default value = 0.0003).
ITURRC(integer): the Spalart-Allmaras turbulence model with/without extended wall function
does not take the rotation and curvature effects into account. Modifications
have been brought in order to consider these effects. The modified Spalart-All-
maras model is marked as SARC model.
0(default): use the Spalart-Allmaras model, which does not take the rotation/
curvature effects into account.
2: use the SARC model, which takes the rotation/curvature effects into account.
ζ
qn1+ qn
–1ζ–()qn
<
qn1+ qn
–1ζ+()qn1+ qn
–()
1qn1+ qn
–
qn
--------------------------
+



---------------------------------------------
=
Mathematical Model Flow Model
FINE™/Turbo 4-7
k-ε models
CMU(real): constant for the k-ε model (default value = 0.09).
CE1(real): constant for the k-ε model (default value = 1.44 automatically set to 1.35 for
the Chien k-ε model).
CE2(real): constant for the k-ε model (default value = 1.92 automatically set to 1.8 for the
Chien k-ε model).
SIGK(real): constant for the k-ε model (default value = 1.).
SIGE(real): constant for the k-ε model (default value = 1.3).
PRT(real): constant for the k-ε model - the turbulent Prandtl Number (default value = 1.).
INEWKE(integer):allows the user to activate the k-ε (Standard wall function) model when the k-ε
(Extended wall function) model is selected in the interface:
0: activate the the k-ε (Standard wall function) model.
10 (default): use the k-ε (Extended wall function) model.
LTM AX(real): maximum turbulent length scale (default = 1.E+6),
-1: control of turbulent length scale with automatic clipping.
IYAP(integer): 1: applies the Yap’s modification to control the turbulent length scale.
0 (default): The value of the expert parameter LTMAX must be the default
value.
TEDAMP(real): 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 in the factor ; a minimum of TEDAMP multipli-
cation factor of the clipping value (EPCLIP) is used for to compute the tur-
bulent viscosity,
<= 0: the minimum values used for and correspond to the expert parameter
EPS,
PRCLIP(real): sets an upper bound for the ratio between production and dissipation (default
value = 50).
LIPROD(integer): corresponds to a linearization of the production term (default = 1) when strain
rate is large (i.e. impinging flow) and PRCLIP has no effect anymore on the
flow field.
EKCLIP(real): clipping value for the turbulent kinetic energy k (default value = 1.E-5).
EPCLIP(real): clipping value for the turbulent dissipation rate ε (default value = 1E-5).
IUPWTE(integer): uses an upwind scheme for the convection of k-ε instead of a centre scheme
(default = 1).
IKENC(integer): solves the k-ε equations with a non-conservative approach (default = 1).
IKELED(integer): (= 1) activates the LED scalar scheme for k-ε instead of the standard central
scheme (default = 0).
IOPTKE(integer): optimized implementation for k-ε (Yang-Shih, Wall function, Lauder Sharma)
(default = 1).
k
1T⁄
ε
k
ε
Flow Model Mathematical Model
4-8 FINE™/Turbo
All the above mentioned limiters are very important for the robustness of k-ε compu-
tations. With the exception of the length scale LTMAX all limiters are given appropriate
defaults and it is not recommend to modify them.
v2-f model
CMUV2F(real): constant for the v2-f model (default value = 0.22),
C1F(real): constant for the v2-f model (default value = 1.4),
C2F(real): constant for the v2-f model (default value = 0.3),
CL(real): constant for the v2-f model (default value = 0.23),
CET(real): constant for the v2-f model (default value = 70.0),
CE2V2F(real): constant for the v2-f model (default value = 1.9),
SIGE(real): constant for the v2-f model (default value = 1.3),
SIGK(real): constant for the v2-f model (default value = 1),
EKCLIP(real): clipping value for the turbulent kinetic energy k (default value = 1.E-5),
EPCLIP(real): clipping value for the turbulent dissipation rate ε (default value = 1E-5),
k-ω (Wilcox)
The parameters for the k-ω (Wilcox) model are hard coded. The user cannot modify the default val-
ues.
Shear Stress Transport (SST)
GAM1(real): constant for the SST model (default value = 0.5532),
GAM2(real): constant for the SST model (default value = 0.4403),
BETA1(real): constant for the SST model (default value = 0.075),
BETA2(real): constant for the SST model (default value = 0.0828),
SICK1(real): constant for the SST model (default value = 0.85),
SICK2(real): constant for the SST model (default value = 1.0),
SIGO1(real): constant for the SST model (default value = 0.5),
SIGO2(real): constant for the SST model (default value = 0.856),
A1SST(real): constant for the SST model (default value = 0.31),
BETSST(real): constant for the SST model (default value = 0.09).
EARSM
GAM1(real): constant for the EARSM model (default value = 0.5532),
GAM2(real): constant for the EARSM model (default value = 0.4403),
BETA1(real): constant for the EARSM model (default value = 0.075),
Mathematical Model Flow Model
FINE™/Turbo 4-9
BETA2(real): constant for the EARSM model (default value = 0.0828),
SICK1(real): constant for the EARSM model (default value = 0.5),
SICK2(real): constant for the EARSM model (default value = 1.0),
SIGO1(real): constant for the EARSM model (default value = 0.5),
SIGO2(real): constant for the EARSM model (default value = 0.856),
A1SST(real): constant for the EARSM model (default value = 1.245),
BETSST(real): constant for the EARSM model (default value = 0.09).
4-2.5 Best Practice for Turbulence Modelling
4-2.5.1 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 Rey-
nolds 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 gen-
eral necessary to predict adequately the turbulence effects on the flow-field behaviour.
To 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,
•if necessary, setting expert parameters to procure convergence.
4-2.5.2 First Step: Choosing a Turbulence Model.
A turbulence model is chosen based on the specific application. Table 4-1 states the most appropri-
ate 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".
According to the method accounting for viscous effects close to the wall, the turbulence models can
be divided into two types: high Reynolds number turbulence models and low Reynolds number tur-
bulence models. Please note that here "high Reynolds number" and "low Reynolds number" refer to
the local turbulent Reynolds number formed by the turbulent fluctuation , turbulent
length scale and kinematic viscosity . The high Reynolds number turbulence models assume
that the flow near the wall behaves like a fully developed turbulent boundary layer and prescribe
boundary conditions by employing wall functions. The viscous sublayer will not be resolved. In
FINE™/Turbo, both standard wall function and extended wall function are available, see the theo-
retical manual for the detailed information. The low Reynolds number turbulence models resolve
the entire boundary layer, including the viscous sublayer where the viscous diffusion is much larger
that the turbulent one. Thus, sufficiently fine grid should be used inside the boundary layer so that
the sharp gradients can be resolved.
Relu'lν⁄=
u'
l
ν
Flow Model Mathematical Model
4-10 FINE™/Turbo
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 (four)-equation models (k-ε, k-ω and v2-f).
When quick turbulence calculations are required, for example, in design-cycle analysis, it is recom-
mended that the Baldwin-Lomax model is used due to its high numerical stability and low compu-
tational expense. To simulate more precisely the turbulent quantities with also a good rate of
convergence the Spalart-Allmaras model should be preferred.
Another model often used in design is the "standard" k-ε model. This model employs an empiri-
cally based logarithmic function to represent the near-wall physics and requires a lower grid resolu-
tion 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 trans-
fer calculations. However, experience has shown quite successful prediction of heat transfer coeffi-
cients when using low Reynolds models.
The Shear Stress Transport (SST) k-ω turbulence model is another most utilized two-equation
model. This model, which combines the advantages of the Wilcox k-ω model and the k-ε model,
has higher accuracy in the separation flow predictions. The user is recommended to use the SST k-
ω model in predicting the onset and the amount of separations under adverse pressure gradient con-
ditions.
The EARSM (Explicit Algebraic Reynolds Stress Model) model is a non linear eddy viscosity 2-
equation model. EARSM is much less demanding than RSM from the computational standpoint
and, at the same time, is capable of reproducing some important features of turbulence (e.g. its ani-
High-Re: Low-Re:
Turbulence Models Spalart-Allmaras (Extended Wall
Function);
SARC (Extended Wall Function);
k-ε (Extended wall function);
k-ε (Standard wall function);
SST (Extended wall function)
EARSM (Extended wall function);
Baldwin-Lomax;
Spalart-Allmaras;
Spalart-Allmaras (Extended Wall
Function);
SARC;
SARC (Extended Wall Function);
k-ε (Extended wall function);
k-ε (Low Re Yang-Shih);
k-ε (Low Re Chien);
k-ε (Low Re Launder-Sharma);
Shear Stress Transport (SST);
SST (Extended wall function);
EARSM;
EARSM (Extended wall function);
k-ω (Wilcox);
v2-f (code friendly)
Most Appropriate
Flows
Quasi-2D;
Weak pressure gradient;
Quick design-cycle calculations
3D;
Strong pressure gradient;
Moderate curvature;
Separating flows
Mathematical Model Flow Model
FINE™/Turbo 4-11
sotropy in the normal stresses), which are beyond the capabilities of linear eddy viscosity turbu-
lence models. The user is recommended to use the EARSM model when strong anisotropy exists in
the computational domain.
