guideline COSMOS by qoolshabi

VIEWS: 367 PAGES: 182


Solver User’s Guide

 Finite Element Fluid Flow
 and Heat Transfer Solver

       Version 4.1

The COSMOS/Flow product is copyrighted and all rights are
reserved by Blue Ridge Numerics, Incorporated. Copyright (c) 1992-
1999 Blue Ridge Numerics, Incorporated. All Rights Reserved.

The distribution and sale of COSMOS/Flow is intended for the use of
the original purchaser only and for use only on the computer system
specified at the time of the sale. COSMOS/Flow may be used only
under the provisions of the accompanying license agreement.

The COSMOS/Flow Solver User’s Guide may not be copied, photo-
copied, reproduced, translated or reduced to any electronic medium or
machine readable form in whole or part without prior written consent
from Blue Ridge Numerics, Incorporated. Blue Ridge Numerics,
Incorporated makes no warranty that COSMOS/Flow is free from
errors or defects and assumes no liability for the program. Blue Ridge
Numerics, Incorporated disclaims any express warranty or fitness for
any intended use or purpose. You are legally accountable for any vio-
lation of the License Agreement or of copyright or trademark. You
have no rights to alter the software or printed materials.

The development of COSMOS/Flow is ongoing. The program is con-
stantly being modified and checked and any known errors should be
reported to Blue Ridge Numerics, Incorporated.

Information in this document is for information purposes only and is
subject to change without notice. The contents of this manual do not
construe a commitment by BRNI.

All brand and product names are trademarks of their respective own-
1            Getting Started

    Congratulations and thank you for choosing COSMOS/Flow as your fluid
    flow analysis tool!

    COSMOS/Flow is designed to be an interactive program with an intuitive
    graphical user interface (GUI) that allows you to communicate effectively
    with the program during the course of a CFD analysis. COSMOS/Flow pro-
    vides graphical data which monitor solution progress and aid in making a
    definitive assessment of convergence.

    COSMOS/Flow User’s Guide • 01/2000                                    1-1
      Chapter 1 Getting Started

      COSMOS/Flow solves the mathematical equations which represent heat
      and momentum transfer in a moving fluid. The finite element method is
      used to discretize the flow domain, thereby transforming the governing par-
      tial differential equations into a set of algebraic equations whose solution
      represent an approximation to the exact (and most often unattainable) ana-
      lytical solution. The numerical formulation is derived from the SIMPLER
      solution scheme introduced by Patanker1. More detail is available in the
      Technical Reference.
      The finite element, geometric, and boundary condition information required
      by the solver must be created or imported using COSMOS/Works, COS-
      MOS/Edge, or COSMOS/DesignSTAR. Results computed by the COS-
      MOS/Flow Solver are visualized in CFDisplay.

      Using COSMOS/Flow
      To perform flow analysis using COSMOS/Flow, you need to go through the
      following steps:
      1 Make the design in a CAD system. If you are using COSMOS/Works,
          create your model in SolidWorks. If you are using COSMOS/Edge, use
          Solid Edge to create your model. If you are using COSMOS/
          DesignSTAR, use your favorite CAD system. COSMOS/DesignSTAR
          supports most CAD systems.
      2 Import the CAD model to COSMOS/DesignSTAR or COSMOS/Edge.
          Skip this step for COSMOS/Works since COSMOS/Works is
          embedded in SolidWorks
      3 Create a thermal study.
      4 Apply flow boundary conditions. The flow boundary conditions are
          mapped on to structural boundary conditions. These mapped boundary
          conditions can be applied in a thermal study. Please refer to attached
          document for details

      1. Patankar, S.V., Numerical Heat Transfer and Fluid Flow, Hemisphere Publish-
         ing, New York, 1980

1-2   COSMOS/Flow User’s Guide • 01/2000
Chapter 1 Getting Started

5 Mesh the model
6 Choose Run COSMOS/Flow from Analysis menu
7 COSMOS/Flow will start. All the mesh and boundary conditions are
    transferred to COSMOS/Flow
8 Run and view the results in COSMOS/Flow and CFDisplay.

COSMOS/Flow Functionality
The following is a list of the funtionality and features in COSMOS/Flow.

Geometric Functionality
• Only three dimensional models can be analyzed with COSMOS/Flow in
  this release.
• Cartesian analysis coordinates.

Flow and Heat Transfer Characteristics
• Incompressible and Compressible flow including Subsonic, Transonic
  and Supersonic flow regimes
• Laminar and Turbulent flows
• Steady-state
• Single-Phase flows
• Multiple fluid capability
• Newtonian and non-Newtonian fluids
• External and/or Internal flow
• Distributed Resistance/Porous Media
• Internal fan/pump regions
• Forced, Natural or Mixed Convection
• Conduction Heat Transfer
• Conjugate Heat Transfer (Solid Conduction simultaneous with Fluid

COSMOS/Flow User’s Guide • 01/2000                                     1-3
      Chapter 1 Getting Started

      •   Radiation heat transfer capability
      •   Boundary Conditions
      •   Inlet/outlets
      •   Walls and moving walls
      •   Arbitrary slip boundaries
      •   Total Pressure boundary condition
      •   Fan/Pump curve boundary condition
      •   Boundary conditions in local coordinates
      •   Heat flux
      •   Film coefficient

      Productivity Enhancers
      •   Multi-threaded user interface
      •   Parallel Multi-processing
      •   Advanced iterative matrix solvers for non-symmetric matrices
      •   Global re-initialization of variables
      •   Integrated postprocessor

      Fluid/Solid Properties
      •   Property definition of distributed resistance elements
      •   Property variations with user-selected independent variable
      •   User-defined look-up tables for functional form of properties
      •   Carreau and Hershel Buckley Non-Newtonian models
      •   User-modifiable fluid property data base
      •   User-modifiable solid property data base
      •   Units of inch-Watt-C added to fluid property data base

1-4   COSMOS/Flow User’s Guide • 01/2000
Chapter 1 Getting Started

CFDisplay Functionality
•   Geometry viewed as surfaces, lines, or points
•   Overlaid mesh lines
•   Filled contours (textured, plain, or shaded)
•   Texture and environment mapping
•   Vector arrows
•   Iso surfaces
•   Clipping plane
•   Particle tracing
•   Animation of transient results sets
•   2D curve plotting
•   Trace lines of vector results
•   Graphical output in TIFF, RGB, PPM, and MPEG
•   Image mirroring about x, y, and z axes.
•   Z-buffer
•   Flat and smooth shading (gouraud shading)
•   Wireframe Display
•   Save Scene to Clipboard
•   Print Command
•   Cutting Plane Vector Density Set in Cutting Plane Dialog
•   Uniform Color Vectors
•   Hidden Line Display
•   Move Model as Outline
•   Part Attributes with Part Highlighting
•   Parts by Property
•   Part Tips
•   Detailed Information Dialog

For a more detailed discussion and definition of some of these terms, refer
to the Solver Technical Reference.

COSMOS/Flow User’s Guide • 01/2000                                       1-5
      Chapter 1 Getting Started

      New Features of CFDisplay 4.1
      • Internal fans/pumps
        You can place internal fans/pumps or more generic momentum/mass
        sources into the interior of the problem domain.
      • Fan/Pump curve boundary condition
        You can represent inlets with a fan curves or pump head/capacity curves.
        COSMOS/Flow will adjust the mass flow across these boundaries
        according to the system pressure
      • Parallel Multi-processor
        If your PC has more than one processor, COSMOS/Flow will detect this
        automatically and use the other processor during the solve cycle.
      • Global re-initialization of field variables
        Many times, you may run an analysis several iterations and then discover
        the initial temperature, for example was at an unrealistic value. This
        feature allows you to change this initial value at any time during the
        analysis.The boundary conditions will be maintained at the user defined
      • Visualizing turbulence intensity in CFDisplay
        The turbulence intensity is a good measure of the level of turbulence and
        can also be used to determine areas where turbulence induced noise
      • Automated 0 iteration run
        You can check your model to make sure you have the proper number of
        inlets/outlets and that there are no disconnected faces.
      • Save-All-As function
        If you use a COSMOS GFM file (generated by COSMOS/Works,
        COSMOS/Edge, or COSMOS/DesignSTAR), this function will save all
        of the files necessary to restart your analysis with a new jobname. This is
        a convenient way to do parametric studies of say, boundary condition
      • Wireframe Display
      • Save Scene to Clipboard
      • Print Command
      • Cutting Plane Vector Density Set in Cutting Plane Dialog

1-6   COSMOS/Flow User’s Guide • 01/2000
Chapter 1 Getting Started

•   Uniform Color Vectors
•   Hidden Line Display
•   Move Model as Outline
•   Part Attributes with Part Highlighting
•   Parts by Property
•   Part Tips
•   Information Dialog

COSMOS/Flow Documentation
COSMOS/Flow is documented in 3 manuals:
q   The COSMOS/Flow Solver User’s Guide
q   The COSMOS/Flow Solver Technical Reference
q   The COSMOS/Flow Tutorial Guide

The COSMOS/Flow Solver User’s Guide covers the fundamentals of creat-
ing a model suitable for a COSMOS/Flow analysis. The user interface is
explained and analysis techniques are described for a large number of dif-
ferent analysis types.

The COSMOS/Flow Technical Reference contains the theory behind COS-
MOS/Flow and the error messages and their explanation.

The COSMOS/Flow Tutorial Guide contains a number of example models
and step-by-step instructions for creating meshes, applying boundary condi-
tions, running analyses, and postprocessing results.

The Solver User’s Guide contains the following chapters:
    •   Chapter 1: Getting Started
    •   Chapter 2: Installing COSMOS/Flow
    •   Chapter 3: Model Guidelines
    •   Chapter 4: The COSMOS/Flow Control File
    •   Chapter 5: Analysis Guidelines

COSMOS/Flow User’s Guide • 01/2000                                      1-7
      Chapter 1 Getting Started

         • Chapter 6 and 7: postprocessing

      This chapter serves as an introduction to COSMOS/Flow. It provides a brief
      description of COSMOS/Flow functionality, instructions for invoking the
      program, and a brief overview of the COSMOS/Flow analysis process.

      Chapter 2 provides a step-by-step installation procedure.

      Chapter 3 describes the pre-processing required by COSMOS/Flow. Topics
      such as meshing and boundary conditions are covered.

      Chapter 4 explains the COSMOS/Flow Solver GUI Menu System. This
      chapter is meant to serve as a supplement to the on-line help system. Fig-
      ures are provided for reference as the menu selections are described.

      In Chapter 5, CFD analysis guidelines are presented and discussed. This is
      an important chapter and should be read before using COSMOS/Flow. At
      the end of Chapter 5 are procedures for troubleshooting an analysis, if prob-
      lems should arise.

      Chapters 6 and 7 cover postprocessing.

      Invoking COSMOS/Flow
      To use COSMOS/Flow, you need COSMOS/Works, COSMOS/Edge, or
      COSMOS/DesignSTAR. If you are using COSMOS/Works or COSMOS/
      Edge, you can create your geometry in SolidWorks or Solid Edge, respec-
      tively. If you are using COSMOS/DesignSTAR, you can import your geom-
      etry from your favorite CAD system. You cannot create geometry in

      After the finite element model is completed in COSMOS/Works, COS-
      MOS/Edge, or COSMOS/DesignSTAR, you can launch COSMOS/Flow to
      perform the analysis.

1-8   COSMOS/Flow User’s Guide • 01/2000
Chapter 1 Getting Started

Ways to start the COSMOS/Flow Solver program:
q   To launch COSMOS/Flow from COSMOS/Works, click FEM, Run
    COSMOS/Flow. This generates a GEO file that is read by COSMOS/
q   To launch COSMOS/Flow from COSMOS/DesignSTAR or COSMOS/
    Edge, choose Define, Run COSMOS/Flow.This generates a GEO file that
    is read by COSMOS/Flow.
q   You can also start COSMOS/Flow as you would start any other
    application in the Windows environment (icon, My Computer, Explorer,

After the analysis is completed, click on the Results icon in the COSMOS/
Flow Solver Main Menu to invoke CFDisplay,.


COSMOS/DesignSTAR is a product of Structural Research and Analysis
Corporation. It is an open-architecture, multiple-document program, that
takes advantage of the well-known Windows Graphical User Interface
(GUI). You will find it familiar, efficient, and easy to use. The open
architecture of COSMOS/DesignSTAR allows integration with third party
analysis software, user customization, and the addition of complementary

COSMOS/DesignSTAR, based on the Parasolid geometry engine, also
supports ACIS and STEP standards. COSMOS/DesignSTAR can directly
open SolidWorks and Pro/Engineer part files as well as IGES files of parts
and assemblies. With these capabilities, COSMOS/DesignSTAR can analyze
parts and assemblies created in almost any CAD system. Once you import
your geometry to COSMOS/DesignSTAR, you can create studies, assign
materials, mesh the model, and apply boundary conditions. For flow
analysis, you need to launch COSMOS/Flow to define analysis options, run
the analysis, and visualize the results.

COSMOS/Flow User’s Guide • 01/2000                                     1-9
       Chapter 1 Getting Started

       About COSMOS/Works

       COSMOS/Works, a product of Structural Research and Analysis
       Corporation, is a design analysis system fully integrated in SolidWorks.
       COSMOS/Works provides one screen solution for many types of analysis.
       Powered by COSMOS/FFE (Fast Finite Element) technology, COSMOS/
       Works lets you solve large problems quickly using your personal computer.
       COSMOS/Works comes in several configurations to satisfy your analysis

       SolidWorksTM, a product of SolidWorks Corporation. is a mechanical design
       automation software that takes advantage of the familiar Microsoft
       WindowsTM graphical user interface. This is easy-to-learn tool makes it
       possible for you to quickly sketch out ideas, experiment with features and
       dimensions, and produce models and detailed drawings.

       About COSMOS/Edge

       COSMOS/Edge is a design analysis system tailored for use with Solid
       Edge. COSMOS/Edge is an open-architecture multiple-document program
       that takes advantage of the well-known Windows Graphical User Interface
       (GUI). You will find it familiar, efficient, and easy to use. COSMOS/Edge
       is powered by fast solvers and state-of-the-art technologies.

       Solid EdgeTM is a computer-aided design (CAD) system for mechanical
       assembly, part modeling, and drawing production.

       Written specifically for Windows®, Solid Edge brings true parametric,
       feature-based solid modeling to the Windows environment. With an
       intuitive interface that emulates a practical mechanical engineering work
       flow. Solid Edge eliminates the command clutter and complicated modeling
       procedures of traditional CAD systems.

       Solid Edge is built on open and inter-operable software technologies so you
       can quickly put it to work with all your other computer-aided tools.

1-10   COSMOS/Flow User’s Guide • 01/2000
Chapter 1 Getting Started

Ending the Analysis

The COSMOS/Flow Solver will automatically run to the number of itera-
tions set in the Analyze window.

The COSMOS/Flow Solver can be terminated at any time during the analy-
sis phase by clicking on the Stop button on the Analyze window. When the
Stop button is hit, COSMOS/Flow will exit gracefully, meaning that the
current iteration or time step will be completed and the output results will
be current with the global iteration or time step that was being executed
when the stop key was hit.

COSMOS/Flow User’s Guide • 01/2000                                      1-11
1-12   COSMOS/Flow User’s Guide • 01/2000
2             Installing COSMOS/Flow

            This chapter shows you how to install COSMOS/Flow.

    Hardware and Software Requirements
    COSMOS/Flow requires the following:

    q   Pentium®-based computer,
    q   A mouse or other pointing device tablet,
    q   A monitor,
    q   CD ROM drive,
    q   Minimum 64 MB of RAM,
    q   About 20 MB of disk space for program installation, and
    q   100 MB of disk space should be available in your computer after
        installation to be able to run medium size problems,
    q   Microsoft Windows® 95, Windows® 98, or Windows® NT 4.0 or higher,
    q   COSMOs/DesignSTAR, COSMOS/Works, or COSMOS/Edge,

    ✍ A license string is required for the installation of COSMOS/Flow.
        Before starting the installation procedure, make sure that your license
        information is available.

    COSMOS/Flow User’s Guide • 01/2000                                      2-1
      Chapter 2 Installing COSMOS/Flow

      Installing Program Files
      ✍ COSMOS/Flow installation requires an existing installation of
          COSMOS/DesignSTAR (version 2.0 or later), COSMOS/Works
          (release code 1999/350 or later), or COSMOS/Edge (version 4.0 or
          later). If none of these products is installed on your computer, the
          installation program issues a warning message and gives you the
          option to quit or continue.

      To install the program files:
      1 Insert the COSMOS/Flow CD-ROM in the drive. The setup program
          starts automatically and a splash screen followed by a welcoming
          message opens.

      ✍ If you have turned off the autorun feature or if the setup does not start
          automatically, go to your CD-ROM drive in Windows Explorer and
          double-click the autorun.exe file.

2-2   COSMOS/Flow User’s Guide • 01/2000
Chapter 2 Installing COSMOS/Flow

2 Welcome: Read the information in the Welcome window, close any
  open windows or programs, and click Next.

3 Select the Installation Type: This window allows you to install the
  program files or the license. Choose Install COSMOS/Flow and click

COSMOS/Flow User’s Guide • 01/2000                                      2-3
      Chapter 2 Installing COSMOS/Flow

      4 Software
          Read the
          agreement and
          click Yes if you
          agree to all
          terms and

      5 Specify
        Folder: The
          default directory is C:\Program Files\Cosmosflow. Change the
          installation folder if desired and click Next.
      6 Select Optional Components: Select the optional components to be
        installed. Click Next .

      ✍ The documentation of COSMOS/Flow consists of 3 manuals:
          COSMOS/Flow User’s Guide, COSMOS/Flow Technical Reference,
          and COSMOS/Flow Tutorial

2-4   COSMOS/Flow User’s Guide • 01/2000
Chapter 2 Installing COSMOS/Flow

7 Select program Folder: The default program group name appears in the
    Program Folder field. Change the default folder, if desired, and click

8 Start Copying Files: Review the settings. Click Back to make changes
  or click Next to continue. The installation program starts copying files
    to their proper destination.

COSMOS/Flow User’s Guide • 01/2000                                       2-5
      Chapter 2 Installing COSMOS/Flow

      9 Setup Complete : Click OK to complete the installation of COSMOS/

      Configuring COSMOS/Flow License
      To configure the COSMOS/Flow license:
      1 Insert the COSMOS/Flow CD in your CD-ROM drive again. The setup
          program starts automatically and a splash screen followed by a
          welcoming message opens. Click Next.
      2 Select Installation Type: Select Configure COSMOS/Flow License.
      3 License File Information: You should have received a license file from
        your sales representative. Make your selection and click Next.
      4 Depending on your selection in step 3, the licensing procedure will
          continue as follow:
         • If you select “A diskette marked Program License File”, you will be
            asked to insert the diskette containing the license file (brni.lic).
            Browse to where the license file is then click Next. You will get a
            message that the license configuration is successful. Click OK to end
            the license configuration procedure.
         • If you select “A sheet of paper entitled Important: Retain for your
            records”, you will be asked to type the authorization string in a text
            editor exactly as it appears on the license sheet. When you finish
            typing, save the file and exit the Notepad. You will get a message that
            the license configuration is successful. Click OK to end the license
            configuration procedure.
         • If you select “A Directory containing the license file”, you will be
            asked to specify the directory where the license file is. Browse to the
            desired directory and click Next. You will get a message that the
            license configuration is successful. Click OK to end the license
            configuration procedure.

2-6   COSMOS/Flow User’s Guide • 01/2000
3             Modeling Guidelines

    The purpose of this chapter is to describe how to create models that will
    work well with the COSMOS/Flow Solver.Throughout this chapter, refer-
    ences are made to specific pull-down menus and windows. The convention
    for identification is illustrated by the title of the window introducing the on-
    line help system: COSMOS/Flow_Help_onHelp. Note that the title of the
    Main Window, COSMOS/Flow, is always first in the hierarchical chain of
    selections linked together by the “_” symbol. A similar convention is used
    for the COSMOS/Works, COSMOS/Edge, and COSMOS/DesignSTAR
    menu system.

    This chapter covers the following areas:
       • Importing and Building Geometry
       • Meshing
       • Applying boundary conditions

    COSMOS/Flow User’s Guide • 01/2000                                          3-1
      Chapter 3 Modeling Guidelines

      Importing and Building Geometry


      ✍ If you are using COSMOS/Flow with COSMOS/Works, use Solid
          Works to create your model. If you are using COSMOS/Flow with
          COSMOS/Edge, use Solid Edge to create your geometry.

      ✍ If you are using COSMOS/Flow with COSMOS/DesignSTAR, use
          your favorite CAD system to create the model.Refer to the on-line
          help of COSMOS/DesignSTAR for details.

      The geometry used for a typical CFD analysis is often somewhat different
      than that used in a structural analysis. To analyze a pipe for example, in a
      structural analysis the walls of the pipe would be meshed and the interior
      would be omitted from the calculation domain. In a CFD analysis however,
      the walls of the pipe are omitted (unless they are to be used as part of a heat
      transfer calculation) and the interior volume of the pipe is what is modeled.
      Another description of the interior volume is this: imagine that the pipe
      were filled with water and the water was allowed to freeze. Now, imagine
      that the pipe walls were chipped away, and all that remained was the solid
      volume of ice. This volume is where the fluid exists, and is the geometry
      that would be created and meshed for a CFD analysis of that pipe flow.

      The other broad classification of CFD analysis geometry is the submerged
      object. The flow over a wing or a submarine are two examples of sub-
      merged objects. In COSMOS/Flow, it is customary to “invert” the geome-
      try, meaning that the object will be made stationary and the flow will be
      blown over it at the equal and opposite speed of the object. To implement
      this as analysis geometry, two pieces of geometry are needed: the object
      itself (missile, submarine, bullet, etc.) and a large calculation domain in
      which the object is positioned. The shape of the domain is usually not very
      critical, and can be a circle, semi-circle, rectangle, sphere, or box. Because
      the flow all around the object is being modeled, it is a good idea to make the
      computational domain be substantially larger than the object itself. More
      detail about the relative size of the calculation domain will be discussed in
      Chapter 4 of this manual.

