ANSYS Fluids Analysis
Guide

ANSYS Release 9.0

002114
November 2004

ANSYS, Inc. is a
UL registered
ISO 9001: 2000
Company.

ANSYS Fluids Analysis Guide

ANSYS Release 9.0

ANSYS, Inc.
Southpointe
275 Technology Drive
Canonsburg, PA 15317
ansysinfo@ansys.com
http://www.ansys.com
(T) 724-746-3304
(F) 724-514-9494

Copyright and Trademark Information

ANSYS, DesignSpace, CFX, DesignModeler, DesignXplorer, ANSYS Workbench environment, AI*Environment, CADOE and any and all ANSYS, Inc. product
names referenced on any media, manual or the like, are registered trademarks or trademarks of subsidiaries of ANSYS, Inc. located in the United States or
other countries. ICEM CFD is a trademark licensed by ANSYS, Inc. All other trademarks and registered trademarks are property of their respective owners.

ANSYS, Inc. is a UL registered ISO 9001: 2000 Company.

ANSYS Inc. products may contain U.S. Patent No. 6,055,541.

Microsoft, Windows, Windows 2000 and Windows XP are registered trademarks of Microsoft Corporation.
Inventor and Mechanical Desktop are registered trademarks of Autodesk, Inc.
SolidWorks is a registered trademark of SolidWorks Corporation.
Pro/ENGINEER is a registered trademark of Parametric Technology Corporation.
Unigraphics, Solid Edge and Parasolid are registered trademarks of Electronic Data Systems Corporation (EDS).
ACIS and ACIS Geometric Modeler are registered trademarks of Spatial Technology, Inc.

FLEXlm License Manager is a trademark of Macrovision Corporation.

This ANSYS, Inc. software product and program documentation is ANSYS Confidential Information and are furnished by ANSYS, Inc. under an ANSYS
software license agreement that contains provisions concerning non-disclosure, copying, length and nature of use, warranties, disclaimers and remedies,
and other provisions. The Program and Documentation may be used or copied only in accordance with the terms of that license agreement.

See the ANSYS, Inc. online documentation or the ANSYS, Inc. documentation CD for the complete Legal Notice.

If this is a copy of a document published by and reproduced with the permission of ANSYS, Inc., it might not reflect the organization or physical appearance
of the original. ANSYS, Inc. is not liable for any errors or omissions introduced by the copying process. Such errors are the responsibility of the party
providing the copy.

Table of Contents

I. CFD

1. Overview of FLOTRAN CFD Analyses .................................................................................................. 1–1

1.1. What Is FLOTRAN CFD Analysis? .................................................................................................... 1–1
1.2. Types of FLOTRAN Analyses .......................................................................................................... 1–1

1.2.1. Laminar Flow Analysis .................................................................................................... 1–1
1.2.2. Turbulent Flow Analysis ................................................................................................. 1–2
1.2.3. Thermal Analysis ............................................................................................................ 1–2
1.2.4. Compressible Flow Analysis ........................................................................................... 1–2
1.2.5. Non-Newtonian Fluid Flow Analysis ................................................................................ 1–2
1.2.6. Multiple Species Transport Analysis ................................................................................ 1–2
1.2.7. Free Surface Analysis ...................................................................................................... 1–2

1.3. About GUI Paths and Command Syntax ......................................................................................... 1–2

2. The Basics of FLOTRAN Analysis ......................................................................................................... 2–1

2.1. Characteristics of the FLOTRAN Elements ...................................................................................... 2–1

2.1.1. Other Element Features .................................................................................................. 2–1

2.2. Considerations and Restrictions for Using the FLOTRAN Elements ................................................. 2–1

2.2.1. Limitations on FLOTRAN Element Use ............................................................................. 2–2

2.3. Overview of a FLOTRAN Analysis ................................................................................................... 2–3

2.3.1. Determining the Problem Domain .................................................................................. 2–4
2.3.2. Determining the Flow Regime ........................................................................................ 2–4
2.3.3. Creating the Finite Element Mesh ................................................................................... 2–4
2.3.4. Applying Boundary Conditions ....................................................................................... 2–5
2.3.5. Setting FLOTRAN Analysis Parameters ............................................................................ 2–5
2.3.6. Solving the Problem ....................................................................................................... 2–5
2.3.7. Examining the Results .................................................................................................... 2–5

2.4. Files the FLOTRAN Elements Create ............................................................................................... 2–5

2.4.1. The Results File .............................................................................................................. 2–6
2.4.2. The Print File (Jobname.PFL) ........................................................................................... 2–6
2.4.3. The Nodal Residuals File ................................................................................................. 2–6
2.4.4. The Restart File .............................................................................................................. 2–7
2.4.5. The Domain File ............................................................................................................. 2–7
2.4.6. Restarting a FLOTRAN Analysis ....................................................................................... 2–7

2.5. Convergence and Stability Tools ................................................................................................... 2–8

2.5.1. Relaxation Factors .......................................................................................................... 2–8
2.5.2. Inertial Relaxation .......................................................................................................... 2–8
2.5.3. Modified Inertial Relaxation ............................................................................................ 2–9
2.5.4. Artificial Viscosity ........................................................................................................... 2–9
2.5.5. DOF Capping ................................................................................................................. 2–9
2.5.6. The Quadrature Order .................................................................................................. 2–10

2.6. What to Watch For During a FLOTRAN Analysis ............................................................................ 2–10

2.6.1. Deciding How Many Global Iterations to Use ................................................................ 2–10
2.6.2. Convergence Monitors ................................................................................................. 2–11
2.6.3. Stopping a FLOTRAN Analysis ....................................................................................... 2–13
2.6.4. Pressure Results ........................................................................................................... 2–13

2.7. Evaluating a FLOTRAN Analysis ................................................................................................... 2–14
2.8. Verifying Results ......................................................................................................................... 2–14

3. FLOTRAN Laminar and Turbulent Incompressible Flow ..................................................................... 3–1

3.1. Characteristics of Fluid Flow Analysis ............................................................................................ 3–1
3.2. Activating the Turbulence Model .................................................................................................. 3–2

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

3.2.1. The Role of the Reynolds Number ................................................................................... 3–2
3.2.2. Determining Whether an Analysis Is Turbulent ............................................................... 3–3
3.2.3. Turbulence Ratio and Inlet Parameters ........................................................................... 3–3
3.2.4. Turbulence Models ........................................................................................................ 3–3

3.2.4.1. Standard k-epsilon Model (default) ........................................................................ 3–4
3.2.4.2. Zero Equation Turbulence Model (ZeroEq) ............................................................. 3–6
3.2.4.3. Re-Normalized Group Turbulence Model (RNG) ...................................................... 3–6
3.2.4.4. k-epsilon Model Due to Shih (NKE) ......................................................................... 3–7
3.2.4.5. Nonlinear Model of Girimaji (GIR) ........................................................................... 3–7
3.2.4.6. Shih, Zhu, Lumley Model (SZL) ............................................................................... 3–8
3.2.4.7. k-omega Turbulence Model ................................................................................... 3–8
3.2.4.8. Shear Stress Transport Model (SST) ........................................................................ 3–9

3.3. Meshing Requirements ................................................................................................................. 3–9
3.4. Flow Boundary Conditions .......................................................................................................... 3–11
3.5. Strategies for Difficult Problems .................................................................................................. 3–14
3.6. Example of a Laminar and Turbulent FLOTRAN Analysis ............................................................... 3–16

4. FLOTRAN Thermal Analyses ................................................................................................................ 4–1

4.1. Thermal Analysis Overview ........................................................................................................... 4–1
4.2. Meshing Requirements ................................................................................................................. 4–1
4.3. Property Specifications and Control .............................................................................................. 4–1
4.4. Thermal Loads and Boundary Conditions ...................................................................................... 4–1

4.4.1. Applying Loads .............................................................................................................. 4–2

4.4.1.1. Applying Loads Using Commands ......................................................................... 4–2
4.4.1.2. Applying Loads Using the GUI ............................................................................... 4–3
4.4.1.3. Solutions ............................................................................................................... 4–3

4.5. Solution Strategies ....................................................................................................................... 4–4

4.5.1. Constant Fluid Properties ............................................................................................... 4–4
4.5.2. Forced Convection, Temperature Dependent Properties ................................................. 4–4
4.5.3. Free Convection, Temperature Dependent Properties ..................................................... 4–5
4.5.4. Conjugate Heat Transfer ................................................................................................. 4–5

4.6. Heat Balance ................................................................................................................................ 4–7
4.7. Surface-to-Surface Radiation Analysis Using the Radiosity Method ................................................ 4–8

4.7.1. Procedure ...................................................................................................................... 4–8
4.7.2. Heat Balances ................................................................................................................ 4–8

4.8. Examples of a Laminar, Thermal, Steady-State FLOTRAN Analysis ................................................... 4–8

4.8.1. The Example Described .................................................................................................. 4–9
4.8.2. Doing the Buoyancy Driven Flow Analysis (GUI Method) ............................................... 4–10
4.8.3. Doing the Buoyancy Driven Flow Analysis (Command Method) ..................................... 4–16

4.9. Example of Radiation Analysis Using FLOTRAN (Command Method) ............................................ 4–17
4.10. Where to Find Other FLOTRAN Analysis Examples ...................................................................... 4–18

5. FLOTRAN Transient Analyses .............................................................................................................. 5–1

5.1. Time Integration Method .............................................................................................................. 5–1
5.2. Time Step Specification and Convergence ..................................................................................... 5–1
5.3. Terminating and Getting Output from a Transient Analysis ............................................................ 5–3
5.4. Applying Transient Boundary Conditions ...................................................................................... 5–3

6. Volume of Fluid (VOF) Analyses .......................................................................................................... 6–1

6.1. Overview ...................................................................................................................................... 6–1
6.2. VFRC Loads ................................................................................................................................... 6–1

6.2.1. Initial VFRC Loads ........................................................................................................... 6–1
6.2.2. Boundary VFRC Loads .................................................................................................... 6–2

6.3. Input Settings ............................................................................................................................... 6–3

6.3.1. Ambient Conditions ....................................................................................................... 6–3

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

ANSYS Fluids Analysis Guide

6.3.2. VFRC Tolerances ............................................................................................................ 6–4
6.3.3. VOF Time Steps .............................................................................................................. 6–4

6.4. Postprocessing ............................................................................................................................. 6–5
6.5. VOF Analysis of a Dam .................................................................................................................. 6–5

6.5.1. The Problem Described .................................................................................................. 6–5
6.5.2. Building and Solving the Model (Command Method) ...................................................... 6–5

6.6. VOF Analysis of Open Channel with an Obstruction ....................................................................... 6–6

6.6.1. The Problem Described .................................................................................................. 6–6
6.6.2. Building and Solving the Model (Command Method) ...................................................... 6–7

6.7. VOF Analysis of an Oscillating Droplet ......................................................................................... 6–10

6.7.1. The Problem Described ................................................................................................ 6–10
6.7.2. Results ......................................................................................................................... 6–10
6.7.3. Building and Solving the Model (Command Method) .................................................... 6–12
6.7.4. Where to Find Other Examples ..................................................................................... 6–13

7. Arbitrary Lagrangian-Eulerian (ALE) Formulation for Moving Domains ............................................ 7–1

7.1. Introduction ................................................................................................................................. 7–1
7.2. Boundary Conditions .................................................................................................................... 7–3
7.3. Mesh Updating ............................................................................................................................. 7–5
7.4. Remeshing ................................................................................................................................... 7–6
7.5. Postprocessing ............................................................................................................................. 7–7
7.6. ALE Analysis of a Simplified Torsional Mirror .................................................................................. 7–8

7.6.1. The Problem Described .................................................................................................. 7–8
7.6.2. Boundary Conditions ..................................................................................................... 7–8
7.6.3. Forces and Moments ...................................................................................................... 7–9
7.6.4. Building and Solving the Model (Command Method) .................................................... 7–12

7.7. ALE/VOF Analysis of a Vessel with a Moving Wall ......................................................................... 7–15

7.7.1. The Problem Described ................................................................................................ 7–15
7.7.2. Results ......................................................................................................................... 7–16
7.7.3. Building and Solving the Model (Command Method) .................................................... 7–16

7.8. ALE Analysis of a Moving Cylinder ............................................................................................... 7–18

7.8.1. The Problem Described ................................................................................................ 7–18
7.8.2. Results ......................................................................................................................... 7–19
7.8.3. Building and Solving the Model (Command Method) .................................................... 7–19

8. FLOTRAN Compressible Analyses ....................................................................................................... 8–1

8.1. Requirements for Compressible Analysis ....................................................................................... 8–1
8.2. Property Calculations .................................................................................................................... 8–1
8.3. Boundary Conditions .................................................................................................................... 8–2
8.4. Structured vs. Unstructured Mesh ................................................................................................. 8–2
8.5. Solution Strategies ....................................................................................................................... 8–3

8.5.1. Inertial Relaxation .......................................................................................................... 8–4

8.6. Example of a Compressible Flow Analysis ...................................................................................... 8–4

8.6.1. The Example Described .................................................................................................. 8–4

8.6.1.1. Fluid Properties ..................................................................................................... 8–4
8.6.1.2. Approach and Assumptions ................................................................................... 8–4

8.7. Doing the Example Compressible Flow Analysis (GUI Method) ....................................................... 8–5
8.8. Doing the Example Compressible Flow Analysis (Command Method) .......................................... 8–11

9. Specifying Fluid Properties for FLOTRAN ........................................................................................... 9–1

9.1. Guidelines for Specifying Properties .............................................................................................. 9–1
9.2. Fluid Property Types ..................................................................................................................... 9–1

9.2.1. Property Types for Specific Heat ..................................................................................... 9–2
9.2.2. Property Types for Density and Thermal Conductivity ..................................................... 9–2
9.2.3. Property Types for Viscosity ............................................................................................ 9–3

ANSYS Fluids Analysis Guide

vii

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

9.2.4. Property Types for Surface Tension Coefficient ............................................................... 9–3
9.2.5. Property Types for Wall Static Contact Angle .................................................................. 9–3
9.2.6. General Guidelines for Setting Property Types ................................................................ 9–3

9.2.6.1. Using a Fluid Property Table .................................................................................. 9–3
9.2.6.2. Specifying Property Types ..................................................................................... 9–4

9.2.7. Density .......................................................................................................................... 9–5
9.2.8. Viscosity ........................................................................................................................ 9–6
9.2.9. Specific Heat .................................................................................................................. 9–7
9.2.10. Thermal Conductivity ................................................................................................... 9–8
9.2.11. Surface Tension Coefficient .......................................................................................... 9–8
9.2.12. Wall Static Contact Angle ............................................................................................. 9–9

9.3. Initializing and Varying Properties ................................................................................................. 9–9

9.3.1. Activating Variable Properties ....................................................................................... 9–10

9.4. Modifying the Fluid Property Database ....................................................................................... 9–10
9.5. Using Reference Properties ......................................................................................................... 9–12
9.6. Using the ANSYS Non-Newtonian Flow Capabilities ..................................................................... 9–13

9.6.1. Activating the Power Law Model .................................................................................. 9–13
9.6.2. Activating the Carreau Model ....................................................................................... 9–14
9.6.3. Activating the Bingham Model ..................................................................................... 9–14

9.7. Using User-Programmable Subroutines ....................................................................................... 9–14

10. FLOTRAN Special Features .............................................................................................................. 10–1

10.1. Coordinate Systems .................................................................................................................. 10–1
10.2. Rotating Frames of Reference .................................................................................................... 10–2
10.3. Swirl ......................................................................................................................................... 10–3
10.4. Distributed Resistance/Source ................................................................................................... 10–4

11. FLOTRAN CFD Solvers and the Matrix Equation ............................................................................. 11–1

11.1. Which Solver Should You Use? .................................................................................................. 11–1
11.2. Tri-Diagonal Matrix Algorithm ................................................................................................... 11–1
11.3. Semi-Direct Solvers ................................................................................................................... 11–2

11.3.1. Preconditioned Generalized Minimum Residual (PGMR) Solver .................................... 11–3
11.3.2. Preconditioned BiCGStab (PBCGM) Solver ................................................................... 11–5

11.4. Sparse Direct Method ................................................................................................................ 11–5

12. Coupling Algorithms ....................................................................................................................... 12–1

12.1. Overview .................................................................................................................................. 12–1
12.2. Algorithm Settings .................................................................................................................... 12–1

12.2.1. Advection Scheme ..................................................................................................... 12–1
12.2.2. Solver ........................................................................................................................ 12–2
12.2.3. Relaxation Factors ...................................................................................................... 12–2

12.3. Performance ............................................................................................................................. 12–2

13. Multiple Species Transport .............................................................................................................. 13–1

13.1. Overview of Multiple Species Transport ..................................................................................... 13–1
13.2. Mixture Types ........................................................................................................................... 13–1

13.2.1. Dilute Mixture Analysis ............................................................................................... 13–1
13.2.2. Composite Mixture Analysis ........................................................................................ 13–1
13.2.3. Composite Gas Analysis .............................................................................................. 13–2

13.3. Doing a Multiple Species Analysis .............................................................................................. 13–2

13.3.1. Establish the Species .................................................................................................. 13–2
13.3.2. Choose an Algebraic Species ...................................................................................... 13–3
13.3.3. Adjust Output Format ................................................................................................ 13–3
13.3.4. Set Properties ............................................................................................................. 13–3
13.3.5. Specify Boundary Conditions ...................................................................................... 13–4
13.3.6. Set Relaxation and Solution Parameters ...................................................................... 13–4

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

viii

ANSYS Fluids Analysis Guide

13.4. Doing a Heat Exchanger Analysis Using Two Species ................................................................. 13–5
13.5. Example Analysis Mixing Three Gases ........................................................................................ 13–7