The v2-f turbulence model was developed to eliminate the need to the damping functions that used
by the low-Reynolds k-ε turbulence models. Through several years of fundamental research, v2-f
turbulence model has been proven to have better behavior in predicting wall induced phenomena
such as heat transfer and flow separation than the other low-Reynolds turbulence models. The user
is suggested to use this model in heat transfer applications.
The v2-f turbulence model has not been extended to some specific modules: Rotor/
Stator interfaces, Full Non-Matching connections and Cooling/Bleed module.
4-2.5.3 Second Step: Generating an Appropriate Grid.
a) Cell Size
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) independ-
ently. 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.
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+(4-5)
where uτ is the friction velocity:
(4-6)
Note that the value of ywall depends on the value of y1+.
ρuτywall
μ
---------------------
=
uτ
τwall
ρ
----------- 1
2
---Vref
()
2Cf
==
Flow Model Mathematical Model
4-12 FINE™/Turbo
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 4.2.5-2 Boundary layer profiles
In Figure 4.2.5-2 it is represented the evolution of u+ against y+ from the measurements of Lind-
gren(1965) with:
u+=/
Low-Re models resolve the viscous sublayer and are well suited for y1+ values less than 10 whereas
high-Re models apply analytical functions to the log-layer and are appropriate to y1+ values ranging
from 20 to 50, even more (depending on the extension of the buffer layer for the considered flow).
When the extended wall function is used, it is strongly advised to locate the first inner node either in
the viscous sublayer (y1+<5) or in the log layer (y1+>20).
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.
logarithmic law
Data of Lindgren (1965)
viscous sub-layer buffer layer log layer
Separating flow
defect layer
u
uτ
Mathematical Model Flow Model
FINE™/Turbo 4-13
TABLE 4-1 Appropriate y1+ values for available turbulence models
One way to estimate ywall as a function of a desired y1+ value is to use a truncated series solution of
the Blasius equation:
y1+... (4-7)
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 a typical length scale since an estimation of boundary layer thickness is implied
in this calculation. For instance, in the case of a turbomachinery simulation one could use the dis-
tance between hub and shroud curves that exist upstream of the first row of blades. This is approxi-
mate, of course, as the thickness of the boundary layers will vary widely within the computational
domain. Fortunately it is only necessary to place y1+ 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 fric-
tion coefficient Cf is related to the Reynolds number:
(4-8)
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. 4-6, and ywall may then be calculated from
Eq. 4-5. 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 y1+, can be expected to drop. Since a certain range is
desired (e.g., 20< y1+<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).
High-Re: Low-Re:
Turbulence Models Spalart-Allmaras (Extended Wall
Function);
SARC (Extended Wall Function);
k-ε (Extended wall function);
k-ε (Standard wall function);
SST (Extended wall function)
EARSM (Extended wall function);
Baldwin-Lomax;
Spalart-Allmaras;
Spalart-Allmaras (Extended Wall
Function);
SARC;
SARC (Extended Wall Function);
k-ε (Extended wall function);
k-ε (Low Re Yang-Shih);
k-ε (Low Re Chien);
k-ε (Low Re Launder-Sharma);
Shear Stress Transport (SST);
SST (Extended wall function);
EARSM;
EARSM (Extended wall function);
k-ω (Wilcox);
v2-f (code friendly)
y1+20-50 <10
ywall 6Vref
ν
---------


78/– Lref
2
---------


18/
=
Cf
0.027
Rex
17/
--------------
=
Flow Model Mathematical Model
4-14 FINE™/Turbo
b) Things to Look Out For
Previous recommendations 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 y1+ 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 (available in solid data output, see section 10-2.1.5). 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 y1+ will be low in such regions. It is generally recommended that turbomachin-
ery blade tip clearances are meshed with uniform spanwise node distributions. In such cases, the
y1+ 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 accelera-
tion.
c) General Advice
•What grid resolution is adequate?
The resolution method employed in the FINE™/Turbo 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 approxi-
mately 9 nodes.
Of course the flow field under study will realistically consist of shear layers of which the width var-
ies substantially throughout the flow field. The user must therefore decide what is important to cap-
ture 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 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.
•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 partic-
ularly important to keep this value within an absolute range of about 1.0-1.6 in regions of high gra-
dients, 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 these instructions it should be possible to generate a grid of reasonable quality for tur-
bulent 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)
Mathematical Model Flow Model
FINE™/Turbo 4-15
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.
4-2.5.4 Defining Initial & Boundary Conditions
Turbulence is commonly modelled by emulating molecular diffusion with a so-called "eddy-viscos-
ity" (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 kinematic turbulent viscosity
ν
t (m2/s) has to be
specified. The kinematic turbulent viscosity ratio is extremely sensitive to the type of application/
configuration. Therefore, if the user has any indication of the actual level of turbulence in the case
configuration, the user should use it. If no information is available on the order of magnitude of the
kinematic turbulent viscosity ratio, estimates can be made based on the following assumptions that:
•For internal flows (e.g. turbomachinery): = 1 to 5.
•For external flows (e.g. vehicle aerodynamics): .
b) k-
ε
, k-
ω
, EARSM and v2-f Models
When the k-ε, k-ω and v2-f models are selected, the boundary values of k and ε have to be specified.
If no information is available on the turbulence properties of the flow, estimates can be made based
on the following formulations.
b.1) Estimation of k
The value of the turbulent kinetic energy k can be derived from the turbulence intensity Tu or from
the wall shear stress.
—From the turbulence intensity: The turbulence intensity Tu can be expressed against the
streamwise fluctuating velocity u' and the streamwise velocity Uref:
(4-9)
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:
(4-10)
—From the wall shear stress: If the wall shear stress is known, the user can use the wall func-
tions defined for the fully turbulent flow:
νt
ν
----
νt
ν
---- 1=
Tu
u'2
Uref
----------
=
k3
2
---u'2


2
=
Flow Model Mathematical Model
4-16 FINE™/Turbo
(4-11)
This value of k could be used as an initial value and also for the inlet boundary condition.
b.2) 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:
(4-12)
For internal flows (such as turbomachinery flow), typical values are .
For external flows (in aerodynamics computations), typical values are .
—Specify the turbulent length scale (only for internal flows):
A typical values is . where DH is the hydraulic diameter of the inlet section
(4-13)
—Derive ε from the asymptotic turbulent kinetic equation:
In a free uniform flow the turbulent kinetic energy equation reduces to
(4-14)
This relation can be used to specify the value of the turbulent dissipation in the following way:
(4-15)
where u is the inlet velocity, Δk the decay of the turbulent kinetic energy over a length L. For
example, in a turbomachine, L is the maximum geometric length and Δk could be set to 10% of
the inlet value of k.
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. . If this condition is not
satisfied, it is advised to scale down or up the value of k inlet or the Δk and compute again the
turbulent dissipation
—Specify the wall shear stress:
If the wall shear stress is known, the user can use the wall functions defined for the fully turbu-
lent flow.
(4-16)
If there is an initial solution file containing and , the and values of this file are used to
initialize the fields.
k
τ
wall
ρ
Cμ
-----------
=
εCμ
μ
μt
---- ρrefk2
μ
--------------
=
μtμ⁄ 50=
μtμ⁄ 1=
l0.1DH
=
εcμ
3
4
---
k
3
2
---
l
----------
=
uk∂
x∂
----- ε–=
εu–Δk
L
------
=
1μt
μ
---- 1000<<
ετwall ρ⁄()
3
2
---
l
-------------------------
=
k
ε
k
ε
Mathematical Model Flow Model
FINE™/Turbo 4-17
The values of the inlet boundary conditions for the and can also be used to set the initial and
fields. However, to reduce the possibility of oscillations in skin friction due to non-physical rela-
minarisation during convergence, it is recommended to insure ≈ 0.1 .