3-2   COSMOS/Flow User’s Guide • 01/2000
Chapter 3 Modeling Guidelines

There may be some editing required to make the model suitable for COS-
MOS/Flow. Editing should be performed on selected entities so no geome-
try data is inadvertently deleted. In general, geometry details that are very
small, i.e. several orders of magnitude smaller than the analysis model,
should be suppressed or deleted. Items such as bolts or burrs should be
smoothed by creating new curves or surfaces unless they are of critical
interest to the analysis.

Meshing is performed in COSMOS/DesignSTAR, COSMOS/Works, or
COSMOS/Edge. This section will cover several aspects of meshing critical
to creating a COSMOS/Flow model.

Mesh Topology

A primary cause of solution divergence is inadequate mesh topology, a term
which refers to the number, size and distribution of finite elements through-
out the solution domain. Many engineers choose to use finite elements in
CFD because they have experience in structural analysis. Applying this
background in CFD is generally helpful but can lead to difficulties, particu-
larly with regard to meshing.

In any finite element analyses, more elements are required in areas of the
model where spatial gradients of the solution variables are high. In CFD, an
additional physical phenomenon called velocity-pressure coupling must
also be accurately represented on the mesh to ensure continuity of fluid
mass over the entire solution domain. This distinction elicits the following
two requirements:
   • Many more elements must occupy the domain than in a typical
     structural analysis;
   • Transitions in element size must be relatively smooth so that the area
     or volume of adjacent elements do not vary substantially.

COSMOS/Flow User’s Guide • 01/2000                                         3-3
      Chapter 3 Modeling Guidelines

      In attempting to satisfy these criteria, engineers sometimes construct very
      large CFD finite element models, particularly when the geometry is com-
      plex. Typical 2D fluid flow analyses will take anywhere from 1,000 to
      25,000 nodes; 3D analyses from 5,000 to 100,000 nodes. These ranges are
      exceeded in some applications. A recent article describing flow over an
      automobile prototype required over 250,000 nodes!

      It is important to note that the sequential solution algorithm in COSMOS/
      Flow solves separately for u, v, w, P, T, k and ε at all nodes in the domain.
      Therefore, the number of degrees of freedom is simply the number of nodes.
      This feature makes COSMOS/Flow several orders of magnitude faster, per
      degree of freedom per iteration, than a typical structural analysis.

      Recommended Procedures

      To prevent construction of an unnecessarily large model and, conversely, to
      ensure that a sufficient number of nodes are present, the following steps are
      recommended when performing any CFD analysis.
         • Determine if there are any symmetries. Check for symmetries that do
           not lie on a Cartesian axis that can be implemented using slip
         • Examine the geometry, identifying probable high and low gradient
           regions for all solution variables (u, v, w, P, T, k and ε ).
         • Identify solid material zones and fluid zones and keep them as
           separate geometric parts.
         • Identify extended attribute (distributed resistances, internal fans/
           pumps, ..) zones and regular fluid zones and keep them as separate
           geometric parts.
         • If there are areas with minute geometric details, try using distributed
           resistances to model these zones, instead of meshing the detail. You
           can also use wall roughness values greater than zero if the detail is
           attached to a wall.
         • Because the outflow boundary conditions assume fully developed
           flow, try to place these boundaries where this is at least
           approximately true. The outlet should be removed from areas where

3-4   COSMOS/Flow User’s Guide • 01/2000
Chapter 3 Modeling Guidelines

     the flow must make a sharp turn. If the outlet is too close to the turn
     or at the turn, the mass balance could be off by as much as 20%.
     Move the outlet out to avoid this condition.
   • Perform an analysis on a coarse mesh (no more than 15,000 nodes) to
     qualitatively assess the flow features present and identify meshing
     needs in high gradient regions without a severe time penalty. Try the
     default element size. If the model does not have too many small
     features, turn on the automatic transition flag.
   • Looking at the results on the coarse mesh, use mesh control to refine
     the mesh in the high gradient regions.
   • To ensure that the final solution is not “mesh-dependent,” compare
     the two solutions from the coarse and fine meshes. If they are
     substantially different, then it is a good idea to construct a mesh that
     has at least 10% fewer nodes than the fine mesh, obtain a solution on
     that mesh and compare. The idea is to have two meshes that vary in
     number of nodes by 10% or more and that give the same solution.
     This solution is then said to be “mesh-independent”.

Locations of Mesh Refinement
Solid Boundaries

Spatial gradients for velocity, pressure, turbulent kinetic energy and turbu-
lent energy dissipation will generally be highest near a solid boundary, typi-
cally a containment wall or the surface of an immersed body. This is
particularly true if the flow is constrained by a tight clearance, forced to turn
around a sharp corner or suddenly brought to rest at a stagnation point.
Accordingly, mesh density must be greatest in these regions.

✍ The Automatic Transition flag in COSMOS/DesignSTAR, COSMOS/
    Edge, and COSMOS/Works, automatically assigns smaller element
    sizes to fillets and small features. Use Automatic transition unless you
    have too many fillets and/or other small features in your model. In
    that case, meshing with automatic transition could generate too many

COSMOS/Flow User’s Guide • 01/2000                                           3-5
      Chapter 3 Modeling Guidelines

      Important Rules
      q Place a minimum of five nodes across any flow passage, no matter how
        small, so that the velocity profile can be correctly resolved. (This rule is
        most important when using the k-epsilon turbulence model, which is the
        default. Fewer nodes can be used across a cross section for laminar flow
        or when using the constant eddy viscosity turbulence model.)
      q Where possible, construct the mesh so that elements adjacent to a solid
        boundary are approximately one-tenth the width (in the direction normal
        to the boundary) of elements in the free stream where the fluid is
        relatively uninfluenced by the boundary. This can save substantially on
        the number of nodes in the model. As noted previously, make sure that
        mesh transitions are smooth.

      Inlet/Outlet Passages

      In general, elements must be concentrated at inlet openings to allow solu-
      tion gradients to develop. In some situations (compressible flows, for exam-
      ple), the regions near outlets should also have a fine mesh. If the outlet has
      been placed far enough out from the solution domain, no refinement is nec-
      essary. The goal is that the outlet should not strongly affect the solution.

      Thermal Boundaries

      Similar to the inlet passages, elements must be concentrated near walls with
      thermal boundary conditons. Usually near these boundaries is where the
      heat transfer rate, which is the temperature gradient, is the highest. You
      should also try to bunch nodes at the edges of these boundaries so the dis-
      continuity in heat transfer can be captured accurately.

      Sudden Change in Boundary Conditions

      The area surrounding the separation point between two boundary condition
      types must have a refined mesh to adequately resolve the discontinuity. An
      example is the point at the intersection of an insulated wall and a specified
      heat flux boundary in a convection analysis.

3-6   COSMOS/Flow User’s Guide • 01/2000
Chapter 3 Modeling Guidelines

Near Distributed Resistances/Porous Media Elements

Because of the extra pressure drop across distributed resistance/porous
media elements, you should refine the mesh in and around these regions to
resolve the velocity and pressure gradients.

Near Internal fans/pumps elements

Because of the extra pressure drop and increased or decreased flow rates
across these regions, you should refine the mesh in and around these regions
to resolve the velocity and pressure gradients.

Boundary Conditions
The units used by COSMOS/Flow and a general description of the bound-
ary types and their conditions are presented. COSMOS/Flow boundary con-
dition mappings are discussed in this chapter.

Units of Boundary Conditions

It is important that you are consistent with both the model geometry dimen-
sions and the specified boundary conditions. Post-processing quantities are
output in the same units as set in the COSMOS/Flow Solver Options win-
dow. COSMOS/Flow gets the system of units automatically from COS-
MOS/DesignSTAR, COSMOS/Works, or COSMOS/Edge. Use the same
system to define additional properties.

COSMOS/Flow User’s Guide • 01/2000                                       3-7
      Chapter 3 Modeling Guidelines

      The units used by the COSMOS/Flow Solver are as follows:.

      Boundary Types

      Boundary conditions are specified in COSMOS/Works, COSMOS/Design-
      STAR, or COSMOS/Edge. Please refer to the The COSMOS/Flow Tutorial
      Guide for detailed examples.

      This section describes the types of boundaries commonly found in COS-
      MOS/Flow analyses. The types of boundary conditions appropriate and
      some general notes are provided for each kind of boundary. The following
      section discusses how to apply each of these boundary conditions to a COS-
      MOS/Flow model.

3-8   COSMOS/Flow User’s Guide • 01/2000
Chapter 3 Modeling Guidelines

   • Specify the non-zero nodal velocity components or the static or total
     pressure at each inlet.
   • All unspecified velocity components will automatically be set to zero,
     if at least one component is set to a non-zero value.
   • For subsonic conditions at the inlet, you should specify either
     velocity or static pressure, not both.
   • For supersonic flows, both the velocity and the static pressure must
     be specified. This is true only if the inlet is supersonic or near sonic.
   • For heat transfer analyses, specify the temperature at all inlets.
   • For compressible flow analyses, the specified inlet temperatures are
     total (stagnation) temperatures, not static temperatures.
   • To activate swirl in a 2D axisymmetric analysis, specify the third
     component of velocity (usually the z-component).

COSMOS/Flow User’s Guide • 01/2000                                         3-9
       Chapter 3 Modeling Guidelines

          • Specify the static or total pressure. Specified pressures are always
            gage pressure; the absolute pressure is the sum of the gage pressure
            and the reference pressure set in COSMOS/Flow (see Chapter 4).
          • We recommend setting a value of zero at the outlet. Pressure is
            relative, so this is a convenient value.
          • No other conditions should be set here.
          • You should try to put the outlet downstream away from sudden turns
            or contractions. If the outlet is too close, the flow cannot reach a fully
            developed state, which is the condition assumed by COSMOS/Flow.
            Also, if the outlet is too close to an expansion area, you will get
            reverse flow at the outlet (flow re-entering). This may cause
            convergence difficulties.

          • AutoWall sets wall conditions automatically on all surfaces that are
            not defined as inlets, outlets, symmetry, slip, periodic, or unknown.
          • Thermal conditions must be set on walls if you are conducting a
            thermal analysis. Walls with no thermal specification will be
            considered adiabatic (perfectly insulating).

          • This type of boundary allows the fluid to follow the wall. The only
            condition is to prevent flow from crossing the boundary. Symmetry
            surfaces must be applied to planes (or edges) that are parallel to the
            coordinate system axes.
          • If axisymmetric elements are used, the symmetry condition is
            automatically set by COSMOS/Flow for all the nodes on the
            symmetry axis.

       Slip Walls
          • This type of boundary allows the fluid to follow the contour of the
            wall. The only condition is to prevent flow from crossing the
          • This boundary condition can be used with a near-zero viscosity to
            simulate Euler or inviscid flow.

3-10   COSMOS/Flow User’s Guide • 01/2000
Chapter 3 Modeling Guidelines

   • Slip walls are also useful to define a symmetry plane, but the surface
     or edge does not have to be parallel to a coordinate axis. This is why
     the slip condition offers more flexibility than the symmetry condition.

Fan/Pump curve inlets/outlets
   • You can represent pushing or pulling fans at these boundaries. You
     will enter the fan/pump curve in COSMOS/Flow and it will
     determine the actual operating point on the curve.

Total pressure inlets/outlets
   • There are many situations where the total pressure at an opening is
     constant or known - not the static pressure. Compressible flow
     problems is one example, natural convection is another.
   • For natural and free convection problems, the total pressure should
     usually be set at openings that will draw the air or convecting fluid.

Unknown inlet/outlet
   • Specify the unknown boundary condition on openings where you are
     not sure whether the flow will be entering or leaving.
   • In many supersonic compressible flow analyses, you do not know the
     outlet conditions before hand. Specify the unknown boundary
     condition on such outlets.
   • Natural convection, compressible and rotating flow analyses may
     contain boundaries of this type.

Internal boundary conditions
   • There are cases in which you may want to specify a boundary
     condition on internal nodes. For example, to represent a fan impeller
     in an axisymmetric problem, you can specify an out-of-plane or swirl
     velocity component (VZ) on all of the nodes located within the
     impeller region.
   • Note that COSMOS/Flow will issue a warning for these nodes, but
     this is only a caution.

COSMOS/Flow User’s Guide • 01/2000                                       3-11
       Chapter 3 Modeling Guidelines

       Thermal boundary conditions
          • Temperature
          For compressible flows, this will be considered the stagnation or total
          temperature by COSMOS/Flow.
          • Heat flux
          These conditions are per area, and are applied to element edges or faces.
          • Film coefficient
          These conditions are per area, and are applied to element edges or faces.
          • Surface radiation
          These conditions are per area, and are applied to element edges or faces.


       For a typical fluid flow analysis, most of the boundary nodes are wall nodes.
       To reduce the number of boundary conditions the user must apply, COS-
       MOS/Flow has an Automatic Wall Specification (AWS) algorithm which
       will invoke a wall or no-slip condition on all unspecified boundary nodes as
       it starts the analysis. Therefore, before starting the analysis, the user should
       be sure that all unspecified nodes are indeed wall nodes. Note, that the AWS
       only applies to the velocity conditions, thermal boundary conditions must
       still be specified.

       The Automatic Wall Specification
       Algorithm does more than just apply
       wall conditions to all unspecified exte-
       rior nodes. It examines the intersection
       of all specified flow conditions and                         wall
       walls and determines that nodes at such
       an intersection are indeed wall nodes
       (even though they have a velocity con-
       dition applied). For example, in the fol-    Specified Velocity inlet condition
       lowing situation:

       The condition at node A was set as a velocity. However, because node A is
       on the wall, it is really a wall condition. Auto Wall will identify node A as a
       wall node and automatically remove the velocity specification at that node.
       It is because of this intelligence in Auto Wall that you should specify the

3-12   COSMOS/Flow User’s Guide • 01/2000
Chapter 3 Modeling Guidelines

inlet condition on all nodes of the inlet edge or surface (which is what hap-
pens automatically when geometry associativity is used) and not manually
remove the condition at the inlet/wall interface.

✍ The COSMOS/Flow Solver applies the wall condition automatically.

COSMOS/Flow User’s Guide • 01/2000                                       3-13
         Chapter 3 Modeling Guidelines

         Mapping of Boundary Conditions from
         COSMOS/DesignSTAR or COSMOS/Edge.
         Boundary                 COSMOS/DesignSTAR or COSMOS/
         Condition                   Edge Boundary Condition

       Velocity                 Restraints, where the X, Y and Z restraints corre-
                                spond to the X, Y and Z components of velocity

       Pressure                 Pressure

       Temperature              Temperature

       Heat Flux                Heat Flux

       Heat Power               Heat Power

       Volume Heat              Volume Heat

       Convection               Convection

       Radiation                Radiation

       Slip Wall and            Directional Force, Use component Normal to
       Symmetry Planes          the Plane (a positive non-zero force should be set).
                                This is only a marker, the value is not impor-
                                tant. Do not use Normal Force. A negative
                                force specifies an unknown boundary condi-

3-14     COSMOS/Flow User’s Guide • 01/2000
  Chapter 3 Modeling Guidelines

  Boundary                 COSMOS/DesignSTAR or COSMOS/
  Condition                   Edge Boundary Condition

Unknown                  Directional Force, Use component Normal to
                         the Plane (a negative non-zero force should be set).
                         This is only a marker, the value is not impor-
                         tant. Do not use Normal Force. A positive
                         force specifies a slip wall or symmetry bound-
                         ary condition.

Fan/Pump Curves          Directional Force in the X-Direction AND
                         Pressure = fan curve ID where the force in X-direc-
                         tion is used to mark the boundary condition and the
                         pressure value (use an integer value) is used as the fan
                         curve ID in COSMOS/Flow.

Total Pressure           Directional Force in the Y-Direction AND
                         Pressure = total pressure value where the force
                         in the Y-direction is used to mark the boundary condi-
                         tion and the pressure value is used as the total pressure
                         value in COSMOS/Flow

  COSMOS/Flow User’s Guide • 01/2000                                             3-15
         Mapping of Boundary Conditions from
         Boundary              COSMOS/Works Boundary Condition

       Velocity            Restraints, where the X, Y and Z restraints correspond
                           to the X, Y and Z components of velocity

       Pressure            Pressure

       Temperature         Temperature

       Heat Flux           Heat Flux

       Heat Power          Heat Power

       Convection          Convection

       Radiation           Radiation

       Slip Wall and       Force_Normal to Plane (a positive non-zero force
       Symmetry Planes     should be set). This is only a marker, the value is
                           not important. A negative force specifies the
                           unknown boundary condition.

       Unknown             Force_Normal to Plane (a negative non-zero force
                           should be set). This is only a marker, the value is
                           not important. A positive force specifies a slip
                           wall or symmetry boundary condition.

3-16     COSMOS/Flow User’s Guide • 01/2000
   Chapter 3 Modeling Guidelines

  Boundary                   COSMOS/Works Boundary Condition

Fan/Pump Curves          Force_Along plane Dir 1 AND Pressure = fan
                         curve ID (use integer value) where the force in Dir 1
                         is used to mark the boundary condition and the pressure
                         value is used as the fan curve ID in COSMOS/Flow

Total Pressure           Force_Along plane Dir 2 AND Pressure =
                         total pressure value where the force in Dir 2 is used
                         to mark the boundary condition and the pressure value is
                         used as the total pressure value in COSMOS/Flow

   COSMOS/Flow User’s Guide • 01/2000                                          3-17
3-18   COSMOS/Flow User’s Guide • 01/2000
4             The COSMOS/Flow
              Control File

    After the geometry, mesh, and boundary conditions are created, you need to
    set up the COSMOS/Flow control file for your analysis. The control file
    contains all the settings necessary to run a COSMOS/Flow analysis. This
    chapter describes how to use the COSMOS/Flow Solver Graphical User
    Interface to construct a control file and covers the following areas:
       •   Opening a COSMOS/Flow Control File
       •   Setting Analysis Parameters
       •   Specifying Property Data
       •   Convergence Assistance
       •   Initialization
       •   Turbulence Settings
       •   Post Processing Settings
       •   The Analyze Window
       •   Convergence Assessment

    Much of the material in this chapter is accessible on-line by selecting the
    Help button in the current window or by pressing <F1>. When a more
    detailed explanation of a particular selection is required, reference is made
    to this and other chapters in the User’s Guide.

    COSMOS/Flow User’s Guide • 01/2000                                         4-1
      Chapter 4 The COSMOS/Flow Control File

      Throughout this chapter, references are made to specific pull-down menus
      and windows. The convention for identification is illustrated by the title of
      the window introducing the on-line help system: COSMOS/
      Flow_Help_onHelp. Note that the title of the Main Window, COSMOS/
      Flow, is always first in the hierarchical chain of selections linked together
      by the “_” symbol.

      Window selections are usually described by group. In the window screen
      display, a group is basically a box with a title that encloses one or more
      selections. In this chapter (and in the on-line documentation), the group
      name serves as a section header for the list of enclosed selections.

      File Management
      This section describes the functions available for creating, retrieving, and
      storing a control file. All of the commands are available from the File pick
      from the main menu:

4-2   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

To Begin

Creating a New Control File...

To create a new control file: In the COSMOS/Flow main menu,
click on the New icon:

You can also pick COSMOS/Flow_File_New. Use the browser
to go to the appropriate directory and name the file.

Opening an Existing Control File...

To open an existing control file, pick the Open icon:

You can also use COSMOS/Flow_File_Open from the main

Use the browser to pick the directory and file:

COSMOS/Flow User’s Guide • 01/2000                            4-3
      Chapter 4 The COSMOS/Flow Control File

      Verifying the Finite Element Model

      Picking COSMOS/Flow_File_Verify displays data relating to the geome-
      try and boundary conditions of the fluid domain.

      Note that verify values can only be displayed after the COSMOS/Design-
      STAR, COSMOS//Works, or COSMOS/Edge model files have been pro-
      cessed by COSMOS/Flow Solver. This happens when the analysis is first
      started. The information presented in this window is obtained from the
      binary restart files which do not exist until at least one analysis run has been
      completed. The following is an explanation of the items in the window:


      The number of nodes and elements in the fluid and solid portions of the

      Face Data

      The number of exterior element faces associated with the current geometry
      are given in this group. An exterior element face is any face belonging to
      only one element. The number of exterior faces associated with each of
      seven exterior face boundary condition types is given in this group.

4-4   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

An inlet face has at least one node with a finite velocity boundary condition
specified. An outlet face has pressure specifications on all nodes. Note that
the sum of the number of inlet, outlet, wall, and symmetry faces should be
less than or more usually equal to the number of exterior faces.

Coord. System

The geometry and calculation coordinate systems are given in this group.
The two coordinate systems may be distinct depending on the coordinate
selections in the finite element modeler. For instance, a cylindrical calcula-
tion is usually performed on a finite element mesh constructed in XYZ
coordinates. The COSMOS/Flow coordinate system labels are:
        • XY - 2D Cartesian
        • XR - 2D Axisymmetric (about X-axis)
        • RY - 2D Axisymmetric (about Y-axis)
        • RT - 2D Cylindrical coordinates
        • XYZ - 3D Cartesian
        • RTZ - 3D Cylindrical


The number of inlet, outlet or unspecified (Unknown) passages are dis-
played here. If any of these numbers is incorrect, there are probably dupli-
cate or unmerged nodes in the finite element model.

Nodal Boundary Conditions

Here, the number of nodal boundary conditions for all solution variables
plus other nodal boundary conditions are displayed.

Element B.C.S

This section lists the number of elements with volumetric heat source condi-
tions applied.

COSMOS/Flow User’s Guide • 01/2000                                         4-5
      Chapter 4 The COSMOS/Flow Control File

      Assigning a Title to the Control File (Optional)

      An optional title can be given a control file in addition to the control file
      name. To do this, pick COSMOS/Flow_File_Modify_Title from the main
      menu, and enter a title in the following window:

      Saving a Control File...

      Manual Save

      To save the current control settings in <jobName>.ctl, pick COSMOS/

      Automatic Save

      When you start the analysis (by hitting GO in the Analyze window), the
      control file settings are saved.

      Save As

      To save the file to a different user-specified file name, use COSMOS/
      Flow_File_Save As. Use the browser to choose the directory to which to
      save the control file. Save As can be used to copy the settings of an existing
      .ctl file to a new jobname or analysis

      Save All As

      To save all of the files required to do a new analysis to a different user-spec-
      ified file name, use COSMOS/Flow_File_Save As. Note that this function
      does also copy the COSMOS geo file. Use the browser to choose the direc-
      tory to which to save the files. Save All As can be used to copy files to a
      new jobname or analysis

4-6   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

The Utilities functions can be used to generate COSMOS GFM files from
the COSMOS/Flow database files.