14. Advection Discretization Options ................................................................................................... 14–1

14.1. Introduction ............................................................................................................................. 14–1
14.2. Using SUPG and COLG .............................................................................................................. 14–1
14.3. Strategies for Difficult Solutions ................................................................................................ 14–2

II. Acoustics

15. Acoustics .......................................................................................................................................... 15–1

15.1. What Is Acoustics? .................................................................................................................... 15–1

15.1.1. Types of Acoustic Analysis .......................................................................................... 15–1

15.2. Solving Acoustics Problems ...................................................................................................... 15–1
15.3. Building the Model ................................................................................................................... 15–1

15.3.1. Harmonic Acoustic Analysis Guidelines ....................................................................... 15–2

15.3.1.1. FLUID29 and FLUID30 ........................................................................................ 15–2
15.3.1.2. FLUID129 and FLUID130 .................................................................................... 15–2

15.4. Meshing the Model ................................................................................................................... 15–4

15.4.1. Step 1: Mesh the Interior Fluid Domain ....................................................................... 15–4
15.4.2. Step 2: Generate the Infinite Acoustic Elements .......................................................... 15–4
15.4.3. Step 3: Specify the Fluid-Structure Interface ................................................................ 15–5

15.5. Applying Loads and Obtaining the Solution .............................................................................. 15–6

15.5.1. Step 1: Enter the SOLUTION Processor ........................................................................ 15–6
15.5.2. Step 2: Define the Analysis Type ................................................................................. 15–6
15.5.3. Step 3: Define Analysis Options ................................................................................... 15–6
15.5.4. Step 4: Apply Loads on the Model ............................................................................... 15–7

15.5.4.1. Applying Loads Using the GUI ............................................................................ 15–8
15.5.4.2. Applying Loads Using Commands ...................................................................... 15–8
15.5.4.3. Load Types ........................................................................................................ 15–9

15.5.5. Step 5: Specify Load Step Options ............................................................................... 15–9

15.5.5.1. Dynamics Options ........................................................................................... 15–10
15.5.5.2. General Options ............................................................................................... 15–10
15.5.5.3. Output Controls ............................................................................................... 15–10

15.5.6. Step 6: Back Up Your Database ................................................................................. 15–10
15.5.7. Step 7: Apply Additional Load Steps (Optional) ......................................................... 15–11
15.5.8. Step 8: Finish the Solution ........................................................................................ 15–11

15.6. Reviewing Results ................................................................................................................... 15–11
15.7. Fluid-Structure Interaction ...................................................................................................... 15–11
15.8. Sample Applications ............................................................................................................... 15–12
15.9. Example 1: Fluid-Structure Coupled Acoustic Analysis (Command Method) .............................. 15–12
15.10. Example 2: Room Acoustic Analysis (Command Method) ....................................................... 15–13

III. Thin Film

16. Thin Film Analysis ........................................................................................................................... 16–1

16.1. Elements for Modeling Thin Films .............................................................................................. 16–1
16.2. Squeeze Film Analysis ............................................................................................................... 16–1

16.2.1. Static Analysis Overview ............................................................................................. 16–2
16.2.2. Harmonic Response Analysis Overview ....................................................................... 16–3
16.2.3. Flow Regime Considerations ...................................................................................... 16–4
16.2.4. Modeling and Meshing Considerations ....................................................................... 16–4
16.2.5. Analysis Settings and Options ..................................................................................... 16–5
16.2.6. Loads and Solution ..................................................................................................... 16–5

ANSYS Fluids Analysis Guide

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

16.2.7. Review Results ........................................................................................................... 16–6
16.2.8. Example Problem ....................................................................................................... 16–6

16.3. Modal Projection Method for Squeeze Film Analysis ................................................................ 16–10

16.3.1. Modal Projection Method Overview .......................................................................... 16–10
16.3.2. Steps in Computing the Damping Parameter Using the Modal Projection Tech-
nique .................................................................................................................................. 16–11

16.3.2.1. Modeling and Meshing .................................................................................... 16–12
16.3.2.2. Perform Modal Analysis ................................................................................... 16–12
16.3.2.3. Extracting Eigenvectors ................................................................................... 16–12
16.3.2.4. Performing a Harmonic Response Analysis and Extracting Damping Paramet-
ers ................................................................................................................................ 16–12

16.3.3. Example Problem Using the Modal Projection Method .............................................. 16–13
16.3.4. Damping Extraction for Large Signal Cases ................................................................ 16–18

16.4. Slide Film Damping ................................................................................................................. 16–18

16.4.1. Slide Film Damping Example .................................................................................... 16–20

Index ................................................................................................................................................. Index–1

List of Figures

2.1. Convergence Monitors Displayed by the GST Feature ........................................................................ 2–12
3.1. Internal Flow ...................................................................................................................................... 3–1
3.2. External Flow ...................................................................................................................................... 3–1
3.3. Structured Mesh ............................................................................................................................... 3–10
3.4. Unstructured Mesh ........................................................................................................................... 3–10
4.1. Diagram of the Square Cavity .............................................................................................................. 4–9
4.2. Plot of the Temperature Solution ...................................................................................................... 4–13
4.3. Plot of Streamline Contours .............................................................................................................. 4–14
4.4. Plot of Velocity Vectors ..................................................................................................................... 4–15
4.5. Plot of Flow Trace ............................................................................................................................. 4–16
6.1. Instantaneous Pressure Distributions at 0.001 ms .............................................................................. 6–11
6.2. Instantaneous Pressure Distributions at 0.012 ms .............................................................................. 6–11
7.1. Torsional Mirror at t = 0 Seconds ......................................................................................................... 7–1
7.2. Torsional Mirror at t = 2.5 Seconds ...................................................................................................... 7–2
7.3. Torsional Mirror at t = 7.5 Seconds ...................................................................................................... 7–2
7.4. Boundary Conditions for Moving Walls ................................................................................................ 7–3
7.5. Torsional Mirror Problem Description .................................................................................................. 7–8
7.6. Torsional Mirror Problem - Boundary Conditions ............................................................................... 7–10
7.7. Square Vessel with a Moving Wall ...................................................................................................... 7–15
7.8. Left Wall Displacement and Velocity .................................................................................................. 7–16
7.9. Moving Cylinder ............................................................................................................................... 7–18
7.10. Elements at 0 Seconds .................................................................................................................... 7–19
7.11. Elements at 22 Seconds ................................................................................................................... 7–19
7.12. Elements at 44 Seconds ................................................................................................................... 7–19
8.1. Three Types of Meshing ...................................................................................................................... 8–3
10.1. Direction of Positive Swirl Velocity VZ for Axisymmetric Models ....................................................... 10–1
10.2. Rotating Flow Problem ................................................................................................................... 10–3
10.3. Problem Schematic with Rotating Coordinate ................................................................................. 10–3
11.1. Typical Debug Files ......................................................................................................................... 11–3
13.1. Environment for a Typical Heat Exchanger Analysis .......................................................................... 13–5
15.1. Example of a 2-D Acoustic Model (Fluid Within a Structure) .............................................................. 15–2
15.2. Example of Absorption Element Application .................................................................................... 15–3

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

ANSYS Fluids Analysis Guide

15.3. Submerged Cylindrical Shell ............................................................................................................ 15–3
15.4. Mesh the Fluid Domain ................................................................................................................... 15–4
15.5. Add the Absorption Element on the Boundary ................................................................................. 15–5
15.6. Specify Fluid-Structure Interface ...................................................................................................... 15–6
16.1. Moving Plate above a Fixed Wall ..................................................................................................... 16–2
16.2. Perforated Plate Structure ............................................................................................................... 16–2
16.3. Pressure Distribution on a Plate at a Low Driving Frequency ............................................................ 16–3
16.4. Damping and Squeeze Stiffness Coefficients vs. Frequency .............................................................. 16–3
16.5. Coupling of Nodes at the Hole Periphery with the Center Node of a FLUID138 Element .................... 16–5
16.6. Pressure Distribution (Real Component) .......................................................................................... 16–7
16.7. Pressure Distribution (Imaginary Component) ................................................................................. 16–8
16.8. Modal Projection Technique for Damping Characterization ............................................................ 16–10
16.9. Damping and Squeeze Stiffness Parameters for a Rectangular Plate ............................................... 16–11
16.10. Fluidic Cross-Talk between Transverse and Rotational Motion ...................................................... 16–13
16.11. Time-Transient Response from Voltage Pulse ............................................................................... 16–17
16.12. Slide Film Damping at Low and High Frequencies ........................................................................ 16–19
16.13. Viscous Slide Film Element FLUID139 ........................................................................................... 16–20
16.14. Comb Drive Resonator ................................................................................................................ 16–21
16.15. Displacement of Central Mass ...................................................................................................... 16–21
16.16. Real and Imaginary Current ......................................................................................................... 16–22

List of Tables

2.1. 2-D Solid Elements .............................................................................................................................. 2–1
3.1. Boundary Conditions at Intersections ................................................................................................ 3–13
4.1. Command Family and GUI Path Used to Apply Loads .......................................................................... 4–2
4.2. Load Commands for a FLOTRAN Thermal Analysis ............................................................................... 4–2
5.1. Specifying Values for Time Steps ......................................................................................................... 5–2
5.2. Saving Analysis Results for Processing ................................................................................................. 5–3
7.1. Interface Boundary Conditions ............................................................................................................ 7–4
7.2. Element Qualities ............................................................................................................................... 7–6
7.3. Remeshing Limitations ....................................................................................................................... 7–7
7.4. Quality Requirements ....................................................................................................................... 7–18
9.1. Units for Thermal Quantities ............................................................................................................... 9–1
9.2. Energy Units for Incompressible Analyses with Viscous Heating ........................................................... 9–2
9.3. Units for the AIR Property Type ........................................................................................................... 9–2
9.4. Property types for Value ...................................................................................................................... 9–4
9.5. Property Database Format ................................................................................................................ 9–11
10.1. Coordinate System Specification ..................................................................................................... 10–1
12.1. Advection Scheme Defaults ............................................................................................................ 12–1
12.2. SIMPLEF and SIMPLEN Performance Results ..................................................................................... 12–2
15.1. Loads Applicable in an Acoustic Analysis ......................................................................................... 15–7
15.2. Commands for Applying Loads in Acoustic Analysis ......................................................................... 15–8
15.3. Load Step Options for a Harmonic Acoustic Analysis ...................................................................... 15–10
16.1. Thin Film Fluid Elements ................................................................................................................. 16–1
16.2. Load Options for Thin Film Fluid Elements ....................................................................................... 16–5
16.3. Beam Model Results Considering Perforated Holes .......................................................................... 16–7
16.4. Modal Damping Parameters for First Two Eigenfrequencies ........................................................... 16–14

ANSYS Fluids Analysis Guide

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

xii

Part I. CFD

Chapter 1: Overview of FLOTRAN CFD Analyses

1.1. What Is FLOTRAN CFD Analysis?

The ANSYS FLOTRAN derived product and the FLOTRAN CFD (Computational Fluid Dynamics) option to the
other ANSYS products offer you comprehensive tools for analyzing 2-D and 3-D fluid flow fields. Using either
product and the FLOTRAN CFD elements FLUID141 and FLUID142, you can achieve solutions for the following:

•

Lift and drag on an airfoil

•

The flow in supersonic nozzles

•

Complex, 3-D flow patterns in a pipe bend

In addition, you can use the features of ANSYS and ANSYS FLOTRAN to perform tasks including:

•

Calculating the gas pressure and temperature distributions in an engine exhaust manifold

•

Studying the thermal stratification and breakup in piping systems

•

Using flow mixing studies to evaluate potential for thermal shock

•

Doing natural convection analyses to evaluate the thermal performance of chips in electronic enclosures

•

Conducting heat exchanger studies involving different fluids separated by solid regions

1.2. Types of FLOTRAN Analyses

You can perform these types of FLOTRAN analyses:

•

Laminar or turbulent

•

Thermal or adiabatic

•

Free surface

•

Compressible or incompressible

•

Newtonian or Non-Newtonian

•

Multiple species transport

These types of analyses are not mutually exclusive. For example, a laminar analysis can be thermal or adiabatic.
A turbulent analysis can be compressible or incompressible.

To solve any analysis involving the flow of fluid, use either of the following:

Command(s): FLDATA1,SOLU,FLOW,TRUE
GUI: Main Menu> Solution> FLOTRAN Set Up> Solution Options

1.2.1. Laminar Flow Analysis

In these analyses, the velocity field is very ordered and smooth, as it is in highly viscous, slow-moving flows. The
flow of some oils also can be laminar.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

1.2.2. Turbulent Flow Analysis

Turbulent flow analyses deal with problems where velocities are high enough and the viscosity is low enough
to cause turbulent fluctuations. The two-equation turbulence model in ANSYS enables you to account for the
effect of the turbulent velocity fluctuations on the mean flow.

Laminar and turbulent flows are considered to be incompressible if density is constant or if the fluid expends
little energy in compressing the flow. The temperature equation for incompressible flow neglects kinetic energy
changes and viscous dissipation.

1.2.3. Thermal Analysis

Often, the solution for the temperature distribution throughout the flow field is of interest. If fluid properties do
not vary with temperature, you can converge the flow field without solving the temperature equation. In a con-
jugate heat transfer problem, the temperature equation is solved in a domain with both fluid and non-fluid (that
is, solid material) regions. In a natural convection problem, the flow results mainly or solely from density gradients
brought about by temperature variations. Most natural convection problems, unlike forced convection problems,
have no externally applied flow sources.

1.2.4. Compressible Flow Analysis

For high velocity gas flows, changes in density due to strong pressure gradients significantly influence the nature
of the flow field. ANSYS uses a different solution algorithm for compressible flow.

1.2.5. Non-Newtonian Fluid Flow Analysis

A linear relationship between the stress and rate-of-strain cannot describe many fluid flows adequately. For such
non-Newtonian flows, the ANSYS program provides three viscosity models and a user-programmable subroutine.

1.2.6. Multiple Species Transport Analysis

This type of analysis is useful in studying the dispersion of dilute contaminants or pollutants in the bulk fluid
flow. In addition, you can use multiple species transport analysis for heat exchanger studies where two or more
fluids (separated by walls) may be involved.

1.2.7. Free Surface Analysis

Free surface analyses deal with problems involving a unconstrained gas-liquid surface. You can use this type of
analysis to solve two dimensional planar and axisymmetric problems such as flow over a dam and tank sloshing.

1.3. About GUI Paths and Command Syntax

Throughout this document, you will see references to ANSYS commands and their equivalent GUI paths. Such
references use only the command name, because you do not always need to specify all of a command's arguments,
and specific combinations of command arguments perform different functions. For complete syntax descriptions
of ANSYS commands, consult the ANSYS Commands Reference.

The GUI paths shown are as complete as possible. In many cases, choosing the GUI path as shown will perform
the function you want. In other cases, choosing the GUI path given in this document takes you to a menu or
dialog box; from there, you must choose additional options that are appropriate for the specific task being per-
formed.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

1–2

Chapter 1: Overview of FLOTRAN CFD Analyses

For the thermal related analyses described in this guide, specify the material you will be simulating using an in-
tuitive material model interface. This interface uses a hierarchical tree structure of material categories, which is
intended to assist you in choosing the appropriate model for your analysis. See Section 1.2.4.4: Material Model
Interface in the ANSYS Basic Analysis Guide for details on the material model interface.

Section 1.3: About GUI Paths and Command Syntax

1–3

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

1–4

Chapter 2: The Basics of FLOTRAN Analysis

2.1. Characteristics of the FLOTRAN Elements

The ANSYS FLOTRAN elements, FLUID141 and FLUID142, solve for 2-D and 3-D flow, pressure, and temperature
distributions in a single phase viscous fluid. For these elements, the ANSYS program calculates velocity compon-
ents, pressure, and temperature from the conservation of three properties: mass, momentum, and energy.

Table 2.1 2-D Solid Elements

DOFs

Shape or Characteristic

Dimens.

Element

Fluid velocity, pressure, temperature, turbu-
lent kinetic energy, turbulent energy dissip-
ation, multiple species mass fractions for up
to six fluids

Quadrilateral, four nodes or triangle, three
nodes

2-D

FLUID141

Fluid velocity, pressure, temperature, turbu-
lent kinetic energy, turbulent energy dissip-
ation, multiple species mass fractions for up
to six fluids

Hexahedral, eight nodes or tetrahedral, four
nodes or wedge, six nodes or pyramid, five
nodes; tetrahedral and hexahedral elements
can be combined by pyramids

3-D

FLUID142

2.1.1. Other Element Features

Other features of the FLOTRAN elements include:

•

A two-equation turbulence model for simulating turbulent flows.

•

Derived results, such as Mach number, pressure coefficient, total pressure, shear stress, y plus at walls,
and stream function for fluid analyses and heat flux and heat transfer (film) coefficient for thermal analyses.

•

Fluid boundary conditions, including velocities, pressures, and the turbulence quantities kinetic energy
and kinetic energy dissipation rate. You may supply specific values of the turbulence quantities at the
inlet, but the FLOTRAN default boundary conditions suffice if the entrance is not close to the regions of
primary interest.

•

Thermal boundary conditions, including temperature, heat flux, volumetric heat sources, and heat transfer
(film) coefficient.

You can solve problems in Cartesian, cylindrical, polar, and axisymmetric coordinate systems. If a problem is
axisymmetric, activating a swirl option allows you to calculate a velocity component normal to the axisymmetric
plane.

2.2. Considerations and Restrictions for Using the FLOTRAN Elements

The FLOTRAN elements have some limitations:

•

You cannot change the problem domain during a single analysis.