Either of the above methods can be applied for setting the boundary conditions in tur-
bomachine applications. However, if the given values of k and ε lead to the damping of
the turbulence shortly after the inlet section, we suggest to apply Eq. 4-15 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. 4-12 and Eq. 4-14 may result in very differ-
ent values for ε. In such a case it is recommended to re-evaluate k and ε in the following
manner:
1. Use relation Eq. 4-15:
(4-17)
This relation expresses that k0 (k at the inlet) is expected to be decreased by about 10% over a
length ΔL that is characteristic to the size of the domain.
2. Use relation Eq. 4-12. In this relation Cμ=0.09 and represents the dynamic laminar viscosity
of the fluid.
3. Combine the relations of the two previous steps to remove ε0, leading to:
(4-18)
4. Using either relation Eq. 4-12 or Eq. 4-15 then easily leads to an estimation of ε0.
4-2.5.5 Setting Expert Parameters to Procure Convergence
Several expert parameters may be set to procure convergence.
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 the convergence rate.
EKCLIP(real): 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.
k
ε
k
ε
ε
εinlet
εu–Δk
ΔL
-------u0.1k
ΔL
----------
==
μ
k0
0.1U
ΔL
------------μt
μ
---- ν
Cμ
------


=
Flow Model Mathematical Model
4-18 FINE™/Turbo
IKELED(integer): 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(integer):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 & v2-f / Baldwin-Lomax Switch
KEGRID = 2(default) Grid 222 - Baldwin Lomax,
Grid 111 - Baldwin Lomax,
Grid 000 - k-ε or v2-f Model.
KEGRID = 3: Grid 222 - Baldwin Lomax,
Grid 111 - k-ε or v2-f Model,
Grid 000 - k-ε or v2-f Model.
Example: k-ε run on the finest grid level (000) with 3 levels of grid (222, 111 & 000) in the multi-
grid procedure. The Baldwin-Lomax model remains active on levels 222 and 111 before k-ε is auto-
matically switched on when the finest grid is reached. This is controlled through the expert parame-
ter 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 trans-
ferred 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. How-
ever, 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
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 initialisation 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-ε model). Limiting this to a finite value enhances
the 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 (real): For most flows: 50 (default),
In turbulent diffusion dominated flows (e.g., seals): 200.
Mathematical Model Flow Model
FINE™/Turbo 4-19
f) Cut-off (clipping) of Maximum Turbulent Viscosity Ratio (
μ
t /
μ
)
The float parameter MUCLIP controls the maximum allowable value of the turbulent viscosity ratio
μt/μ. Limiting this to a finite value enhances the convergence rate by removing the possibility of
unbounded spikes occurring during the numerical transient. At the end of the computation however,
the value of μt/μ should not be clipped anymore. During the convergence process, the user can
check the output of the computation to see if the maximum value for the turbulence ratio has been
reached. If this is the case, the output will contain a line: "MUT/MU CLIPPED FOR # CELLS".
MUCLIP can then be put to a higher value, to increase the limit. However, care must be taken to
apply reasonable limits. Recommended values are:
MUCLIP (real): For most flows: 5000 (default). It can be increased if necessary.
4-2.6 Laminar-Transition Model
4-2.6.1 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 Laminar-
Turbulent 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, a laminar-transition model is proposed in the FINE™/Turbo solver in order to take into
account the effect of the laminar-turbulent transition. The following four choices are possible in the
Transition Model page under Optional Models:
—Fully Turbulent
—Fully Laminar
—Forced Transition
—Abu-Ghannam and Shaw (AGS) Model
The present transition model can be used only with the low Reynolds number Spalart-Allmaras,
Yang-Shih k-epsilon, Wilcox k-omega and SST turbulence models.
The transition model in FINE™/Turbo is mainly devoted to turbomachinery applications using
AutoGrid™ mesh. Both the pressure and suction sides of the blade need to be set with the transition
model. Chapter 8-9 describes the interface for the transition model. More information on the
transition model can be seen in Chapter 3-8 in the theoretical manual.
However, the transition model in FINE™/Turbo is also available for the other cases, such as flat
plate, wings and hydrofoils, etc. In the next section a best practice will be given to describe how to
model transition on non-turbomachinery cases.
4-2.6.2 How to model transition on non-turbomachinery cases
Use of the transition model is restricted to the pressure and suction sides of the turbomachinery
blade using AutoGrid™ mesh. Modeling transition on non-turbomachinery cases can therefore only
be performed by considering the object to be a pseudo "blade" and modifying the mesh files manu-
ally. The limitation on the mesh of non-turbomachinery cases is:
Flow Model Mathematical Model
4-20 FINE™/Turbo
•The mesh topology should be similar to a Autogrid™ mesh topology (with at least a proper
mesh in spanwise direction).
•The transition is along a pseudo "blade", so the user has to add the "blade" definition in the
mesh files manually.
Example: Mesh for modeling transition on a flat plate
Considering transition flow over a flat plate (Figure 4.2.6-3). The computational domain corre-
sponds to an external flow with a constant velocity blowing towards the flat plate.
Note that for the flat plate case the user has to consider the two faces of the plate since the transition
model needs a pressure side and a suction side.
FIGURE 4.2.6-3 Computational domain for a flat plate
In order to be compatible with the transition model, a 3D mesh should be used for this case with a
correct orientation: i perpendicular to the flat plate with i=1 on the flat plate and with j and k along
the plate: k in streamwise direction and j perpendicular to main flow direction.
The .bcs file of the mesh should be modified in order to include the turbomachinery blade defini-
tion. At the end of the .bcs file the line "NUMBER_OF_BLADES 0" should be modified: the "0"
should be change in a "1" as the flat plate will be considered as one blade (of zero thickness).
Mathematical Model Flow Model
FINE™/Turbo 4-21
Next lines need to be added as shown here:
4-2.7 Gravity Forces
When gravity should be taken into account the box Gravity Forces should be checked. If gravity is
activated, 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 and
are respectively introduced in the momentum and energy conservation equations where ρ
is the density, the gravity vector and the velocity vector.
If the fluid is a liquid, the density is constant and there is no influence of the pressure or temperature
on the flow by interaction with the gravity. To simulate these interactions, one can use the Boussin-
esq approximation in the gravity source terms. With this approximation, the density is developed in
the first order of the MacLaurin series. It becomes:
(4-19)
with α the compressibility and β the dilatation coefficients specified in the fluid properties.
ρg
ρgv⋅()
g
v
ρρ
ref 1αpp
ref
–()β–TT
ref
–()+()=
Flow Model Characteristic & Reference Values
4-22 FINE™/Turbo
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 is the char-
acteristic density specified in the Configuration/Flow Model page. and are the reference
values in the Configuration/Flow Model page.
When the gravity is taken into account, a reference pressure must be specified at a ref-
erence altitude to add the hydrostatic pressure in the initial pressure field. The reference
pressure is the reference value in the Configuration/Flow Model page. The reference
altitude is specified in the expert parameter IREFPT in meter [m].
4-2.8 Low Speed Flow (Preconditioning)
This option appears in the Flow Model page only if the fluid type is compressible.
Preconditioning is automatically used for incompressible fluids.
In the low 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 com-
parison with the acoustic speeds, time marching compressible codes converge very slowly.
Two low speed preconditioners, Hakimi and Merkle preconditioners, have been implemented in the
FINE™/Turbo solver in order to provide fast convergence characteristics and accurate solutions as
the Mach number approaches zero:
•The Hakimi preconditioner is of sufficient generality and can treat any type of fluids and
flows. Efficient convergence rates and accurate solution can be 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.
•Compared with the Hakimi preconditioner, the Merkle preconditioner has the advantage that it
is not only effcient at all Mach number but also at all Reynolds and Strouhal numbers. With the
Merkle preconditioner, the user can perform a fast and accurate computation of supersonic
flows with regions at very low speed. Moreover the Merkle preconditioner doesn't require any
user inputs.
Merkle preconditioning is not compatible with:
•barotropic fluids
•unsteady mode
•cavitation model
For the detailed parameter settings, please refer to section 6-2.2.4.
4-3 Characteristic & Reference Values
4-3.1 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 a useful information to choose the suitable model (section 4-2.5). These characteristic val-
ues can be used for other purposes as well.
ρref
pref
Tref
Characteristic & Reference Values Flow Model
FINE™/Turbo 4-23
The characteristic length is used:
—in the outlet boundary condition for which the mass flow is imposed with pressure adapta-
tion,
—in the computation of CP1 and CP3 for cylindrical cases.