To Exit COSMOS/FlowCOSMOS/Flow...
Pick the command COSMOS/Flow_File_Exit to leave COSMOS/Flow.
Note that the exit function does not save any modifications. If COSMOS/
Flow_Analyze_GO was not used, use COSMOS/Flow_File_Save to save
any changes that have been made to the COSMOS/Flow control file.

Setting Analysis Options
Under this menu, you will set the operating conditions for the analysis and
any special boundary conditions.

_Analysis Selections (Options)
The Analysis Selections window is where the CFD problem formulation is
defined and applicable equations are selected. This window is accessible in
two manners: from the main menu, pick COSMOS/Flow_Options_ Anal-
ysis Selections:

Click the Options icon:

COSMOS/Flow User’s Guide • 01/2000                                       4-7
      Chapter 4 The COSMOS/Flow Control File

      This dialog box contains the parameters and options for defining the type of
      analysis to be performed. The following sections contain an explanation of
      each of the items on this window.

      _Analysis Units

      The units of the analysis are set in this drop menu. This is the only place
      where units are set. Because COSMOS/Flow has multiple fluid capability, it
      is imperative that only one system of units be set for the analysis. All of the
      fluids and solids input in the Properties windows should be in this unit sys-

4-8   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

The available unit systems are:

                      m-kg-s        meter-kilogram-second
                      cm-g-s       centimeter-gram-second
                     mm-g-s        millimeter-gram-second
                      in-lb-s            in-pound-second
                      ft-lb-s            foot-pound-second
                     in-watt-k           inch-Watt-Kelvin

✍ You should use the same unit system that you have used in COSMOS/
    DesignSTAR, COSMOS/Edge, or COSMOS/Works. If you try to
    select a different unit system from the drop-down menu, you will get a
    warning message.

_Flow Parameters

...will solve the pressure and momentum equations for the fluid motion if
you select Internal Flow or External Flow. Internal Flow refers to fluid
motions through a rigid body. External Flow refers to a body submerged in
a fluid. If both are present, select Internal Flow. Flow should be Off for
conduction heat transfer analyses.

...will simulate laminar flow when Laminar is selected, or turbulent flow
when Turbulent is selected.

Several turbulence models are available. The turbulence model and its asso-
ciated parameters can be changed by picking COSMOS/
Flow_Preferences_Turbulence from the COSMOS/Flow Solver main



...characterizes any flow for which the maximum Mach number in the fluid
domain is less than 0.3.

COSMOS/Flow User’s Guide • 01/2000                                      4-9
       Chapter 4 The COSMOS/Flow Control File

       _Subsonic Compressible

       ...for flows which are compressible but contain no shocks.

       In particular, the fluid velocity must be low enough so that heat generation
       due to viscous shearing work on the fluid is negligible. Typically, a Mach
       number of 0.7-0.8 is the maximum for which this is true. If there is heat
       transfer, the static Temperature equation is solved. This equation neglects
       viscous dissipation and pressure work effects. If there is no heat transfer, the
       total temperature is held constant and the static temperature is determined

         T = T       + ---------                                                  (2-1)
          0    static 2c

       ...applies to all flows having a maximum Mach number greater than 0.8
       with or without heat transfer and shocks.

       If there is heat transfer, the total Temperature equation is solved. This equa-
       tion includes terms for viscous dissipation and pressure work. The static
       temperature is determined from Eq. 1 shown above.

       _Compressible Liquid

       ...applies to liquid flows which contain pressure wave phenomena as in
       water hammer problems. Remember to set a bulk modulus in the fluid prop-
       erty window for this type of flow.

       _Heat Transfer

       Heat transfer will not be solved for if Adiabatic is picked, and will be
       solved for if Thermal is picked. Selecting Thermal will solve for any con-
       duction, radiation, forced convection, mixed convection, and natural con-
       vection. (For internal radiation, also select Radiation from the Radiation
       group.) Picking Thermal also activates the fields in the Gravitational Vec-
       tor group below. Do not specify a value for gravitational vector if you
       are do not wish to consider buoyancy effects, a good assumption for
       many forced flow problems.

4-10   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

_Gravitational Vector

Assigns values to the three spatial components of gravitational acceleration,
remembering to use units consistent with the geometry and boundary condi-
tions. These values should only be specified, when solving a mixed or natu-
ral convection heat transfer analysis.


Select Radiation to include radiation effects in a heat transfer analysis.
Radiation can only be picked if Thermal is selected as well.

_Special Boundary Conditions
Under this menu, you can set the fan/pump curve data.

COSMOS/Flow User’s Guide • 01/2000                                           4-11
       Chapter 4 The COSMOS/Flow Control File

       _Boundary Conditions_Fan/Pump Curve BC
       To enter the fan or pump
       curve data for this type of
       boundary condition, click
       on Fan Curves .... This
       will open the External
       Fan/Pump Curve Speci-
       fication window.
       In this window, you can
       input a fan or pump curve
       (head-capacity curve) as
       a boundary condition,
       and let COSMOS/Flow
       determine the operating
       point of the system on
       that curve. Multiple fan
       curves are permitted in a
       Recall in Chapter 2 of this guide that you mark a boundary as having a fan
       curve by assigning a:
       Directional Force in the X-direction and a Pressure (COSMOS/Design-
       STAR and COSMOS/Edge). Where the integer value of the Pressure is
       used as the unique Fan Curve ID.

       Force in along plane Dir 1 and a Pres-
       sure (COSMOS/Works). Where the inte-
       ger value of the Pressure is used as the
       unique Fan Curve ID.

       To define a fan curve:
       1 Click on the Add button to create the
           Fan Curve ID.
       2 Click on the Insert Before or Insert
           After buttons to add editable fields.

4-12   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

3 Select the units of Flow Rate and Pressure, and enter the values.
4 Click on the Plot button to check the head/capacity curve.

The points can be entered either in flow rate ascending or descending order,
and to specify that the fan is directing flow out of the domain (a “puller”
fan), use negative values for the flow rates and pressures.

Fluid and solid properties, both constant and variable, are specified from the
COSMOS/Flow_Properties menu selection.

COSMOS/Flow User’s Guide • 01/2000                                        4-13
       Chapter 4 The COSMOS/Flow Control File

       The Fluid Properties window can be accessed by either choosing
       COSMOS/Flow_Properties_Fluid or by clicking on the
       Fl_Prop icon:
       Fluid properties are set in the following dialog box:

       _Fluid ID

       COSMOS/Flow has the ability to analyze multiple fluids. The number of
       the “current” fluid is listed in the Fluid ID box. The “current” fluid is the
       fluid that is being defined in the Fluid Properties window.

4-14   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

For assembly models, each
part (assembly component) is
assigned a material id. To see
the material assignments and
define new material proper-
ties, click the New button.

The Fluid ID number corre-
sponds to the Material Prop-
erty Number (MP) assigned
COSMOS/Works, or COSMOS/Edge to each of the meshed parts in the

✍ Two fluids of different ID numbers can not be in direct contact with
    one another, and must be separated by a solid property type. Two or
    more fluids can be thermally connected by a solid property, however.
    It is possible to have a fluid and a distributed resistance fluid in
    contact, two (or more) different distributed resistance property types
    in contact, or two or more solid property types in contact.

To specify additional Fluid ID’s:
1 Click the New button in the
    Fluid Properties dialog box.
2 From the Pre-processor
    Property Ids drop-down
    menu, select the desired
    assembly component. The id
    of the selected part will
    appear in the New property
    id field.
3 Click OK.
4 In the Fluid Properties dialog box, select a material from the library or
    define the desired material properties of the new material.
5 Repeat steps 1-4 to define other materials if desired.
6 Click OK.

COSMOS/Flow User’s Guide • 01/2000                                     4-15
       Chapter 4 The COSMOS/Flow Control File

       ✍ The Existing Property Ids drop menu lists the Property ID’s that
           have already been defined as a fluid or as a solid (and hence should
           not be used again). Once a Property ID is created as a Fluid ID, that
           property number can not be used as a Solid ID unless it is deleted
           from the Fluid Properties window first. The opposite is true as well:
           once a Property ID is created as a Solid ID, it can not be used as a
           Fluid ID. You can have as many or as few Fluid ID’s as you want.

       To delete unwanted Fluid Property ID’s:
       1 In the Fluid Properties dialog box, select the unwanted Fluid Property
           ID from the Fluid ID drop-down menu.
       2 Click the Delete button.

       ✍ By default, Fluid 1 is active, but the Fluid 1 property ID can be
           removed by clicking the Delete button. You would want to do this if
           you were solving a pure solid conduction model containing no fluids
           at all. The Property ID 1 would then be used as a Solid ID.


       Select a fluid from those available in the pull-down menu at the top of this
       group. In the COSMOS/Flow fluid property database are properties for AIR
       and H2O both constant and variable using the units set defined in the
       Options window. Unless the word “Not_STP”, “Moist” or “Steam/Liquid”
       is part of the name, the properties are evaluated at the equivalent of 1 atmo-
       sphere and 293K.

4-16   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

The data base properties are shown in the following table:

                       Name           Units       Property Formulation

                    User Defined

                        AIR           units             Constant

                        AIR           units            Buoyancy

                        AIR           units              Moist

                        AIR           units            Not_STP

                        H2O           units             Constant

                        H2O           units            Buoyancy

                        H2O           units          Steam/Liquid

                        H2O           units            Not_STP

The distinction between Constant and Buoyancy exists so that COSMOS/
Flow will automatically generate the appropriate settings in the Properties
Specification group (described below). A Buoyancy property formulation
should be selected when Thermal is chosen under COSMOS/Flow_
Options and you want to include buoyancy effects. It should not be chosen
if you only want to consider forced convection effects. The Not_STP selec-
tion is for fluid flow analyses at temperatures and/or pressures far from the
standards. The property variation functional forms for the Not_STP proper-
ties are probably the most representative for a particular fluid.
Note that the reference pressure is automatically updated if a data base
property is selected. If one of the COSMOS/Flow database property selec-
tions is made, then all fields in the Properties Specification group are
made unselectable.
For radiation analyses, enter a value in the Emissivity property window.
For fluid properties, the specified emissivity will be the Emissivity of the
walls surrounding the fluid. If the fluid contacts a solid material property,
the emissivity of that surface will be the emissivity set on the solid property
window for that material. Only the fluid exterior walls use the emissivity set
on this window.

COSMOS/Flow User’s Guide • 01/2000                                         4-17
       Chapter 4 The COSMOS/Flow Control File

       Selecting User_Defined makes all fields in the Properties Specification
       group editable.

       _Length unit

       The length unit is never modifiable on the Fluid Properties window, but is
       displayed for the user’s information. All fluids and solids in an analysis use
       the set of units defined on the Options screen. Properties will be automati-
       cally updated if the units on the Options screen are changed.

       _Reference pressure

       This value is determined by the length unit or can be set using any of the
       following functional forms: Equation of State, Adiabatic Equation of State
       or Steam/Liquid. The default is STP.

       To change the reference pressure:
       1 Make the Name be User_Defined in the drop menu near the top of the
       2 Change the variation on Density to Equation of State or Adiabatic
           Equation of State using the drop menu adjacent to Density.
       3 Change the Reference
           Pressure in the following
       4 Click on OK.
       5 If you want the Density to be
           Constant in the analysis, now
           change the Density variation
           back to constant, and enter
           the correct density value if

4-18   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

_Properties Specification

Changes to the properties specifications may be made only when
User_Defined is selected in the Name menu. For each property, select
either Constant or, for a variable property, one of the available functional
forms. COSMOS/Flow will evaluate the following functional forms for
property variation (not all forms apply to each property):

      Equation of State                            ρ = --------
                                            P                  V
      Adiabatic Equa-                ρ = -------- ,T = T
                                                -                   -
                                                             – ------
                                         RuT             stag 2C
      tion of State

                                           α         T 1.5 T o + S
      Sutherland’s                        ----- ≈  ---- 
                                              -        -                -
                                          α o  T o        T+S

                                                  α         T n
      Power Law                                  ----- ≈  ---- 
                                                     -        -
                                                 α o  T o

                                                                    2         5
     Polynomial                α – α 0 = a0 + a1 T + a2 T + … + a5 T

                                                       a1 a2             a5
     Inverse Polynomial          ( α ⁄ α 0 ) =  a 0 + ---- + ---- + … + ---- 
                                                          -      -          -
                                                       T T2             T

     Piece-Wise Linear         Linear interpolation between input data points

                                                    α        RT
     Arrhenius                                         -
                                                  ------ = e

COSMOS/Flow User’s Guide • 01/2000                                                4-19
       Chapter 4 The COSMOS/Flow Control File

                                                                      µ       p
            Non-Newtonian                                            ---- = γ
            Power Law

            Hershel-Buckley                                     µ = µ o + Kγ

                                                                             (n – 1)
                                    µ – µ∞                         2
            Carreau                ----------------- = [ 1 + ( λγ ) ]
                                   µo – µ ∞

            team/Liquid                                          steam tables

       Variables α and α o represent property values where α o is a reference
       value. R is the gas constant, T is static temperature, E is an activation
       energy and γ is the rate of deformation of the fluid.
       To set the property variations, choose the method from the drop menu adja-
       cent to each property. Click on the property button to bring up the window
       used to specify a constant property value or provide data relating to the
       selected functional form. Examples of the windows are shown below.

       ✍ Ratio Cp/Cv applies only in
           Subsonic Compressible and
           Compressible flows


       To change the value, click on the
       value in the window and type in the
       modified value. Then click on OK.
       Equation of State

       For Equation of State property variations:
         ρ = --------
                    -                                                                        (2-2)

4-20   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

Enter P = Reference Pressure, R
= Gas Constant, and T = Refer-
ence Temperature in the window.
✍ The Reference Temperature
    is only used to calculate an
    initial reference density.
    Therefore, it is only used at
    start-up. The field value of
    temperature is used during the
    calculation cycle. On the
    other hand, the Reference Pressure is used both to calculate an initial
    reference density and is used throughout the calculation cycle to
    determine the absolute pressure. Check the pressure definitions in the
    Technical Reference Guide.

For Adiabatic Equation of State, the window looks the same as the Equa-
tion of State window and the same values need to be input. The Reference
Temperature is again used to calculate the initial reference density. How-
ever, during the calculation cycle, the static temperature used to calculate
density is determined from the local stagnation and dynamic temperatures.
See the Technical Reference for a discussion of Adiabatic Compressible


COSMOS/Flow User’s Guide • 01/2000                                      4-21
       Chapter 4 The COSMOS/Flow Control File

           α         T 1.5 T o + S
          ----- ≈  ---- 
              -        -                -
                           --------------                                       (2-3)
          α o  To         T+S

       Enter a Reference Value (of the property) = α o , the Sutherland con-
       stant=S and a Reference Temperature = To

       ✍ The current reference temperature will be displayed here as the
             default. If you change this value, the reference temperature for the
             problem will also be changed. This is true for all of the property
             functional forms which use a reference temperature. Therefore, if you
             change the reference temperature for, say viscosity, and then change it
             again for conductivity, the reference temperature value for viscosity
             will be different than what was entered during the viscosity editing.

       Power Law

       For the power law variation,

        α         T n
       ----- ≈  ---- 
           -        -
       αo       T o

       enter a Reference Value (of the property) = α o , the Power Law Exponent
       = n, and a Reference Temperature = To. See the note above regarding
       changing the reference temperature.

       Polynomial and Inverse Polynomial

4-22   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

If Polynomial or Inverse polyno-
mial is selected, then data points
must be entered for COSMOS/Flow
to formulate a polynomial or
inverse polynomial expression for
property variation. Density, con-
ductivity, and specific heat can vary
with temperature, pressure, or sca-
lar. Viscosity can vary with temper-
ature, pressure, scalar, and strain
The table shown in the figure is for
entering data points to formulate a
polynomial expression for density
as a function of temperature. When entering data in this table, use the Insert
Before and Insert After buttons. You can delete data rows using the Delete
button. The dependent variable (density, viscosity, conductivity, or specific
heat) is entered in the left column and the dependent variable (temperature,
pressure, or scalar) is entered in the right column.
The polynomial order is specified in the Order field. The polynomial order
should be less than the number of data points to get a good fit. You should
also try to enter a range of values that encompasses the range of the inde-
pendent variable (temperature, pressure, or scalar) of your analysis. COS-
MOS/Flow will automatically clip the property value if it exceeds the upper
and lower values of the independent variable.
For variable properties, it is always a good idea to plot the property values
to see if they follow the expected trends. Polynomial orders greater than 3
are generally not useful. To see the form of the polynomial fit, click on the
Plot button. The following plot shows results from the data entered
above.The plot will show inflection points in the curve fitted to the data.
Note, that in the case shown, the density value is increasing with tempera-
ture at the lower end of the temperature, but decreasing with temperature at
the upper end.

COSMOS/Flow User’s Guide • 01/2000                                        4-23
       Chapter 4 The COSMOS/Flow Control File

       The grid can be displayed by selecting On from the Grid drop menu at the
       top of the window.

       Piecewise Linear

       Unlike the polynomial and inverse
       polynomial functional forms, the
       piecewise linear variation results in
       a linear interpolation between data
       points. Data points are entered in
       the same manner as polynomial
       and inverse polynomial data. The
       key difference is that instead of
       specifying an order of the equation,
       the number of segments is set auto-
       matically, and is one less than the
       number of data points.

       Density, specific heat, and conductivity can be varied with temperature,
       pressure, or scalar. Viscosity can vary with temperature, pressure, scalar,
       and strain rate. The choice of independent variable is made using the drop
       menu (showing Temperature in the above example).

4-24   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

Clicking the Plot
button will pro-
duce a plot of the
data points:

If the data you
are entering is in
form, the data
can be displayed
in logarithmic
form as well by
selecting Log
from the menus
on both axis. Likewise, if the data is in semi-log form, select Log from one
of the axes to plot the data in the appropriate format.


To use the Arrhenius functional form,

    α        RT                                                         (2-4)
  ------ = e

COSMOS/Flow User’s Guide • 01/2000                                      4-25
       Chapter 4 The COSMOS/Flow Control File

       enter a Reference Value (of the property) = αo and the Activation Energy
       = E. The gas constant for the selected length units will automatically be
       selected for use with this functional form.

       Non-Newtonian Power Law

       For the non-Newtonian formula-

          µ       p
         ---- = γ
            -                          (2-5)

       enter the Viscosity Coefficient =
       µ o and the Power Law Exponent
       = p (exponent of 0 equals a New-
       tonian fluid). Note that the vis-
       cosity coefficient becomes the
       viscosity reference value. Non-Newtonian fluids are often described in
       terms of a power law index, n. The quantity to be entered here, the power
       law exponent, is related to the power law index as follows: p = n-1. (A
       power law index of 1 describes a Newtonian fluid.)

       Two other values to specify are: Cutoff Viscosity and Cutoff Strain Rate.
       These two parameters add the capability to model a non-Newtonian fluid
       that has a constant viscosity-strain relationship that starts to vary at a given
       strain rate:

          µ        p
         ---- = kγ                                                                 (2-6)

       If a cutoff is present in the relationship, enter the constant k in the Viscosity
       Coef (k) field.

       If no viscosity cutoff is present, simply enter the Viscosity Coefficient and
       the Power Law exponent and leave the Cutoff Strain rate as the default.
       Enter the value of the Viscosity Coef as the Cutoff Viscosity as well.

4-26   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File


For the Herschel-Buckley varia-
tion of viscosity,

  µ = µ o + Kγ                                          (2-7)

enter the Zero-Strain Value = µ o ,
the Exponent = p, and the Coeffi-
cient = K. Often the power law
index, n, is known. The relation-
ship between the Exponent, p, and
the power law index is: p = n-1.


For the Carreau variation of viscosity,

                                            ( n – 1)
   µ – µ∞                         2
  ----------------- = [ 1 + ( λγ ) ]
                  -                                                       (2-8)
  µ o – µ∞

enter the Zero Strain Viscosity = µ o , the Infinite Strain Viscosity = µ ∞ ,
the Time Constant = λ , and the Power Law Index = n.

COSMOS/Flow User’s Guide • 01/2000                                        4-27
       Chapter 4 The COSMOS/Flow Control File

       User Defined Fluid Property Database

       If User Defined is the name shown in the Fluid Property Name group, then
       the properties shown can be written to a user-customized property database.
       The user-customized database will be stored in the same directory contain-
       ing the current control file. If you want to work in a different directory and
       want to use the database, simply copy the file userfprop.fdb to that direc-

       To enter a property into your own fluid database:
       1 Click on the Add button in the
           Database group:
       2 In the Adding Fluid to
           Database window, enter a
           title that is at least five
           characters long. Comments
           are optional, but are a good
           way to remind yourself of
           what a fluid is later.
       3 Click OK.

       When a fluid is entered into the
       database, it can then be picked
       from the Name menu for subse-
       quent use. If the Analysis Units
       were changed in the
       Options_Analysis Selections
       window, the properties of the user-
       database properties will be converted to match the new set of units.

       To remove a user-defined property from the database:
       1 Pick the fluid to be removed from the Name menu.
       2 Click on the Remove button in the Database group.

4-28   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

Extended Attributes_Resistance

In some fluid flow problems, the actual flow passages may contain a large
number of obstructions. For example in a shell-and-tube heat exchanger,
there may be as many as 50,000 tubes for the shell side fluid to flow around.
To model each and every flow passage would be tedious, expensive and

The flow through this tubed region can be modeled using distributed resis-
tances. In this method, each finite element in this region is assigned a resis-
tance parameter usually based on the free area ratio (proportion of free to
blocked or total area). This resistance simulates the effect of the obstruc-
tions without using an inordinate number of elements. Other examples of
porous media include radiators, vents, screens, filters and packed beds.