•

Certain features of the ANSYS program do not work with the FLOTRAN elements.

•

You cannot use certain commands or menu paths with the FLOTRAN elements.

•

If you use the ANSYS GUI, only the features and options called for in the FLOTRAN SetUp portion of the
menus and dialog boxes will appear.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

2.2.1. Limitations on FLOTRAN Element Use

When you are using the FLOTRAN elements, you should avoid using certain ANSYS features and commands, or
if you do choose to use them, be aware that they have slightly different uses with the FLOTRAN elements. This
does not mean that every command not listed here will work with FLOTRAN elements. ANSYS informs you if you try
to issue a command that is invalid.

When using the FLOTRAN elements, keep the following points in mind:

•

You cannot combine the FLOTRAN elements with other elements.

•

The nodal coordinate system must be identical to the global coordinate system.

•

The /CLEAR command does not destroy an existing FLOTRAN results file (Jobname.RFL), thus preventing
you from inadvertently destroying a results file that took much time and effort to create. Existing Job-
name.RFL file names will become Jobname.RFO file names if the number of nodes in the model has
changed since the Jobname.RFL file creation. You should remove unwanted results files at the system
level.

•

In FLOTRAN, the CP command enforces periodic boundary conditions by coupling all degrees of freedom
between two nodes. You should not use the CP command to couple more than two nodes or to couple
a subset of the degrees of freedom. You should only use this command to couple all degrees of freedom
of one node on a periodic boundary face to one other node on another periodic boundary face.

You cannot couple nodes on the same element, and you may have difficulty coupling nodes on adjacent
elements.

•

The ADAPT macro does not work with FLOTRAN.

•

You cannot use the ANTYPE command to invoke a transient analysis with the FLOTRAN element. (See
Chapter 5, “FLOTRAN Transient Analyses”.)

•

FLOTRAN analyses do not support automatic time stepping. For more information, see Chapter 5, “FLOTRAN
Transient Analyses”.

•

If you specify nodal heat generation loads via commands BFCUM, BFDELE, or BFUNIF, ANSYS uses load
values specified with the BFE command instead.

•

The commands CE, CECMOD, CEDELE, and CEINTF do not work with FLOTRAN.

•

The CNVTOL command does not set convergence tolerances with FLOTRAN as it does for other analyses.
For information about FLOTRAN convergence, see Section 2.6.1: Deciding How Many Global Iterations to
Use.

•

The symmetry and antisymmetry conditions that the DSYM command specifies are not appropriate for
FLOTRAN. Chapter 3, “FLOTRAN Laminar and Turbulent Incompressible Flow” explains how to specify
flow symmetry boundary conditions for FLOTRAN.

•

FLOTRAN does not support angular acceleration vectors for rotating coordinate systems.

•

In a FLOTRAN analysis, the command FLDATA4,TIME (rather than the DELTIM command) specifies a time
step for a load step.

•

For FLOTRAN, you cannot use the DESOL command or the PRESOL command to modify HEAT, FLOW, or
FLUX nodal results.

•

FLOTRAN does not permit extrapolation of integration point results to nodes (via the ERESX command).

•

FLOTRAN does not allow you to generate elements through reflections. Although not recommended,
FLOTRAN will execute properly if you generate reflected elements using a different element type and you
subsequently switch to the FLOTRAN element type.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

2–2

Chapter 2: The Basics of FLOTRAN Analysis

•

In FLOTRAN analyses, you cannot ramp loads via the KBC command. The FLOTRAN command
FLDATA4,TIME,BC, however, is analogous to the ANSYS command KBC, except that the default for FLOTRAN
is a step change.

•

Load case operations, such as those performed by the LCCALC, LCDEF, LCFACT, and LCFILE commands,
are not allowed in a FLOTRAN analysis.

•

Do not use the LSWRITE or LSSOLVE command in a FLOTRAN analysis. Use the SOLVE command to start
a FLOTRAN solution.

•

The convergence tool invoked with the NCNV command does not apply to the FLOTRAN segregated
solver.

•

Do not use the NEQIT command, which defines the number of equilibrium iterations for a nonlinear
solution, in a FLOTRAN analysis.

•

FLOTRAN requires the nodal and global Cartesian coordinate systems to be the same. Therefore, you
cannot use the rotational fields on the N, NMODIF, and NROTAT commands.

•

In a FLOTRAN analysis, the commands FLDATA2,ITER, FLDATA4,TIME, and FLDATA4A,STEP control items
written to the results files (Jobname.RFL and Jobname.PFL

•

FLOTRAN does not permit user programmable elements, such as those specified via the NSVR command.

•

In a FLOTRAN analysis, the commands FLDATA2,ITER and FLDATA4,TIME control items written to the
database.

•

The PRNLD command does not apply to FLOTRAN, because it does not store boundary conditions as
printable element nodal loads.

•

Node reaction solutions, such as those produced by the PRRSOL command, are not available for FLOTRAN.

•

The partial and predefined solution option (called by the PSOLVE command) does not apply to the FLO-
TRAN segregated solver.

•

The TIME command, which associates boundary conditions with a particular time value, does not apply
to FLOTRAN.

•

FLOTRAN analyses use the FLDATA1,SOLU command instead of the TIMINT command to specify transient
load steps.

•

FLOTRAN analyses use the FLDATA4,TIME command instead of the TRNOPT command to specify transient
analysis options.

•

The RESCONTROL command does not apply to FLOTRAN. Some of the functionality of RESCONTROL is
provided with the FLDATA32,REST command.

•

For FLOTRAN, you cannot use the DK command to define DOF constraints at keypoints.

2.3. Overview of a FLOTRAN Analysis

A typical FLOTRAN analysis consists of seven main steps:

Determine the problem domain.

Determine the flow regime.

Create the finite element mesh.

Apply boundary conditions.

Set FLOTRAN analysis parameters.

Solve the problem.

Section 2.3: Overview of a FLOTRAN Analysis

2–3

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Examine the results.

2.3.1. Determining the Problem Domain

You need to determine the proper domain for each problem you analyze. Locate the boundaries of the problem
where conditions are known. If you do not know precise conditions and must make assumptions about them,
do not locate boundaries too close to the regions of greatest interest or near regions that have steep gradients
in the solution variables.

Sometimes, you may not realize that steep gradients occur too near the outlet or in some other region until you
see the analysis results. Should this happen, you can re-analyze the problem with a different problem domain.

For specific recommendations on determining problem domain, see the sections discussing the various flow
phenomena.

2.3.2. Determining the Flow Regime

You need to estimate the character of the flow. The character is a function of the fluid properties, geometry, and
the approximate magnitude of the velocity field.

Fluid flow problems that FLOTRAN solves will include gases and liquids, the properties of which can vary signi-
ficantly with temperature. The flow of gases is restricted to ideal gases. You must determine whether the effect
of temperature on fluid density, viscosity, and thermal conductivity is important. In many cases, you can get
adequate results with constant properties.

To assess whether you need the FLOTRAN turbulence model, use an estimate of the Reynolds number, which
measures the relative strengths of the inertial and viscous forces. (See Chapter 3, “FLOTRAN Laminar and Turbulent
Incompressible Flow” for more information.)

To determine whether you need to use the compressible option, estimate the Mach number. (See Chapter 8,
“FLOTRAN Compressible Analyses”) The Mach number at any point in the flow field is the ratio of the fluid speed
and the speed of sound. At Mach numbers above approximately 0.3, consider using the compressible solution
algorithm. At Mach numbers above approximately 0.7, you can expect significant differences between incom-
pressible and compressible results. You may want to compare results from each algorithm for a representative
problem.

2.3.3. Creating the Finite Element Mesh

You will need to make assumptions about where the gradients are expected to be the highest, and you must
adjust the mesh accordingly. For example, if you are using the turbulence model, then the region near the walls
must have a much denser mesh than would be needed for a laminar problem. If it is too coarse, the original mesh
may not capture significant effects brought about through steep gradients in the solution. Conversely, elements
may have very large aspect ratios with the long sides along directions with very low gradients.

For the most accurate results, use mapped meshing. It more effectively maintains a consistent mesh pattern
along the boundary. You can do this by issuing the command MSHKEY,1 (Main Menu> Preprocessor> Meshing>
Mesh>

entity

> Mapped).

In some cases, you may wish to use hexahedral elements to capture detail in high-gradient regions and tetrahedral
elements in less critical regions. As described in Section 7.3.9: Creating Transitional Pyramid Elements in the
ANSYS Modeling and Meshing Guide you can instruct ANSYS to automatically create pyramid elements at the in-
terface.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

2–4

Chapter 2: The Basics of FLOTRAN Analysis

For flow analysis, especially turbulent, you should not use pyramid elements in the region near the walls because
it may lead to inaccuracies in the solution.

Wedge elements can be useful when a complex area can be easily meshed with triangles that are then extruded.
For a quick solution, you can use wedge elements in the region near the walls. However, for accurate results,
you should use hexahedral elements in those regions.

Wedge elements are considered to be degenerate hexahedral elements. When using the ANSYS MeshTool (Main
Menu> Preprocessor> Meshing> MeshTool) to sweep triangles into wedges, you must select Hex elements.

2.3.4. Applying Boundary Conditions

You can apply boundary conditions before or after you mesh the domain. Consider every model boundary. If a
condition is not specified for a dependent variable, a zero gradient of that value normal to the surface is assumed.

You can change boundary conditions between restarts. If you need to change a boundary condition or accidentally
omit it, you do not need to restart your analysis unless the change causes instabilities in the analysis solution.

2.3.5. Setting FLOTRAN Analysis Parameters

In order to use options such as the turbulence model or solution of the temperature equation, you must activate
them. Specific items to be set, such as fluid properties, are a function of the type of flow problem at hand. Other
sections in this document recommend parameter settings for various types of flow.

2.3.6. Solving the Problem

You can monitor solution convergence and stability of the analysis by observing the rate of change of the solution
and the behavior of relevant dependent variables. These variables include velocity, pressure, temperature, and
(if necessary) turbulence quantities such as kinetic energy (degree of freedom ENKE), kinetic energy dissipation
rate (ENDS), and effective viscosity (EVIS).

An analysis typically requires multiple restarts.

2.3.7. Examining the Results

You can postprocess output quantities and examine the results in the output files. Use your engineering judgment
when examining the results to evaluate the plausibility and consistency of the overall analysis approach, how
specific properties are used, and the conditions imposed.

2.4. Files the FLOTRAN Elements Create

You perform most fluid flow analyses in ANSYS by stopping the analysis job and then restarting it multiple times.
Often, analysts change parameters such as relaxation factors or turn options (such as solution of the temperature
equation) on or off between restarts. Each time you continue a job, the ANSYS program appends data to all of
the files that its FLOTRAN element creates.

The following list explains all files that a FLOTRAN element creates. A discussion of the residual file appears at
the end of this section.

•

The results file, Jobname.RFL, contains nodal results.

•

The print file, Jobname.PFL, contains input convergence monitors, and inlet/outlet summaries.

•

The wall file, Jobname.RSW, contains wall shear stress and Y-plus information.

Section 2.4: Files the FLOTRAN Elements Create

2–5

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

•

The residual file, Jobname.RDF, contains the nodal residuals.

•

The debug file, Jobname.DBG, contains information about algebraic solver performance.

•

The results backup file, Jobname.RFO, contains a copy of the results file data.

•

The restart file, Jobname.CFD, contains FLOTRAN data structures.

•

The domain file, (jobname.pv_0000

) for use by ICEM CFD's PV3 postprocessing visualization tool.

2.4.1. The Results File

The results of a FLOTRAN analysis are not stored in the ANSYS database automatically. At the end of every solution,
the ANSYS program adds a set of results to the results file, Jobname.RFL. You have some control over the content
of the results file and how often ANSYS updates it. The defaults given in the description of the FLDATA5,OUTP
command in the ANSYS Commands Reference reflect FLOTRAN's determination of what the results file should
store based on the options you choose.

The ANSYS program is flexible about how many sets of results you can store for a steady-state FLOTRAN analysis.
Keeping sets of results from earlier executions has advantages: you can compare changes that occurred between
sets of results, and you can continue an analysis from its earlier stages using different options or relaxation
parameters.

The ANSYS program stores a set of results when you begin an analysis (before the first iteration), then stores
results again when one of the termination criteria is reached. Between those events, you can append the results
to the Jobname.RFL file. Storing intermediate sets of results enables you to continue the analysis from an
earlier stage with different options and features activated, for example to enhance stability.

We recommend that you use ANSYS' overwrite frequency option because it allows you to periodically store and
update a temporary set of results. Using this option ensures that a useful set of results will exist should you need
to restart an analysis after a power failure or other system interruption. The next regularly scheduled output of
results overwrites the temporary results set. You can accomplish the same thing by instructing ANSYS to append
data to the results file more often; however, this method inflates the size of the results file.

To set the overwrite frequency, use either of the following:

Command(s): FLDATA2,ITER,OVER,

Value

GUI: Main Menu> Solution> FLOTRAN Set Up> Execution Ctrl

To set the append frequency, use either of the following:

Command(s): FLDATA2,ITER,APPE,

Value

GUI: Main Menu> Solution> FLOTRAN Set Up> Execution Ctrl

2.4.2. The Print File (Jobname.PFL)

The Jobname.PFL file contains a complete record of all FLOTRAN input parameters, including properties and
solution options. This information is recorded each time a SOLVE is issued so as to provide a complete account
of the analysis history. In addition, all convergence monitors are recorded for all active values. A results summary,
showing maximum and minimum values of each property and degree of freedom, is provided at a user-determined
frequency. Average values are also recorded. The mass flow boundaries are identified and a mass balance is
calculated. Finally, all heat transfer information is summarized for all heat transfer and heat sources.

2.4.3. The Nodal Residuals File

The nodal residuals file, Jobname.RDF, shows you how well the current solution is converged. At every stage
in the solution procedure, the flow, property, and temperature fields are used to calculate coefficient matrices

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

2–6

Chapter 2: The Basics of FLOTRAN Analysis

and forcing functions for each DOF. If a solution is converged completely, these matrices and forcing functions
will produce the same velocity field used to generate them and the residuals of the matrix equation will be very
small. You must request at least one global iteration to obtain a nodal residual file.

If a solution oscillates, however, the magnitude of the residuals shows where the maximum errors are. (The main
diagonal entries of the matrix normalize the residuals.) This normalization enables you to compare directly the
value of the DOF and the value of its residual.

To calculate residuals for every active degree of freedom and output them to the residuals file, do either of the
following:

Command(s): FLDATA5,OUTP,RESI,TRUE
GUI: Main Menu> Solution> FLOTRAN SetUp> Additional Out> Residual File

To read the residuals file, either issue the FLREAD command (Main Menu> General Postproc> FLOTRAN 2.1A).
The residuals are postprocessed with the label associated with the DOF (for instance, TEMP or PRES for the
temperature or pressure residuals).

2.4.4. The Restart File

By default, FLOTRAN calculates data structures at the beginning of a restart of an analysis. These calculations
may take considerable time for large models. To avoid recalculation, you can opt to have FLOTRAN store the
data structures in the Jobname.CFD file. FLOTRAN creates this file from information in the ANSYS database (but
the file is not required for restarts).

To write to or read from the Jobname.CFD file, use either of the following methods before the restart:

Command(s): FLDATA32,REST,RFIL,T
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Restart Options> CFD Restart File

You can toggle the RFIL state on (TRUE) or off (FALSE). If is on, ANSYS reads the restart file when FLOTRAN begins
to execute. If no restart file exists, one will be created.

If you are restarting an analysis with updated boundary conditions, you must overwrite an existing .CFD file in
order to use the new conditions. To overwrite the file, use either of the following methods:

Command(s): FLDATA32,REST,WFIL,T
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Restart Options> CFD Restart File

This will cause FLOTRAN to create a new restart file during the next load step, and automatically sets the RFIL
state to False. After the restart that has created the new file completes, issue the FLDATA32,REST,RFIL,TRUE
command so that subsequent restarts use the new Jobname.CFD restart file.

2.4.5. The Domain File

Domain files are used by ICEM CFD's PV3 postprocessor visualization tool. In addition to nodal results these files
contain information to define the finite element model, including node locations, element topology, element
connectivity, and family information concerning predefined ANSYS components. They also contain load step,
substep, cumulative iteration, and time point values.

2.4.6. Restarting a FLOTRAN Analysis

You can restart the FLOTRAN analysis from any set of results in the Jobname.RFL file or from a different .RFL
file. You can base the restart on the set number (

Label

= NSET), the global iteration number (

Label

= ITER), the

load step/subset numbers (

Label

= LSTP), or the transient analysis time (

Label

= TIME). You determine the restart

criteria by doing either of the following:

Section 2.4: Files the FLOTRAN Elements Create

2–7

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

•

Issue the command FLDATA32,REST,

Label

Value

. Specify one of the labels listed above in place of

Label

The

Value

argument causes values associated with the other criteria to be zeroed. Once invoked, the

behavior is turned off in the database by setting all the criteria to zero. If you are restarting from a different
results file, you also need to specify the filename, extension, and directory of that file.

•

Choose menu path Main Menu> Preprocessor> FLOTRAN Set Up> Restart Options> Restart/Iteration
(or Restart/Load step, Restart/Set, etc.)

If you specify invalid criteria, ANSYS notifies you and (if the program is operating in batch mode) terminates the
analysis.