—in the transition model, to set the free stream turbulent intensity.
The characteristic velocity is used:
—in the preconditioning method to compute the parameter β,
—in the computation of the solid data Cf (normalized by ).
The characteristic velocity should be set to the highest value in the flow domain.
The characteristic density is used:
— in the Boussinesq approximation for incompressible fluid (Eq. 4-19),
— in the computation of the solid data Cf (normalized by ),
—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.
4-3.2 Reference Values
The reference values have been introduced for preconditioning, to define a gauge pressure and a
gauge total energy.
A value of Reference temperature Tref of the order of magnitude of the expected tem-
perature field will reduce the machine round-off errors influence on the temperature
field.
The value of Reference pressure 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 sec-
ond order artificial dissipation term. A value of Pref close to the real pressure level is
therefore recommended.
These reference values also have some additional uses which are described hereafter:
—in the Boussinesq approximation for incompressible fluid (Eq. 4-19),
—in the outlet boundary condition for which the mass flow is imposed with pressure adapta-
tion,
ρrefUref
22⁄()
ρrefUref
22⁄()
Flow Model Characteristic & Reference Values
4-24 FINE™/Turbo
—in the definition of the heat transfer coefficient when the expert parameter HTCDEF is set to
2, see section 10-2.1.5.
FINE™/Turbo 5-1
CHAPTER 5: Boundary Conditions
5-1 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 in the Boundary Conditions
page. In section 5-2, the page is described. For expert use, section 5-3 gives an overview of the
available expert parameters. In section 5-4, some advice is provided on the combinations of bound-
ary conditions to use.
5-2 Boundary Conditions in the FINE™/Turbo
GUI
When selecting the Boundary Conditions page the "parameters area" appears as shown in
Figure 5.2.0-1. Five tabs are available, depending on the boundary condition types defined in the
mesh. There are currently five types of boundary conditions available in the FINE™/Turbo solver:
inlet, outlet, periodic (connection with or without rotational or translational periodicity), solid walls
and external (far-field). Each of those is described in the next sections.
Note that the connecting (matching (CON) and non-matching (NMB)) boundary con-
ditions (without periodicity) do not appear in this menu, because they do not require any
input from the user. Only the "periodic" conditions (PER & PERNM) appear in the Peri-
odic tab page.
Note that the full non matching and periodic full non matching connections defined
within IGG™ (refer to IGG™ User Manual for details on limitations) are appearing in
the Solid tab page.
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 tab page. A patch can be identified either by the name of the block face to which it
Boundary Conditions Boundary Conditions in the FINE™/Turbo GUI
5-2 FINE™/Turbo
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 5.2.0-1 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
FINE™/Turbo. If the patches have been grouped in IGG™, by giving the same name to
many patches, they will appear ungrouped in FINE™/Turbo (with block, face and patch
number shown after the name) to avoid contradiction between grouping in IGG™ and
FINE™/Turbo. Ungroup button will toggle the IGG™ name of the selected patch(es)
with the default FINE™/Turbo name (block, face and patch number).
If the Use Grid Configuration option is activated when linking the mesh for the first
time (see section 2-2.3), a default grouping by row is proposed by FINE™/Turbo. For
Boundary Conditions in the FINE™/Turbo GUI Boundary Conditions
FINE™/Turbo 5-3
the solid boundaries, the rotation speed specified in IGG™ or AutoGrid™ is automati-
cally transferred to FINE™/Turbo. This limits the user input to a strict minimum. This
automatic grouping cannot be modified by the user.
If the graphics area 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.
FIGURE 5.2.0-2 Two patches will be 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 gases. FINE™/Turbo will automatically disable the boundary conditions
that are not available, depending on the type of fluid selected in the Fluid Model page.
Also the type of boundary conditions are adjusted according to the selection for Carte-
sian 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.
(1)
(2)
(3)
Boundary Conditions Boundary Conditions in the FINE™/Turbo GUI
5-4 FINE™/Turbo
5-2.1 Inlet Condition
5-2.1.1 Available Types
The inlet boundary condition page is customized according to the configuration of the project (Car-
tesian or cylindrical) as shown in the following two figures. The user has the freedom to access both
types of configuration in the Boundary Conditions page independently of the mesh properties.
FIGURE 5.2.1-3 Subsonic inlet boundary conditions page for cylindrical problems.
FIGURE 5.2.1-4 Subsonic inlet boundary conditions page for Cartesian problems.
Boundary Conditions in the FINE™/Turbo GUI Boundary Conditions
FINE™/Turbo 5-5
The upper part of the inlet boundary condition page allows the user to select the type of inlet condi-
tion 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 super-
sonic, the velocity component normal to the boundary should be considered.
Total quantities imposed condition applicable to supersonic inlets is not compatible
with condensable fluid.
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 sim-
ulation using a k-ε, k-ω or v2-f 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 the absolute quantities
•A special condition is available, for which the values can be entered in the upstream rotational
frame of reference
Six major types of inlet boundary conditions can be identified:
•velocity components and the static temperature
•total pressure, total temperature and the flow direction
Total quantities imposed boundary conditions with V-extrapolated is incompatible
with a model which streamwise direction is in negative Z.
•total enthalpy, dryness fraction and the flow angles (only for condensable fluid)
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
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).
•mass flow, static temperature and the flow direction (see the next paragraph for detail on cou-
pling with the outlet)
The mass flow imposed in the GUI will be used for the whole inlet. For example, if
the user has a rotational periodicity of 40, the mass flow for only one passage will be the
mass flow specified in the GUI divided by 40.
•distributions of the flow variables for the non-linear harmonic method. For more detail, please
refer to Chapter 8-4.2.2.
Boundary Conditions Boundary Conditions in the FINE™/Turbo GUI
5-6 FINE™/Turbo
•conditions set from a rotor-stator interface (SubProjects only, see Chapter 8-11)
Inlet boundary condition Velocity normal to inlet is not compatible with the following
expert parameter value:
•INITRB=0
•IMASFL=1
•INMFTT=1
Moving grid is not compatible with relative velocity normal to inlet when using mass
flow imposed.
5-2.1.2 Coupling Temperature with Outlet
When the 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 aver-
age temperature Taverage is computed at the specified outlet and imposed at the inlet as Tinlet = Taver-
age + ΔT (see Figure 5.2.1-5). The quantity ΔT is a constant temperature difference (>=0 or <0)
specified by the user. This is done in FINE™/Turbo by choosing Mass Flow Imposed as boundary
condition type for the subsonic inlet in cylindrical configuration 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 ΔT.
This option is only working if both inlet and coupled outlet patch have the mass flow
imposed as a boundary condition.
FIGURE 5.2.1-5 Meridional view of the "Coupling with Outlet ID" functionality
5-2.1.3 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 2-7 for a
Taverage + ΔT
Taverage
Outlet
Inlet
Boundary Conditions in the FINE™/Turbo GUI Boundary Conditions
FINE™/Turbo 5-7
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 5.2.1-6 The Profile Manager
The option 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. More details on the
required file format are available in Appendix A.
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 tab page. In such
a case a default constant value is used in the computation.
5-2.2 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.
Five types of subsonic outlet boundary condition are available, as shown in Figure 5.2.2-7. These
five 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 enter-
ing flow is controlled so that the entering and outgoing flows globally have the same total tempera-
ture.
Backflow Control is only compatible with compressible fluid. When condensable or
incompressible fluids are used, it is suggested to use the expert parameter BCKFLO to
control backflow at outlet, see Chapter 5-3.5 for more detail.
Backflow Control is applied separately on each outlet patch when an uniform static
pressure is imposed (it is applied to a group of patches if averaged static pressure and
mass flow are imposed).
Boundary Conditions Boundary Conditions in the FINE™/Turbo GUI
5-8 FINE™/Turbo
Backflow Control is not available for the outlet boundary conditions where static
pressure is imposed with radial equilibrium.
FIGURE 5.2.2-7 Outlet boundary conditions page.
5-2.2.1 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 tempera-
ture and the absolute velocity components are extrapolated. As described for the inlet condi-
tions, 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 appro-
priate approximation of the physical pressure distribution at the outlet, an averaged static pres-
sure 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.
 The outlet patches have to be grouped in one group to use this boundary condition.
•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 pro-
file of the static pressure. Please note that the given radius should be between hub and shroud.
Otherwise the outlet static pressure will be imposed on the corresponding extreme radius of
the outlet instead of the given radius. A constant static pressure is imposed along the circum-
ferential direction.