Each set of distributed resistance elements has its own property ID number,
and this number cannot be used as solid property ID. This number corre-
sponds to the Material Property ID assigned by COSMOS/DesignSTAR,
COSMOS//Works, or COSMOS/Edge to each meshed part of the assembly.
Distributed resistance elements can have their own unique properties. The
standard Fluid Properties window is used to specify the properties. To dis-
tinguish a property type as distributed resistance, simply check both the
Extended Attribute box and the Resistance Box in the Extended
Attribute group at the top of the Fluid Properties window, as shown

COSMOS/Flow User’s Guide • 01/2000                                         4-29
       Chapter 4 The COSMOS/Flow Control File

        To mark as
        a resistant

       To set the element properties representing the distributed resistances/porous
       media models, click on the Edit button, and use the following window to
       make settings:

4-30   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

There are 3 different ways to model these flow resistances. The first and
most common is the loss coefficient method, where losses through the
media can be written in terms of an additional pressure gradient:

   ∂p            ui
  ------ = K i ρ -----
       -             -                                                     (2-9)
  ∂x i             2

where Ki is the loss coefficient in the global i coordinate direction. Each
global coordinate direction can have its own unique loss coefficient. For the
example of the shell-and-tube heat exchanger, the losses in the direction of
the tube axis will be lower than those in the cross-tube direction. The set-
tings in the above window indicate that a loss coefficient in the x direction
of 0.8 occurs over a 0.25 inch (or whatever length unit) length in the
model. The loss coefficient in the Y and Z directions is considerably larger
than the through flow direction, indicating a much greater loss.

✍ The values for Ly and Lz are again the lengths (element size) over
    which the loss occurs in the model.

Note that the units on the Ki are length-1. Normally, you would find values
for loss coefficient that are unit-less. The equation describing these losses is
written in terms of a pressure drop instead of a pressure gradient:

             u i2
  ∆p = ζ i ρ ----
                -                                                         (2-10)

Values for ζ can be found in many fluids text books and the hydraulic resis-
tance reference, Handbook of Hydraulic Resistance, 3rd Edition by I.E.
Idelchik, published by CRC Press, 1994 (ISBN 0-8493-9908-4). To imple-
ment this type of loss coefficient, enter the value for ζ in the box for K and
the length of the elements over which this resistance acts in the box for L.

This is a good method to use if measured data for pressure drop versus flow
rate is available. You can use the equation for pressure drop shown above:

             u i2
  ∆p = ζ i ρ ----
                -                                                         (2-11)

COSMOS/Flow User’s Guide • 01/2000                                          4-31
       Chapter 4 The COSMOS/Flow Control File

       Substitute in the values for pressure and velocity that you have measured to
       determine a ζ value. Enter this value in the box for K and the length of the
       element region in your analysis model over which the resistance acts in the
       L box.

       If measured data is not available, a good reference for determining ζ values
       is the Handbook of Hydraulic Resistance, 3rd edition by I.E. Idelchik, pub-
       lished by CRC Press, 1994 (ISBN 0-8493-9908-4). This reference lists loss
       coefficients for a wide variety of geometries. To implement them in COS-
       MOS/Flow, enter both the loss coefficient value ζ as K and the length over
       which this loss occurs as L.

       The second method for representing distributed resistance is the friction fac-
       tor method. In this method, the excess pressure drop is written as:

          ∂p         f ui
         ------ = ------ ρ -----
              -        -       -                                               (2-12)
         ∂x i     DH 2

       where f is the friction factor and DH is the hydraulic diameter of the
       obstructions. Both of these values must be provided to COSMOS/Flow. The
       friction factor can be calculated in one of two ways. In the first method, the
       Moody formula for friction factor is used. Here the obstruction roughness
       height must be entered in the correct length units (as set in the Options win-
       dow). In the second method, the friction factor is determined from:

         f = aRe                                                               (2-13)

4-32   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

where Re is the Rey-
nolds number based
on the hydraulic diam-
eter of the obstruction.
If this method is cho-
sen, a and b must be

For this case, the
Resistance Property
window will appear as
shown here

✍ Note that the friction factor is dimensionless but the hydraulic
    diameter should be entered in the correct length units.

The third method for modeling distributed resistances is the Darcy Equa-

  ------ = Cµu i
       -                                                               (2-14)
  ∂x i

where C is the permeability coefficient, µ is the viscosity (the value from
the Fluid Properties window is used) and ui is the velocity in the global i
coordinate direction. To use this form of distributed resistance model, enter
a value for C. Note that the units of viscosity are the same as those for the
fluid properties. The units on C are 1/length2 in the correct length units.

Once all of the properties have been specified, click on the OK button on
the Fluid Properties window.

COSMOS/Flow User’s Guide • 01/2000                                       4-33
       Chapter 4 The COSMOS/Flow Control File

       Internal fans/pumps

       This is a method for you to represent the boost of momentum caused by a
       fan or pump internal to the solution domain. For example, if you were mod-
       eling an electronic enclosure which contained a power supply with its own
       cooling fan, you can include such a fan inside the problem domain as a sep-
       arate part in the assembly. This internal fan or pump is identified using the
       MP number assigned by COSMOS/DesignSTAR, COSMOS//Works, or
       COSMOS/Edge to this part, similar to a distributed resistance area.

       From the Fluid Properties window in COSMOS/Flow,

4-34   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

click on Extended Attributes, and select Internal Fan/Pump. Then, click
on the Edit button, bringing up the Internal Fan/Pump Properties window

On this dialog, choose the Fan Flow Direction either in the Global coordi-
nate system (0) or the specified Local Coordinate System. If the Fan Flow
Direction is not aligned with the global coordinate system, you need to cre-
ate a local coordinate system in Geostar that is aligned with the fan flow
direction, and specify its ID (assigned in Geostar) in the Local Coordinate
System field. Then, specify the Flow Rate and choose the Units (e.g., CFM)
for this flow rate, and the Fan Speed in RPM.


COSMOS/Flow will model the heat transfer in solid materials as well as
fluids. This is called conjugate heat transfer. COSMOS/Flow will recognize
solids during cold flow analyses and not solve for velocities at the solid
material nodes. Each set of solid material elements has its own property id,
corresponding to a property id assigned by COMOS/DesignSTAR, COS-
MOS/Works, or COSMOS/Edge to a meshed part. The solid property ID
numbers have to be unique (different from fluid property ID numbers).

The Solid Properties window is accessible by either picking
COSMOS/Flow_Properties_Solid or by clicking on the Solid

The property values are entered using the Solid Properties dialog box.

COSMOS/Flow User’s Guide • 01/2000                                       4-35
       Chapter 4 The COSMOS/Flow Control File


       Opens the AutoAdd dialog box to let you import material properties defined
       in the preprocessor.

       Begin by entering the property IDs assigned by COSMOS/DesignSTAR,
       COSMOS/Works, or COSMOS/Edge.

4-36   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

To import material sets defined in the pre-processor:
1 Click the AutoAdd button in
    the Solid Properties dialog
    box. The AutoAdd Property
    dialog box opens.
2 From the Property ID to add
  drop-down menu, select All
    to add all material sets
    defined in the preprocessor or
    select an individual
3 Click OK. You will return to the Solid Property dialog box.
4 Click OK.

✍ You can modify the material properties imported from the pre-
    processor but the changes you make in COSMOS/Flow will not be
    reflected in the pre-processor.

To define additional Fluid ID’s:
1 Click the New button in
    the Solid Properties
    dialog box.
2 From the Pre-processor
    Property Ids drop-down
    menu, select the desired
    assembly component. The
    id of the selected part will
    appear in the New
    property id field.
3 Click OK.
4 In the Solid Properties dialog box, select a material from the library or
    select User-Defined and define the desired material properties of the
    new material.
5 Repeat steps 1-4 to define other materials if desired.
6 Click OK.

COSMOS/Flow User’s Guide • 01/2000                                      4-37
       Chapter 4 The COSMOS/Flow Control File

       Once the solid ids have been entered, you can enter new values or edit exist-
       ing values for the properties. Just as in the Properties_Fluid dialog box,
       clicking on the pull-down arrow next to the property shows the various
       functional forms available for representing the material properties. The
       information required for these functional forms is the same as for the fluid
       properties. Thermal material properties defined in the pre-processor will be
       used by COSMOS/Flow.

       ✍ COSMOS/Flow supports orthotropic solid materials. The default is
           isotropic conductivities. These properties can be non-linear depending
           upon the functional form chosen for the property.

       ✍ For steady-state flows, only the conductivity is needed.

       ✍ For radiation heat transfer analyses, an emissivity of the material must
           also be specified.

       A user-customizable solid property data base is available. The use of the
       data base is the same as in the Fluid Properties window. The operation of
       the solid property data base is the same as the fluid property data base. The
       only difference is that you can add solid material property sets automati-
       cally using the AutoAdd button.

4-38   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

The Control section contains two selections: a Convergence Control tool to
improve solution convergence characteristics by adjusting the solution rate
and an Initialization tool.

_Convergence used to set the convergence rate for the solution variables.

Convergence control of a solution variable is accomplished by reducing the
solution progression rate so that the chance of divergence is minimized.
Values can be adjusted by either moving the slider bar toward “Slower” or
“Faster”, or by inputting a value between 0 and 0.5 (or in some cases, 1.0).

COSMOS/Flow User’s Guide • 01/2000                                      4-39
       Chapter 4 The COSMOS/Flow Control File

       ✍ If you specify 0, the degree of freedom will not be allowed to progress
           with the solution at all.

       The default values are the best settings for most analyses. However, solu-
       tion difficulties can often be resolved by reducing the progression rate.
       Lowering the progression

       rate for pressure to 0.1-0.3 is generally the most effective way to minimize
       solution difficulties, particularly if they occur in the early iterations of a cal-
       culation. Reducing the rate on the velocity components, in conjunction with
       pressure, to 0.1-0.3 may be necessary in some cases.

       The progression rate on the variables and properties can be adjusted only if
       it is changing in the analysis. For example, the temperature rate can only be
       adjusted if Thermal is selected on the Options_Analysis Selections win-
       dow. Likewise, the progression rate on the properties Density, Specific heat
       (Cp), and Conductivity can only be adjusted if these properties are variable,
       as set in the Fluid Property window.

       The value you specify is applied to the solution in the following manner:

         φ = rφ ne w + ( 1 – r )φ ol d                                             (2-15)

       where r is the control parameter, φ is the dependent variable, the new sub-
       script refers to the latest solution and the subscript old refers to the previous
       solution. Values greater than 0.5 (default) are not used for most solution

       For compressible analyses, an additional method of control is also avail-
       able: Pressure Control and Temperature Control. (Temperature Control
       is available for incompressible analyses as well.) A value between 1e-3 and
       1e-6 can be selected for these parameters. They are necessary for compress-
       ible analyses because the numerical conditioning for such analyses can
       often be poor. For most compressible analyses, a value of 1e-3 is adequate
       for pressure (and temperature if Thermal is switched on in the
       Options_Analysis Selections window). However, if convergence difficul-
       tites persist, it may be necessary to reduce the value further.

4-40   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

The value set for Pressure and Temperature control is a sort of pseudo-tran-
sient relaxation that is implemented in the solution in the following manner:

         ρ i N dΩ 
   A + ----------------------- φ +
                                                             ρ i N dΩ
                              - i        A i, j φ j = F i + ----------------------- φ i
   i, i ∆t                                                ∆t inertia                      (2-16)
             inertia

This sort of solution control is most often referred to as “inertial relaxation.”

_Initialization used to initialize the
velocity components, tem-
perature and scalar variable.

The velocity components,
temperature and scalar vari-
ables can be initialized
throughout the fluid domain
(on all nodes). Of course,
nodes having boundary con-
ditions will not be affected.
Initialization of pressure and
the turbulence quantities is performed internally by COSMOS/Flow. This is
to ensure that the smoothest possible start-up occurs for a wide range of
CFD problems.

It is a good practice to initialize temperatures in heat transfer problems. This
will shorten the overall time required to achieve a solution.

By checking a box in the Re-initialize column and entering a value in the
appropriate field, the quantity will be reset to the specified value throughout
the entire domain. This is especially handy if after running a flow and ther-
mal calculation, you decide that you want to keep the flow solution, but dis-
card the temperature field. By re-initializing the temperature, you can do
this without having to re-run the flow calculation from scratch. If the Re-
initialize box is not checked, this initialization only takes place at the very
beginning of the analysis (iteration 0).

COSMOS/Flow User’s Guide • 01/2000                                                           4-41
       Chapter 4 The COSMOS/Flow Control File

       Default values for the velocity components and scalar variable are zero; the
       default temperature is 293.

       The COSMOS/Flow_Preferences selection contains various options for
       treating and selection of input/output information. By clicking on the Pref-
       erences menu, you should see the selections available.

4-42   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

_Optional Output_Post-Processing
...allows the user to select which quantities are to be sent to the post-proces-
sor after the analysis is completed. These selections will be used in generat-
ing the output files for CFDisplay and FieldView.

Velocity, pressure, and temperature are on by default. All of the quantities
in a group can be selected at once by clicking on the “All” button, and any
or all of them can be deselected by picking the “None” button in the group.

Note the addition of “Turbulent Intensity”. This is a measure of the effect of
turbulence on the model. Turbulence induced noise is proportional to the
turbulent intensity. See the COSMOS/Flow Technical Reference for a
description of this parameter.

This window is also accessible by picking the Output icon from
the main menu:

COSMOS/Flow User’s Guide • 01/2000                                         4-43
       Chapter 4 The COSMOS/Flow Control File

       _Optional Output_Film Coefficient

       ...turns on the cal-
       culation of film
       coefficients and the
       output of heat flux
       by COSMOS/Flow.

       The film coeffi-
       cients will be cal-
       culated one of two
       ways. The first
       method available is
       to use the energy equation solution in the fluid and calculate the residual
       heat going to the walls which, of course will include the solid/fluid inter-
       face. This method is described in the Technical Reference.

       In the second method, an empirical formulation of the form:

                   a   b
         Nu = cRe Pr                                                            (2-17)

       is used, where Nu is the Nusselt number, Re is the local Reynolds number
       and Pr is the Prandtl number. The fluid flow solution is used to calculate the
       Reynolds and Prandtl numbers. The user can either use the default values
       shown for a b c or select new values. Note that the definition of Reynolds
       number and Nusselt number requires the use of a length constant. If you are
       unsure what to use for these length scales, leave a value of 1.

4-44   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

_Optional Output_Residual Output

...allows nodal residual data associated with
any of the 7 solution variables (u, v, w, P, T, k
and ε ) to be selected for output.

The nodal residual is defined in the Technical

Select the solution variables for which resid-
ual output is desired. Nodal residuals for the
chosen variables are output to the appropriate
post-processing file. Occasionally, it is useful
to plot residuals to identify areas of the finite
element mesh at which solution instabilities or
even divergence occur for a particular vari-
able. Nodal residuals can be post-processed in
By default, there is no residual output.

...selects the pre-processor used to generate the geometry and boundary
condition data. The post-processor is also defined so that the solution can be
written out in the appropriate format.

COSMOS/Flow User’s Guide • 01/2000                                        4-45
       Chapter 4 The COSMOS/Flow Control File


       Choose from available pre-processor interfaces. For all pre-processor selec-
       tions, the COSMOS/Flow <jobName>.gm and <jobName>.bc files are
       generated from the pre-processor analysis model information. Another
       selection available is CFDesignTK which reads 2 generic list-directed for-
       matted files, <jobname>.gmi and <jobname>.bci. For more information
       regarding this format, contact Blue Ridge Numerics Inc. directly. All files
       must have the same path as the control file, <jobName>.ctl.


       Choose from available post-processor file formats. Post-processing files are
       written out in the required format. Choosing CFDisplay will cause the
       results to be written in a format readable by CFDisplay. You can also
       choose to output a Tecplot-readable file or FieldView-readable file for

       _Turbulence used to select the turbulence
       model and to modify the default
       values for the turbulence model
       parameters. This window is only
       selectable if Turbulence is
       selected on the Options_Analysis
       Selections window.

       _Model used to select the turbulence model. The available models include:
       • A constant eddy viscosity model which is less accurate than the other
         two models (except possibly for electronic cooling analyses), but more
         numerically stable. This is a good choice if one of the other two models
         caused divergence.

4-46   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

• The default k-epsilon turbulence model is usually more accurate than the
  constant eddy viscosity, but more computationally intensive and less
• The RNG turbulence model is more computationally intensive, but
  generally more accurate than the k-epsilon model, particularly for
  separated flows. In general, you should start with the k-epsilon model
  and after this model is fairly well converged, turn on the RNG model.

Turb./Laminar Ratio

The Turb./Laminar Ratio is the ratio of the effective viscosity to the lami-
nar value. This is used to estimate the effective viscosity at the beginning of
the turbulent flow analysis. In most turbulent flow analyses, the effective
viscosity is 2-3 orders of magnitude larger than the laminar value. The
default value is generally suitable for most flows.

Turbulence Intensity

The Turbulence Intensity Factor controls the amount of turbulent kinetic
energy in the inlet stream. Its default value is 0.05 and should rarely exceed
0.5. The expression used to calculate turbulent kinetic energy at the inlet,
k in , is:

         1 2 2       2   2
  k in = -- I ( u + v + w )
          -                                                              (2-18)

where I is the Intensity Factor and u, v and w are velocity components.


The Roughness is the average height (in correct length units) of the scale or
roughness from the wall. This value is used for all wall elements. A default
of zero indicates that the walls are smooth.

COSMOS/Flow User’s Guide • 01/2000                                        4-47
       Chapter 4 The COSMOS/Flow Control File

       Auto Startup

       ...activates the COSMOS/Flow Automatic Turbulent Start-Up (ATSU)

       This algorithm goes through a number of steps to obtain turbulent flow
       solutions. The algorithm starts by running 10 iterations using a constant
       eddy viscosity model, so the k and epsilon equations are not solved. With
       this solution as an initial guess, the two-equation turbulence model selected
       by the user is started. So, at iteration 10, a spike in the convergence moni-
       toring data will appear at least for the k and epsilon equations. Other steps
       are then taken to gradually arrive at the converged result. These steps may
       involve spikes in the convergence monitoring data at iterations 10, 20 and
       50 if the On choice is made. After 50 iterations, the ATSU is turned off
       automatically if On is the choice.

       If the Lock On choice is made, the ATSU stays on during the entire analysis
       until the user manually clicks it off. The default is to use On. If there are
       convergence difficulties after iteration 50, then change this selection to
       Lock On. If the ATSU is turned on, you should run at least 200 iterations to
       ensure convergence of the turbulent flow solution. Use the algorithm on any
       turbulent flow problem, particularly when the solution appears unstable in
       the early iterations.

       If Extend is selected, an extended version of the ATSU is put into effect.
       This method is useful for difficult to converge analyses, particularly com-
       pressible analyses. The minimum number of iterations that should be run if
       this algorithm is chosen is 400.


       There are a number of other quantities that can be changed in the turbulence
       model. They are accessible through the Advanced button. All of the param-
       eters listed in this window are described in the COSMOS/Flow Technical
       Reference. The parameters that are most likely to be changed include the
       Turb./Laminar Ratio, Intensity Factor, and Roughness, as shown on the
       Turbulence window.

4-48   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File


...contains all of the settings necessary
to define a transient analysis.

Max Transient Inner Iterations used to set the termination criterion
for the inner iterations during a tran-
sient analysis. Because we use an
implicit method to discretize the tran-
sient terms in the governing equations,
we need to iterate on the solution at
each time step. This inner iteration is
similar to the global iteration per-
formed during steady state calculations. All of the governing equations are
solved at each inner iteration as they are for each global iteration in a steady
state problem. The difference is that far fewer inner iterations are needed in
a transient solution since we are only looking for an approximate solution,
and primarily because the transient equations are much more stable numeri-
cally. Typically, 10-20 inner iterations is sufficient for a transient analysis.
If the convergence monitor indicates that this is not enough (the conver-
gence plot does not decrease to near zero), you can increase this number
preferably only in increments of 10. If the convergence monitor shows that
this is too many inner iterations (plot stays at zero for several iterations),
you can decrease this number.

Results and Summary Output Frequency

...choose how often results and summary information is output to the disk
by COSMOS/Flow. The intermediate summary information is available in
the summary file. The intermediate results files are saved in a form that can
be used either for restarting COSMOS/Flow or creating animation files for
post-processing. Be careful not to ask for so many that you fill your hard
disk. If you are running a transient analysis, the number entered here refers
to time steps.

COSMOS/Flow User’s Guide • 01/2000                                         4-49
       Chapter 4 The COSMOS/Flow Control File

       For steady-state analyses, the number refers to iterations. This is useful for
       saving multiple iterations through the course of a run. Any intermediate
       results file (steady-state or transient) can be used for restart or to create an
       animation file for post-processing.

       Program execution is begun from the COSMOS/Flow_Analyze
       window or simply by picking the Analyze icon:

       The following shows the complete run-time collection of windows:

4-50   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

The Analyze window has been redesigned
from version 3.0, but maintains the same


This group allows you to restart the analysis
from the existing analysis files. The alterna-
tive is to start over from scratch.


Activate the Model Restart by clicking on
the Model box (a check will indicate that it is on). You can and should do
this if the mesh and boundary conditions did not change since the last time
the analysis was started.

Checking the Model restart box causes a <jobName>.gm geometry file and
a <jobName>.bc boundary condition file to be read in. These are binary file
that contain the node, element and boundary condition data read in from

If the flag is checked and no <jobName>.gm <jobName>.bc files exist,
they will automatically be created from the selected pre-processor file

COSMOS/Flow User’s Guide • 01/2000                                      4-51
       Chapter 4 The COSMOS/Flow Control File


       ...when turned ON, the drop-down box next to Starting From will be
       selectable. You can choose which set of results (identified by either the

                       Starting From

       steady-state iteration number (s#) or the transient time step number (t#))
       from which you want to restart. The default will be the last set that was cre-
       ated. Note that all of the intermediate results files saved according to the
       parameters set on the COSMOS/Flow_Preferences_Transient_Output
       Frequency window are included in the list.

       If you restart from a result set other than the last one, all of the sets after the
       one from which you restarted will be deleted from the disk. For example, if
       there were three results sets saved (s100, s75, and s50), and you selected
       s50 to restart from, s75 and s100 would be deleted from your disk and can-
       not be used for subsequent restarts. Before deleting the files, however, a
       window will come up listing the files to be deleted.