When you restart an analysis, ANSYS copies the original results file to the file Jobname.RSO and places the restart
point, all previous results sets, and all subsequent results sets in the new Jobname.RFL file. If the

Value

input

on the FLDATA32,REST command is negative, creation of the Jobname.RSO file is blocked. FLOTRAN uses the
absolute value of the number specified for

Value

If a results file name is entered in the

Fname

field of the FLDATA32,REST command, FLOTRAN interpolates those

results onto the current mesh in the database, regardless of whether or not the mesh has changed. This causes
the convergence monitors to start again from zero. This restart is different than a restart without a file name
specification. However, the results quickly converge to the original solution.

2.5. Convergence and Stability Tools

The ANSYS program offers several tools to help with convergence and solution stability. The ANSYS, Inc. Theory
Reference explains how they are implemented.

2.5.1. Relaxation Factors

The relaxation factor is the fraction of the change between the old solution and the newly calculated solution
that is added to the old solution, giving the results for the new global iteration. The relaxation factors for every
component must be between 0.0 (resulting in no update to the degree of freedom or property) and 1.0 inclusive.
You set relaxation factors via either of the following:

Command(s): FLDATA25,RELX,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Relax/Stab/Cap> DOF Relaxation
Main Menu> Preprocessor> FLOTRAN Set Up> Relax/Stab/Cap> Prop Relaxation
Main Menu> Solution> FLOTRAN Set Up> Relax/Stab/Cap> DOF Relaxation
Main Menu> Solution> FLOTRAN Set Up> Relax/Stab/Cap> Prop Relaxation

Note — See the description of the FLDATA25,RELX command in the ANSYS Commands Reference for lists
of degree of freedom and property component names.

2.5.2. Inertial Relaxation

Inertial relaxation of the equation set for a DOF provides diagonal dominance to make a solution stable. Hypo-
thetically, when a solution is converged in the absence of round off-error, the inertial relaxation applied does
not affect the value of the answer. However, in real situations, some round off-error always occurs, so the inertial
relaxation may affect your solution.

You can apply inertial relaxation to the momentum equations (MOME), turbulence equations (TURB), the pressure
equation (PRES), and the temperature equation (TEMP). To do so, use either of these methods:

Command(s): FLDATA26,STAB,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Relax/Stab/Cap> Stability Parms
Main Menu> Solution> FLOTRAN Set Up> Relax/Stab/Cap> Stability Parms

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

2–8

Chapter 2: The Basics of FLOTRAN Analysis

The inertial relaxation factor is in the denominator of the term added, so smaller values have a greater effect.
Typical useful values range between 1.0 (mild) and 1.0 x 10

-7

(severe).

2.5.3. Modified Inertial Relaxation

Modified inertial relaxation adds a local positive value to the diagonal term to guarantee a positive diagonal.

You can apply modified inertial relaxation to the momentum equations (MOME), turbulence equations (TURB),
and the temperature equation (TEMP). To do so, use either of these methods:

Command(s): FLDATA34,MIR,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Relax/Stab/Cap> MIR Stabilization
Main Menu> Solution> FLOTRAN Set Up> Relax/Stab/Cap> MIR Stabilization

A larger modified inertial relaxation factor gives a more robust scheme, but it may yield a slower convergence.
The recommended range is 0.1 to 1.0.

You should consider inertial relaxation and modified inertial relaxation to be mutually exclusive.

2.5.4. Artificial Viscosity

Artificial viscosity smooths the velocity solution in regions of steep gradients. It has proven useful in aiding
convergence of compressible problems and in smoothing velocity solutions in incompressible problems with
distributed resistances. For incompressible analyses, you should keep the artificial viscosity within an order of
magnitude of the effective viscosity.

To apply artificial viscosity, use either of these methods:

Command(s): FLDATA26,STAB,VISC,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Relax/Stab/Cap> Stability Parms
Main Menu> Solution> FLOTRAN Set Up> Relax/Stab/Cap> Stability Parms

2.5.5. DOF Capping

DOF capping allows you to prevent variables from going out of boundaries you specify. You can limit the velo-
cities, pressure, and temperature degrees of freedom (VY, VY, VZ, PRES, TEMP). To do this, use either of these
methods:

Command(s): FLDATA31,CAPP
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Relax/Stab/Cap> Results Capping
Main Menu> Solution> FLOTRAN Set Up> Relax/Stab/Cap> Results Capping

Velocity capping eliminates the effects of velocity spikes on properties, which may occur in the early stages of
convergence. Capping is especially suited to compressible analyses, where velocity spikes can cause kinetic energy
terms great enough to produce negative static temperatures. When a degree of freedom is capped, ANSYS prints
a message along with the convergence monitor printout.

The pressure value calculated by the solution of the pressure equation is capped, not the relaxed value. Therefore,
if you introduce pressure capping upon restarting an analysis, pressure values may still be outside the caps.

Capping applies to relative values of pressure and absolute values of temperature.

You should cap the total temperature when performing compressible thermal analyses. It will help ensure neg-
ative properties do not enter the calculations.

Caution: When velocities are capped, conservation of mass may not be enforced.

Section 2.5: Convergence and Stability Tools

2–9

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

2.5.6. The Quadrature Order

You have control over the quadrature order. In axisymmetric problems, the quadrature order automatically is
set to 2 upon solution. This is because quadrature orders of 2 produce more accurate results for problems with
irregularly shaped elements. The quadrature order is also automatically set to 2 upon solution for 3-D problems
using cylindrical coordinates.

If you notice anomalous results near a region of skewed hexahedral elements, reset the quadrature order to 2.
There might be a problem with the results when the included angles of the hexahedra exceed 120 degrees.

You can change the quadrature order for momentum diffusion or source, pressure diffusion or source, thermal
diffusion or source, turbulent diffusion or source, using either of the following:

Command(s):

FLDATA30,QUAD,

Label

Value

(

Label

is the element integral to change quadrature for, and

Value

is the number of integration points).

GUI:

Main Menu> Preprocessor> FLOTRAN Set Up> Mod Res/Quad Ord> CFD Quad Orders
Main Menu> Solution> FLOTRAN Set Up> Mod Res/Quad Ord> CFD Quad Orders

For more information on quadrature order, refer to the description of the FLDATA30,QUAD command in the
ANSYS Commands Reference.

2.6. What to Watch For During a FLOTRAN Analysis

This section describes what happens in a FLOTRAN analysis and how to evaluate how the analysis is proceeding.

2.6.1. Deciding How Many Global Iterations to Use

A FLOTRAN analysis is nonlinear and uses a sequential solution, so the first thing you must do is decide how
many global iterations should be executed. A global iteration is the solution, in sequence, of all relevant governing
equations followed by any fluid property updates that are needed.

In a transient simulation, a time step loop exists around the global iteration loop.

During a global iteration, the ANSYS Multiphysics program or ANSYS FLOTRAN obtains approximate solutions
to the momentum equation and uses them as forcing functions to solve a pressure equation based on conservation
of mass. ANSYS uses the resulting pressures to update the velocities so that the velocity field conserves mass. If
you request it, the ANSYS program solves the temperature equation and updates temperature dependent
properties.

Finally, if you have activated the turbulence model, the equations are solved and the program uses the turbulent
kinetic energy and dissipation rate to calculate the effective viscosity and thermal conductivity. Effective viscosity
and thermal conductivity replace, respectively, the laminar viscosity and thermal conductivity to model the effect
of turbulence on the mean flow.

To specify how many global iterations a FLOTRAN analysis should execute, use either of the following:

Command(s): FLDATA2,ITER,EXEC,

Value

(

Value

is the number of iterations.)

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Execution Ctrl
Main Menu> Solution> FLOTRAN Set Up> Execution Ctrl

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

2–10

Chapter 2: The Basics of FLOTRAN Analysis

2.6.2. Convergence Monitors

As a FLOTRAN simulation proceeds, ANSYS calculates convergence monitors for each degree of freedom every
global iteration. Convergence monitors are computed for velocities (VY, VY, VZ), pressure (PRES), temperature
(TEMP), turbulent kinetic energy (ENKE), kinetic energy dissipation rate (ENDS), and any active species transport
equations (SP01-SP06).

The convergence monitors are a normalized measure of the solution's rate of change from iteration to iteration.
Denoting by the general field variable,

Φ, any DOF, the convergence monitor is defined as follows:

ConvMon

−

∑

The convergence monitor represents the sum of changes of the variable calculated from the results between
the current

th iteration and the previous (

-1)

iteration, divided by the sum of the current values. The summation

is performed over all

nodes, using the absolute values of the differences.

Available in both batch and interactive sessions, the Graphical Solution Tracking (GST) feature displays the
computed convergence monitors while the solution is in process. Be default, GST is ON for interactive sessions
and OFF for batch runs. To turn GST on or off, use either of the following:

Command(s): /GST
GUI: Main Menu> Solution> Load Step Opts> Output Ctrls> Grph Solu Track

Figure 2.1: “Convergence Monitors Displayed by the GST Feature” shows two typical GST displays:

Section 2.6: What to Watch For During a FLOTRAN Analysis

2–11

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Figure 2.1 Convergence Monitors Displayed by the GST Feature

(a) Steady-state simulation, (b) Transient simulation

In Figure 2.1: “Convergence Monitors Displayed by the GST Feature” (b), a plot of a transient FLOTRAN solution,
each "spike" on the plot indicates the beginning of a new time step.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

2–12

Chapter 2: The Basics of FLOTRAN Analysis

After perhaps some initial fluctuations, convergence monitors will decrease as the analysis approaches conver-
gence. How small the numbers become depends on several factors, such as:

•

Complexity of the geometry

•

Adequacy of the finite element mesh in regions with steep gradients

•

The severity of the turbulence levels, indicated by the flow Reynolds number

•

Development of the flow near outlet boundaries

Points to remember when using graphical solution tracking include:

•

The GST feature is available for FLOTRAN analyses and also for structural, thermal, and electromagnetic
analyses containing nonlinearities. For information about using GST to track convergence in non-FLOTRAN
analyses, see the ANSYS Thermal Analysis Guide, the ANSYS Low-Frequency Electromagnetic Analysis Guide,
and the ANSYS Structural Analysis Guide.

•

GST can display up to ten curves at the same time. (Your model can include more than ten DOFs, but only
the first ten will be displayed.)

•

When the GST begins its plotting, ANSYS displays a dialog box with a STOP button. You can stop the
solution at any time by clicking on this button. To restart it, issue SOLVE or choose Main Menu> Solution>
Run FLOTRAN.

•

The time label which is positioned above the graph reveals the time at the last iteration.

2.6.3. Stopping a FLOTRAN Analysis

You can choose a target value for terminating a FLOTRAN analysis, based on the convergence monitors for each
degree of freedom falling below a certain value. To specify these values, use the following:

Command(s): FLDATA3,TERM,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Execution Ctrl
Main Menu> Solution> FLOTRAN Set Up> Execution Ctrl

See the ANSYS Commands Reference for the default values. Termination checks do not include inactive degrees
of freedom or degrees of freedom set to a negative value.

The analysis must satisfy convergence criteria for all active degrees of freedom, or complete the specified number
of global iterations requested. FLOTRAN terminates on the first condition satisfied. For information on terminating
transient analyses, see Chapter 5, “FLOTRAN Transient Analyses”.

To stop a FLOTRAN batch or background job in progress, place a file named Jobname.ABT in the subdirectory
from which the ANSYS job has been executed. The first line of this file should contain the word "terminate," and
should be left-justified. On Windows systems, you should also add a blank line at the end of the Jobname.ABT
file. FLOTRAN looks for the Jobname.ABT file during every global iteration. If it finds the file and reads the word
"terminate," it will finish that global iteration and terminate normally, writing the results to the Jobname.RFL
file and extending the Jobname.PFL file.

2.6.4. Pressure Results

For locked tetrahedral elements (those at a corner where two walls meet) there is a slight pressure anomaly.
ANSYS takes those elements out of the solution domain because all the nodes have boundary conditions. The
solution is correct in the domain. Use hexahedral elements to avoid this pressure anomaly.

Section 2.6: What to Watch For During a FLOTRAN Analysis

2–13

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

2.7. Evaluating a FLOTRAN Analysis

The two basic questions an analyst must answer are:

When is the analysis completed?

Has it been done correctly?

These questions are interrelated, since convergence may not be achieved it you have not set up and executed
the analysis correctly.

If you have set the input parameters and boundary conditions correctly, the analysis is complete when the con-
vergence monitors for all variables stop decreasing and the average, maximum, and minimum values of the
solution variables no longer increase or decrease. There is no guarantee, however, that you will achieve a single
exact answer because nature does not guarantee that a single exact answer exists. Oscillatory problems (for ex-
ample, vortex shedding behind a cylinder) may not yield stationary results from a steady-state or a transient
solution algorithm. You may wish to continue executing the analysis to verify whether a solution has a stable or
a fluctuating nature.

The ANSYS program stores the average, minimum, and maximum values of the solution variables in the file
Jobname.PFL. This file also records the FLOTRAN input plus the convergence monitors which have been calcu-
lated. The results summary includes all the DOF, as well as laminar and effective properties. You determine how
often ANSYS issues the results summary by using one of these methods:

Command(s): FLDATA5,OUTP,SUMF,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Additional Out> RFL Out Derived
Main Menu> Solution> FLOTRAN Set Up> Additional Out> RFL Out Derived

The

Value

argument is the number of global iterations that pass before ANSYS issues the next results summary.

You may also want to map your results onto a path through your model. See Section 5.3.5: Mapping Results onto
a Path in the ANSYS Basic Analysis Guide for more information on reviewing results along a path.

2.8. Verifying Results

You, the analyst, are responsible for verifying results. If your FLOTRAN analysis produces unexpected results,
take the actions listed below. You can accomplish many of these actions at the beginning of the analysis. ANSYS
creates a Jobname.PFL file and checks inputs even if the number of iterations executed is zero.

Check the mass balance printed as part of the results summary. Internal checks will determine if any
mass flow can potentially cross a model boundary. Boundary conditions admitting mass flow are:

•

Specified velocity boundaries

•

Specified pressure boundaries

•

Unspecified boundaries (These can result if you inadvertently omit a boundary condition.)

The ANSYS program tabulates the number of inlets/outlets, which should correspond to expectations.

Check boundary conditions within ANSYS to ensure that they are accurate.

Check that you specified the properties correctly and that they can vary with temperature and pressure
if necessary. The results summary in the Jobname.PFL file is a convenient place to check this.

Check that the length units used to build the model are consistent with those used in specifying properties.

In some cases, you need to verify that equations associated with the options chosen are solved correctly
(for instance, the pressure equation in compressible flow).

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

2–14

Chapter 2: The Basics of FLOTRAN Analysis

If the unexpected result of your analysis is divergence, the finite element mesh may not have sufficient
resolution, or significant gradients may exist near outlets. To resolve this, you may need to use conver-
gence aids such as relaxation. Later sections in this document discuss various relaxation techniques.

If you get a diverged solution for a particular variable, you can re-initialize that variable to a single value
and continue. To do so, use one of these methods:

Command(s): FLDATA29,MODV
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Mod Res/Quad Ord> Modify Results
Main Menu> Solution> FLOTRAN Set Up> Mod Res/Quad Ord> Modify Results

Section 2.8: Verifying Results

2–15

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

2–16

Chapter 3: FLOTRAN Laminar and Turbulent
Incompressible Flow

3.1. Characteristics of Fluid Flow Analysis

A laminar or turbulent flow analysis calculates the flow and pressure distribution in a 2-D or 3-D geometry. Flow
problems require you to specify density and viscosity. Problems may be internal or external in nature. For internal
flows, wall or symmetry planes bound the flow (for example, flow in a pipe), except for the inlet and outlet
boundaries. (Figure 3.1: “Internal Flow” shows an example). The boundaries of external problems generally are
either far-field velocity or pressure boundary conditions. The flow surrounding an airfoil is an external flow (See
Figure 3.2: “External Flow”).

Figure 3.1 Internal Flow

Figure 3.2 External Flow

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

The distinction between incompressible and compressible flow lies in both the equation of state and the solution
algorithm.

•

In an incompressible flow, density variations can drive the flow only through gravitational acceleration.
Temperature changes cause variations of density.

•

In a compressible flow, the density changes caused by pressure variations significantly affect the momentum
and temperature equations.

In any event, the incompressible algorithm can measure flow of an ideal gas, complete with small density changes
due to pressure. See Chapter 8, “FLOTRAN Compressible Analyses” for more information.

3.2. Activating the Turbulence Model

The distinction between laminar and turbulent flow lies in the ratio of the inertial transport to the viscous
transport. As this ratio increases, instabilities develop and velocity fluctuations begin to occur. A turbulent
model accounts for the effect of these fluctuations on the mean flow by using an increased viscosity, the effective
viscosity, in the governing equations. The effective viscosity is the sum of the laminar viscosity (which is a property
of the fluid) and turbulent viscosity (which is calculated from a turbulence model).

= µ + µ

Generally, the more turbulent the flow field, the higher the effective viscosity.

3.2.1. The Role of the Reynolds Number

The dimensionless Reynolds number measures the ratio of inertial and viscous forces to help determine whether
or not the turbulence model should be activated. The Reynolds number is defined in terms of the properties of
the fluid, a characteristic velocity, and a characteristic dimension:

= ρ

The density

ρ (mass/length

) and absolute viscosity µ (mass/length-time) are properties of the fluid. For internal

flow problems, the characteristic dimension is the hydraulic diameter, defined as:

L =D =

4 (Cross-Sectional Flow Area)

Wetted Perimeter

For example, the hydraulic diameter of a pipe is simply the diameter. As a general guideline for internal flow
problems such as flow in pipes, the turbulence model should usually be activated if the Reynolds number is in
excess of about 2300.

For an external flow problem, such as the flow over an airfoil, the characteristic length is a parameter such as the
length of the airfoil (wing cross section for a 2-D analysis).