This boundary condition is only valid on surfaces with mesh lines at constant radius.
 This boundary condition is not compatible with the radius r=0.
Boundary Conditions in the FINE™/Turbo GUI Boundary Conditions
FINE™/Turbo 5-9
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 ( ) right next to the input
text box. The Profile Manager will appear as described in section 5-2.1.3.
5-2.2.2 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 ’Static Pressure Imposed’
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 con-
dition is used.
When using the mass flow imposed outlet boundary condition and restarting a compu-
tation from a file, only one group of patches can be used in the initial solution page and
the reset convergence history has to be deactivated
The outlet patches have to be grouped in one group to use this boundary condition.
The mass flow imposed in the GUI will be used for the whole outlet. For example, if
the user has a rotational periodicity of 40, the mass flow for only one passage will be the
mass flow specified in the GUI divided by 40.
5-2.2.3 Averaged Mach Number
When imposing the averaged Mach number at the outlet, the user must group all the related patches
for each outlet. This permits to have several groups of patches, each of the groups constituting an
outlet through which the averaged Mach number can be controlled.
Two options are available:
•Absolute Mach Number with Pressure adaptation: the absolute Mach number is imposed at
the outlet boundary. The exit pressure is automatically modified during the resolution process
so that after convergence, the prescribed absolute Mach number is obtained.
•Relative Mach Number with Pressure adaptation: the relative Mach number is imposed at
the outlet boundary. The exit pressure is automatically modified during the resolution process
so that after convergence, the prescribed relative Mach number is obtained.
The initial pressure asked in addition to the imposed Mach number is used in the full multigrid ini-
tialisation. This value is also used for the turbomachinery initial solution.
During the pressure adaptation process, the exit pressure can be imposed in different ways:
•Constant Profile: this boundary condition is identical to the ’Static Pressure Imposed’
boundary condition.
Boundary Conditions Boundary Conditions in the FINE™/Turbo GUI
5-10 FINE™/Turbo
•Radial Equilibrium: this boundary condition is identical to the ’Radial Equilibrium’ bound-
ary condition.
•Extrapolated Profile: this boundary condition is identical to the ’Averaged Static Pressure’
boundary condition.
The averaged Mach number boundary condition at outlet is not compatible with
incompressible fluid.
5-2.2.4 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 or real gas in the Fluid Model page.
Figure 5.2.2-8 shows as an illustration performance curves for a centrifugal compressor. Near chok-
ing 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 pres-
sure 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.
FIGURE 5.2.2-8 Example of performance curves for centrifugal compressor
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 out-
let mass flow and a target outlet pressure (at point 2 in Figure 5.2.2-8) and the pressure at zero mass
flow (point 1 in Figure 5.2.2-8). Based on these three parameters, a simple parabolic curve is gener-
ated. This curve is then used to apply the boundary condition allowing to impose a relation between
the mass flow and the pressure at the outlet.
(static pressure)
(mass flow)
Boundary Conditions in the FINE™/Turbo GUI Boundary Conditions
FINE™/Turbo 5-11
5-2.2.5 From Rotor/Stator
The outlet boundary condition From Rotor/Stator can only be used in the frame of the SubProject
module. This boundary condition is set automatically, no user intervention is required. For more
details, see Chapter 8-11.
5-2.3 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™/Turbo interface, with the advantage that the user does not need to specify any input con-
cerning these boundary conditions.
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 5.2.3-9 Periodic boundary condition page.
In case some input is required this section explains how to define the periodic conditions using the
PERIODIC tab page.
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
identical, and if all the corresponding points along these patches coincide (PER type within
IGG™). The Non Matching connection (PERNM type within IGG™) requires the use of an inter-
polation process to establish the connection, whereas a matching one consists of a single communi-
cation of the flow variables. The interpolation used for non matching periodic boundaries consists
on a linear interpolation from the four nearest cells.
Some additional characteristics need to be given to fully determine the periodic boundary condi-
tion:
Boundary Conditions Boundary Conditions in the FINE™/Turbo GUI
5-12 FINE™/Turbo
•For Cartesian (rectangular) 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.
5-2.4 Solid Wall Boundary Condition
The solid wall boundary condition page is customized essentially according to the type of calcula-
tion (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 condi-
tions. The type of boundary conditions determines the way the velocity and thermal conditions are
defined for the solid boundary.
5-2.4.1 Cylindrical Boundary Condition
a) Area Defined Rotation Speed
The wall rotation velocity can be constant or area defined (see Figure 5.2.4-10). The area defined
option allows to attribute a specific rotation velocity to a rectangular zone in the meridional plane
independently of the grid structure.
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 outside the
domain and to 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 lim-
its such that they include the full solid (hub) patch.
ω1
ω2
Boundary Conditions in the FINE™/Turbo GUI Boundary Conditions
FINE™/Turbo 5-13
FIGURE 5.2.4-10 Solid boundary conditions page in case of a cylindrical boundary condition
b) Thermal Condition
Four options are available for the thermal condition:
•Adiabatic
•Imposed Heat Flux (in W/m2)
A positive heat flux indicates that the direction of the heat flux is from the solid wall to the
fluid.
•Imposed Temperature (isothermal)
•Imposed heat transfer coefficient (W/K/m2)
,
where is the local heat flux, the local temperature at the wall and the refer-
ence temperature inputted by the user.
The imposed heat flux, temperature or heat transfer coefficient 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 5-2.1.3.
5-2.4.2 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.
hqw
Tref Twall
–()
---------------------------------
=
qw
Twall
Tref
Boundary Conditions Boundary Conditions in the FINE™/Turbo GUI
5-14 FINE™/Turbo
5-2.4.3 Force and Torque
Below the box, a Compute force and torque option is provided that permits to include the selected
patches in the calculation of the global solid boundary characteristics.
The contribution of patches included in a full non-matching connection will not be
taken into account for the computation of the force and torque. Those patches will how-
ever appear as solid in the boundary condition page.
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:
.(5-1)
The computed force is the one from fluid on solid. The force is considered as positive
when in the direction of the z-axis.
The projection of the torque along a given direction , i.e. the couple exerted by the global force
along the rotation axis:
(5-2)
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 5-3).
When using an area defined rotation speed, the expert parameter TORRO can be used to compute
the force and torque on the complete patch, or on the rotating part only (see section 5-3).
Within the FINE™/Turbo solver it is possible to calculate and to store the partial torque in the cor-
responding ".wall" file of the computation through the use of the expert parameter IFRCTO within
the FINE™/Turbo GUI.
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).
Fn
z
⋅
S
z
rF×
S



z⋅
Boundary Conditions in the FINE™/Turbo GUI Boundary Conditions
FINE™/Turbo 5-15
FIGURE 5.2.4-11 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 5.2.4-11.
The force and torque computed on the selected surface(s) and included in ".wall" file
are based on the full 360 degrees, so taking into account the periodicity when the blocks
concerned are presenting a periodicity.
5-2.4.4 Properties of Solid for Turbulence
In addition, when turbulence models with extended wall function are 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 the
theoretical manual.
Two methods considering the wall function for roughness is implemented. With the old method
(default, IROUGH=0), the constant B has to be computed after obtaining the value of y+. And the
value of B will also correct y+. The user has to iterate this procedure and converge to the desired
IFRCTO = 0
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
Total Torque and Force on Suction Side
Boundary Conditions Boundary Conditions in the FINE™/Turbo GUI
5-16 FINE™/Turbo
value of B. This is not straighforward and a new approach has been introduced in the flow solver in
order to simplify the computations with roughness. To use the new method, the user has to set the
expert parameter IROUGH to 1.
When a rough wall is specified, if IROUGH=0, the distance from the wall to the cell-
centre of the first inner cell should be bigger than k0 + d0; if IROUGH=1, the distance
from the wall to the cell-centre of the first inner cell should be bigger than ks + d0. In
general, the first inner cell should be located within the fully turbulent layer.
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 (see section 4-2).
5-2.5 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 5.2.5-12.
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 varia-
bles. 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 5.2.5-12 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 gases are not compatible with external boundary condition.
The boundary condition External Constant Wind with Incidence Relative to Axis
Z is only compatible with NLH.
Expert Parameters Boundary Conditions
FINE™/Turbo 5-17
5-3 Expert Parameters
5-3.1 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 bound-
ary conditions. This procedure is only available when 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.