4-52   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

This warning will also appear if the Results Restart box is turned off if there
are results sets saved from previous starts. The window that comes up looks

  Results file
  about to be

                                                      Confirm deletion to
                                                      proceed with analysis

If you confirm that those files are to be deleted, the analysis can proceed. If
you click on Cancel, the analysis will not proceed and you will be returned
to the Analyze window.

The restart results capability allows you to run the analysis to get a prelimi-
nary set of results for examining in the post-processor. After checking these
initial or intermediate results, changes can be made to some of the parame-
ters discussed in previous sections and the analysis can then continue. For
example, a turbulent flow problem can be run 100 iterations using the k-
epsilon turbulence model. These results can be plotted to see where separa-
tion and reattachment occur. These results can then be restarted using the
RNG turbulence model and the effect of this turbulence model on separa-
tion can be seen in the post-processor. Restart results can also be used to
start a similar analysis with new boundary conditions.

The “Iterations” box is the number of steady state iterations to be performed
in this analysis.

COSMOS/Flow User’s Guide • 01/2000                                         4-53
       Chapter 4 The COSMOS/Flow Control File


       Begin the fluid flow analysis and saves the <jobName>.ctl file. Note that
       after the analysis is started, this button changes to a Stop button. Clicking
       on the Stop button stops the analysis at the end of the current iteration or
       time steps.

       Because the graphical user interface is multi-threaded, certain items from
       the COSMOS/Flow main menu are still pickable even after the analysis has
       started. It is possible to access and change the Convergence Control set-
       tings as well as the Preferences_Optional Output settings while the analy-
       sis is running. Also note that if the Convergence monitor window is
       obscured by another window or the screen saver, redisplay of the window is
       almost instantaneous.

       In this window, status messages are written out during input processing.
       This information will fill you in as to what is happening between hitting the
       “GO” button and seeing the arrow in the convergence monitor window. The
       information will be available for you to scroll through after the analysis has
       started. Note that summary information regarding model size is now con-
       tained in this window.

4-54   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

Graphical Convergence Monitor
The information that is displayed in the Convergence Monitor are the SUM-
MARY VALUES of the data:

In addition to graphical convergence monitoring, we display the average,
min, and max numerical value of each degree of freedom over the range of
iterations. This way, the user always knows the scale of each curve on the
review axis.

The numerical data that is presented in the Convergence Monitor are the
average, average minimum, and average maximum values for each degree
of freedom over the completed range of iterations. Note that the extrema are
not the true maximum and minimum but rather the average of all of the
maximum and minimum values, respectively.

_CFDisplay Controls
After Go is hit, CFDisplay and the
CFDisplay Controls window will
appear if you are a licensed user of
CFDisplay. Your analysis model
with results will be displayed in the
graphics window, and will be
updated with every iteration or time
step to show the progress of the anal-
ysis. The CFDisplay Controls win-
dow, displayed below,

is used to manipulate the displayed
image and to change the plotted

The display of the model can be moved within the graphics window by
pressing one of the mouse buttons and moving the mouse: Left mouse but-
ton = Pan. Middle mouse button = zoom, and Right mouse button =

COSMOS/Flow User’s Guide • 01/2000                                      4-55
       Chapter 4 The COSMOS/Flow Control File


       Choose which result to display in the graphics window. Only the most basic
       degrees of freedom are selectable in this utility. The items picked in the
       COSMOS/Flow_Preferences_Optional Output_Post Processing win-
       dow will be sent to the post processor after the analysis is completed.


       How the model is displayed is chosen here. If Surfaces are chosen, the
       model will be represented by showing its surfaces with some degree of
       transparency. If Edge is chosen, the lines forming the outline of the model
       will be displayed. The latter pick is most useful for decreasing the display
       time of very large models.


       Choose the method of results display. Vectors and/or Contours can be cho-
       sen. If vectors are chosen in a three dimensional model, the vectors will be
       displayed on a cutting plane. If a two dimensional model is running, all of
       the vectors will be displayed. The vectors will be scaled according to the
       largest vector in the analysis domain. For this reason, displayed vectors may
       seem to change size as the analysis is running, particularly in the early itera-


       This drop menu contains different viewing positions. Picking one of these
       viewing positions aligns the model with a Cartesian axis, making viewing
       easier. The Reset View button changes the viewing position back to default
       and centers the model in the graphics window.

       CFDisplay Active

       The CFDisplay graphics window is updated after each iteration. This can
       cause the analysis to slow down especially for large models. To speed up
       the calculation, you can turn off this update (for example, for overnight
       runs). If the box is checked, the window will be updated. If it is unchecked,
       the CFDisplay update will be skipped.

4-56   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

_Cutting Plane

The Orientation and the Position of the cutting plane are chosen here. The
slider bar can be used to sweep the cutting plane across the model to give
you a quick idea of the trends throughout the analysis model. The orienta-
tion of the plane can be changed to be parallel to any of the Cartesian planes
(x, y, or z). The Visible switch governs the display of contours on the cut-
ting plane.

To display contours only on a cutting plane: In the Display group, make
sure only Contour is checked. In the Cutting Plane group, make sure Visi-
ble is checked. The cutting plane will be displayed as a contour. Change the
location of the plane by moving the slide bar. Change the orientation of the
plane by selecting the Y direction.

To display only vectors on a cutting plane: In the Display group, check
Vectors. In the Cutting Plane group, uncheck Visible. The location and
orientation of the cutting plane can be adjusted as you like.

Other commands

During the analysis, you can activate other
CFDisplay commands by holding the Control
key down and doing a right mouse click in the
CFDisplay window. When you do this, you
will see a small menu pop up:

COSMOS/Flow User’s Guide • 01/2000                                        4-57
       Chapter 4 The COSMOS/Flow Control File

       Clicking the top item will bring up the Info window:

       There are a number of tabs on this window. Perhaps one of the most useful
       is the Polygon tab. If you click this tab, you will see information about the
       currently selected polygon. To select a polygon, hold the Control key down
       and click the left mouse button somewhere on the cutting plane. You will
       see the window will get updated information about the polygon just
       selected. The top window shows the node Id’s and the global coordinates of
       the selected polygon. The bottom window shows the selected results for the
       nodes on this polygon. In the figure, Pressure was selected in the Results
       window. So, the Scalar column shows the pressure values at the nodes on
       this polygon. The Vector columns are always the velocity vector results.
       You can use this window to query local results in the model.

4-58   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

The polygons that you select with the <Ctl> left mouse button are always on
the cutting plane. So you can position the cutting plane in the area of the
model to be queried and begin selecting.

If you click on the Element tab, the same information as for the Polygon is
now displayed for the entire element.

If you click on the Results tab, you will see the minimum/maximum for the
selected scalar results (Pressure in the example above) over the entire
model. You also get the minimum/maximum for the velocity vector.

Another useful tool in the special commands
popup menu:

is the Change Part Attributes. If you click
this selection, the Change Part Attributes
window will open:

All of the surface elements in the model have been typed by COSMOS/
Flow. We group these elements by contiguous elements with the same type
and that is classified as a separate CFDisplay “Part”. For example, all of the
wall element faces that touch in your model (say the outer skin) will be
typed as a single part. In the poppet valve model above, Part 2 contains all
of the outlet elements.

COSMOS/Flow User’s Guide • 01/2000                                        4-59
       Chapter 4 The COSMOS/Flow Control File

       Under Draw Style, you can change how that part is drawn. In the example,
       only the Outline is drawn. You might try clicking on Surface. Then, you
       should see the entire surface drawn with the Results selected (VMag, for
       example) contours on that surface.

       In the Part Attributes group, you can choose to make this part invisible or
       Visible. You can display the Shaded part, Fringe contours, Vector arrows,
       the Mesh or the mesh on the surface (Outline mesh). You can also change
       make the part Transparent. If you click on the Transparent box, you can
       change the transparency and a whole lot of other stuff by clicking on the
       Material button on the right.

       You should try out some of these buttons to see what happens. One note is
       that nothing will happen until you click on the Apply button. So, you can
       make all of your selections and then click on the Apply button to see the
       results of your selections. This feature is particularly useful for models cre-
       ated from assemblies where each part of the assembly will be a separate part
       in CFDisplay.

       The final command on the special commands popup menu:

       is to the ability to change the Rotation Point in the model. If you click on
       this selection, you will see the Rotation popup window:

4-60   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

In the figure above, we have already clicked on the Show option. CFDis-
play has drawn the 6-pointed star to indicate the location of the center of
rotation for the part. We can change this center of rotation to say be on the
Selected Part. In the example above, the rotation point would be moved to
the outlet face. The ability to move the rotation point around makes viewing
results easier.

After the analysis is finished, there are other options available on this spe-
cial window. You should try some of these to make the display more useful
to you.

COSMOS/Flow User’s Guide • 01/2000                                        4-61
       Chapter 4 The COSMOS/Flow Control File

       This group of commands access selected analysis output files for review:


       This item displays plots of the residual norm and summary plots.
       The window is also accessible by picking on the Check icon:

       There are two criteria which should be used to determine conver-
       gence, each exhibited in the two plots below. The first is that the residual
       norm data for all solution variable should not be changing as iterations
       elapse. Similarly, the second criterion requires that the average, minimum
       and maximum nodal values of the solution variables not change as iterations
       elapse. The solution exhibited below is converged.

4-62   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

To plot the convergence and summary data for individual variables:
Select the appropriate variable in the pop-down menu at the upper left of
each plot. When you do this, the Min and the Max value will be written in
the Min and Max fields at the top of each plot.

To plot average, maximum, and minimum nodal values in the summary
plot: Pick the desired quantity from the menu at the right of the window.

To plot the values for a selected range of iterations: Click in the Start
and End boxes and replace the numbers there. After each number is
changed, hit the Enter key to produce the plot for that range of iterations.

To close the window: Click on the OK button.

COSMOS/Flow User’s Guide • 01/2000                                        4-63
       Chapter 4 The COSMOS/Flow Control File


       ...loads the status file,

       <jobName>.st, for review. This file contains any error messages that may
       occur during a program run. The file also lists the files used for the analysis
       as well as general information indicating the operations performed.

4-64   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File


Last Run

This loads the most recent summary file, <jobName>.sum, for review. This
file contains calculation units, tabulated minimum, maximum, and average
nodal values for selected variables. It also contains global summary calcula-
tions such as mass flow through inlet and outlet passages, bulk pressures
and temperatures, Reynolds number, wall heat transfer, a global energy bal-
ance and the fluid forces. The end of the file also contains the CPU and
memory statistics such as analysis times and the amount of RAM used in
the analysis.

✍ You should use the same unit system that you have used in COSMOS/
    DesignSTAR, COSMOS/Edge, or COSMOS/Works. If you try to
    select a different unit system from the drop-down menu, you will get a
    warning message.

COSMOS/Flow User’s Guide • 01/2000                                      4-65
       Chapter 4 The COSMOS/Flow Control File

       Run History

       ...loads the summary history <jobName>.shs, for review. This is a collec-
       tion of all of the summary files created with this jobname. Each time you
       restart a run, a new summary file is added to this file. This file allows to
       track the progress of your mass balance, for example.

       ...allows you to perform special operations on the COSMOS/Flow results.

4-66   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

Create Animated Results

...can be used to create the animation file for post-processing using the
stored intermediate results files or time steps.

The saved results files appear in the left window marked Available Results.
The results are listed according to how many iterations (steady-state runs,
marked with an “s” in parentheses) or time steps (transient runs, marked
with a “t”) are contained in the result file. The frequency of the iterations or
time steps that are available is determined by the Results Output Fre-
quency. Results sets have to be moved into the Animated Results window
to be animated.

There are three ways to select results to be animated:
1 The first method is to select a result and click on the arrow button.
    Using this method, each result is moved into the Animated Results
    window individually. This method can be used to deselect results sets as
    well (move them from Animated Results back to Available Results.)
2 The second method is to click on the Move All button. All of the results
    will be moved into the Animated Results window. To deselect all of
    the results, click on the Move All button under Animated Results.

COSMOS/Flow User’s Guide • 01/2000                                          4-67
       Chapter 4 The COSMOS/Flow Control File

       3 The third method is to use the Parametric Selection of Available
           Results utility. Every result set has a bracketed number assigned to it.
           This number indicates its order in the Available Results list. Enter a
           From, To, and Increment value to move as many or as few results sets
           as you want. The From and To numbers refer to the bracketed numbers
           and not the iteration or time step numbers.

       After you have selected all of the results that you want to include in the ani-
       mation file, click on OK. This will over-write the current post-processing
       file with the animation file.

       Post Process

       ...starts CFDisplay, the COSMOS/Flow post processor. A
       reduced-functionality version of CFDisplay serves as the run-
       time results monitor, but when COSMOS/
       Flow_Review_Results_Post Process or the Results icon is selected the full
       version of CFDisplay is started. The Analyze window does not have to be
       closed before starting CFDisplay.

       If animation results were created, a
       dialog box will pop up when the
       Results icon is clicked asking if you
       want to post process Single Iter/
       Time Step or Animated Iter/Time
       Steps. If you pick Single Iter/Time
       Step, the last saved result set will be
       sent to CFDisplay, and only that
       result set can be post-processed. If
       Animated Iter/Time Steps is
       selected, the animation set created
       containing the results to be animated will be sent to CFDisplay. The anima-
       tion set can contain either transient time steps or steady state iterations.

4-68   COSMOS/Flow User’s Guide • 01/2000
Chapter 4 The COSMOS/Flow Control File

The COSMOS/Flow Help System under COSMOS/Flow_Help is orga-
nized to access information about selections in the COSMOS/Flow pull-
down menus and windows. Also, under _onHelp, _General and
_TroubleShoot, an overview of the help system usage mechanics, general
information about COSMOS/Flow, and techniques for troubleshooting an
analysis may be found.

COSMOS/Flow User’s Guide • 01/2000                                 4-69
       Chapter 4 The COSMOS/Flow Control File

4-70   COSMOS/Flow User’s Guide • 01/2000
5             Analysis Guidelines

    The purpose of this chapter is to offer tips and suggestions for a number of
    different types of flow analyses. While the previous chapters in this Guide
    discussed the general operation of the code, this chapter discusses some of
    the details of specific flow environments. The suggestions offered in this
    chapter should be used in conjunction with the example problems in the
    Tutorial Manual. The following analysis types are discussed in this chapter:
            • Internal and external incompressible flows
            • Heat transfer (conduction and convection)
            • Porous Media
            • Multiple fluids
            • Internal fans/pumps
            • Fan/pump curves
            • Boundary layer flows
            • Radiation heat transfer
            • Internal and external compressible flow

    The final section discusses troubleshooting procedures.

    COSMOS/Flow User’s Guide • 01/2000                                       5-1
      Chapter 5 Analysis Guidelines

      Incompressible Flows
      Internal Flow

      Internal flow is a very general category which describes any fluid that is
      contained by and passes through a solid structure. There may be one or sev-
      eral inlet/outlet passages through which fluid enters and leaves the solution
      domain. The solutions to internal flow problems are among the most diffi-
      cult to achieve in CFD, particular for turbulent and, even more so, for com-
      pressible flows. The reason is that the final solution may exhibit widely
      varying mathematical characteristics in a single domain.

      COSMOS/Flow has several tools to aid convergence for a wide range of
      internal flow problems. The most powerful is the Automatic Turbulent
      Start-Up algorithm previously described. This algorithm is on by default,
      and will often prevent solution instability or divergence, particularly in the
      early iterations. Other troubleshooting techniques are described in a later
      section of this chapter

      Boundary Condition Specification

      There are many different types of boundary condition specifications for
      internal flows. Regions where problems arise most commonly are at inlet/
      outlet passages.

      Important Notes
      • First, when using the k-epsilon turbulence model (the default) there be at
        least five elements across inlet and outlet passages so that the gradients
        there can be properly resolved.
      • Second, it is good practice to refine the mesh toward the inlets so that the
        boundary conditions will correctly affect the interior of the domain.
      • Third, at the outlet (specified pressure boundary), where a uniform
        pressure is commonly applied, there must not be any flow features which
        will conflict with this uniform pressure boundary. The aim should be to
        have velocity vectors at nodes on the specified pressure boundary be
        approximately normal to the plane of this boundary. Sometimes the
        boundary must be extended to achieve this effect.

5-2   COSMOS/Flow User’s Guide • 01/2000
Chapter 5 Analysis Guidelines

The following figure illustrates these concepts.

For incompressible flows, pressure is commonly specified at the outlet and
either velocity or pressure (not both) is specified at the inlet. When specify-
ing velocity or pressure, all nodes on the inlet/outlet surface or edge must be
included. The Automatic Wall Specification Algorithm will internally
determine and adjust the condition at nodes at the interface of a wall and a
flow boundary.

For flow situations in which a small jet is blowing into a large room, it has
been found to be helpful to change the Turb/Lam Ratio to 1000 or greater
(the default is 100). This can be found under Preferences_Turbulence.

External Flows

External flows are characterized by a solid body immersed in fluid that is
moving relative to the body. Nearly all aerodynamic problems in engineer-
ing design are external flows, e.g. noise generated by a car mirror at high-
way speeds. These problems generally require the greatest number of nodes
of any CFD calculation since the velocity and pressure boundary conditions
applied at the exterior of the flow domain must not affect flow features
around the immersed body. Generally, the exterior or “far-field” boundary
must be located 50-200 times the longest chord of the immersed body.
Higher Reynolds number flows will require far-field distances in the upper
portion of this range.

COSMOS/Flow User’s Guide • 01/2000                                          5-3
      Chapter 5 Analysis Guidelines

      It is important to transition the element sizes in the mesh quite substantially
      to conserve nodes. It is common for elements on the body surface to be sev-
      eral thousand times smaller than elements at the far-field. Lift and drag
      forces calculated by COSMOS/Flow will be dependent upon the mesh size
      near the body. Transitioning must be smooth for solution stability and accu-
      racy, as described in chapter 3, and care must be taken to prevent elements
      from having aspect ratios much greater than 500:1 and these only at the far-
      field boundary.

      Boundary Condition Specification

      For incompressible and
      subsonic compressible
      flow problems with sub-
      sonic inlets, velocity and
      pressure boundary condi-
      tions must not be applied
      to the same node. They
      will, however, be applied
      at adjacent nodes on the
      far-field boundary as
      shown in the following
      figure. To aid conver-
      gence, it is useful to spec-
      ify the velocity boundary condition around a greater portion of the flow
      domain than for pressure, as shown in the following figure:

5-4   COSMOS/Flow User’s Guide • 01/2000
Chapter 5 Analysis Guidelines

Basic Heat Transfer
This section discusses conduction and the different varieties of convection.
Radiation is discussed in a later section.

There are several variations of heat transfer analyses that can be performed
using COSMOS/Flow. They include: conduction, natural convection,
forced convection and mixed convection. Some of these can occur together
in the same analysis. For example, conjugate heat transfer includes both
fluid convection and solid conduction. The following discussions offer
some hints on performing each of these types of heat transfer analysis.

You can do a conduction heat transfer analysis with COSMOS/Flow on
either fluid or solid material elements. In either case, the correct properties
should be set (thermal conductivity). If the analysis is done on the solid
material, you should be sure to add the solid material property number to
the Properties_Solid window. Whether using a solid or a fluid material, you
should turn Flow to No Flow and Heat Transfer to Thermal on the
Options window. If the material properties are constant, you should only
need 1 or 2 global iterations on the Analyze window. To be safe, you can set
the number of iterations to 2 or 3.

Natural Convection

Natural and free convection flows are largely dominated by buoyancy
forces. The buoyancy forces are generated by density gradients which vary
primarily with temperature since pressure gradients are relatively small in
these flows. Natural convection flows may be laminar or turbulent depend-
ing on the Grashof number associated with the flow. The Grashof number is
defined as

       gβL ∆T
  Gr = -------------------
                         -                                                (4-1)

COSMOS/Flow User’s Guide • 01/2000                                          5-5
      Chapter 5 Analysis Guidelines

      where g is the local acceleration of gravity, β is the thermal coefficient of
      volume expansion, L is a characteristic length of the surface in the direction
      of gravitational acceleration, ∆T is the temperature difference between the
      heated surface and the undisturbed fluid and ν is the kinematic viscosity.
      The Grashof number is a measure of the ratio of net buoyancy forces to vis-
      cous forces. Transition to turbulence occurs at around Gr ≈ 4 × 10 8 .

      Some prefer to use the Rayleigh number to characterize the flow. The Ray-
      leigh number is the product of the Grashof and Prandtl numbers, the latter
      being defined as

             µC p
        Pr = ---------                                                             (4-2)

      For most gas flows, Pr ≈ 1 .

      Boundary condition specification is generally straightforward for mixed or
      enclosed natural convection flows. For free convection flows (where the
      fluid can be drawn in or expelled from the domain), apply constant pressure
      to all openings in the domain. One suggestion with regard to constructing
      the mesh is that, in most cases, more elements will be required in the inte-
      rior of the domain (away from the solid boundaries) than for a pressure
      driven flow. The reason is that accurate representation of the small density
      gradients is critical to computing the driving buoyancy forces correctly.

      The number of iterations required, and hence the total solution time, will be
      greater for a natural convection than for a pressure-driven flow analyses.
      Solution progression is slowed by the fact that buoyancy forces are gener-
      ally significantly larger than pressure forces.

      In the COSMOS/Flow_Options_Analysis Selections window, be sure to
      set Heat Transfer to Thermal and to set a gravity vector in the analysis
      units. Be sure to select a property with Buoyancy on the Fluid Property
      window or select Equation of State as the variation for density. In the
      COSMOS/Flow_Preferences_Turbulence window, it may be necessary
      to set the Turb/Lam Ratio to a higher value, at least 2-5 times the default.
      It is also helpful to initialize the temperature field to a value close to what is
      expected. Do this by picking COSMOS/Flow_Control_Initialization and
      entering an appropriate value.

5-6   COSMOS/Flow User’s Guide • 01/2000
Chapter 5 Analysis Guidelines

Forced Convection

If the heated or cooled air is being blown (by a fan, for example) through
the solution domain, this is usually forced convection. In forced convection
heat transfer, the temperature does not influence the fluid material proper-
ties. For this reason, the energy equation can and should be solved alone
(Flow is Off on the Options window) after the flow solution (velocity,
pressure) has converged. As with the conduction heat transfer analyses,
you probably only need 1 iteration to converge on temperature. To be safe,
you should set the number of iterations to 2 or 3.