For flow over a flat plate, the dimension is the length along the plate from the leading edge, with the transition
to turbulence occurring at a Reynolds number of approximately 500,000.

For more information, see the ANSYS, Inc. Theory Reference.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

3–2

Chapter 3: FLOTRAN Laminar and Turbulent Incompressible Flow

3.2.2. Determining Whether an Analysis Is Turbulent

Determining if an analysis is laminar or turbulent is your responsibility. What happens if turbulence is not activated
when it should be, or vice versa? What are the indications and the consequences?

If turbulence is needed but not activated, the analysis probably will diverge. If this occurs, the momentum and
pressure convergence parameters will approach 1.0 and the values of velocities and pressure will become very
large. You should start over with the turbulence model activated.

In some cases, convergence occurs even without the turbulence model. This can happen if no geometrical features
such as bends disturb the flow. Physically, some flows retain laminar characteristics unless they are slightly dis-
turbed in some fashion.

Conversely, although the turbulence models are not low Reynolds number models and do not "automatically"
resort to laminar behavior at low Reynolds numbers, in such cases the turbulence models predict low values of
effective viscosity. If the final average effective viscosity is less than five times greater than the laminar value,
you should rerun the case without the turbulence model and evaluate the differences.

You can postprocess the effective viscosity with the label EVIS. It is also tabulated in the results summary output
provided in the Jobname.PFL file. Therefore, you can observe the average behavior of effective viscosity as the
solution proceeds. You also can postprocess it to see its variation throughout the flow field.

3.2.3. Turbulence Ratio and Inlet Parameters

Be aware that when an analysis begins, the effective viscosity initializes as a multiple of the laminar value. This
initialization occurs whether a turbulence model is or is not active. The default value of this multiple (also called
the turbulence ratio) is 1000; a reasonable value for most turbulent analyses. The algorithm calculates lower or
higher values as conditions dictate. However, the accuracy of the initial estimate affects how long the program
takes to compute the final value.

To set the turbulence ratio, use either of these methods:

Command(s): FLDATA24,TURB,RATI,Value
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Turbulence> Turbulence Param

The two-equation turbulence models require boundary conditions for the turbulent kinetic energy (ENKE) and
turbulent kinetic energy dissipation rate (ENDS) at an inlet. If known values are available at the inlet, you can
specify ENKE and ENDS, Otherwise, you must specify an inlet intensity (ININ), which is the ratio of the fluctuating
velocity to the inlet velocity, and an inlet scale factor (INSF), which is the ratio of a length scale inlet region to
the hydraulic diameter of the inlet. ININ and INSF default to 0.01.

To set the inlet intensity and inlet scale factor, you use either of the following:

Command(s): FLDATA24,TURB,ININ,

Value

FLDATA24,TURB,INSF,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Turbulence> Turbulence Param

3.2.4. Turbulence Models

FLOTRAN offers several turbulence models:

Standard k-

ε Model

Zero Equation Turbulence Model (ZeroEq)

Re-Normalized Group Turbulence Model (RNG)

ε Model due to Shih (NKE)

Section 3.2: Activating the Turbulence Model

3–3

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Nonlinear Model of Girimaji (GIR)

Shih, Zhu, Lumley Model (SZL)

ω Turbulence Model

Shear Stress Transport Turbulence Model (SST)

Turbulence modeling is activated by either of the following:

Command(s): FLDATA1,SOLU,TURB,T
GUI: Main Menu> Preprocessor> FLOTRAN Setup> Solution Options
Main Menu> Solution> FLOTRAN Setup> Solution Options

To select a model, you use either of the following:

Command(s): FLDATA24,TURB,MODL,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Setup> Turbulence> Turbulence Model
Main Menu> Solution> FLOTRAN Setup> Turbulence> Turbulence Model

Normally, the Standard k-

ε Model is the first model to apply. It usually provides a realistic picture of the flow. It

is fine for the analysis of turbulent flow in pipes and channels. However, it over predicts the amount of turbulence
in a number of situations. For example, the flow in a converging nozzle undergoes significant normal strain and
the Standard k-

ε Model over predicts the amount of turbulence. The resulting kinetic energy is over predicted,

and the resulting effective viscosity prevents simulation of shock waves in some cases.

In general, the RNG, NKE, GIR, and SZL turbulence models produce significantly more realistic and reliable results
in regions of large strain. This is particularly important for cases where the flow is strongly accelerated or decel-
erated (e.g. a converging nozzle) or where there is significant separation or recirculation (e.g. a duct that goes
through a 180 degree change of direction). Other situations where the Standard k-

ε Model encounters difficulties

include flows with stagnation points.

The RNG, NKE, GIR, and SZL turbulence models control the excess turbulence by applying adjustments to C µ
and the source term of the dissipation equation. The adjustments are made in accordance with the local rate of
strain.

The k-

ω turbulence model has the advantage near the walls to accurately predict the turbulence length scale in

the presence of an adverse pressure gradient. The k-

ω model is much more sensitive to the free-stream turbulence

levels than the k-

ε model. The Shear Stress Transport model (SST) combines the k-ω model near the wall and the

ε model away from the wall to overcome the deficiencies of both models.

See the ANSYS Commands Reference and the ANSYS, Inc. Theory Reference for more information on the models.

3.2.4.1. Standard k-epsilon Model (default)

The Standard k-

ε Model, the Zero Equation Turbulence Model, and the k-ω Model are the simplest models. The

other models are all extensions of the Standard k-

ε Model and the k-ω Model. The Standard k-ε Model is the default

model.

To select the Standard k-

ε Model, you use either of the following:

Command(s): FLDATA24,TURB,MODL,1
GUI: Main Menu> Preprocessor> FLOTRAN Setup> Turbulence> Turbulence Model
Main Menu> Solution> FLOTRAN Setup> Turbulence> Turbulence Model

Cµ, C1, C2, SCTK, and SCTD are Standard k-

ε Model constants that are defined as follows:

Cµ -

Value

is the k-

ε turbulence model constant

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

3–4

Chapter 3: FLOTRAN Laminar and Turbulent Incompressible Flow

which is used in the update of the turbulent viscosity.

C1 -

Value

is the k-

ε turbulence model C1 constant. It is the multiplier of the shear rate generation term of the

turbulent kinetic energy dissipation rate equation.

C2 -

Value

is the k-

ε turbulence model C2 constant. It is the multiplier of the dissipation source term in the tur-

bulent kinetic energy dissipation rate equation.

SCTK -

Value

is the Schmidt number for the turbulent kinetic energy. The diffusion term in the turbulent kinetic

energy equation is divided by this factor.

SCTD -

Value

is the Schmidt number for the kinetic energy dissipation rate. The diffusion term in the dissipation

rate equation is divided by this factor.

To set the Standard k-

ε Model constants Cµ, C1, C2, SCTK, and SCTD, you use either of the following:

Command(s): FLDATA24,TURB,

Label,Value

GUI: Main Menu> Preprocessor> FLOTRAN Setup> Turbulence> Turbulence Model
Main Menu> Solution> FLOTRAN Setup> Turbulence> Turbulence Model

The following five wall parameters control turbulence wall modeling. The wall parameters apply for all turbulence
models except the Zero Equation Turbulence Model.

KAPP -

Value

is the law of the wall constant. It is the slope of the plot of normalized shear velocity (u

) versus

the nondimensionalized distance from the wall (y

). See ANSYS, Inc. Theory Reference for details.

EWLL -

Value

is the law of the wall constant. It is related to the y intercept value for a plot of normalized shear

velocity (u

) versus the nondimensionalized distance from the wall (y

). See the ANSYS, Inc. Theory Reference for

more details.

WALL -

Value

is the choice of wall conductivity model. The default model is the Van Driest model (

Value

VAND), used most often for high Prandtl number fluids. The second choice is the Spalding model (

Value

= SPAL),

applicable to low Prandtl number fluids. The third choice is the Equilibrium model (

Value

= EQLB). The equilib-

rium model is also automatically invoked for the wall viscosity by this command.

VAND -

Value

is the constant in the Van Driest wall conductivity model. See the ANSYS, Inc. Theory Reference for

details.

TRAN -

Value

is the magnitude of y

marking the outer boundary of the laminar sublayer. Used only for the

Equilibrium Wall model.

To set the wall parameters KAPP, EWILL, WALL, VAND and TRAN, you use either of the following:

Command(s): FLDATA24,TURB,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Setup> Turbulence> Wall Parameters
Main Menu> Solution> FLOTRAN Setup> Turbulence> Wall Parameters

The following three buoyancy terms control buoyancy modeling. The buoyancy terms apply for all turbulence
models except the Zero Equation Turbulence Model.

Section 3.2: Activating the Turbulence Model

3–5

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

BUC3 -

Value

is the k-

ε buoyancy model constant. A value of zero means that there is no contribution to the

turbulent kinetic energy dissipation rate equation. The default value of one is appropriate for stable thermally
stratified flows. A value of zero is appropriate for unstable thermally stratified flows.

BUC4 -

Value

is the k-

ε multiplier applied to the buoyancy term of the turbulent kinetic energy equation. A value

of 1.0 is appropriate for the calculation of stable thermally stratified flows. The default value is zero.

BETA -

Value

β, the coefficient of thermal expansion

= ∂

∂

This term is used in the buoyancy terms of the k-

ε model.

To set the buoyancy terms BUC3, BUC4, and BETA, you use either of the following:

Command(s): FLDATA24,TURB,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Setup> Turbulence> Buoyancy Terms
Main Menu> Solution> FLOTRAN Setup> Turbulence> Buoyancy Terms

See the ANSYS, Inc. Theory Reference and the ANSYS Commands Reference for more information.

3.2.4.2. Zero Equation Turbulence Model (ZeroEq)

The Zero Equation Turbulence Model (ZeroEq) is the simplest and fastest turbulence model. It applies to problems
with fairly simple geometry and flow characteristics. The model does not give accurate results if there is significant
separation or recirculation.

To select the Zero Equation Turbulence Model, you use either of the following:

Command(s): FLDATA24,TURB,MODL,2
GUI: Main Menu> Preprocessor> FLOTRAN Setup> Turbulence> Turbulence Model
Main Menu> Solution> FLOTRAN Setup> Turbulence> Turbulence Model

The Zero Equation Turbulence Model contains an automatic calculation of the length scale or you can specify
the length scale. Generally, the turbulence ratio can be set to 2.0 when you are using the Zero Equation Turbulence
Model.

See the ANSYS, Inc. Theory Reference and the ANSYS Commands Reference for more information.

3.2.4.3. Re-Normalized Group Turbulence Model (RNG)

The Re-Normalized Group Turbulence Model (RNG) is effective where the geometry has a strong curvature (e.g.,
a duct that goes through a 180 degree change in direction. If you have tried the SZL Model and the results are
unsatisfactory, it is generally recommended that you try the RNG Model.

To select the RNG Model, you use either of the following:

Command(s): FLDATA24,TURB,MODL,3
GUI: Main Menu> Preprocessor> FLOTRAN Setup> Turbulence> Turbulence Model
Main Menu> Solution> FLOTRAN Setup> Turbulence> Turbulence Model

To set the constants for the RNG Model, you use either the FLDATA24A,RNGT command or the foregoing GUI.

The RNG Model is an extension of the Standard k-

ε Model. Seven constants are assigned values. The Cµ, C1, C2,

SCTK, and SCTD constants are assigned values that are separate from the Standard k-

ε Model. The following two

constants are added:

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

3–6

Chapter 3: FLOTRAN Laminar and Turbulent Incompressible Flow

BETA -

Value

is the RNG model constant,

∞

ETAI -

Value

is the asymptotic value of the strain rate parameter eta.

Inlet parameters and wall parameters are the same as the Standard k-

ε Model.

See the ANSYS, Inc. Theory Reference and the ANSYS Commands Reference for more information.

3.2.4.4. k-epsilon Model Due to Shih (NKE)

The k-

ε Model due to Shih (NKE) features a variable Cµ term which helps to reduce the excess normal strain terms

in the Standard k-

ε Model. The NKE model also employs a different dissipation source term than the Standard

ε Model.

The NKE and GIR models are recommended for rotating flows.

To select the NKE Model, you use either of the following:

Command(s): FLDATA24,TURB,MODL,4
GUI: Main Menu> Preprocessor> FLOTRAN Setup> Turbulence> Turbulence Model
Main Menu> Solution> FLOTRAN Setup> Turbulence> Turbulence Model

To set the constants for the NKE Model, you use either the FLDATA24B,NKET command or the foregoing GUI.

The NKE Model is an extension of the Standard k-

ε Model. Four constants are assigned values. The C2, SCTK, and

SCTD constants are assigned values that are separate from the Standard k-

ε Model. The following constant is

added:

C1MX - Value is the maximum allowed value of the C1 constant in the turbulent kinetic energy dissipation rate
equation.

Inlet parameters and wall parameters are the same as the Standard k-

ε Model.

See the ANSYS, Inc. Theory Reference and the ANSYS Commands Reference for more information.

3.2.4.5. Nonlinear Model of Girimaji (GIR)

The Nonlinear Model of Girimaji (GIR) is suggested for cases with secondary vortices in the flow. The GIR and NKE
models are recommended for rotating flows.

To select the GIR Model, you use either of the following:

Command(s): FLDATA24,TURB,MODL,5
GUI: Main Menu> Preprocessor> FLOTRAN Setup> Turbulence> Turbulence Model
Main Menu> Solution> FLOTRAN Setup> Turbulence> Turbulence Model

To set the constants for the GIR Model, you use either the FLDATA24C,GIRT command or the foregoing GUI.

The GIR Model is an extension of the Standard k-

ε Model. Seven constants are assigned values. The SCTK, and

SCTD constants are assigned values that are separate from the Standard k-

ε Model. The following five constants

are added:

G0 -

Value

is the

constant.

G1 -

Value

is the

constant.

G2 -

Value

is the C

constant.

Section 3.2: Activating the Turbulence Model

3–7

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

G3 -

Value

is the C

constant.

G4 -

Value

is the C

constant.

Inlet parameters and wall parameters are the same as the Standard k-

ε Model.

See the ANSYS, Inc. Theory Reference and the ANSYS Commands Reference for more information.

3.2.4.6. Shih, Zhu, Lumley Model (SZL)

The SZL Model is simpler than the NKE and GIR models. It produces the lowest level of turbulence. The SZL
model is numerically efficient, but in some cases the resulting low effective viscosity has an adverse effect on
stability. Generally, if the SZL model does not give satisfactory results, it is recommended that you try the RNG
model.

If conditions of large strain exist in the flow field, you may want to try the SZL Model after trying the RNG, NKE
or GIR models. If the SZL Model gives significantly different results, it is recommended that you refine the mesh
in the regions where the turbulence field is strongly altered.

To select the SZL Model, you use either of the following:

Command(s): FLDATA24,TURB,MODL,6
GUI: Main Menu> Preprocessor> FLOTRAN Setup> Turbulence> Turbulence Model
Main Menu> Solution> FLOTRAN Setup> Turbulence> Turbulence Model

To set the constants for the SZL Model, you use either the FLDATA24D,SZLT command or the foregoing GUI.

The SZL Model is an extension of the Standard k-

ε Model. Five constants are assigned values. The SCTK, and SCTD

constants are assigned values that are separate from the Standard k-

ε Model. The following three constants are

added:

SZL1 -

Value

is the numerator constant used in the calculation of Cµ. It is the A

szl1

constant.

SZL2 -

Value

is the denominator constant used in the calculation of Cµ. It is the A

szl2

constant.

SZL3 -

Value

is the strain rate multiplier. It is the A

szl3

constant.

Inlet parameters and wall parameters are the same as the Standard k-

ε Model.

See the ANSYS, Inc. Theory Reference and the ANSYS Commands Reference for more information.

3.2.4.7. k-omega Turbulence Model

The k-

ω model is one of the simplest turbulence models. It provides better modeling of the turbulent boundary

layer than the standard k-

ε model, but is more sensitive to the free-stream turbulence levels.

To select the k-

ω Model, you use either of the following:

Command(s): FLDATA24,TURB,MODL,7
GUI: Main Menu> Preprocessor> FLOTRAN Setup> Turbulence> Turbulence Model
Main Menu> Solution> FLOTRAN Setup> Turbulence> Turbulence Model

To set the constants for the k-

ω Model, use either the FLDATA24E,SKWT command or the foregoing GUI.

The k-

ω Model solves for the ω equation rather than the ε equation in the standard k-ε Model. Four constants

are assigned values. The SCTK constant is an assigned value that is separate from the Standard k-

ε Model. The

following three constants are added:

SCTW -

Value

is the Schmidt number for the specific dissipation rate.

BETA -

Value

is the BETA factor.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

3–8

Chapter 3: FLOTRAN Laminar and Turbulent Incompressible Flow

GAMA -

Value

is the GAMMA factor.

Inlet parameters and wall parameters are the same as the Standard k-

ε Model.

See the ANSYS, Inc. Theory Reference and the ANSYS Commands Reference for more information.

3.2.4.8. Shear Stress Transport Model (SST)

The SST Model combines advantages of both the Standard k-

ε Model and the k-ω Model. It automatically switches

to the k-

ω Model in the near region and the Standard k-ε Model away from the walls.

To select the SST Model, you use either of the following:

Command(s): FLDATA24,TURB,MODL,8
GUI: Main Menu> Preprocessor> FLOTRAN Setup> Turbulence> Turbulence Model
Main Menu> Solution> FLOTRAN Setup> Turbulence> Turbulence Model

To set the constants for the SST Model, use the FLDATA24F,SST1, FLDATA24G,SST1 and FLDATA24H,SST2
commands, or the foregoing GUI. Similar to the k-

ω Model, the SST Model solves for the ω equation rather than

the

ε equation in the Standard k-ε Model. Nine constants are assigned values. The SCTK

and the SCTK

constants

are assigned values that are separate from the Standard k-

ε Model. The following seven constants are added.