The following parameters have to be defined:
INLREL(integer): allows to specify relative angles for the cylindrical inlet boundary conditions
with
= 0 (default):total quantities imposed,
= 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(real): data use with the expert parameter INLREL (for stator only). This variable con-
tains three values:
•1st real: relaxation angle (in degrees),
•2nd real: distance (%) from hub where the absolute flow angle is extrapo-
lated,
•3rd real: distance (%) from shroud where the absolute flow angle is extrapo-
lated.
5-3.2 Inlet Mass Flow Boundary Condition
IMASFL(integer): expert parameter specially dedicated to radial inlets. The mass flow is extrapo-
lated 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.
INMFTT(integer): specify static temperature or total temperature when using mass flow imposed
inlet BC,
= 0 (default): static temperature is specified.
=1: total temperature is specified.
5-3.3 Outlet Mass Flow Boundary Condition
RELAXP(real): is the under-relaxation for the outlet boundary condition where the mass flow is
imposed with the exit pressure adaptation (default value = 1.).
VELSCA(real): is the maximum value allowed for the velocity scaling (outlet boundary condi-
tion with mass flow imposed by scaling velocity) (default value = 2.)
Boundary Conditions Expert Parameters
5-18 FINE™/Turbo
5-3.4 Outlet Averaged Mach Number Boundary Condition
RELAXP(real): is the under-relaxation for the outlet boundary condition where the averaged
Mach number is imposed with the exit pressure adaptation (default value = 1.).
5-3.5 Control of backflows
BCKFLO(integer): defines whether an Euler wall boundary condition is used at all outlet cells
where back flow is detected:
= 0 (default): don’t use the control of backflow,
= 1: use an Euler wall boundary condition at all cells where backflow is
detected.
BCKFLU(integer): defines whether the backflow control at inlet is activated or not. The use of
BCKFLU is limited to turbomachinery cases meshed with AutoGrid4™/
AutoGrid5™.
= 0 (default): don’t use the control of backflow at inlet
= 1: use the control of backflow at inlet, based on pitchwise averaging of the
solution.
5-3.6 Torque and Force
IDCDP(real): 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(real): direction (x,y,z) for lift (not used if cylindrical project and IINT=1),
IDCMP(real): direction (x,y,z) for moment,
IFRCTO(integer): calculate and to store the partial torque in the corresponding ".wall" file. More
detail in Chapter 5-2.4.3.
IXMP(real): coordinate (x,y,z) of the point around which the moment has to be calculated.
The coordinates are expressed in meters.
TORRO(integer): = 0 (default): Compute force and torque on the complete patch
= 1: Compute force and torque only on the part of the patch which is defined
through an area defined rotation (the part corresponding to ω2).
IMUWAL(integer):if set to 1, the ".wall" file will be saved at each iteration on the finest grid level
(current grid level specified in the Numerical Model page) when performing a
steady simulation. The corresponding .wall file (_iter#.wall) will be saved in
the computation directory.
5-3.7 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 the theoretical manual. Note
that the default (active in Standard Mode) is a Navier-Stokes wall.
Best Practice for Imposing Boundary Conditions Boundary Conditions
FINE™/Turbo 5-19
5-3.8 Pressure Condition at Solid Wall
When the interface is in Expert Mode, two toggle buttons are provided to select the type of pres-
sure condition at the wall: extrapolated or computed from the normal momentum equation. The
default (active in Standard Mode) is the extrapolation of the pressure.
5-4 Best Practice for Imposing Boundary
Conditions
The quality of the flow simulation depends 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 a calculation is diverging, it is strongly recommended to check by post
processing of the solution (in CFView™), that the appropriate boundary conditions have
been imposed.
5-4.1 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 pres-
sure 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 mass-
flow 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 a fine grid.
A solution to overcome this drawback is to impose the mass-flow at the outlet. This can be done in
two ways:
•Velocity Scaling: for a 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 backflows are
detected along the exit. If this is the case, the next option is better suited.
•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.
Boundary Conditions Best Practice for Imposing Boundary Conditions
5-20 FINE™/Turbo
5-4.2 Incompressible or Low Speed Flow
For incompressible 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 inlet-outlet conditions has a
stabilizing effect on calculations and is also well adapted to provide initial solutions for multi-stage
calculations.
5-4.3 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 activating Backflow Control in the FINE™/
Turbo GUI on the Boundary Conditions page under the OUTLET tab page.
FIGURE 5.4.3-13 Example of case with strongly varying radius in the inlet1
When end-walls in the inlet regions are strongly varying in radius (e.g. centripetal turbines as in
Figure 5.4.3-13) 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 Control Variables page in Expert Mode).
This option is adapted when the inlet boundary conditions fixes the absolute total quantities (pres-
sure, temperature) and is only valid for non-preconditioned computations. When it is activated, the
mass-flow is extrapolated instead of the velocity.
 Inlet patches have to be grouped in one group to use the extrapolation of mass flow
boundary condition.
1. Picture from D. Japikse, N.C. Balines, Introduction to Turbomachinery, Concept ETI Inc. and Oxford Uni-
versity Press, 1994.
Radial turbine
FINE™/Turbo 6-1
CHAPTER 6: Numerical Scheme
6-1 Overview
This chapter describes the interface and settings that can be used to specify the numerical parame-
ters and the time configuration for the simulations:
•Numerical Model defines the numerical aspects of the computations
•Time Configuration defines the time dependence of the equations to solve.
This chapter is organised as follows:
•section 6-2 describes the interface and settings for the definition of the numerical model,
•section 6-3 describes the interface and best practice for unsteady computations.
6-2 Numerical Model
6-2.1 Introduction
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.
Numerical Scheme Numerical Model
6-2 FINE™/Turbo
FIGURE 6.2.1-1 Numerical model interface
In expert user mode (Expert Mode) additional parameters are available as shown in Figure 6.2.1-2:
additional multigrid parameters and unsteady parameters. These interfaced expert parameters are
described in section 6-2.3. 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 Chapter 5-2 in the theoretical manual.
FIGURE 6.2.1-2 Numerical Model page in expert mode
6-2.2 Numerical Model in the FINE™/Turbo GUI
6-2.2.1 CFL Number
This box allows to tune the CFL (Courant-Friedrich-Levy) number to be employed in the compu-
tation. 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.
Numerical Model Numerical Scheme
FINE™/Turbo 6-3
6-2.2.2 CPU Booster
FINE™/Turbo includes an innovative breakthrough in convergence acceleration. Based on
enhanced implicitness, it leads to a drastic reduction in computational time with respect to the cur-
rent advanced technologies in FINE™/Turbo. If the user activates the option CPU Booster, the
default value of the CFL number will be 1000.
The CPU Booster is available only in case of perfect gas or real gas without precondi-
tioning.
The CPU Booster is not recommended when modelling low speed flows without pre-
conditioning
For the turbulence simulations, the CPU Booster is compatible only with the 0-equa-
tion and 1-equation turbulence models.
The CPU Booster is not compatible with the phase-lagged and NLH simulations.
When simulating flow with real gas, the results obtained with CPU Booster may be
less accurate if either the allowed temperature range is too large or if the properties are
expected to vary significantly in the allowed temperature range. In this case, the results
obtained with CPU booster could be different from a computation run without CPU
booster.
6-2.2.3 Multigrid Parameters
In the left part of the Numerical Model page, three boxes are visible. The first one is an informa-
tion 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 the
Current grid level for each of the i, j and k directions.
•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:
0 0 0 17*33*33 (18,513 points)
1 1 1 9*17*17 (2,601 points)
2 2 2 5*9*9 (405 points)
3 3 3 3*5*5 (75 points)
4 4 4 2*3*3 (18 points)
4 5 5 2*2*2 (8 points)
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 coars-
est 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. It is however not recommended to use such hybrid levels (e.g.
010 or 211) since it deforms the mesh in a preferential direction and thus possibly
Numerical Scheme Numerical Model
6-4 FINE™/Turbo
increasing the aspect ratio. Consequently, the quality of the resulting mesh can be
decreased.
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 compu-
tational 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 level(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 option 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 auto-
matically 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.
6-2.2.4 Preconditioning Parameters
This box allows the user to choose the Hakimi or Merkle preconditioners. The 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 activated on the Flow Model page.
The upwind spatial scheme (Numerical Model page) is not available if the precondi-
tioning option is chosen.
a) Hakimi Preconditioning
When choosing Hakimi preconditioning, extra parameters have to be defined. The variables that the
user controls are reference pressure , reference temperature , β coefficient and charac-
teristic velocity .
and are accessible through the Flow Model page.
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 computa-
tions 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 compu-
tation, 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 6.2.2-3).