Note that you should not specify a gravity vector for forced convection
analyses (leave the component values at 0).

Mixed Convection

In some heat transfer analyses, the heated or cooled air is blown but may
contain local temperature gradients that will cause some appreciable buoy-
ancy effects. This type of heat transfer is known as mixed convection, since
it has features of both natural and forced convection. There is not a good
way to tell apriori if the heat transfer is mixed or just forced. To check, you
should run a mixed convection analysis after the forced convection analysis
is finished. The steps required are:
1 Get a converged flow solution with Thermal set to Off on the Options
    window and constant fluid properties on the Properties_Fluid window.
2 Turn off the Flow and turn Heat Transfer to Thermal on the Options
    window and run <5 iterations.
3 Set Flow to Internal Flow, keep Heat Transfer on Thermal and set
    the gravitational acceleration vector on the Options window. Select a
    fluid property with Buoyancy in its name from the fluid property data
    base or choose Equation of State for the functional form for density .
    For the latter, set the appropriate parameters for this functional form.
4 Run 25-50 more iterations and examine the results for changes.

COSMOS/Flow User’s Guide • 01/2000                                          5-7
      Chapter 5 Analysis Guidelines

      Many electronic cooling applications are in the mixed convection regime.
      The above steps are recommended for these analyses. Temperature results
      should be reviewed carefully after step 2 to ensure that unrealistic tempera-
      tures have not been predicted. This is generally an indication that buoyancy
      effects are significant. In this case, continue on to step 3, BUT choose the
      previous iteration from the Starting At menu on the Analyze window to start
      the thermal solution from a constant temperature field instead of the unreal-
      istic values.

      Conjugate Heat Transfer
      For conjuagate heat transfer analyses, the solid material conduction and the
      fluid convection are analyzed simultaneously. For this type of analysis, the
      type of fluid convection: natural, forced or mixed determines the analysis
      parameters. If the fluid convection is forced, you should again get a con-
      verged flow solution and then run the forced convection analysis with the
      flow turned off for a few more iterations. If the fluid convection is natural
      convection, you need to run the thermal equation analysis with the flow
      turned on for all iterations. For mixed fluid convection, follow the steps out-
      lined above.

      Porous Media Flows
      For fluid flow analyses that include a great many flow obstacles, you should
      consider using porous media elements to represent these obstacles. This
      eliminates the need to model each obstacle with enough finite elements to
      adequately resolve the flow around or through each obstacle.

      To use porous media or distributed resistance elements, identify or select
      the region with the obstacles and assign a unique Material Property ID (MP)
      in Geostar. Then, enter the resistance parameters in the Resistance window
      under the Fluid Properties window. Distributed resistance elements can
      have physical properties that are different from the surrounding fluid. Typi-
      cally, you would want to change only the thermal conductivity of distrib-
      uted resistance elements. An example of such a situation would be if you
      were modeling flow through a porous ceramic filter. The ceramic material
      would have a different conductivity from that of the surrounding fluid, and
      that can now be represented.

5-8   COSMOS/Flow User’s Guide • 01/2000
Chapter 5 Analysis Guidelines

There are 3 ways to enter flow resistances for these obstacles:

K-factor approach

A good reference for calculating or estimating K-factors is: Handbook of
Hydraulic Resistance, 3rd edition by I.E. Idelchik, published by CRC Press,
1994 (ISBN 0-8493-9908-4). To use this data, enter the value of the loss
coefficient as K, and the length of the element region over which it acts in
the model as L.

If measured data for pressure drop versus flow rate is available, this can be
used to calculate the K-factor. This is done using the following equation:
                                 ∆P = ζ i ρ ----
                                               -                         (4- 3)

If you know the pressure drop, the velocity, and the density, you can back
out the value of ζ . Enter this value for K, and the length of the element
region over which it acts IN THE MODEL as the value for L.

Often, as in the case of a mesh filter for example, the loss in one direction
will be significantly less than the loss in the other two directions. In such a
situation, enter the calculated or estimated loss coefficient for the through
flow direction and some value 3 or 4 orders of magnitude in the cross direc-
tions. This will allow the flow to go in the desired direction, and impede it
in the other directions.

Friction Factor Approach
In this method, the pressure drop is written as:
                                 ∂p         f ui
                                ------ = ------ ρ ----
                                     -        - -                        (4- 4)
                                ∂x i     DH 2

where f is the friction factor and DH is the hydraulic diameter of the
obstructions. Both of these values must be provided to COSMOS/Flow

COSMOS/Flow User’s Guide • 01/2000                                         5-9
       Chapter 5 Analysis Guidelines

       Solver. The friction factor can be calculated in one of two ways. In the first
       method, the Moody formula is used. Here the obstruction roughness height
       must be entered in the correct length units. In the second method, the fric-
       tion factor is determined from:

                                       f = aRe                                  (4- 5)

       where Re is the Reynolds number based on the hydraulic diameter of the
       obstruction. If this method is chosen, a and b must be entered. For this case,
       note that the friction factor is dimensionless but the hydraulic diameter
       should be entered in the correct length units.

       Darcy Equation Approach

       The Darcy equation:

                                       ------ = Cµu i                           (4- 6)
                                       ∂x i

       where C is the permeability coefficient, µ is the viscosity (as set in the
       Fluid Properties window), and u is the velocity. Enter a value for C. The
       units of C are 1/length^2 in the correct units.

       Multiple Fluids
       COSMOS/Flow has the ability to handle multiple fluids in one model. Note
       that fluids with different property numbers cannot come in physical contact
       with each other unless one or more is a distributed resistance. Non-distrib-
       uted resistance fluids can however be connected thermally (separated by a
       solid material).

       To implement multiple fluids into an analysis, each fluid must have its own
       unique Material Property ID (MP) number. Each fluid is defined on its own
       Fluid Property window in COSMOS/Flow Solver.

5-10   COSMOS/Flow User’s Guide • 01/2000
Chapter 5 Analysis Guidelines

To add property ID’s, click on the New button. Once a property ID is cre-
ated, it cannot be used for another property (either fluid or solid) unless that
ID is deleted.

Examples of types of analyses where this functionality might be useful are
an air-water heat exchanger or flow blown over a sealed electronics compo-
nent box. In the latter example, natural convection might be important
inside the sealed box, and forced convection may play a role outside the

Note that a pressure boundary condition must be set in all fluid regions. For
a totally enclosed area with no inlets or outlets, it is a good idea to specify
the pressure on at least one node somewhere in the enclosure. This will
decrease the analysis time significantly.

Internal Fans/Pumps
For fluid flow analyses that include some sort of momentum source like a
fan or a pump or an actuator, you can use the internal fan/pump feature in
COSMOS/Flow to represent these sources. This eliminates the need to cut
out these areas and apply boundary conditions to them.

To use internal fans/pumps, identify or select the region with the source and
make this a separate part in SolidWorks so that Cosmos/Works will assign a
unique Material Property ID (MP). If the axis of the fan is not lined up with
the global coordinate system, you should define a local coordinate system
which is lined up with the fan. When you enter the internal fan/pump data
on the COSMOS/Flow windw, use the local coordinate system and identify
the direction in this system of positive flow.

You can analyze completely closed loops with an internal fan or pump to
generate the flow. However, for problems with internal fans and pumps that
have unknown openings, i.e., flow could be sucked in or blown out, you
should use specified total pressure boundary conditions on these openings.
This will bound the problem, while specifying static pressure at these open-
ings will not bound the solution.

COSMOS/Flow User’s Guide • 01/2000                                          5-11
       Chapter 5 Analysis Guidelines

       Fan/Pump Curves
       You can use a fan curve or a pump head-capacity curve as a boundary con-
       dition in COSMOS/Flow. You need only identify the boundary as such in
       Cosmos/Works. See Chapter 2 of this guide to see the mapping of the Cos-
       mos/Works boundary condition for fan curve boundary conditions. To
       model a pushing fan, enter the data as positive flow rates and positive pres-
       sure heads. The data can be entered in any order, but it may be more read-
       able to you if you enter it in the same order as the manufacturer presents it.
       To model pulling or sucking fans, enter both the flow rate and the pressure
       head as negative numbers.

       For problems with fan/pump curve boundaries and that have unknown
       openings, i.e., flow could be sucked in or blown out, you should use speci-
       fied total pressure boundary conditions on these openings. This will bound
       the problem, while specifying static pressure at these openings will not
       bound the solution.

       Boundary Layer Flows
       Boundary layers flows are performed in a fashion similar to external flows
       with one important exception. Since the pressure field is generally uniform
       throughout the domain in these types of flows, the nodal pressures must be
       initialized to the same value (usually zero) and not updated during the cal-
       culation. The solution relaxation for pressure must be set to zero to maintain
       the initial pressure field.
                                       ∂P ∂P          ∂P
       Note that there will be finite ------ , ------ and ------ terms in the governing flow
                                      ∂x ∂y               ∂z
       equations since “intermediate” pressures are used in their computation.
       “Intermediate” refers to a point in the middle of a sequential solver iteration
       when pressure gradients are established to conserve mass. At the end of
       each sequential solver iteration, these pressure gradients will not be present
       since pressure relaxation is set to zero.

5-12   COSMOS/Flow User’s Guide • 01/2000
Chapter 5 Analysis Guidelines

To use radiation, simply select Radiation from the Options window and
specify an emissivity for every solid material type in the model. If there are
no solids present, specify an emissivity for the surrounding walls. This
emissivity is specified in the Fluid Properties window. The radiation algo-
rithm does not allow the fluid medium to participate, so the emissivity spec-
ified in the Fluid Properties window is really that of the exterior walls
touching the fluid.

Radiation can be run with or without flow, but should be run with Heat
Transfer set to Thermal.

Note that for large models, the start up time can be somewhat longer
because the program has to calculate view factors for every element. Note
also that radiation does not currently work for axisymmetric or symmetric
2D and 3D geometries. It does however work for full 2D planar and full 3D

Compressible Flows
In “Compressible” flow, density varies with pressure. In COSMOS/Flow,
we distinguish between Subsonic Compressible flow where the pressure-
density affects are weak and Compressible flow where the pressure
strongly affects the density. Subsonic Compressible contains no shocks.
The local Mach number is always less than 1.0. Compressible flow may
have shocks and contains regions where the local Mach number is greater
than 1.0. This type of flow may be either transonic or supersonic. In super-
sonic flows, pressure effects are transported downstream. The upstream
flow is not affected by downstream conditions. The mathematical implica-
tions of compressible flow is that downstream boundary conditions should
not be fixed. In this case, the downstream boundary should be set either
using the Unknown or the Total Pressure boundary condition. The
unknown condition will allow the static pressure value to float; its only con-
straint is continuity. The total pressure condition also allows the static pres-
sure to float but maintains both a continuity and a momentum constraint.

COSMOS/Flow User’s Guide • 01/2000                                         5-13
       Chapter 5 Analysis Guidelines

       If you switch from a Compressible flow to an Incompressible flow on the
       COSMOS/Flow_Options_Analysis Selections window, you should
       remember to reset the density functional form on the COSMOS/
       Flow_Properties_Fluid window. It is automatically changed to Equation
       of State for Compressible and Subsonic Compressible flows.

       For subsonic compressible and full compressible problems with Heat
       Transfer set to Adiabatic in the Options window, it is necessary to specify
       a stagnation temperature in the Options window. The equation to determine
       the stagnation temperature is:

                                       T t = T + --------                       (4- 7)
                                                 2C p


                                                γ–1 2
                                  T t = T  1 + ---------- M 
                                                   2                          (4- 8)

       To include heat transfer in a compressible analysis, set Heat Transfer to
       Thermal in the Options window. Temperatures set in Geostar are always
       TOTAL (STAGNATION) temperatures for compressible analyses so a
       stagnation temperature does not have to be set in the Options window. Note
       that when heat transfer is present in a compressible analysis, viscous dissi-
       pation, pressure work, and kinetic energy terms are solved for. It is only
       necessary to set Thermal if you are solving for heat transfer or for Mach
       numbers greater than 3. The latter condition is applicable only if viscous
       dissipation is important.

       Internal Flow
       The practices outlined in the Incompressible flow section about internal
       flow modeling should be followed for compressible flows as well, with the
       important exception of the boundary conditions.

       For compressible flows, if the inlet is supersonic, either the total pressure
       and the velocity or the static pressure and velocity must be specified at the

5-14   COSMOS/Flow User’s Guide • 01/2000
Chapter 5 Analysis Guidelines

inlet because pressure signals only travel downstream in a supersonic flow.
Usually, you do not want to specify the outlet static pressure for compress-
ible flows for the same reason. You can however use the unknown or speci-
fied total pressure boundary condition at the outlet.

There are situations, however, in which the inlet and/or the outlet may be
subsonic, while flow within the domain goes supersonic. For a subsonic
inlet that is well below sonic, it is a good idea to specify only velocity. For a
subsonic inlet that is near sonic, both velocity and pressure can be specified.
If the outlet is very far downstream of supersonic flow, you should specify a
total pressure. In some instances it is possible to add an extension on the
exit to be able to set a uniform static pressure at the domain exit. If such an
extension is used, it is good practice to set the slip condition on the walls of
the extension to prevent any Fanno flow effects. If, however, the outlet is
fairly close to supersonic flow, you should set either the total pressure or the
unknown boundary condition.

External Flow

Please refer to the general information about external flows in the Incom-
pressible flow section of this chapter. The key difference between incom-
pressible and compressible external flow modeling is the boundary
conditions. In supersonic flows, you should specify both pressure (static or
total) and velocity upstream of the object. Downstream of the object you
should set either the total pressure or the unknown boundary condition. An
example of this looks like:

COSMOS/Flow User’s Guide • 01/2000                                           5-15
       Chapter 5 Analysis Guidelines

       ✍ If the domain is not adequately large, you may have to make the inlet
           condition (velocity and pressure) extend over a greater portion of the

       Another approach that can be used for subsonic and transonic flows is to
       specify velocity and static pressure upstream of the object and total pressure
       downstream of the object. This is valid if the domain is at least 50 chord
       lengths away from the object. The analysis run scheme for this type of anal-
       ysis is to run 50 iterations as subsonic compressible then switch to full com-
       pressible and run for 300 or so more iterations. Convergence Control
       should be set to 0.1-0.2 for velocity and pressure. This method has been
       found to be quite stable for flows around Mach 1.

       Higher velocity flows (greater than Mach 1.5) should be run with velocity
       and static pressure specified upstream and either total pressure or the
       unknown set downstream (as shown in the preceding figure). Also, Pres-
       sure Control should be set to 0.001 and Convergence Control on velocity
       and pressure should be set to 0.1 in the Control_Convergence window.

       Sometimes you may find it more convenient to use a rectangular shaped
       domain instead of a semi-circular or spherical shape. This has been found to
       work quite well for some situations, and the boundary conditions should be
       applied as shown in the following graphic:

5-16   COSMOS/Flow User’s Guide • 01/2000
Chapter 5 Analysis Guidelines

This section identifies problems which can arise when first using COS-
MOS/Flow and outlines procedures for solving them. It is helpful to first
review Chapter 1 of the Technical Reference for an explanation of the COS-
MOS/Flow input/output data files.

One beginning note is that most of the convergence problems are related to
the mesh. Finer meshes will usually (not always) produce a more converged
solution. This is probably where to begin the trouble shooting. However, if
you feel you have an adequate mesh, here are some other possible culprits.

Divergence Before 1 Iteration
Once the analysis phase has started, the start up processing steps are dis-
played in the information window of the Analysis window. When all input
processing is completed, the black arrow should appear next to U Vel, V
Vel, etc. On the PC, the machine may be hung if you don’t see this arrow
after a brief setup time (This is dependent on problem size. Note: radiation
analyses can take a very long time to process initially. For very large mod-
els (500,000 elements) the start up time could be as high as 2 hours.).

On some PC’s, you can check by hitting the caps lock key. If the caps lock
indicator light does not respond, the machine is probably hung. One prob-
lem that may cause this behavior is if your hard disk has some lost alloca-
tion units. If you do a ScanDisk command to clean up the disk, this problem
should go away. Another possible cause of the machine hanging is if the
hard disk is nearly full. If your disk is nearly full, the machine may hang
when it tries to write the file.

If you don’t get the black arrow but you do get the COSMOS/Flow error
box after you hit the GO button on the Analyze window, select COSMOS/
Flow_Review_Status to see the error message noted in the status file,
<jobName>.st. Typically, one of the pre-processor files containing the
geometry and/or boundary condition information does not have the correct
path or model data. These pre-processor files must be in the same path as
the control file, <jobName>.ctl.

COSMOS/Flow User’s Guide • 01/2000                                       5-17
       Chapter 5 Analysis Guidelines

       Another cause of this scenario is that the program has not been installed
       properly and some COSMOS/Flow files are missing. You may need to re-
       install the software.

       If there is not enough in-core memory available for the CFD problem being
       run, the message “Maximum available memory may have been exceeded”
       will be printed in the <jobName>.st file. If the memory limit is exceeded,
       COSMOS/Flow can be run using a virtual memory manager to “page” to
       the hard disk.

       Divergence Before Iteration 10

       One common cause for early divergence is mis-matching units. Check the
       Reynolds number and property values (a zero viscosity frequently causes
       quick divergence) in the summary file. Also, make sure the length unit spec-
       ified on the Options window is correct.

       If you are using variable properties, the temperature should be initialized to
       some appropriate value. A temperature of zero will definitely cause prob-
       lems. Specified temperatures should be in absolute units if variable proper-
       ties are used.

       If a turbulent flow is analyzed without using one of the turbulence models,
       the solution will diverge rather quickly. Try turning on a turbulence model.
       Also, make sure the automatic turbulent start up is turned on.

       Finally, for some compressible flow analyses, you may need to adjust the
       Turb/lam Ratio in Preferences_Turbulence.

       Divergence After Iteration 10

       If there are unmerged nodes or crossed element faces between fluid vol-
       umes in the model, the solution may take some time to diverge, depending
       upon where these nodes are. It is always a good idea to check carefully for
       unmerged nodes or crossed element faces if the solution diverged. Often the
       result of unmerged nodes is internal walls. Plots of the velocity magnitude

5-18   COSMOS/Flow User’s Guide • 01/2000
Chapter 5 Analysis Guidelines

or simply the walls themselves in CFDisplay should make the internal walls
visible. The unmerged nodes will be at the boundaries of the meshed geom-
etry. Note that you may have to change the tolerance on the merging com-
mand or remesh the domain to solve this problem properly.

If the inlets or outlets contain recirculation zones, the problem is not well-
posed mathematically and may eventually diverge. You may have to move
these boundaries out, as described earlier in this chapter.

If there are gaps which have fewer than 3 interior nodes, the solution may
also diverge. This is usually only true if the gap is in a critical area of the

If the solution gets a large spike soon after iteration 50 and continues to
grow or at least does not converge, you should try choosing Lock On for the
Automatic Turbulent Startup Procedure. (COSMOS/Flow_Preferences_

Though many CFD analyses, including turbulent ones, may be performed
with the default COSMOS/Flow control settings, some require special treat-
ment to achieve a solution. When necessary, the following steps are recom-
mended to aid convergence, particularly when the solution is unstable or
diverging in the early iterations (these steps should be implemented individ-
ually in the order given):
1 Lower the convergence control on the pressure equation from the
    default value of 0.5 to 0.1-0.3 by selecting COSMOS/Flow_Control_
    Convergence and changing the slider bar position.
2 Try setting the Auto Turb to Extend in the Preferences_Turbulence
    window. This is a variation of the Automatic Turbulent Startup
    algorithm that is particularly useful for some compressible flow

COSMOS/Flow User’s Guide • 01/2000                                          5-19
       Chapter 5 Analysis Guidelines

       3 Observe the solution results in the Run-time CFDisplay window.
           Wherever you see errant velocity vectors or splotches of high or low
           pressures is where the solution is having difficulty. Often refining the
           mesh in these locations solves the problem. If necessary, you may have
           to re-run the analysis and stop just before divergence occurs (1-2
           iterations). The turbulence quantities (TKE and EPS) can also be
       4 Turn on the calculation of the nodal residuals and plot these in
           CFDisplay. Where the largest values appear, the mesh should be

       Oscillating Results

       There are three scenarios which cause results to appear to oscillate in the
       Run-time CFDisplay window:

       The first is that the mesh is not fine enough. By observing where the solu-
       tion changes in the Run-time CFDisplay window, you can quickly locate
       areas of the mesh in need of refinement, while the analysis is running. Dis-
       play vectors, and note where the directions are changing. Often you will see
       one or a small number of vectors in some critical location such as a wake
       oscillating back and forth. Plotting the nodal residuals should also provide
       you with which areas need refinement (largest residuals).

       Another scenario which causes this condition is recirculation zones crossing
       inlet/outlet planes. Again, this can be quickly diagnosed by observing the
       Run-time CFDisplay window. If these zones can be eliminated in your
       model, the solution should converge.

       The third cause of oscillating residuals is vortex shedding. If you switch to
       transient, you should be able to obtain a converged solution.

       Finally, the solution may be converged enough for the purpose of the analy-
       sis. If you check the summary information in the Convergence Monitor and
       under COSMOS/Flow_Review_Convergence, and the plots have all flat-
       tened, the solution is converged for this mesh. The summary information is
       the best indicator of convergence.

5-20   COSMOS/Flow User’s Guide • 01/2000
6             CFDisplay Commands

    CFDisplay is a results-visualization tool of COSMOS/Flow. There are two
    modes of CFDisplay, the Run-Time and the Post-Processor. The commands
    and operation of the Run-Time CFDisplay are discussed in Chapter 3. This
    chapter will focus on the commands and User Interface of the Post-Proces-
    sor CFDisplay.

    This chapter will cover the following areas:
       • The CFDisplay graphical user interface
       • CFDisplay commands

    CFDisplay Graphical User Interface
    This section describes the components of the User Interface. The Graphics
    Window, Select Results dialog, Toolbar icons, and the mouse functions are

    COSMOS/Flow User’s Guide • 01/2000                                     6-1
       Chapter 6 CFDisplay Commands

       User Interface

       The following is the CFDisplay graphics window:

      Main Menu                                                 Toolbar


                                          Graphics Window

                                                                      Displayed Result


            Number                    Select Results Dialog

              • Main Menu: All commands are found there. Every command will be
                described in this chapter subsequently.
              • Toolbar: Many of the more commonly used commands are accessible
              • Graphics Window: The model is shown here.
              • Model: Your analysis model.
              • Title: The COSMOS/Flow 4.0 name and the job title are shown here.
              • Legend: When fringes (filled contours) are on, the scale is displayed
              • Status Line: Lists status of current or last operation.