CLMT -

Value

is the turbulent production clip factor.

SCTW

Value

is the Schmidt number for the specific dissipation rate in the k-

ω regime.

SCTW

Value

is the Schmidt number for the specific dissipation rate in the k-

ε regime.

BETA

Value

is the BETA factor in the k-

ω regime.

BETA

Value

is the BETA factor in the k-

ε regime.

GAMA

Value

is the GAMMA factor in the k-

ω regime.

GAMA

Value

is the GAMMA factor in the k-

ε regime.

Inlet parameters and wall parameters are the same as the Standard k-

ε Model.

See the ANSYS, Inc. Theory Reference and the ANSYS Commands Reference for more information.

3.3. Meshing Requirements

The meshing requirements for turbulence are more restrictive than those for laminar flow. The most important
areas obviously are those with the higher gradients, in particular the regions near walls.

Structured meshes, as contrasted with free meshes, can provide more consistent representation at the walls.
Figure 3.3: “Structured Mesh” and Figure 3.4: “Unstructured Mesh” compare the structured and unstructured
meshes for a region near the wall.

Section 3.3: Meshing Requirements

3–9

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Figure 3.3 Structured Mesh

This mesh was produced with MSHAPE,0,2D and MSHKEY,1 commands.

Figure 3.4 Unstructured Mesh

This mesh was produced with MSHAPE,1,2D and MSHKEY,0 commands.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

3–10

Chapter 3: FLOTRAN Laminar and Turbulent Incompressible Flow

You can evaluate the adequacy of the mesh near the walls. Applying the turbulence model near walls involves
the "Log Law of the Wall," the relationship between a nondimensionalized distance from the wall Y

, and the

log of a nondimensionalized velocity in a region near the wall. This law calculates a near wall viscosity that is
consistent with experimentally determined velocity profiles near the wall. Values of Y

are relevant only for wall

nodes and are available for postprocessing (YPLU).

Optimum values of Y

are between approximately 30 and 1000. If the pressure is decreasing in the direction of

flow, values up to 5000 are acceptable. FLOTRAN handles the case where Y

is less than 30 for the near wall node

by assuming that the near wall node is in the laminar sublayer or the overlap region. In the former case, the near
wall viscosity is simply the laminar value.

If Y

is very small, perhaps below 1, more elements than necessary are being used to resolve the flow distribution

field. If Y

is greater than 5000, decrease the mesh spacing near the wall.

Caution: Use enough elements to resolve the flow field in the regions of interest. You should use at
least four elements to span the cross sections of long thin channels. Use more than four elements where
thin channels connect to larger regions.

3.4. Flow Boundary Conditions

Each boundary of the problem domain requires treatment. You specify some combination of DOF (VX, VY, VZ
and PRES) at the boundary types listed below. (If suitable values are available, you can specify turbulent kinetic
energy (ENKE) and turbulent kinetic energy dissipation rate (ENDS) at an inlet.) The derivative of all dependent
variables normal to the surface is zero if you apply no conditions at the boundary surface.

To set DOF constraints at nodes, use either of the following:

Command(s): D
GUI: Main Menu> Preprocessor> Loads> Define Loads> Apply>

boundary condition type

You can set boundary conditions on the solid model using any of the following:

Command(s): DA and DL
GUI: Main Menu> Preprocessor> Loads> Define Loads> Apply>

boundary condition type

> On

Areas
Main Menu> Solution> Define Loads> Apply>

boundary condition type

> On Areas

Main Menu> Preprocessor> Loads> Define Loads> Apply>

boundary condition type

> On Lines

Main Menu> Solution> Define Loads> Apply>

boundary condition type

> On Lines

This enables you to redo the analysis with a different mesh, without reapplying boundary conditions on a nodal
basis. These commands or GUI paths allow you to specify the condition on the endpoints of a line or the edge
of an area.

Take care to ensure that the proper conditions are applied at intersecting boundaries. You have control over
whether or not boundary conditions are applied at the ends of lines or at the edges of areas. A nonzero velocity
component at the end of a line or at the edge of an area will not replace an existing zero velocity condition at
the associated nodes. Where a wall intersects an inlet, the wall condition will automatically prevail.

If you apply new (and different) boundary conditions to a solid model of a finite element mesh, you should delete
existing nodal boundary conditions before transferring the new loads.

Specified Flow: You specify all velocity components at the boundary. Use this method to specify a flow at an
inlet. Knowledge of the mass flow at the inlet requires you to know the density.

Section 3.4: Flow Boundary Conditions

3–11

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Specified Pressure: Typically, you apply a relative pressure (usually zero) as an outlet boundary condition. In
the absence of gravity and a rotating reference frame, the absolute pressure is the sum of the FLOTRAN (relative)
pressure and the reference pressure. See the ANSYS, Inc. Theory Reference for a more complete discussion of
pressure. A problem may also be pressure driven, in which case one of the pressure boundaries is an inlet.

Note — If significant gradients are calculated near a boundary, a mass imbalance can occur. This is due
to the implied condition of fully developed flow for a constant pressure boundary. If the flow has not
fully developed, FLOTRAN is forced to adjust it across the last row of elements to satisfy the boundary
condition. Occasionally, this adjustment may cause a mass imbalance.

To prevent this from occurring, you can add a development length to the exit. This addition does not actually
need to match the physical flow geometry. You can subtract the pressure drop in this "chimney" to obtain the
desired pressure drop. The pressure drop in the "chimney" will vary over its full cross section. You will have to
choose a representative value of the pressure drop to match the desired outlet conditions. You will not know
this pressure drop, of course, until after you examine the results from the chimney. You can opt to apply an exit
pressure profile, based on these results, to the original geometry.

You can calculate the required length of the chimney (L) using the characteristic diameter (D) from the develop-
ment length formula:

Laminar flow: L/D ~ 0.06 Re
Turbulent flow: L/D ~ 4.4 Re

1/6

Typically, a chimney 20 to 25 diameters long will be sufficient. Although the mesh in this region may be coarse,
you should avoid drastic changes in element size by using a size ratio in the chimney. The important feature is
the chimney length, not the number of nodes in it.

Symmetry Boundary: The velocity component normal to the boundary is specified as zero. Leave all other degrees
of freedom unspecified.

Generalized Symmetry Boundary Conditions: You can also apply generalized symmetry boundary conditions.
Velocity components are set tangential to the symmetry surface if the ALE formulation is not activated. They are
set equal to the mesh velocity if the ALE formulation is activated. To apply generalized symmetry boundary
conditions, use one of the following commands or the GUI equivalent:

NODE

,ENDS,-1

DL,

LINE

AREA

,ENDS,-1,

Value2

DA,

AREA

,ENDS,-1,

Value2

With one exception, if any velocity component is specified at the same boundary, the generalized symmetry
boundary conditions are overwritten. In a 2-D swirl problem, specification of a velocity component VZ does not
overwrite generalized symmetry conditions.

Stationary Wall: This is also referred to as a no-slip condition. All the velocity components are set to zero.

Moving Wall: Specify the velocity component tangent to the wall and set all other velocity components to zero.
As a flag to indicate this is a moving wall, set the turbulent kinetic energy to -1 on a moving wall. This specification
is as a flag only; it does not affect the performance of the wall turbulence model. If you are using the GUI, indicate
a moving wall when specifying the velocities.

Unspecified Boundary: In this case, neither the relative pressure nor the velocities are known. The most common
application for this is at downstream boundaries in compressible supersonic flow.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

3–12

Chapter 3: FLOTRAN Laminar and Turbulent Incompressible Flow

Periodic Boundary: Conditions are unknown but identical at two boundaries. You select the nodes at one
boundary and then issue the macro PERI,DX, DY, DZ, where DX, DY, and DZ are the offsets of the second
boundary from the first. The offsets are input in the established FLOTRAN coordinate system. The meshes at the
two boundaries must be identical.

Intersections: At the intersection of surfaces where two different boundary conditions are applied, either the
boundary conditions are merged or one takes precedence over the other. The following table provides guidance
on what boundary conditions are applied at the intersection.

Table 3.1 Boundary Conditions at Intersections

Action

Intersecting Boundary 2

Intersecting Boundary 1

Overwrite inflow with wall

Wall:
VX, VY, VZ = 0

Inflow:
VX, VY, VZ values specified

Combine inflow with symmetry

Symmetry:
VX or VY or VZ = 0

Inflow:
VX, VY, VZ values specified

Enforce inflow condition, not outflow

Outflow:
P = 0

Inflow:
VX, VY, VZ values specified

Combine symmetry and outflow

Outflow:
P = 0

Symmetry:
VX or VY or VZ = 0

Overwrite symmetry with the wall

Wall:
X, VY, VZ = 0

Symmetry:
VX or VY or VZ = 0

Combine wall and outflow conditions

Outflow:
P = 0

Wall:
VX, VY, VZ = 0

Combine the generalized symmetry and outflow
conditions

Outflow:
P = 0

Generalized Symmetry

Note — Inflow, symmetry , and wall boundary conditions all overwrite generalized symmetry conditions.

Inlet Values: If you activate the turbulence model, boundary conditions are required. The ANSYS program supplies
default values based on the inlet velocity and a scale factor. Given an inlet velocity magnitude

, the inlet kinetic

energy is specified as:

[(ININ)V]

inlet

The default value of the factor ININ is 0.01, corresponding to a level of turbulence of 1 percent at the inlet. The
inlet value of the kinetic energy dissipation rate

ε is calculated from:

inlet

INSF L

C k

(

)

The INSF value is a user-controlled scale factor. To specify the factors ININ and INSF, use either of the following
methods:

Command(s): FLDATA24,TURB,ININ,

Value

and FLDATA24,TURB,INSF,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Turbulence> Turbulence Param

Section 3.4: Flow Boundary Conditions

3–13

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Main Menu> Solution> FLOTRAN Set Up> Turbulence> Turbulence Param

You can set specific values of the turbulent kinetic energy (ENKE) or the dissipation rate (ENDS) using either the
FLDATA24 command or the menu paths in Section 3.2.2: Determining Whether an Analysis Is Turbulent.

Occasionally, you may wish to activate the turbulence model for the case, but deactivate it for certain regions.
To deactivate the turbulence model in regions, set the kinetic energy (ENKE) to zero and the dissipation rate
(ENDS) to 1.0. It is never valid to set the dissipation rate to zero, and FLOTRAN prohibits it. ENDS will be set to
1.0, if ENKE is set to zero.

Wall Roughness:

The FLOTRAN default condition is smooth walls. To specify wall roughness values, you must use the equilibrium
wall turbulence model. You activate it using the FLDATA24,TURB,WALL,EQLB command.

To apply a uniform wall roughness in length units to all walls, you can use the FLDATA24,TURB,KS,Value command.
In addition to being the actual roughness, the KS parameter determines the regime of roughness (smooth,
transitional, or fully rough). The default value of 0.0 implies a smooth wall.

You can also apply an empirical dimensionless factor (CKS) between 0.5 and 1.0 that specifies the degree of
nonuniformity of the surface. The default value of 0.5 means that the roughness signified by KS is uniformly
distributed. Higher values increase the roughness losses without changing the flow regime implied by the value
of KS. You can use the FLDATA24,TURB,CKS,Value command to specify this factor.

The following two methods are available if you have surfaces that require different roughness values.

The first method utilizes real constants for all the wall elements. You apply suitable KS and CKS values to the near
wall elements as real constants. A different real constant set will exist for each set of wall roughnesses. Note that
roughness constants applied to elements that are not near wall will be ignored. Also, any KS and CKS values
specified by the FLDATA24,TURB command will be ignored.

The second method is for cases where most of the surfaces have the same roughness condition and only a few
are different. First, set the values appropriate for most of the surfaces with the FLDATA24,TURB command. Then
use real constants to apply roughnesses to the walls that have different conditions. The real constants will
overwrite the FLDATA24,TURB values. Note that if the same value of CKS is applied to all the surfaces (as is typ-
ical), it can be controlled with the FLDATA24,TURB command and the real constant can be omitted.

3.5. Strategies for Difficult Problems

The most common problems are divergence or oscillation of the pressure and/or velocity field.

The following strategies have proven helpful in getting difficult turbulent problems to converge.

Activate the turbulence option if you have not done so.

Turbulence modeling is activated by either of the following:

Command(s): FLDATA1,SOLU,TURB,T
GUI: Main Menu> Preprocessor> FLOTRAN Setup> Solution Options
Main Menu> Solution> FLOTRAN Setup> Solution Options

Use a mapped mesh if a free mesh has given poor results. Resolve the boundary layer so that the value
of Y

is less than 5000.

To set the Y+ output option, use the following:

Command(s): FLDATA5,OUTPUT,YPLU,

Value

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

3–14

Chapter 3: FLOTRAN Laminar and Turbulent Incompressible Flow

GUI: Main Menu> Preprocessor> FLOTRAN Setup> Additional Out> RFL Out Derived
Main Menu> Solution> FLOTRAN Setup> Additional Out> RFL Out Derived

Set the turbulence inertial relaxation factor to 1.0. Values as low as 1.0

-2

may help. (For incompressible

flow problems, you may not need to vary this factor.)

To set the turbulence inertial relaxation factor, use the following:

Command(s): FLDATA26,STAB,TURB,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Relax/Stab/Cap> Stability Parms
Main Menu> Solution> FLOTRAN Set Up> Relax/Stab/Cap> Stability Parms

Use pressure and momentum relaxation factors less than 0.5. If values as low as 0.2 do not help, going
lower probably will not help either.

To set the pressure and momentum relaxation factors, use the following:

Command(s): FLDATA25,RELX,PRES,

Value

FLDATA25,RELX,VX (or VY, VZ),

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Relax/Stab/Cap> DOF Relaxation
Main Menu> Solution> FLOTRAN Set Up> Relax/Stab/Cap> DOF Relaxation

Begin the problem with a higher turbulence ratio (meaning a higher initial effective viscosity). Do not
set values for this parameter, which takes effect only at problem startup, above 1.0 x 10

. The ratio set

controls the initial effective viscosity no matter when you activate the turbulence model.

To set the turbulence ratio, use either of these methods:

Command(s): FLDATA24,TURB,RATI,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Turbulence> Turbulence Param
Main Menu> Solution> FLOTRAN Set Up> Turbulence> Turbulence Param

After initializing with the correct properties, solve the problem with a higher viscosity and the turbulence
model turned off. When the flow field is partially converged, the turbulence model is activated. You may
need to reduce the relaxation factor of the effective viscosity to 0.1 or 0.0 for some global iterations to
allow partial convergence of the turbulence equations. Refer to the foregoing strategies for command
information.

Difficulties can involve large changes in properties due to large fluctuations in pressure or temperature.
Preventing property variations early in the analysis (until the large fluctuations calm down) can stabilize
the analysis significantly.

You also can invoke velocity capping to prevent large values of velocities or pressures. This is particularly
useful in compressible analyses, where velocity spikes can cause negative static temperatures.

To implement velocity capping, use either of the following methods:

Command(s): FLDATA31,CAPP,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Relax/Stab/Cap> Results Capping
Main Menu> Solution> FLOTRAN Set Up> Relax/Stab/Cap> Results Capping

If you use the FLDATA31 command,

Label

represents a capping parameter such as VELO (velocity), or

TEMP (temperature).

Value

is either the capping flag (T or F) or the capping parameter value. Pressure

capping applies to relative values of pressure. Temperature capping applies to absolute values of tem-
perature.

Problems involving pyramid, wedge or in particular tetrahedral element shapes may require tighter
convergence of the pressure equation. Values as low as 1.E-18 may be required (FLDATA21,CONV,PRES,1.E-
18). You should reduce the convergence criterion until, from one global iteration to the next, the number
of iterations required to solve the equation varies by less than 10 percent (as per the Jobname.DBG file).

Section 3.5: Strategies for Difficult Problems

3–15

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

The solution of the pressure equation may affect the mass balance. The mass balance may be incorrect
(as per the Jobname.PFL file) if large aspect ratio elements are near significant flow area changes. Mass
imbalances may also occur if inlet or outlet regions are too coarsely meshed or if the flow tends to exit
at an angle at outlets.

10. If FLOTRAN displays a message stating that the coefficient matrix has a negative diagonal and the solution

is probably divergent, try turning on modified inertial relaxation in the momentum equation or turbulence
equation. Set the

Value

between 0.1 and 1.0. To achieve a faster convergence rate, use the smallest

Value

possible.

To set the turbulence inertial relaxation factor, use the following:

Command(s): FLDATA34,MIR,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Relax/Stab/Cap> MIR Stabilization
Main Menu> Solution> FLOTRAN Set Up> Relax/Stab/Cap> MIR Stabilization

11. If you notice anomalous results for 3-D problems, you should increasing the quadrature order to 2.

12. Specifying the Streamline Upwind/Petrov-Galerkin (SUPG) approach for momentum may help conver-

gence. Specifying the SUPG approach for temperature may also yield more accurate energy solutions
and hence more accurate energy balances. For more information on the SUPG approach, see Chapter 14,
“Advection Discretization Options”.

3.6. Example of a Laminar and Turbulent FLOTRAN Analysis

Access the CFD Tutorial to perform an example analysis of laminar and turbulent flow in a 2–D duct.

Before you begin the laminar/turbulent example, note the following:

•

The example problem is only one of many possible FLOTRAN analyses. It does not illustrate every technique
you might use in a FLOTRAN analysis, and is intended only to show the kinds of tasks a FLOTRAN analysis
typically requires.