With low Reynolds number, β∗ has to be increased. But this increases the dissipation
and therefore alters the precision of the solution.
Pref
Tref
β∗
Uref
Pref
Tref
Numerical Model Numerical Scheme
FINE™/Turbo 6-5
FIGURE 6.2.2-3 Typical variation of the preconditioning parameter with Reynolds
number
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. Note, for the user’s convenience, the constant Uref is always equal to the
reference velocity specified in the Flow Model page, which means that one of them (Uref/reference
velocity in the Flow Model page) is changed, the other one will be changed automatically.
The choice of Uref has an influence on the convergence.
Another expert parameter ALPHAP (α) is accessible in the Control Variables page under Expert
Mode. According to several computations accomplished with the central scheme, good conver-
gence rates were obtained for values of α lying in the range [-1,1]. So far the best value is found to
be α=-1.
b) Merkle Preconditioning
When choosing the Merkle preconditioner, no extra inputs are required.
6-2.3 Expert Parameters
6-2.3.1 Interfaced Expert Parameters
a) Multigrid Strategy
If the option 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:
•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.
For the Convergence criteria on each grid level, both the RMS and maximum resid-
uals are checked when passing from one grid level to the next one in full multigrid ini-
tialization. The flow solver jumps to the next grid level when both criteria has decreased
β∗
Uref
Numerical Scheme Numerical Model
6-6 FINE™/Turbo
e.g. 3 orders of magnitude.
•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 is applied. 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.
b) Spatial Discretization
Two types of spatial discretization are available:
•central scheme (default) and
•upwind scheme.
A new way of calculating the artificial dissipation based on the primitive variables can be accessed
by switch expert parameter IARTVS to 2 when a central scheme is chosen. Such a new way can
limit or remove strong overshoot in temperature in the vicinity of holes when running blade cooling
configurations with the source term approach.
This method is restricted to non-preconditioned perfect gas and real gas implementa-
tions. And it is not applicable with NLH method.
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 sec-
tion for more detail on those different schemes.
Condensable and preconditioned fluids are not compatible with the use of upwind
schemes for space discretization.
c) 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 step-
ping (default) and Global time stepping. See section for more detailed information on the tempo-
ral discretization. In general the default scheme is recommended.
If the computation is an unsteady computation, unsteady parameters box appears. Please refer to
chapter section 6-3.1 for a description of those unsteady parameters.
Numerical Model Numerical Scheme
FINE™/Turbo 6-7
6-2.3.2 Non-interfaced Expert Parameters
Additional parameters related to the numerical model are available in the list on the Control Varia-
bles page in Expert Mode.
a) Multigrid
IMGDIR(integer): Indicates if coarsening will be applied in the specified I, J or K direction (three
values):
1 1 1 (default): coarsening applied in all directions
0 0 0: no coarsening applied in all directions
1 1 0: coarsening applied only on I and J directions
IPROLO(integer): Indicates the order of the prolongation within the multigrid approach. The
default value is depending on the selected fluid type and turbulence model.
0: piecewise constant prolongation,
1: linear prolongation with damping,
-1: linear prolongation without damping,
2: linear prolongation except at boundaries(-2).
When used with a preconditioned formulation, this damping option is somewhat use-
less and can be damaging. FINE™/Turbo therefore sets it to off when preconditioning is
used.
When used with k-ε turbulence model and preconditioning, the linear prolongation
with damping is recommended.
IRESTR(integer): Gives the order of the restriction operator of the multigrid.
= 0 (default): corresponds to linear restriction,
= 1: to quadratic restriction.
MGRSTR(integer):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 saw-
tooth. Default: MGRSTR=1.
MGSIMP(integer):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 2nd order upwind scheme is used) or central
scheme with increased 4th order dissipation on solid walls (if central scheme is
used). If MGSIMP=2, in addition to the simplification for MGSIMP=1, viscous
and source terms (of turbulence) are neglected on coarser levels. No simplifica-
tion for MGSIMP=0. Default: MGSIMP=1
RSMPAR(real): Residual smoothing parameter σ*/σ. A value less or equal to zero means no
residual smoothing.
SMCOR(real): 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.
b) Spatial Discretization
IFACE(integer): = 1(default): Cell face gradients are used for the viscous fluxes,
Numerical Scheme Numerical Model
6-8 FINE™/Turbo
= 0: cell corner gradients.
IWAVVI(integer): 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.
IWAVCO(integer): If IWAVCO=0 a variable averaging is performed. If IWAVCO=2 a flux averag-
ing is used instead.
c) Central Discretization
CDIDTE(real): 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
EXPMAR(real): Exponent in the multi-dimensional scaling model of Martinelli of the dissipa-
tion used in central schemes. Default EXPMAR=0.5 i.e. multi-dimensional
scaling not used.
IARTV2(integer): Defines whether the second order artificial dissipation switch should be based
on both pressure and temperature gradients (parameter IARTV2=1) or on pres-
sure 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.
VIS2(real): Coefficient κ(2) for 2nd order dissipation in the central scheme (default
VIS2=1.0).
VIS2KE(real): 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
VIS2SW(integer): This parameter switches off all second order dissipation for incompressible flu-
ids (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 incom-
pressible fluids. Sometimes it may be stabilizing to use some second order dis-
sipation. In that case set this parameter to zero.
VIS4(real): Coefficient κ(4) for 4th order dissipation in the central scheme. Default
VIS4=0.1
VIS4KE(real): 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
VISNUL(integer): Eliminates 2nd order dissipation fluxes along the physical boundaries (central
scheme). Default VISNUL=1. If VISNUL=0, the procedure is not applied.
d) Upwind Discretization
ENTRFX(real): Entropy coefficients. The first value is the entropy fix 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.
IRATIO(integer): Vector of two values, that indicate which effective ratio is to be used. The first
value applies to the linear field, the second to the non-linear field.
IRATIO is only active for second-order upwind schemes.
Numerical Model Numerical Scheme
FINE™/Turbo 6-9
IROEAV(integer): =1 indicates that Roe averages are to be used to calculate cell face data. If
IROEAV=0 (default), arithmetic averaging will be used.
e) Time Discretization
IBOTH(integer): used in combination with ISWV. The latter parameter indicates whether the dis-
sipation 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 dissipa-
tion. The default value = 2 means that the dissipation term contains only the
artificial dissipation. The physical dissipation is computed once per time step.
IRKCO(real): 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:
1st order upwind - Van Leer:
4stage .0833 .2069 .4265 1.
5stage .0533 .1263 .2375 .4414 1.
2nd order upwind - Van Leer:
4stage .1084 .2602 .5052 1.
5stage .0695 .1602 .2898 .5060 1.
central scheme - Jameson:
4stage .25 .3333 .5 1.
5 stage .25 .1666 .375 .5 1.
both central and upwind - Eliasson:
4stage .125 .306 .587 1.
5stage .0814 .191 .342 .574 1.
NSTAGE(integer): number of stages for the explicit Runge-Kutta scheme. In practice, 4 or 5 stage
schemes are mostly used.
= 4: ISWV = 1 1 0 ...(ISWV can be modified afterwards independently)
= 5: ISWV = 1 0 1 0 1 0 ...(ISWV can be modified afterwards independently)
IRSMCH(integer): specifies the type of residual/correction smoothing.
= 1: standard version
= 2 (default only if Hakimi preconditioning): Radespiel & Rossow
= 3 (default): Zhu, time step dependent coefficients
= 4: Swanson & Turkel viscous
= 5: Vatsa. On meshes without high aspect ratio.
ISWV(real): 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 recalcula-
tion of dissipative residual (latest available value will be used); 1 means recal-
culation. 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) respec-
tively. 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 combina-
tion with IBOTH.
RSMPAR(real): residual smoothing parameter σ*/σ. A value less or equal to zero means no
residual smoothing. Default value = 2.
Numerical Scheme Time Configuration
6-10 FINE™/Turbo
6-3 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 or Harmonic should be selected which gives
access to additional parameters respectively for unsteady flow simulation. All parameters in the
FINE™/Turbo interface related to Unsteady computations are described in the following section.
The parameters related to Harmonic computations are described in section 8-4.
6-3.1 Interface for Unsteady Computation
When selecting Unsteady time configuration in the Flow Model page the following additional
parameters become accessible in the FINE™/Turbo interface:
a) Rotating Machinery
On the Rotating Machinery page, under the Rotor-Stator tab, 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.
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:
•fct(time) to define a constant value in space but varying in time. Click on the profile data but-
ton ( ) 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 tabs,
and to set the periodicity of the signal entered in FINE™/Turbo through the expert parameter
NPERBC.