6-2    COSMOS/Flow User’s Guide • 01/2000
Chapter 6 CFDisplay Commands

   • Iteration Number: The iteration number from the results set is shown.
   • Select Results Dialog: Choose the displayed result and set animation
   • Displayed Result: Informational dialog which shows the displayed

✍ The Title and Displayed Result box can be turned off by unchecking

Select Results Dialog

   • Scalar: Select the scalar quantity to display from this drop menu.
   • Vector: Select the displayed vector quantity.
   • Step: Select the desired time step or steady state iteration if multiple
     sets were sent to CFDisplay.
   • Apply: Activates changes
   • Animation: Brings up the Animation Setup dialog for animating
     results sets.
   • Close Dialog: Normally this button should no be pressed. If the
     Select Results dialog is closed, it can be reopened by clicking
     Window_Results Dialog.
   • Auto Apply: Applies commands as soon as they are entered, instead
     of having to click the Apply button.

COSMOS/Flow User’s Guide • 01/2000                                        6-3
      Chapter 6 CFDisplay Commands


      The most frequently used menu commands can be accessed directly from
      the toolbar buttons.
          Select Region               Deformed Display     Animation Setup
      opy Scene to                 Fringe Display              Animation Control Panel
      nt Scene                  Mesh Display
                                                                         Enter Commands

                                       Hidden Line                   Command and Message D
       Open Command
        File                        Wireframe            Move Model as Outline
      en Secondary              Display As Points
      le                                             Toggle Navigation Mode
                            Display As Lines
       Primary File       Display As Surfaces

          • Open Primary File: Generally not used. CFDisplay is always started
            from the COSMOS/Flow Solver User Interface (Results icon), so the
            appropriate files are read in automatically based on the control file
            name. To switch to a different model, open the control file in
            COSMOS/Flow Solver, and launch CFDisplay.
          • Open Secondary File: Not used. See Open Primary File.
          • Open Command File: Not used. See Open Primary File.
          • Print Scene: Opens dialog for printing scene.
          • Copy Scene to Clipboard: Copies image to clipboard buffer for later
            use. Image can be pasted into Paint, word processing applications,
          • Select Region: Choose desired part of display to be printed or copied
            to clipboard.
          • Display as Surfaces: Show model as surfaces (solid)
          • Display as Lines: Show model as element edges
          • Display as Points: Show model as node point locations
          • Wireframe: Show model as wireframe.

6-4   COSMOS/Flow User’s Guide • 01/2000
              Chapter 6 CFDisplay Commands

   •   Hidden Line: Show model as element edges with hidden lines removed.
   •   Mesh Display: Shows mesh. Most useful in conjunction with Surface Display.
   •   Fringe Display: Activates color fringes (colored results display)
   •   Deformed Display: Not used.
   •   Toggle Navigation Mode: Toggle between standard mouse navigation mode
       and “Walk-around” mode.
   •   Move Model as Outline: When model is rotated, translated, or zoomed, it is
       shown as a wireframe image. (On by default.)
   •   Animation Setup: Brings up the Animation Setup dialog for animating results
   •   Animation Control Panel: Brings up the dialog to control forward and reverse
       animation of transient and multi-step steady-state result sets.
   •   Command and Message Dialog: Diagnostic tool if errors occur.
   •   Enter Commands: Because CFDisplay is command-driven, this field is
       available for commands. All relevant commands are available through the
       menus and icons, however, so this field is not very useful.

Mouse Functions

The mouse controls model navigation and several other useful functions.

Mouse-only Navigation Functions:
  • Left mouse button: Pans the image.
  • Middle mouse button (both buttons on a 2 button mouse): Zoom in and out of
    the image.
  • Right mouse button: Rotate the image about the center of rotation.
  • Double click right mouse button: toggle between standard navigation mode and
    Walk-Around Mode.

              COSMOS/Flow User’s Guide • 01/2000                                      6-5
      Chapter 6 CFDisplay Commands

      Mouse+Keyboard Control Key Functions:
        • Ctrl+Left mouse button On the model: Selects a polygon and
          highlights a CFDisplay part. A part is marked as selected by a white
          bounding box surrounding it. (Parts in CFDisplay are distinct
          boundary conditions. For example each inlet is a part, each outlet is a
          part, each separate wall is a part, etc.)
        • Ctrl+Left mouse button Off the model: Deselects all parts.
        • Ctrl+Right button if no parts are selected:
          Brings up the following menu:
              •   Show Model Info: Brings up the Info
                  window with Model tab. Presents a
                  brief summary of the model. For fur-
                  ther description, see the section about Window_Info Window.
              •   Change Part Attributes: Brings up the Change Part
                  Attributes dialog. This is useful for modifying the display and
                  visibility of CFDisplay parts. See Model_Change Part
                  Attributes for more information.
              • Rotation Point: Controls the display of the rotation point and
                resets to default location.
         • Ctrl+Right button if a part is selected: Brings up the following menu:

              •   Show Model Info: Brings up the Info window with Model tab.
                  Presents a brief summary of the model. For further description,
                  see the section about Window_Info Window.
              •   Show Part Info: Brings up the Info window with Part tab.
                  Shows the part name and number, the number of polygons and
                  edges, and the display attributes.

6-6   COSMOS/Flow User’s Guide • 01/2000
Chapter 6 CFDisplay Commands

       •   Show Polygon Info: Brings up the Info window with Polygon
           tab, and shows results values at the selected point.
       •   Hide Part #: Turns off display of selected part.
       •   Hide # Unselected Parts: Turns off display of all unselected
       •   Change Part Attributes: Brings up the Change Part
           Attributes dialog. This is useful for modifying the display and
           visibility of CFDisplay parts. See Model_Change Part
           Attributes for more information.
       •   Trace Nodes in Part #: Not used.
       •   Plot Nodes in Part #: Only useful for X-Y plotting across mul-
           tiple result sets. To create X-Y plots of single-result set infor-
           mation, import results into Modeler.
       •   Rotation Point: Controls display of center of rotation, and
           allows the rotation point to be changed to one of the nodes in
           the selected polygon.

COSMOS/Flow User’s Guide • 01/2000                                       6-7
      Chapter 6 CFDisplay Commands

      CFDisplay Commands


      The File menu contains the interaction items for input of geometry, scalar,
      vector/displacement, transformation, and command files. An image can be
      stored as TIFF, PPM or IRIS RGB image file format.

      _Open Primary Files

      This command is generally not used. CFDisplay is always started from the
      COSMOS/Flow Solver User Interface (Results icon), so the appropriate
      files are read in automatically based on the control file name. To switch to a
      different model, exit CFDisplay, open the desired control file in COSMOS/
      Flow Solver, and launch CFDisplay again. This command can be used to re-
      open the Select Results dialog by selecting the .glr file.

      _Open Secondary Files

      Most of the file types in this dialog are not accessible to the user. This com-
      mand is seldom used.

6-8   COSMOS/Flow User’s Guide • 01/2000
Chapter 6 CFDisplay Commands

   _View file:

Open a .vif file which contains one pre-defined view angle command. The
view angle is saved with the menu option File/Save File/Save View.
   _Attributes file:

Opens an .atr file which contains appearance settings in terms of CFDis-
play commands for the model (parts colors, light settings, etc.).

_Open Command File

Not Used. The correct Command file is loaded automatically when CFDis-
play is launched from COSMOS/Flow Solver.

_Save file
   _Save View:

Saves the current viewpoint of the model in a .vif file. This file saves the
orientation of the model.
   _Save Attributes:

Saves the current appearance attributes for the present model (colors, light
settings, transparency, etc.) in an .atr file.

_Export to file
   _VRML file:

Saves the current geometry to a VRML file (wrl suffix).

_Save image to file:

Saves the current view on the screen to a specified image format. Note that
the different image formats are pixel based and that the resolution is depen-
dent upon the actual window size. Note also that the CFDisplay window
must not be obscured since the pixels are read directly from the screen.
        •    BMP: Saves the current view as a Windows Bitmap file.

COSMOS/Flow User’s Guide • 01/2000                                        6-9
       Chapter 6 CFDisplay Commands

                •   TIFF: Save the current view to a TIFF file.
                •   RGB: Save the current view to a IRIS RGB file.
                •   PPM: Save the current view to a PPM file (Portable PixMap).

       _Close Files

       Closes all files and puts CFDisplay in an empty state.


       Brings up the Print dialog:

       Clicking the Print Setup button brings up the standard Windows Print
       Setup dialog.

       _Page Setup

       Allows modification to the printable image.

6-10   COSMOS/Flow User’s Guide • 01/2000
Chapter 6 CFDisplay Commands


Exits CFDisplay.


The Display menu contains items which impact the general display modes
for the model and for the background: Light settings, background color, part
tips, spin mode, etc. Node numbers and performance numbers are also
selectable from this menu.


Toggles the display of the Displayed Result box and the Title in the CFDis-
play graphics window. The Displayed Result box displays the CFDisplay
program version, time, minimum and maximum values of scalar and vector
results for all time steps.
   •    SMN Minimum scalar value.
   •    SMX Maximum scalar value.
   •    VMN Minimum vector value (sum of x-, y- and z-components).
   •    VMX Maximum vector value (sum of x-, y- and z-components).

COSMOS/Flow User’s Guide • 01/2000                                      6-11
       Chapter 6 CFDisplay Commands


       Display the coordinate axis of the model.


       Enable/disable display of performance numbers in the graphics window
       (number of polygons, polygons per second, frames per second).

       _Node numbers

       Display the node numbers of the model. Please note that displaying node
       numbers for all nodes in a large model, decreases the graphics performance.

       _Polygon normals

       Display normal vectors for every polygon. Please note that displaying poly-
       gon normals for all polygons decreases the graphics performance.

       _Part Tip

       When checked, displays the name of the part the mouse is over.

       _Perspective view

       Enables/disables perspective view (default = enabled).


       Enable/disable spin mode (default = disabled).


       Enable/disable color dithering (default = enabled). On displays with insuffi-
       cient color depth, OpenGL will simulate the missing colors by dithering.

6-12   COSMOS/Flow User’s Guide • 01/2000
Chapter 6 CFDisplay Commands

_Use Zbuffer

Enable/disable Z-buffer depth buffer) (default = enabled). Using the Z-
buffer ensures that the model is displayed with the correct depth ordering.

_View from

View the model from six preset angles:
        •   x-axis View from positive x-axis
        •   –x-axis View from negative x-axis
        •   y-axis View from positive y-axis
        •   –y-axis View from negative y-axis
        •   z-axis View from positive z-axis
        •   –z-axis View from negative z-axis

_Reset view

Reset the view of the model to the initial view.


   • Color: Set the background to one solid, user specified color. (default
     = black).
   • Top/Bottom: Enable a two-colored graded background from bottom
     to top.
   • Top/middle/bottom: Enable a three-colored graded background
     from bottom to middle to top.

COSMOS/Flow User’s Guide • 01/2000                                      6-13
       Chapter 6 CFDisplay Commands

          • Corners: Enable four-colored graded background from corner to
          • Radial: Enable two-colored graded background from edge to center.


       Six different light sources are available and can be enabled/disabled inde-
       pendently. During the modeling process, normals of neighboring polygons
       are sometimes accidentally specified so that they point in opposite direc-
       tions. This may cause different and unintended light reflections when a sur-
       face consists of several polygons. This phenomenon can be avoided by
       using two-sided light.
          • Front: Enable/disable front light (light 1, default = enabled).
          • Back: Enable/disable back light (light 2, default = enabled).
          • Bottom left: Enable/disable bottom left light (light 3, default =
          • Bottom right: Enable/disable bottom right light (light 4, def. =
          • Top right: Enable/disable top right light (light 5, default = disabled).
          • Top left: Enable/disable top left light (light 6, default = disabled).
          • Two-sided light: Enable/disable two-sided light (default = enabled).
          • Properties... Set advanced light settings independently for the six
            different light sources.

6-14   COSMOS/Flow User’s Guide • 01/2000
Chapter 6 CFDisplay Commands


These items impact the model geometry and the appearance of the model:
surface, lines or points mode, smooth shading and smoothed lines, mesh
and lines color. Part attributes may be set independently for selected parts
by using the Change Parts Attributes option.


Toggles between the image and a bounding box. This is useful when zoom-
ing, rotating or translating large models on computers with low graphics

_Move as

When moving the model (zoom, rotate, translate), the model changes
appearance to either bounding box, points or lines. When the mouse buttons
are released, the current display setting reappears.

COSMOS/Flow User’s Guide • 01/2000                                       6-15
       Chapter 6 CFDisplay Commands

          •   Bounding box: Moves the model as bounding box.
          •   Points: Moves the model as points (vertices).
          •   Lines: Moves the model as lines.
          •   Outline: Moves model as wireframe display.
          •   Model Moves the model in the same mode as the current viewing

       _Show as Surface

       View the model in surface mode (solid model):

       _Show as lines

       View the model as elements (element edge lines).

6-16   COSMOS/Flow User’s Guide • 01/2000
Chapter 6 CFDisplay Commands

_Show as points

View the model as points (polygon vertices).

_Show as outline

View the model as outline (wireframe).

_Show as hidden lines

View the model as element edges with hidden lines removed.

COSMOS/Flow User’s Guide • 01/2000                           6-17
       Chapter 6 CFDisplay Commands

       _Show outline mesh

       Displays the wireframe lines over the surface display.

       _Show mesh

       Display overlayed mesh lines. This is most useful in conjunction with sur-
       face display.

       _Smooth shading

       Enable gouraud shading when viewing the model in surface mode.

       _Smooth lines

       Enable smoothed lines when viewing the model in line mode or when mesh
       is enabled. The command uses antialiasing and softens the edges of the

6-18   COSMOS/Flow User’s Guide • 01/2000
Chapter 6 CFDisplay Commands

_Change Part Attributes

Opens the Part Attributes Dialog. It is possible to change any appearance
and attribute for each selected part. “Parts” in CFDisplay are distinct bound-
ary conditions. Parts are further categorized by their element property ID’s.
For example, models with multiple solid types would have walls with each
property ID listed independently.

Each part “remembers” its settings. It is possible to display each part in a
different manner, or to display only one part if desired. To rapidly select all
of the parts, click the Select All Parts button. To select individual parts,
either pick them from the list, or hold down the keyboard control key, posi-
tion the mouse cursor over the desired part, and click the left mouse button.
Selected parts are surrounded by a white bounding box in the display and
are highlighted in the list.

To de-select all parts, position the mouse in the display window off the
model, hold down the keyboard control key, and click the left mouse button.
   • Part Types
        •   Inlet: any specified velocity entering or leaving the domain
        •   Outlet: any specified pressure entering or leaving the domain
        •   Wall: any external surface and any fluid/solid interface
        •   Slip: any slip or symmetry condition
        •   Unknown: any specified unknown entering or leaving
        •   Shell Side 1: one side of a duplicated shell surface
        •   Shell Side 2: other side of a duplicated shell surface

COSMOS/Flow User’s Guide • 01/2000                                         6-19
       Chapter 6 CFDisplay Commands

             • Shells: any shell element that could not be duplicated
          • Draw Style
              •   Surface: show part as surface
              •   Lines: show part as element edges
              •   Points: show part as points
              •   Outline: show as wireframe
              •   Hidden Lines: show as element edges with hidden lines
          • Part Attributes
              •   Visible: toggles visibility of part
              •   Smooth Shading: enables gouraud shading of part
              •   Displacements: not relevant
              •   Fringes: toggles display of color fringes (results display)
              •   Vector Arrows: toggles display of vectors
              •   Mesh: overlays mesh if surface display is enabled
              •   Outline mesh: overlays wireframe display if surfaces are
              •  Transparent: shows the part with 70% transparency (only active
                 when part is shown in surface mode)
          • Color
             • Set color for the selected part(s).
          • Material

              •   Ambient reflection RGB [0.0–1.0].
              •   Diffuse reflection RGB [0.0–1.0].

6-20   COSMOS/Flow User’s Guide • 01/2000
Chapter 6 CFDisplay Commands

        •   Specular reflection RGB [0.0–1.0].
        •   Emission RGB [0.0–1.0].
        •   Shininess [0.0–128.0].
      • Transparency [0.0–1.0]
   • Texture

        •   Load texture: Load an IRIS RGB texture file for the selected
        •   Remove texture: Remove selected loaded textures.
        •   Mapping: Apply image as a texture map.
        •   Plane: Select the plane to apply the texture map
        •   Tile: Select the display type of texture display
        •   Mode: Select the mode of texture display

_Mirror Model

Mirror the current model along the x-, y- or z-axis. This command dupli-
cates all positive coordinate values to the corresponding negative value (and
vice versa). The option is useful when working with a smaller part of a
model (e.g. one fourth of a circular model) and later on presenting the full
model. Note that only one mirroring is allowed simultaneously.
   • Mirror off Disable mirroring.
   • X-axis Mirror the model along x=0.

COSMOS/Flow User’s Guide • 01/2000                                       6-21
       Chapter 6 CFDisplay Commands

          • Y-axis Mirror the model along y=0.
          • Z-axis Mirror the model along z=0.

       _Line width

       1–5 Sets line width (lines and mesh).

       _Point size

       1–5 Set the point size.

       _Show all model points

       Show all nodes in the model including nodes that are not referenced by the
       polygon definition.

       _Mesh color

       Set the color of the mesh lines.


       Open the Z-clip Dialog where the rear clipping plane (back plane) and the
       front clipping plane can be set. This is a way to cut into a model and to see
       its interior.
          • Front Plane: Increasing this value moves the clipping plane away
            from the user’s eye, removing from view what is between the user
            and the plane. No material is removed for values less than the Model
            Min, and the entire model will disappear if the value is larger than the
            Model Max.

6-22   COSMOS/Flow User’s Guide • 01/2000
Chapter 6 CFDisplay Commands

   • Back Plane: Increasing this value moves the clipping plane toward
     the user’s eye (from behind the model), removing from view material
     behind the model.
   • Model Min and Max: These values are the bounds of the model.
     They change when the image is zoomed in and out.

The following graphic illustrates use of the Z-clip:
                        Front Plane               Back Plane


               Direction when         Visible Region   Direction when
               Front Plane                             Back Plane
               Value is increased                      Value is increased

CFDisplay_Scalar menu

The Scalar menu contains options for how the scalar results will be dis-
played: fringes (filled contours), textured fringes, contour lines, fringe and
contour ranges. For three dimensional models, iso surfaces and cut planes
may be visualized.

COSMOS/Flow User’s Guide • 01/2000                                          6-23
       Chapter 6 CFDisplay Commands

       _Color fringes

       Display scalar results as fringes (filled contours).

       _Contour lines

       Display scalar results as contour lines. The appearance is somewhat similar
       to isobars and is useful to see how different values are distributed on the

       _Fringe shade

       Enable shading of the model when scalars are displayed as fringes.

       _Textured fringes

       The scalar results are displayed as a color map with 16 different colors. This
       option gives a more distinct separation between the different scalar values.

       _Average Element Results

       Displays results averaged across elements.

       _Set Scalar Ranges

       Change the Fringe Range and Contour Range.
          • Fringe Range: is automatically set to the minimum and maximum
            value of the results in the scalar file.
          • New Scalars Force Full Range: Uncheck to keep the specified
            fringe range when loading a new scalar

6-24   COSMOS/Flow User’s Guide • 01/2000
Chapter 6 CFDisplay Commands

   • Set Full Range: Use to reset the Fringe Range to the minimum and
     maximum values.
   • Contour Range: By default the contour range is set to automatically
     follow the current fringe range. This can be overridden by entering
     values for the minimum and maximum contour range.
   • Contours Follow Fringes: Force contours to follow the fringe range.


Toggles the display of the color Fringe Legend.

_Legend text

Display legend label annotations (fringe values on the legend bar).

_Cutting plane

Set a cutting plane through a 3D model. Cutting planes are very useful for
displaying information through cross sections of three dimensional results.
Contours and/or vectors can be displayed on cutting planes.
   • Point on the Plane: Use the slider bars to locate the plane. Values
     can be typed into the fields adjacent to the bars.
   • Normal: Set the orientation of the plane by entering a normal vector
     to the plane. The plane can be set in any orientation with this field.
   • Vectors: When checked, vectors are displayed on the plane.
   • Color vectors by scalar: When checked, vectors are colored by the
     active scalar. When unchecked, vectors are a uniform color.

COSMOS/Flow User’s Guide • 01/2000                                      6-25
       Chapter 6 CFDisplay Commands

          • Hide Plane: When checked, color fringes are not displayed. Only
            vectors are shown (if the Vectors box is checked).
          • Grid: Vectors on cutting planes are displayed as an ordered grid for
            clarity. Modify the density of the grid by increasing or decreasing the
            number of grid points.

       An example of a cutting plane:


       Generate an iso-surface of a specified scalar value. An iso-surface is a sur-
       face of common value. Such surfaces are useful for visualizing velocity and

6-26   COSMOS/Flow User’s Guide • 01/2000
Chapter 6 CFDisplay Commands

temperature distributions, helping to identify areas of constant value. An
example of an iso surface is shown below.


The Vector menu contains options for how the vector results should be dis-
played. Use this menu to adjust the vector scale, and to display particle
traces (for 3D geometry).


Not relevant for flow models.

COSMOS/Flow User’s Guide • 01/2000                                       6-27
       Chapter 6 CFDisplay Commands

       _Vector arrows

       Display vector results as vector arrows. This option enables vector display
       on boundaries. To display vectors on a cutting plane, see the Cutting Plane

       _Arrow heads

       Toggles the display of arrow heads on vectors.

       _Show undeformed model

       Not relevant for flow models.

       _Vector Settings

          •   Scaling Factor: adjusts length of vectors relative to model
          •   Arrow head size: adjusts size of arrow head
          •   Relative to model: auto-scales vectors relative to the model
          •   Vector arrows: toggles display of arrow heads

       _Trace nodes

6-28   COSMOS/Flow User’s Guide • 01/2000
Chapter 6 CFDisplay Commands

Trace the trajectory of a user specified node. Use picking to get polygon/
node numbers (Ctrl + left mouse).