•

You can use many techniques in a FLOTRAN analysis that are not shown in this problem. For example,
you can integrate pressure and shear stress on an airfoil to determine the lift and drag forces (see the
description of the INTSRF command in Section 5.3.3: Integrating Surface Results in the ANSYS Basic Ana-
lysis Guide).

•

The values you enter in this example are specific values for this example only. The characteristics of the
individual problem you are solving dictate what values you should specify for a particular FLOTRAN ana-
lysis.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

3–16

Chapter 3: FLOTRAN Laminar and Turbulent Incompressible Flow

Chapter 4: FLOTRAN Thermal Analyses

4.1. Thermal Analysis Overview

In a thermal analysis, you solve the temperature equation to determine temperature. Even if the temperature
itself is not important, the variation of fluid properties with temperature may be important enough to warrant
a thermal analysis.

In addition to calculating a temperature field, a thermal analysis provides heat fluxes at problem boundaries and
heat transfer coefficients based on an assumed bulk or ambient temperature.

You activate solution of the temperature equation via one of the following:

Command(s): FLDATA1,SOLU,TEMP,TRUE
GUI: Main Menu> Solution> FLOTRAN Set Up> Solution Options

FLOTRAN automatically includes viscous heating for compressible flows. For information on activating viscous
heating for incompressible flows, see Section 4.5.2: Forced Convection, Temperature Dependent Properties and
the description of the FLDATA1 command in the ANSYS Commands Reference.

4.2. Meshing Requirements

The ANSYS program has no formal criteria for evaluating the finite element mesh. However, thermal gradients
are often extremely high near thermal boundaries, especially heat flux boundaries. Therefore, the mesh should
usually be denser near thermal boundaries.

4.3. Property Specifications and Control

In addition to density and viscosity, thermal flow problems require the specification of thermal conductivity and
specific heat. You must determine whether or not fluid properties should vary with temperature.

To set properties for non-fluid regions, use one of these methods:

Command(s): MP
GUI: Main Menu> Preprocessor> Loads> Load Step Opts> Other> Change Mat Props
Main Menu> Preprocessor> Material Props> Material Models> CFD> Conductivity> Isotropic
Main Menu> Preprocessor> Material Props> Material Models> CFD> Specific Heat
Main Menu> Solution> Load Step Opts> Other> Change Mat Props

4.4. Thermal Loads and Boundary Conditions

The ANSYS program supports six types of thermal boundary conditions:

Constant temperatures

Constant heat fluxes

Applied heat transfer (film) coefficients with associated ambient temperatures

Ambient radiation with associated surface emissivities and ambient temperatures

Surface-to-surface radiation with associated emissivities and enclosure number.

Adiabatic boundaries (the default condition)

In addition, constant volumetric heat sources may be located in both fluid and non-fluid regions.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

The applicable commands are summarized below.

You can apply your boundary conditions via TABLE type array parameters (see Section 2.3.4.2.1: Applying Loads
Using TABLE Type Array Parameters in the ANSYS Basic Analysis Guide). You can also apply your boundary conditions
using function boundary conditions (see Section 2.6.15: Applying Loads Using Function Boundary Conditions
in the ANSYS Basic Analysis Guide).

You can define a TABLE type array parameter to apply your boundary conditions in a FLOTRAN analysis. Attempting
to use tabular boundary conditions in a FLOTRAN analysis will create erroneous results.

4.4.1. Applying Loads

The table below lists the loads you can apply in a thermal FLOTRAN analysis.

Table 4.1 Command Family and GUI Path Used to Apply Loads

GUI Path

Cmd

Family

Category

Load Type

Main Menu> Solution> Define Loads> Apply> Temperature

Constraints

Temperature (TEMP)

Main Menu> Solution> Define Loads> Apply> Thermal>
Convection
Main Menu> Solution> Define Loads> Apply> Thermal>
Heat Flux
Main Menu> Solution> Define Loads> Apply> Thermal>
Ambient Rad
Main Menu> Solution> Define Loads> Apply> Thermal>
Surface Rad

Surface Loads

Convection (CONV),
Heat Flux (HFLU),
Radiation (RAD),
Surface-to-surface
radiation (RDSF)

Main Menu> Solution> Define Loads> Apply> Fluid/CFD>
Heat Generat

Body Loads

Heat Generation Rates
(HGEN)

In an analysis, you can apply, remove, operate on, or list loads.

4.4.1.1. Applying Loads Using Commands

The table below lists all the commands in detail you can use to apply loads in a FLOTRAN thermal analysis.

Table 4.2 Load Commands for a FLOTRAN Thermal Analysis

Apply Set-
tings

Operate

List

Delete

Apply

Entity

Solid Model
or FE

Load Type

DLIST

DDELE

Nodes

Finite Element

Temperature

SFLDELE

SFL

Lines

Solid Model

Convection, Heat
Flux, Ambient Radi-
ation, or Surface-to-
surface Radiation

SFGRAD

SFTRAN

SFALIST

SFADELE

SFA

Areas

Solid Model

SFLIST

SFDELE

Nodes

Finite Element

SFSCALE

SFELIST

SFEDELE

SFE

Elements

Finite Element

SFSCALE

SFELIST

SFEDELE

SFE

Elements

Finite Element

Heat Generation
Rates

BFTRAN

BFLLIST

BFLDELE

BFL

Lines

Solid Model

BFTRAN

BFALIST

BFADELE

BFA

Areas

Solid Model

BFTRAN

BFVLIST

BFVDELE

BFV

Volumes

Solid Model

BFLIST

BFDELE

Nodes

Finite Element

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

4–2

Chapter 4: FLOTRAN Thermal Analyses

BFSCALE

BFELIST

BFEDELE

BFE

Elements

Finite Element

Note — You must use tabular boundary conditions if you are applying tapered heat flux or convection
loads.

4.4.1.2. Applying Loads Using the GUI

You access all operations except List through a series of cascading menus. From the Solution Menu, you choose
the operation (Apply, Delete, etc.), then the load type (temperature, heat flux, etc.), and then the object (node,
line, or area) to which you are applying the load.

For example, to apply a temperature load to lines, follow this GUI path:

Main Menu> Solution> Define Loads> Apply> Thermal> Temperature> On Lines

To list loads, follow this GUI path:

Utility Menu> List> Loads>

load type

4.4.1.3. Solutions

The following list describes what is known and what is calculated as a function of the type of boundary specified.

•

For temperature boundary conditions, heat flux and heat transfer coefficient are calculated.

•

For heat flux boundary conditions, temperature and heat transfer coefficient are calculated.

•

For ambient radiation boundary conditions, temperature and heat flux are calculated.

•

For surface-to-surface radiation boundary conditions, temperature and heat flux are calculated.

•

For heat transfer boundary conditions, temperature and heat flux are calculated.

•

For adiabatic boundary conditions, temperature is calculated.

When you apply a heat transfer (film) coefficient, you also specify an associated ambient temperature. The ANSYS
program uses this along with the surface temperature to calculate the heat flux at that boundary.

You specify heat flux and heat transfer coefficients at external model boundaries. You cannot specify them at
general internal surfaces. You can specify heat flux and heat transfer coefficients at internal boundary faces (such
as fluid/solid interface surfaces), but FLOTRAN will issue a warning because they are probably incorrect. In a
standard FLOTRAN analysis the heat transfer at a fluid/solid boundary is a desired result, not a boundary condition.
If you wish to apply a heat flux or a heat transfer coefficient, you should apply it at the external solid material
boundary, or at the edge of the fluid region without modeling the solid material in the analysis. If you specify a
film coefficient or a heat flux at an internal fluid/solid interface, FLOTRAN interprets it to be a line/area heat
source or sink. You can prescribe temperatures anywhere.

In cases where you must calculate the heat transfer coefficient at a surface, ANSYS uses the surface temperature
along with the bulk temperature you specify using either of the following methods:

Command(s): FLDATA14,TEMP,BULK,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Flow Environment> Ref Conditions
Main Menu> Solution> FLOTRAN Set Up> Flow Environment> Ref Conditions

If the analysis is compressible, boundary condition temperatures are in terms of total temperature, and the
temperature equation is formulated and solved in terms of total temperature.

Section 4.4: Thermal Loads and Boundary Conditions

4–3

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

The FLOTRAN ambient radiation load simulates radiation heat transfer to space at a constant temperature. You
specify the constant temperature with the SF command. You specify the Stefan-Boltzmann constant with the
STEF command (defaults to 0.119E-10 Btu/hr/in

/ °R

). The form factor is 1.0 by assumption.

Since radiation can pass through a fluid region and impact on a solid, you can apply the ambient radiation load
on a fluid/solid interface, as well as on external model boundaries. In this case, you should apply the surface load
to either the fluid or solid element faces, or the solid model entity defining the interface. If you apply the load
to more than one face, FLOTRAN applies the boundary conditions on only one face and issues a message that
it skipped duplicate boundary conditions.

4.5. Solution Strategies

The most efficient way to solve thermal-flow problems depends on the degree to which the fluid properties
depend on the temperature.

4.5.1. Constant Fluid Properties

In this case, the flow solution does not depend at all on the temperature field and can be converged without
activating the temperature equation solution.

Once the flow solution is complete, the temperature equation become linear. You can then solve it in one
global iteration after you set the relaxation factor for temperature to 1 using either method shown below:

Command(s): FLDATA25,RELX,TEMP,1.0
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Relax/Stab/Cap/DOF Relaxation
Main Menu> Preprocessor> FLOTRAN Set Up> Relax/Stab/Cap/Prop Relaxation
Main Menu> Solution> FLOTRAN Set Up> Relax/Stab/Cap/DOF Relaxation
Main Menu> Solution> FLOTRAN Set Up> Relax/Stab/Cap/Prop Relaxation

This is often best accomplished with a semi-direct solution algorithm.

See Chapter 11, “FLOTRAN CFD Solvers and the Matrix Equation” for more information.

The flow equations need not be solved during the solution of the temperature equation. Executing two global
iterations should result in a very small change, if any, in the answer during the second calculation. This will be
reflected in a large decrease in the convergence monitors for temperature in the second iteration.

4.5.2. Forced Convection, Temperature Dependent Properties

The flow pattern will be a mild function of the temperature field. You can choose to solve the temperature
equation every global iteration or converge the flow field calculations before activating solution of the temper-
ature equation. In the latter case, you will still need to solve the flow and temperature equations together to refine
the flow field with the property variations. If difficulties with the temperature equation are encountered early in
the solution, it is then best to start over and partially converge the flow solution before allowing the properties
to vary with temperature.

For incompressible flows, viscous heating is generally not important for cases with low Prandtl numbers or low
to moderate velocities. However, you should turn on viscous heating whenever the Prandtl number is greater
than 2 or the velocities are high (e.g., greater than 100 m/s in air). FLOTRAN automatically includes viscous
heating for compressible flows. To include viscous heating for incompressible flows, use one of the following:

Command(s): FLDATA1,SOLU,IVSH,T
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Solution Options
Main Menu> Solution> FLOTRAN Set Up> Solution Options

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

4–4

Chapter 4: FLOTRAN Thermal Analyses

For information on the energy units required for thermal quantities when an incompressible analysis includes
viscous heating, refer to Section 9.2: Fluid Property Types.

4.5.3. Free Convection, Temperature Dependent Properties

In this case, the driving force for the flow is the density change brought about by temperature variations. You
must turn on both options.

You also must do the following:

•

Specify acceleration due to gravity, using one of the following:

Command(s): ACEL
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Flow Environment> Gravity
Main Menu> Solution> FLOTRAN Set Up> Flow Environment> Gravity

•

Activate the variable density option using one of the following:

Command(s): FLDATA13,VARY,

Label

,TRUE (

Label

= fluid property)

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Fluid properties
Main Menu> Solution> FLOTRAN Set Up> Fluid properties

Buoyancy property types, which use a constant pressure to evaluate the density from the ideal gas law are
provided for AIR. (See Chapter 9, “Specifying Fluid Properties for FLOTRAN”.) Pressure fluctuations are thus pre-
vented from causing instabilities in density calculations. Natural convection cases converge slowly, and may be
more stable if the TDMA algorithm is used for pressure and temperature. The number of sweeps used may be
set to Number of Nodes/10, but should be at least 100.

4.5.4. Conjugate Heat Transfer

When the thermal properties of the non-fluid material are several orders of magnitude different from those of
the fluid, this is called an ill-conditioned conjugate heat transfer problem. In this situation, the TDMA method
probably will not yield useful results, no matter how many sweeps you specify. You access the TDMA method
using either of the following:

Command(s): FLDATA18,METH,TEMP,1
GUI: Main Menu> Solution> FLOTRAN Set Up> CFD Solver Controls> Temp Solver CFD

The Conjugate Residual method offers more functionality and requires little more memory than the Tri-Diagonal
Matrix Algorithm (TDMA) method. To access it, use either of the following:

Command(s): FLDATA18,METH,TEMP,2
GUI: Main Menu> Solution> FLOTRAN Set Up> CFD Solver Controls> Temp Solver CFD

You can control several parameters, such as convergence criteria and the number of search vectors used, to en-
hance performance. (See the discussion of FLDATA18 in the ANSYS Commands Reference for more information
about these parameters.) However, the conjugate residual method, although fairly fast, is not suited for difficult
problems.

A more robust choice for solving ill-conditioned heat transfer problems is the Preconditioned Conjugate Residual
method, which requires much more memory than either the TDMA or Conjugate Residual methods. The PCR
method allows you to control the number of search vectors used, up to a maximum of 30. To use it, use either
of the following:

Command(s): FLDATA18,METH,TEMP,3
GUI: Main Menu> Solution> FLOTRAN Set Up> CFD Solver Controls> Temp Solver CFD

Note — For nodes connected only to solid nodes, the value stored in the Jobname.RFL file under the
density (DENS) label is the product of the density and specific heat.

Section 4.5: Solution Strategies

4–5

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

You can evaluate performance of the Conjugate Residual and Preconditioned Conjugate Residual methods by
looking at the Jobname.DBG file (described in Chapter 11, “FLOTRAN CFD Solvers and the Matrix Equation”).

The most robust, but most memory-intensive, method for solving conjugate heat transfer problems is the Pre-
conditioned Generalized Minimum Residual method. You can access it via either of the following:

Command(s): FLDATA18,METH,TEMP,4
GUI: Main Menu> Solution> FLOTRAN Set Up> CFD Solver Controls> Temp Solver CFD

The Preconditioned Generalized Minimum Residual (PGMR) solution method is the default choice for temperature.

Although the same user controls exist for the PGMR method as for the PCCR solver, the default values are different.
For PGMR, the least restrictive convergence criterion allowed is 1.E-10. If you try to use a less restrictive convergence
criterion, FLOTRAN will change it to 1.E-10. A convergence criterion as low as 1.E-20 may be necessary for some
problems. In addition, you should use at least 12 search vectors, and FLOTRAN ensures this. For the PGMR solver,
12 search vectors is the default and the allowable range is 12 to 20.

FLOTRAN non-fluid elements support both temperature dependence and orthotropic variation. That is, KXX,
KYY, and KZZ can assume different values and temperature variations. FLOTRAN considers conductivity as an
element quantity, evaluated at the quadrature points in the element. However, in fluid elements, FLOTRAN
considers thermal conductivity to be a nodal quantity.

To specify the variable and orthotropic conductivities, you use the following commands or GUI paths:

Command(s): MP or MPDATA
GUI: Main Menu> Preprocessor> Loads> Load Step Opts> Other> Change Mat Props
Main Menu> Preprocessor> Material Props> Material Models> CFD> Conductivity> Orthotropic
Main Menu> Solution> Load Step Opts> Other> Change Mat Props
Main Menu> Preprocessor> Loads> Load Step Opts> Other> Change Mat Props

Note — Thermal analysis problems having variable thermal conductivity are nonlinear and require multiple
iterations to solve. Variable solid thermal conductivities are not relaxed.

For a conjugate heat transfer problem, it is wise to obtain an initial temperature solution before solving the
coupled energy/momentum equations. To achieve the temperature solution, use the following:

Command(s): FLDATA1,SOLU,FLOW,F
GUI: Main Menu> Solution> FLOTRAN Set Up> Solution Options
Command(s): FLDATA1,SOLU,TEMP,T
GUI: Main Menu> Solution> FLOTRAN Set Up> Solution Options
Command(s): FLDATA25,RELX,TEMP,1.0
GUI: Main Menu> Solution> FLOTRAN Set Up> Relax/Stab/Cap> DOF Relaxation
Command(s): FLDATA2,ITER,EXEC,1
GUI: Main Menu> Solution> FLOTRAN Set Up> Execution Ctrl
Command(s): FLDATA18,METH,TEMP,3
GUI: Main Menu> Solution> FLOTRAN Set Up> CFD Solver Contr> TEMP Solver CFD

In the above steps, an initial temperature solution is obtained from a solution of the heat conduction equation.

FLOTRAN can calculate film coefficients at walls in conjugate heat transfer problems. Two algorithms are available
for this purpose: the conductivity matrix algorithm and the temperature field algorithm. The conductivity matrix
algorithm uses the thermal conductivity matrix to calculate heat fluxes and film coefficients. It is the default.
Generally, it produces satisfactory results for well shaped elements. However, if the elements are not well shaped,
it can produce non-smooth results. You should then switch to the temperature field algorithm. It calculates film
coefficients directly from thermal gradients. To set the algorithm, use the following:

Command(s): FLDATA37,ALGR,HFLM,Value

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

4–6

Chapter 4: FLOTRAN Thermal Analyses

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Algorithm Ctr
Main Menu> Solution> FLOTRAN Set Up> Algorithm Ctr

4.6. Heat Balance

Using information in the Jobname.PFL file, you can calculate a heat balance for your problem. For any flow
problem with the thermal option activated, the energy flow into and out of the problem domain at the inlets/out-
lets is calculated and tabulated. Also calculated for the flow boundaries is the heat conduction across the
boundary faces. The difference between the energy flow into the system and out of the system at the flow
boundaries should equal the total energy added through sources and sinks.