The FINE™/Turbo solver allows only one rotation speed (combined with a zero rota-
tion speed) when performing an unsteady simulation using the Domain Scaling method
or Phase lagged method.
The inlet/outlet unsteady boundary condition circumferential profile has to be
imposed on a range covering the initial blade passage location and the blade passage
location after one period of the signal.
Time Configuration Numerical Scheme
FINE™/Turbo 6-11
Example:
FIGURE 6.3.1-4 Circumferential signal
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 phys-
ical time step in the FINE™/Turbo 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 calcula-
tion with the period of the varying inlet or outlet boundary conditions different from the blade pass-
ing period, the Phase Lagged option should be activated in the Rotating Machinery page and the
periodicity of the signal entered in FINE™/Turbo has to be specified through the expert parameter
NPERBC.
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.
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 turbomachin-
ery 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 6-3.3.4.
v2.2
θ
02π
π
t0
T
t0+T
v2.2
θ
02π
π
t0
T
t0+T
θ1 θ2 θ3 θ4
Numerical Scheme Time Configuration
6-12 FINE™/Turbo
•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 Bound-
ary 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 output files will be overwritten, every time the solution is saved. In order to keep
the successive unsteady solutions, the multiple output (Multiple Files) option has to be acti-
vated.
•Include Time Averaged Solution in Output: When activated the time averaged solution will
be saved in a "_tav.cfv" file. This option is only available when Rotor/Stator interfaces are
detected or the Rotating Boundary Condition is activated.
The option Include Time Averaged Solution in Output is not available when the
phase lagged approach is used. A tool has been provided, which allows the user to com-
pute the time averaged solution for the phase lagged computation. For more information,
refer to Chapter 6-3.3.6.
•Outputs For Visualization:
—At end only and Intermediate Restart Files: One File: During the computation, one set of
output files is saved1 for a possible restart of the unsteady computation. Output files for vis-
ualization in CFView™ are only available at the end of the computation. No second order
restart possible.
—At end only and Intermediate Restart Files: Multiple Files: During the computation, mul-
tiple sets of output files are saved1 for restart of the unsteady computation. Output files for
visualization in CFView™ are only saved at the end of the computation. This option allows
a second order restart (see paragraph e).
—Intermediate and One Output File: One set of output files is saved2 for restart of the
unsteady computation and visualization in CFView™ during the computation. No second
order restart possible.
—Intermediate and Multiple Files: Multiple sets of output files are saved2 for restart of the
unsteady computation. and visualization in CFView™ during the computation. This option
allows a second order restart (see paragraph e). This combination has to be chosen to be able
to make an animation of the saved time steps in CFView™.
•Number Of Steady Iterations: the number of iterations to initialize the unsteady computa-
tion. Such initialisation is performed with the steady state algorithm, using fixed geometry and
mesh as well as constant inlet/outlet boundary conditions. In case this initialisation procedure
is used the steady state iterations can even be proceeded by a full multigrid process allowing a
rapid initialisation of the flow.
•Save Steady Solution Every: the number of iterations at which the solution of steady initiali-
sation is saved
By default only one output file is created. For the generation of multiple output files,
the Multiple Files option has to be selected.
1. The solution is saved every x time steps as specified in Save Solution Every ... time steps
2. The solution is saved every x time steps as specified in Save Solution Every ... time steps
Time Configuration Numerical Scheme
FINE™/Turbo 6-13
e) Second Order Accurate in Time
The FINE™/Turbo solver performs second order accurate simulations in time. In order to allow 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 pre-
vious time step. When requesting a restart of an unsteady computation the FINE™/Turbo solver
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 a limited output is saved when selecting Multiple Files with Output
For Visualization/At end only. If a solution is requested every x time steps, only solu-
tion files with extension ".cgns" are written every x time steps instead of a full set of
solution files. This limited output still allows to restart from this solution (see section 12-
2). The full set of solution files will be written at the end of the computation.
6-3.2 Expert Parameters for Unsteady Computations
6-3.2.1 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. 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.
•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 iteration process is automatically stopped after this maximum number of iterations if
the convergence criteria has not been satisfied before.
6-3.2.2 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.
ICYOUT(integer): can be equal to 0 or 1 (default):
0: name of output changes with suffix _t#iter,
1(default): each solution is overwritten every cycle.
IFNMB(integer): can be equal to 0 (default) or 1:
0 (default): to keep all PERNM or NMB boundaries,
1: to transform all PERNM boundaries into periodic full non matching ones or
all NMB boundaries into full non matching ones.
NPERBC(integer): can be equal to 1 (default) or integer value:
1 (default): when the inlet/outlet unsteady boundary condition is a rotating cir-
cumferential profile (activating Rotating Boundary Condition and specifying
the rotational speed in Rotational Speed Unsteady respectively under the
INLET and OUTLET tabs) and the boundary condition is entered in the
FINE™/Turbo interface for the full range [0,2π].
Numerical Scheme Time Configuration
6-14 FINE™/Turbo
N: when the inlet/outlet unsteady boundary condition is a rotating circumferen-
tial profile (activating Rotating Boundary Condition and specifying the rota-
tional speed in Rotational Speed Unsteady respectively under the INLET and
OUTLET tabs) and the boundary condition is entered in the FINE™/Turbo
interface for part of the range [0,2π/N] covering one or multiple periods of the
signal.
RELPHL(real): 0.5 (default) if necessary, under-relaxation factor can be applied on Periodic
and R/S boundary conditions by reducing the two values of the expert parame-
ter for respectively the periodic and the R/S boundary conditions.
6-3.3 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 8-3.2.3.
6-3.3.1 General Project Set-up for Time Accurate Computations
1. Create a new project,
2. Select the fluid to use in the Fluid Model page,
3. Select Unsteady time configuration in the 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 4-2 and section 4-
3.
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 8.
5. Set the steady or unsteady boundary conditions. For more detail on time dependent boundary
conditions and phase lagged approach see section 6-3.3.2.
6. Concerning the initial solution for unsteady computations there are three possibilities:
—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 initialisation procedures see section 6-3.3.3.
7. All outputs available in steady mode are also available in unsteady mode (see Chapter 10).
8. On the Control Variables page set:
—the physical time step or number of angular position (see section 6-3.3.4) and the number of
time steps or periods,
—the amount of output files (see section 6-3.3.5),
—amount of iterations in steady state initialisation (see section 6-3.3.3).
6-3.3.2 Time Dependent Boundary Conditions
Unsteadiness can be generated by means of time varying inlet/outlet boundary conditions. Two dif-
ferent situations can be encountered:
1. The time variation is imposed as an amplitude factor of the space variation,
2. The time variation is imposed by rotating the inlet and/or outlet boundary condition. The abso-
lute rotation speed of the boundary condition(s) is imposed in the Boundary Conditions page.
Time Configuration Numerical Scheme
FINE™/Turbo 6-15
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 the
Phase Lagged approach.
2. The period of the time varying inlet/outlet boundary condition is different from the blade pass-
ing 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™/Turbo 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 on θ, z-θ or r-θ. The
profile is rotating at the speed, specified in the Boundary Conditions page (Rotational
Speed Unsteady).
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 Figure 6.3.1-4).
6-3.3.3 Initialisation Procedure
a) Start From 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 ade-
quate 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 the time-marching approach based on a local time stepping, which is proposed 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 6-3.3.1. In step 6
select in the Initial Solution page from file and select the solution of the steady computation. In
step 8 (section 6-3.3.1) it is also possible to select additional steady state initialisation in the Con-
trol 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 9-4.
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 acti-
vated in unsteady calculations the ".cfv" and ".cgns" files 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 the FINE™/Turbo solver 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.
c) Steady State Initialisation in Unsteady Computation
The steady state initialisation is automatically performed before starting the time accurate computa-
tion (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 Initialisation parame-
ters on the Control Variables page.
Numerical Scheme Time Configuration
6-16 FINE™/Turbo
6-3.3.4 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 the Domain Scaling method, 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 8-3.2.3 for more details).
When working with the Phase Lagged method, the Number Of Angular Positions is the number
of time iterations per 2π (see Chapter 8-3.2.4 for more details).
The following examples show the settings of Number Of Angular Positions and Number Of
Time Steps when using an unsteady inlet boundary condition.
Example 1: single blade row calculation involving phase-lagged boundary conditions
When working with a 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
revolutions. 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 rev-
olution (2π)
Example 2: complet