_Particle tracing

Trace a particle through the volume of a model. Note that particle tracing is
only available for 3D geometry. The following shows an example of parti-
cle traces:

COSMOS/Flow User’s Guide • 01/2000                                       6-29
       Chapter 6 CFDisplay Commands

          Startpoint Tab:

       The “Startpoint” tab in the Particle Trace dialog allows specification of
       one or more startpoints for the particle trace(s) to be computed.

       When Vector_Particle Tracing is invoked, a white start point will appear in
       the model. The particle trace will grow from this seed point. The location of
       the start point is controlled with the slider bars and the coordinate text
          • Preview startpoint: this must be checked to preview the specified
            start point(s).
          • Specify as Box: Check to create multiple start points. The lower set
            of slider bars will become active. Both sets of slider bars will control
            the size and location of the box.
          • Lock Coordinates: Clicking this button locks the size of the start-
            point box. Further movements of the slider bars will only move the
          • Nx, Ny, Nz: Controls the number of start points in each direction.
            These fields are active only when Specify as Box is checked.
          • Reset: Returns all settings back to the defaults.

       Note: If the Particle Trace dialog is closed, any traces will remain in place
       on the model. However, when the dialog is opened again, it will be reset to
       the defaults.

6-30   COSMOS/Flow User’s Guide • 01/2000
Chapter 6 CFDisplay Commands

   Particle Trace Display Setup

The settings in this dialog box affect how the computed trace lines are visu-
alized in CFDisplay.
   • Show: Toggles the display of the computed traces on/off
   • Animate: enables or disables animation of the trace lines. When
     animation is on, the number of time steps can be specified.
   • Complete trace: determines whether the entire computed trace line
     should be shown
   • Incremental trace: allows the trace line to be drawn progressively.
   • Show startpoints: Toggles the display of the trace start points.
   • Animate Using Line: A line (worm) will traverse the particle trace.
   • Animate Using Points: A set of points will traverse the particle trace.

COSMOS/Flow User’s Guide • 01/2000                                      6-31
       Chapter 6 CFDisplay Commands

       Particle Trace_Options:

       The “Options” tab allows the setting of various options regarding how the
       particle traces are computed.
          • Method: can be set to RK32, Euler (default) or Linear.
          • Direction: Traces can be computed in either the forward or backward
            (or both) directions in the vector field.
          • Points inside elements: Selects whether computed points lying
            inside volume elements should be displayed.
          • Interpolation: the method to use can be set, but for most purposes
            the default, L2, is the best choice.
          • Maximum Number Of Points: can be set to prevent calculation of
            particles caught in vortexes from which there is no escape to go on

6-32   COSMOS/Flow User’s Guide • 01/2000
Chapter 6 CFDisplay Commands


The Animation menu contains all options related to animation, included cre-
ation of MPEG video sequences. The required information prior to the ani-
mation is defined in the Animation Setup menu. Options for the animation
can be accessed through the Animation Run menu.

_Animation setup

Open the Animation Setup Dialog.
   • From step: Start step of the loaded animation.
   • To step: End step of the loaded animation.
   • Skip by: Skip n number of steps (e.g. when skip by 3, steps 1, 4, 7,
     10, etc. are loaded.)
   • Start Delay: Controls, in seconds, the delay of animation start
   • Stop Delay: Controls, in seconds, the delay of animation stop
   • Max FPS: Controls the animation speed.

COSMOS/Flow User’s Guide • 01/2000                                     6-33
       Chapter 6 CFDisplay Commands

       _Mode Shape Animation Setup

       Not used for flow analyses.

       _Animation Control

       Open the Animation Control Dialog. The controls are: Play forward, back-
       ward, stop, pause, step forward and backwards.

       _Fixed Viewpoint Speed Up

       256 or more colors are required to activate Fixed viewpoint speed up.

       _Animation Settings

       Several animation parameters are set here. This dialog is accessible during
       an animation.

       _Save animation to file

       Save the animation to a MPEG file. The model should not be manipulated
       during the MPEG creation process since it is difficult to control the model

6-34   COSMOS/Flow User’s Guide • 01/2000
Chapter 6 CFDisplay Commands


None of the controls in this menu are relevant to COSMOS/Flow flow cal-
culations. To create 2D X-Y plots, the results should be brought into Mod-
eler, and the plots created in Modeler. For more information, please see
Chapter 4 of this manual.


Using commands from the Special menu, all commands and actions per-
formed in CFDisplay can be logged to a specified file. The actions are saved
in terms of available CFDisplay commands. A few other miscellaneous
commands are also available.

_Start logging commands

Saves a command file. The file will record all actions, entered commands
and menu operations as CFDisplay commands. The file may be re-loaded to
re-produce the actions of the recorded session.

_Stop logging of commands

The menu option stops the logging of commands to file.

_ Copy Scene to Clipboard

Copies current display to the clipboard.

COSMOS/Flow User’s Guide • 01/2000                                      6-35
       Chapter 6 CFDisplay Commands

       _Paste Background Image From Clipboard

       Changes the background image by pasting the contents of the clipboard to
       the background.

       _Show Continuous Picking Info

       By holding the keyboard control key and the left mouse button, information
       about the part the cursor is touching is displayed and updated in the Status
       bar. Also, when Polygon Info is activated (Window_Info
       Window_Polygon) the displayed nodal results are updated as the mouse is
       moved over the model.

       _Keep Settings on New Primary File

       This command maintains the current settings when a new .glr file is loaded
       into CFDisplay.


       In the Window menu, the user can enable/disable the Toolbar, Status bar
       and the Command and Message Dialog box. The Results Dialog and the
       Info Window are also accessible from this menu.

6-36   COSMOS/Flow User’s Guide • 01/2000
Chapter 6 CFDisplay Commands

_Commands and Messages dialog

Opens the Commands and Messages dialog. Every command issued by the
user as well as information and error messages are listed in this window.
Also, commands can be entered in the editable field.

_Results Dialog

Opens the Results Dialog if it is accidently closed.

_Info Window

This is a useful window displaying model information and numerical results
   Model Tab

This displays the jobname, the current iteration, and the geometric bounds.
The number of Polygons, etc. found under Geometry Information is not the
number of nodes and elements found in the original model.
   Results Tab

The min and max of the current scalar and vector quantities are displayed.
   VTF File

Lists the attributes of any loaded VTF files.

COSMOS/Flow User’s Guide • 01/2000                                     6-37
       Chapter 6 CFDisplay Commands


       Displays the attributes for the selected part.

       Holding down the control key and selecting with the left mouse button will
       display the results from a surface in the Polygon tab. This is a method of
       extracting results from CFDisplay. If Show Continuous Picking Info is acti-
       vated, holding down the control key will enable the Polygon display to be
       updated with the mouse position.

       This is another method of results extraction. Instead of showing the results
       from the polygon nodes (like Polygon), the results from all nodes of a
       selected element are displayed.


       Toggles the display of the toolbar.

       _Status bar

       Toggles the display of the status bar.

6-38   COSMOS/Flow User’s Guide • 01/2000
7             Using CFDisplay

    The purpose of this chapter is to explain how to use CFDisplay. While the
    previous chapter listed and explained all of the CFDisplay commands, this
    chapter provides more detail about how to use the commands. This chapter
    covers the following areas:
       •   Launching CFDisplay
       •   Getting Started
       •   Displaying Results
       •   Image and Video Output
       •   Increasing Graphics Performance

    Launching CFDisplay
    CFDisplay is started from the COSMOS/Flow main menu by
    clicking on the Results icon:

    If the analysis was run steady state, CFDisplay will simply start. If the anal-
    ysis was run transient, a dialog box will come up prompting you for which

    COSMOS/Flow User’s Guide • 01/2000                                         7-1
      Chapter 7 Using CFDisplay

      post-processing mode you want: single set or animation of the time steps
      chosen in the Create Post Processing Results dialog.

      CFDisplay cannot be launched outside of COSMOS/Flow. However, if only
      the CFDisplay files were saved (.gl*) from an analysis, the results can still
      be viewed in CFDisplay. To do this start COSMOS/Flow and create a con-
      trol file of the same name. No settings need to be made, so simply click on
      the Results icon to launch CFDisplay. As long as all of the .gl* files are in
      the current directory, CFDisplay will start and the results will be loaded in.

      Getting Started
      When CFDisplay first starts, all of the necessary files are automatically
      loaded. There are two things however that should be done prior to post-pro-
      cessing results: Activate Color fringes, and select a result from the Select
      Results dialog.

      Scalar_Color Fringes
      This activates color fringes (filled contours) and launches the legend.
      Invoke this command by either clicking on Scalar_Color Fringes, or by
      clicking the Color Fringes icon from the Toolbar:

7-2   COSMOS/Flow User’s Guide • 01/2000
Chapter 7 Using CFDisplay


Select a scalar result quantity from the Select Results dialog, and click

Displaying Results
The most common way to display results is either as fringes (filled con-
tours), contour lines, or as vector arrows. Scalar data is displayed as fringes
or contour lines; vector results are displayed as vector arrows.

CFDisplay has the ability to visualize internal scalar and vectorial data of a
3D model. This can be done in several ways. In CFDisplay you can calcu-
late cutting planes and iso-surfaces for scalar data and particle traces for
vectorial data. All of these visualization techniques can be used in connec-
tion with animation. The details of this will be explained in the following

COSMOS/Flow User’s Guide • 01/2000                                          7-3
      Chapter 7 Using CFDisplay

      Cutting planes

      The Cuttingplane Dialog is launched by selecting Scalar_Cuttingplane.

      The primary parameters of the Cutting Plane dialog are the location of one
      point on the plane and the normal vector to the plane. The loaded scalar val-
      ues are then mapped onto the cut plane. When this window is started, it may
      be necessary to click the Apply button or to click one of the slider bars to
      cause the plane to appear.

      An example of a cutting plane through a 3D model is shown:

7-4   COSMOS/Flow User’s Guide • 01/2000
Chapter 7 Using CFDisplay

Checking the Automatic update box makes CFDisplay update the cut
plane while the slider bars are being justified. While this provides for better
feedback when fine tuning the position of the plane, it can be turned off if
you experience long delays when adjusting the slider bars.

If the Vectors box is checked, vectors will be displayed on the cutting
plane. The vector density can be controlled by the x and y values in the
Grid field, where x and y are the number of vectors in the two planar direc-
tions of the cutting plane. The defaults of x and y are 30 and 30.

If the Hide Plane box is unchecked, fringes will be displayed on the cutting
plane. When the Hide Plane box is checked, contours will not be displayed,
but vectors will be displayed if the Vectors box is checked.

If a new scalar field is chosen from the Select Results dialog, these data are
mapped on the existing plane.

The plane can be removed by pressing the Reset button; closing the dialog
box will not remove the plane.

Cutting planes present during a results animation will participate in the ani-
mation. This is accomplished by calculating a new cut plane for each time
step. New parameters can be set for the cut plane while the animation is run-
ning, causing the cut plane to be updated accordingly.

Selecting Scalar_Isosurface brings up the dialog box for calculating iso

The dialog box allows specification of the scalar value for which the iso-
surface is defined. The scalar field chosen from the Select Results dialog

COSMOS/Flow User’s Guide • 01/2000                                          7-5
      Chapter 7 Using CFDisplay

      box is then used to create the iso-surface for the selected value. If a new sca-
      lar field is chosen from the Open Results box or read from a file, the iso-
      surface already calculated is removed. However, the iso surface dialog box
      is not removed, and a new iso-surface can be calculated by applying a new
      value in the legal range.

      The Clear button and the Auto Apply check box have the same functions
      as for the cut plane.

      If the you utilize animation, the iso-surface is able to participate in the same
      way as for the cut plane. As long as an iso-surface is defined during or
      before the animation, it will be updated according to the values of the cur-
      rent time step.

      The following is an example of velocity iso-surfaces:

7-6   COSMOS/Flow User’s Guide • 01/2000
Chapter 7 Using CFDisplay

Particle traces

The dialog box for setting up particle traces can be accessed via the
Vector_Particle Tracing. This dialog involves several settings, both for
the calculation method used to generate the traces and the animations that
can be done with the traces. The user should keep in mind that the calcula-
tions needed to apply the particle traces are CPU demanding, and thus could
take some time for large models, complicated traces or numerous start
points. It is also important to note that this option applies to a time-indepen-
dent field. The animation described below is thus a description of a station-
ary vector field. Shown is an example of a particle traces:

Defining start points

When the Particle Trace dialog appears, the Startpoint sheet is shown.
Here you can specify where to start the particle trace by moving the scroll-
bars corresponding to the x, y and z directions. If you wish to calculate
more than one streamline, check Specify as box. When you now use the
scrollbars, the shape of a line/plane/cube is manipulated. When it has the

COSMOS/Flow User’s Guide • 01/2000                                          7-7
      Chapter 7 Using CFDisplay

      right size and shape, the shape can be locked with the Lock coordinates
      button. Now the scrollbars are used to move the plane/cube around in the
      model space.

      The three fields, nx, ny and nz are used to specify how many start points in
      each direction of the line/plane/cube are desired.

      To hide the preview of the starting points, the uncheck Preview startpoint.
      To calculate particle traces from the chosen start points, press Apply.

      Animation of particle traces

      If the Display setup button is pressed, the Particle Trace Display Setup
      dialog appears. This is used to control and apply animation of the already
      calculated particle traces. The default option is to have the check boxes
      Show and Complete trace activated, which means that the complete trace

7-8   COSMOS/Flow User’s Guide • 01/2000
Chapter 7 Using CFDisplay

is to be visualized as is. If you want to apply animation, the check the Ani-
mate box. When this is done, several other options are available.

   • The Animate using line (worm)
                 •    Tail: activates a worm to animate the particle traces of
                      the vector field. This worm has length corresponding to
                      the number of time steps chosen in the Timesteps field.
                      When animated, you can extract information of the
                      strength of the field in the current position both by
                      color and by length of the worm.
                 •    Single color: When checked, the worm is completely
                 • Linewidth: adjusts the width of the worm
   • Complete trace: Tells CFDisplay to also show the complete trace
     when animating. The user can change the number of time steps to
     tune the animation for the case at hand.

In the Animate using points part of the sheet, the same options as described
above appear. The difference is that these options apply to a set of points on
the particle trace path. In this case CFDisplay does not draw lines between
the points, in contrast to the worm animation. If the Complete trace check
box is turned off and the Incremental trace box is checked, the worms/
points appear to be drawing the particle trace as they move in the vector
field. When none of these boxes are checked, the effect is that the worms/
particles drift in the vector field; stretched if the field is strong, and packed
if it is weak.

COSMOS/Flow User’s Guide • 01/2000                                            7-9
       Chapter 7 Using CFDisplay

       To turn on and off the cube/plane used to define the start points, the Show
       startpoints box is used. Changes to the appearance of the animation can be
       done while an animation is running, and in order to apply any changes done,
       you must press the Apply button. The Reset button puts the values of the
       sheet back to its default values.

       Even further combinations of the options in the Particle Trace Display
       Setup dialog box can be utilized, and effects such as worms with white
       heads, etc. can be achieved. The user is encouraged to experiment with the
       options to get the desired results.

       Defining Calculation Options

       In the Options sheet of the Particle Trace dialog, information concerning
       the calculations of the particle traces is specified.

       The Method part of the Options sheet is devoted to the choice of solver for
       the ordinary differential equation (ODE). Three choices are possible:
          • The RK32 method is a third order Runge Kutta method with second
            order embedding. When using this method the error of the calculation
            can be controlled and an upper limit must be given as Error tol. You

7-10   COSMOS/Flow User’s Guide • 01/2000
Chapter 7 Using CFDisplay

     must also apply a starting step length Start h. In order to get the best
     result one must experiment with these values. If a very small Error
     tol is given, the calculation may take considerably longer time.
   • The Euler method is an ODE solver using constant step length inside
     each element of the model. The step length is chosen by the user in
     the Steps per element box. This is a safer choice than the RK32
     method, but have no error control mechanism. If you experience
     numerical instabilities with the RK32 method, you could try the Euler
     method instead.
   • The Linear method is a fast and simple method, which simply jumps
     from border to border of each element.

The Direction part of the Options sheet has checkboxes Forward and
Backward for the direction of the particle trace. CFDisplay offers the abil-
ity to calculate particle traces both forward and backward in the vector field.
This is convenient when you want to learn where the particles in the defined
start points came from. Both options can be checked at the same time as
well as one or the other.

In the Appearance part of the Options sheet you can select whether you
want CFDisplay to draw lines between the calculated points inside each ele-
ment of the model, or if lines should be drawn only between the edges of
each element. This does not alter the accuracy of the method, but eases the
task of displaying the result of extensive particle trace calculations for large

You can choose which interpolation method to use for the calculations in
the Interpolation part of the sheet. When choosing the L2 method, CFDis-
play tends to take more into consideration of the effect of the nodal points
near the current calculation point than if using the L1 interpolation method.
With knowledge of how the data were created, the expert user may be able
to decide which method that gives the highest accuracy, but with no knowl-
edge of this kind, we suggest the use of the L2 method, since this yields the
smoothest curve across element borders.

The last available parameter is Max. number of points. This is added to
prevent the calculation to go on forever if the particle trace is caught in a
vortex which it can not escape. A number of 5000 tells CFDisplay that one

COSMOS/Flow User’s Guide • 01/2000                                         7-11
       Chapter 7 Using CFDisplay

       particle trace can contain maximum 5000 calculated points, and if this is
       exceeded the particle trace stops.

       Image and video output

       MPEG video output
       A MPEG video stream can be created from any model with results data con-
       taining two or more time steps. The model cannot be manipulated during
       the creation of the MPEG video (zoom, rotation, translation).

       To create an MPEG video, after CFDisplay is started from COSMOS/Flow
       and the scalar and background color, etc. are setup, start the animation.
       From the Animation menu, select Save animation to file. The animation
       will start from step 1 (or the steps you have selected) and run through the
       whole animation.

       The size and resolution of the MPEG video is solely dependent upon the
       actual size of the CFDisplay window (number of pixels) and the actual color
       resolution in Windows (e.g. 256 color, 16-bit color, 24-bit color). Please
       note that the CFDisplay window must not be obscured during the creation
       of the MPEG stream.

       The MPEG file is by default saved in the directory of the current model.

       Image output

       The image output feature allows the user to save an image of the model to
       BMP, TIFF, PPM, IRIS RGB or EPS format. The file formats save all the
       information within the graphics window: background color, text, step num-
       ber, info box and legend bar.

       As in the MPEG feature, the size (pixel resolution) of the output image is
       dependent upon the actual size (number of pixels) of the CFDisplay win-

7-12   COSMOS/Flow User’s Guide • 01/2000
Chapter 7 Using CFDisplay

dow. The color resolution is dependent upon the resolution (e.g. 256 color,
16-bit color, 24-bit color) set by Windows (see Control Panel/Display/Set-
tings). Again, please note that the CFDisplay window must not be obscured
when saving the image.

To save an image, select the File_Save Scene to file. Select the desired file
format, location and file name.

Note that most Windows programs (word processors and presentation pro-
grams) accept the TIFF format. IRIS RGB is useful when exporting images
to UNIX workstations or for more advanced image processing in a photo
editor (e.g. the shareware program XV for UNIX). The PPM format is
mostly used for the creation of MPEG videos.


To create hard copy output, click on File_Print. The Print dialog will come

The image can be printed directly to a printer or to a file by checking the
Save to PostScript box. Other parameters such as Image Size and Image

COSMOS/Flow User’s Guide • 01/2000                                       7-13
       Chapter 7 Using CFDisplay

       Position are also controlled from this dialog. Choose the Render quality
       and Appearance parameters from this dialog. To print, click the Ok button.

       Click the Print Setup button to bring up the standard Windows Printer
       Setup dialog.

       Increasing Graphics Performance
       If no graphics hardware supporting OpenGL 3D acceleration is installed,
       the graphics performance of CFDisplay is solely dependent on the processor
       speed and the amount of installed RAM. This may be frustrating when visu-
       alizing large models and results on a low-end computer.

       However, there are ways to get around these limitations and—to some
       extent—increase the graphics speed (or at least make it easier to manipulate
       the models):
          • Move model as outline.
          • Change display mode (use lines or points).
          • Animation: Skip steps of large results files; display analysis steps one
            by one.
          • Visualizing large geometries: Use structured mesh if possible.
          • Examining large models: Hide (unpost) selected parts.

       The features cannot be applied to all models, but it may be useful to be
       aware of them in the design and pre-processing phase.

       Move model as outline

       Large geometries are often difficult to move, translate or zoom. To facilitate
       the manipulation of such geometry, use the option Model_Move
       as_Outline. The model will automatically change appearance to an outline
       when the geometry is moved.

       Note that Move Model as Outline is set by default.

7-14   COSMOS/Flow User’s Guide • 01/2000
Chapter 7 Using CFDisplay

Change Display Mode to Outline

This mode shows the wireframe view of the geometry, and is often very
informative way to display the model. Redisplaying outline edges is much
quicker than redisplaying surfaces, and the plot is usually quite satisfactory.


Many analysis output files contain numerous time steps. In many cases, it is
not possible to visualize every single analysis step due memory (RAM) lim-

A feasible solution is to visualize steps at some interval. The animation will
not run as smoothly as compared to an animation with all analysis steps
available. However, the feature is useful if the major purpose is to get an
overview of the analysis sequence.

To visualize every tenth time step, select the Animation Setup from the
Animation menu. Enter 10 in the Skip by field.


Settings that decrease graphics performance

The following menu settings should not be used when displaying large
model files on low-end computers without extra OpenGL graphics hard-
   • Texture and environment mapping

COSMOS/Flow User’s Guide • 01/2000                                        7-15
       Chapter 7 Using CFDisplay

          •   Textured fringes (one-dimensional texture)
          •   Vector arrows and polygon normals
          •   Node numbers
          •   Contour lines
          •   Smoothed points (antialiased points)
          •   Smooth shading (gouraud shading)
          •   Smooth lines (antialiased lines)
          •   Fringe shade

7-16   COSMOS/Flow User’s Guide • 01/2000

To top