The accuracy of the energy balance depends on the approach used to discretize the advection term in the energy
equation. In general, the Streamline Upwind/Petrov-Galerkin (SUPG) approach provides a more accurate energy
balance than the Monotone Streamline Upwind (MSU) approach. If you desire an exact energy balance, use the
Collocated Galerkin (COLG) approach. For steady-state incompressible flows, it provides an exact energy balance,
even with a coarse mesh. However, SUPG or COLG may suffer from oscillatory thermal solution near walls with
a coarse mesh. Use the FLDATA40,WADV command to minimize such spatial oscillation.

Energy flowing into or out of the system at mass flow boundaries is equal to the product of the mass flow, the
specific heat, and the temperature. A temperature offset specified by the TOFFST command does not enter this
calculation. Positive numbers mean heat flows into the system.

Energy sources include volumetric heat sources in either fluids or solids. Specified wall temperatures and specified
film coefficient boundaries are either sources or sinks, depending on the temperature gradient. Heat fluxes are
sources or sinks depending on the sign.

Heat transfer to/from wall faces refers to boundaries of fluid regions which are not inlets or outlets.

Heat transfer at wall faces refers to fluid boundaries, regardless of whether or not the boundary is a no-fluid
element or simply a no-slip condition. Positive numbers mean heat flows into the fluid.

Volumetric heat generation can be applied to solid regions or fluid regions. Be careful, when calculating the
energy balance to avoid accounting for heat generation in solids twice.

For example, suppose a conjugate heat transfer problem featured a volumetric heat source in a solid region
which is cooled by a fluid flow. The difference between the energy flow in and out should equal heat transfer to
wall faces. This number should also match the volumetric heat generation in the solid.

For all cases, the difference between the energy flowing into the system at flow boundaries and flowing out at
the boundaries should equal heat transfer to wall faces plus fluid volumetric heat sources plus the heat conduction
effects normal to the flow direction at the flow boundaries.

Essentially, FLOTRAN performs a heat balance on the fluid region only. Heat fluxes and film coefficients are
solution outputs for the external fluid boundaries only. Heat fluxes applied on external boundaries are not part
of the solution output.

The effects of viscous dissipation on a heat balance are not explicitly tabulated. The associated heat generation
is manifested in terms of an increased temperature, which in turn affects the energy departure at the outlet and
the heat transfer at wall faces if applicable. With adiabatic walls, for example, the temperature of the fluid will
increase from viscous dissipation, even though no heat sources will be apparent.

Section 4.6: Heat Balance

4–7

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

4.7. Surface-to-Surface Radiation Analysis Using the Radiosity Method

Surface-to-surface radiation analysis in FLOTRAN can be used for solving generalized radiation problems involving
two or more radiating surfaces in single or multiple open or closed enclosures. The method is supported for both
3-D and 2-D FLOTRAN elements FLUID141 and FLUID142. The thermal solution option has to be on for radiation
analysis. You can switch radiation analysis off using the FLDATA1, SOLU, RDSF command. The command defaults
to on.

Surface-to-surface radiation analysis in 2-D is supported for planar and axisymmetric geometry about YR and XR
coordinate systems. Radiation analysis is not supported for 3-D/2-D compressible flow thermal analysis and for
R-

θ and R-θ-Z coordinate system in 2-D and 3-D analysis respectively.

Elements supported for the radiosity method include:

FLOTRAN

FLUID141
FLUID142

4.7.1. Procedure

The Radiosity Solution method consists of four steps:

Define the radiating surfaces.

Define Solution options.

Define View Factor options.

Calculate and query view factors.

See Section 4.7: Using the Radiosity Solver Method in the ANSYS Thermal Analysis Guide for a detailed explanation
of these steps.

4.7.2. Heat Balances

Jobname.PFL file provides information of the net positive and negative radiation heat transfer from both solid
and fluid surfaces.

See Section 4.9: Example of Radiation Analysis Using FLOTRAN (Command Method)

4.8. Examples of a Laminar, Thermal, Steady-State FLOTRAN Analysis

This chapter describes a laminar, thermal, steady-state fluid flow problem and two ways to solve it: by choosing
items on the ANSYS GUI menus or by issuing a series of ANSYS commands.

Before you begin reading about the example, note the following:

•

The example problem described is only one of many possible FLOTRAN analyses. It does not illustrate
every technique you might use in a FLOTRAN analysis, and is intended only to show the kinds of tasks a
FLOTRAN analysis typically requires.

•

The values you enter in this example via commands or dialog boxes are specific values for this example
only. The characteristics of the individual problem you are solving dictate what values you should specify
for a particular FLOTRAN analysis.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

4–8

Chapter 4: FLOTRAN Thermal Analyses

4.8.1. The Example Described

This example evaluates buoyancy-driven flow in a square cavity with differentially heated vertical sides. It is a
laminar steady-state analysis that uses the FLUID141 2-D element. The physics modeled in this problem govern
a number of practical problems, including solar energy collection, the ventilation of rooms, and so on.

Figure 4.1 Diagram of the Square Cavity

Density variations resulting from the temperature difference across the cavity drive the laminar flow. The Rayleigh
number for this flow is 1.01E+05, and is defined as follows:

Ra = g

β ∆TL

/k µ

The symbols in this equation are:

g = gravitational acceleration

β = 1/T

∆T = T

HOT

- T

COLD

L = cavity length

ρ = density
C

= specific heat

k = thermal conductivity
µ = viscosity

Other example analysis conditions are:

•

Cavity: dimensions 0.03m x 0.03m; gravitational acceleration 9.81 m/s

•

Operating conditions: nominal temperature 193K; reference pressure 1.0135E+05 Pa

•

Fluid: Air in SI units

•

Loads: no slip walls (Vx = Vy = 0); left wall of cavity maintained at T

HOT

= 320K; right wall of cavity maintained

at T

COLD

= 280K

Section 4.8: Examples of a Laminar, Thermal, Steady-State FLOTRAN Analysis

4–9

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

4.8.2. Doing the Buoyancy Driven Flow Analysis (GUI Method)

To do the example buoyancy-driven flow analysis using the menus, perform the steps discussed in the next few
sections.

Step 1: Establish an Analysis Title and Preferences

When you have entered the ANSYS program, do these tasks:

Choose menu path Utility Menu> File> Change Title. The Change Title dialog box appears.

Enter the text "Buoyancy driven flow in a square cavity."

Click on OK.

Choose menu path Main Menu> Preferences. The Preferences for GUI Filtering dialog box appears.

Click the button for FLOTRAN CFD to "On."

Click on OK. You have just instructed the ANSYS program to do a FLOTRAN analysis.

Step 2: Define Element Types

Next, you need to specify which elements your analysis will use. The example uses only one element, FLUID141.
To define it:

Choose menu path Main Menu> Preprocessor> Element Type> Add/Edit/Delete. The Element Types
dialog box appears.

Click on Add. The Library of Element Types dialog box appears.

In the two scrollable lists, highlight (click on) FLOTRAN CFD and "2D FLOTRAN 141."

Click on OK. ANSYS returns you to the Element Types dialog box.

Click on Close.

Step 3: Create Areas

Next, create the areas you need. Our example requires an area representing the square cavity. To create it, perform
these tasks:

Choose menu path Main Menu> Preprocessor> Modeling> Create> Areas> Rectangle> By Dimen-
sions. The Create Rectangle by Dimensions dialog box appears.

Enter the X coordinates from 0.0 to 0.03.

Enter the Y coordinates from 0.0 to 0.03.

Click on OK. The square area you have just created will appear in the Graphics Window.

Step 4: Define Lines, Mesh, and Plot Elements

This step meshes the square cavity area so that you can apply temperature loads to it. Follow these steps:

Choose menu path Main Menu> Preprocessor> Meshing> MeshTool. Under the Size Controls section
of the MeshTool, click Lines,Set. The Element Size on Picked Lines picking menu appears.

Click Pick All. The Element Size on Picked Lines dialog box appears.

Set the number of element divisions to 25.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

4–10

Chapter 4: FLOTRAN Thermal Analyses

Click on OK.

In the MeshTool, select Areas from the Mesh drop down menu. Then click Quad and Free. Then click
MESH. The Mesh Areas picking menu appears.

Click on Pick All to generate the mesh.

Click on Close on the MeshTool.

Click SAVE_DB on the ANSYS Toolbar.

Step 5: Apply Velocity Boundary Conditions

In this step and Step 6, you apply boundary conditions to your model, starting with the exterior nodes. Do the
following:

Choose menu path Utility Menu> Select> Entities. The Select Entities dialog box appears.

Select Nodes and Exterior.

Click on OK.

Choose menu path Main Menu> Preprocessor> Loads> Define Loads> Apply> Fluid/CFD> Velocity>
On Nodes. The Apply V on Nodes picking menu appears.

On the picking menu, click on Pick All. The Velocity Constraints on Nodes dialog box appears.

Set the VX velocity component and VY velocity component fields to 0.

Click on OK.

Step 6: Apply Thermal Boundary Conditions

Now you need to apply temperature loads on the left and right edges of the model. To do so:

Choose menu path Main Menu> Preprocessor> Loads> Define Loads> Apply> Thermal> Temperat-
ure> On Nodes. The Apply TEMP on Nodes picking menu appears.

Click on Box. Doing this enables you to select the nodes to which you are applying loads by drawing a
box around them.

Press and drag your left mouse button to draw a box around the nodes on the left edge of the meshed
area.

Click on OK.

In the Apply TEMP on Nodes dialog box, enter 320 as the temperature value.

Click on OK.

Choose menu path Main Menu> Preprocessor> Loads> Define Loads> Apply> Thermal> Temperat-
ure> On Nodes. The Apply TEMP on Nodes picking menu appears.

On the menu, click on Box. Doing this enables you to select the nodes to which you are applying loads
by drawing a box around them.

Press and drag your left mouse button to draw a box around the nodes on the right edge of the meshed
area.

10. Click on OK.

11. In the Apply TEMP on Nodes dialog box, enter 280 as the temperature value.

12. Click on OK.

Section 4.8: Examples of a Laminar, Thermal, Steady-State FLOTRAN Analysis

4–11

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

13. Choose menu path Utility Menu> Select> Everything. This step is important; it ensures that ANSYS

includes all nodes and elements in the analysis.

14. Click on the SAVE_DB button on the Toolbar.

Step 7: Set FLOTRAN Solution Options and Execution Controls

In this step and the next few steps, you set up conditions for the FLOTRAN analysis. You first specify what type
of FLOTRAN analysis you are doing and what values will control FLOTRAN execution.

Choose menu path Main Menu> Preprocessor> FLOTRAN Set Up> Solution Options. The FLOTRAN
Solution Options dialog box appears.

Set the "Adiabatic or thermal?" field to Thermal.

Click on OK.

Choose menu path Main Menu> Preprocessor> FLOTRAN Set Up> Execution Ctrl. The Steady State
Control Settings dialog box appears.

Set the Global Iterations (EXEC) field to 200.

Set the .RFL File Overwrite Freq field to 50.

Set the Output summary frequency (SUMF) field to 50.

Click on OK.

Step 8: Set Fluid Properties

To set the fluid properties for the example analysis, do the following:

Choose menu path Main Menu> Preprocessor> FLOTRAN Set Up> Fluid Properties. The Fluid Prop-
erties dialog box appears.

Set the "Density," "Viscosity," "Conductivity," and "Specific heat" fields to AIR-SI.

Set the "Allow density variations?" field to Yes.

Click on Apply. The CFD Flow Properties dialog box appears.

Read the information about how coefficients will be calculated, then click on OK.

Step 9: Set FLOTRAN Flow Environment Parameters

To set the flow environment parameters, follow these steps:

Choose menu path Main Menu> Preprocessor> FLOTRAN Set Up> Flow Environment> Gravity. The
Gravity Specification dialog box appears.

Set the "Accel in Y direction" field to 9.81.

Click on OK.

Step 10: Solve the Problem

Set controls for the FLOTRAN solver before you initiate the solution process. Follow these steps:

Choose menu path Main Menu> Preprocessor> FLOTRAN Set Up> CFD Solver Contr> PRES Solver
CFD. The PRES Solver CFD dialog box appears.

Choose TDMA.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

4–12

Chapter 4: FLOTRAN Thermal Analyses

Click on OK. The TDMA Pressure dialog box appears.

Make sure that the value of the "No. of TDMA sweeps for pressure" field is 100. If so, click on OK.

Click on the SAVE_DB button in the Toolbar.

Choose menu path Main Menu> Solution> Run FLOTRAN.

Wait for the solution to finish, then review the information in the ANSYS Output Window. Click Close in
the Solution is done window.

Step 11: Read In Results and Plot the Temperature Solution

Perform these steps:

Choose menu path Main Menu> General PostProc> Read Results> Last Set.

Choose menu path Main Menu> General PostProc> Plot Results> Contour Plot> Nodal Solu. The
Contour Nodal Solution Data dialog box appears.

In the "Item to be Contoured" list, click on (highlight) DOF Solution.

In the scrollable list, scroll down and choose TEMP.

Click on OK. The Graphics Window shows you the following contour plot:

Figure 4.2 Plot of the Temperature Solution

Step 12: Plot Streamline Contours

Choose menu path Main Menu> General PostProc> Plot Results> Contour Plot> Nodal Solu. The
Contour Nodal Solution Data dialog box appears.

Click on (highlight) "Other quantities."

In the scrollable list, select "Strm func2D STRM" (stream function).

Section 4.8: Examples of a Laminar, Thermal, Steady-State FLOTRAN Analysis

4–13

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Click on OK. The Graphics Window shows you the following contour plot:

Figure 4.3 Plot of Streamline Contours

Step 13: Plot Velocity Vectors

For better viewing of the analysis results for the example, switch to vector plotting as described below:

Choose menu path Utility Menu> PlotCtrls> Device Options. The Device Options dialog box appears.

Set Vector mode (wireframe) to "On."

Click on OK.

Choose menu path Main Menu> General PostProc> Plot Result> Vector Plot> Predefined. The Vector
Plot of Predefined Vectors dialog box appears.

Verify that the items "DOF solution" and "Velocity" are highlighted. If so, click on OK. The display in the
Graphics Window now looks similar to the one below.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

4–14

Chapter 4: FLOTRAN Thermal Analyses

Figure 4.4 Plot of Velocity Vectors

Step 14: Plot Particle Traces Contoured by Temperature

In the example analysis, the dimensions of the problem are small (.03 x .03). Therefore, before plotting particle
trace points, you should change the working plane to give a better view from which to choose those points.

Choose menu path Utility Menu> WorkPlane> WP Settings. The WP Settings dialog box appears.

Set Snap Increment to 0.0005.

Set Spacing to 0.0001.

Set Tolerance to 0.00005.

Click on OK.

Choose menu path Utility Menu> Plot> Elements.

Choose menu path Main Menu> General Postproc> Plot Results> Flow Trace> Defi Trace Pt.

Using your mouse, pick five or six points anywhere within the upper half of the problem domain.

Click on OK in the picking menu.

10. Choose menu path Main Menu> General Postproc> Plot Results> Flow Trace> Plot Flow Trace. The

Plot Flow Trace dialog box appears.

11. In the scrollable list, click on (highlight) "Temperature TEMP".

12. Click on OK. The Graphics Window shows a plot that resembles the plot shown below. Your plot may

look different, depending on the location of the points you picked. If a warning message appears telling
you that the maximum number of loops has been exceeded, review it and click Close. For the purposes of this
problem, the particle trace is stuck in a loop by definition, so you can ignore this message.

Section 4.8: Examples of a Laminar, Thermal, Steady-State FLOTRAN Analysis

4–15

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Figure 4.5 Plot of Flow Trace

Step 15: Plot Particle Traces Contoured by Velocity Magnitude

Choose menu path Main Menu> General PostProc> Plot Results> Flow Trace> Plot Flow Trace. The
Plot Flow Trace dialog box appears.

In the scrollable list, choose "VSUM."

Click on OK. The plot shown in the Graphics Window is now contoured by velocity magnitude. How your
plot looks will depend on the location of the points you picked. If you receive another warning message
about the maximum number of loops being exceeded, click Close.

If you wish, you can use animation to enhance your analysis of particle flow. Choose menu path Util-
ity Menu> PlotCtrls> Animate> Particle Flow. When the Animate Flow Trace dialog box appears, enter
the desired animation data and click OK. (To animate particle flow, you must have at least one trace point
defined. To complete the sample analysis, simply take the defaults and click on OK.)

When you are done viewing the animation, click Stop and then Close in the Animation Controller. If ad-
ditional warning messages appear, close them.

To exit ANSYS, click Quit on the ANSYS Toolbar. Choose an exit option and then click on OK.

See Section 5.10, Doing the Sample Analysis (Command Method), for an example problem.

4.8.3. Doing the Buoyancy Driven Flow Analysis (Command Method)

To do the example buoyancy-driven flow analysis, you issue these ANSYS commands:

/TITLE,Buoyancy driven flow in a square cavity

/PREP7

ET,1,FLUID141 ! Set 2-D fluid element type

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

4–16

Chapter 4: FLOTRAN Thermal Analyses

RECTNG,,0.03,,0.03 ! Create square area

LPLOT

LESIZE,ALL, , ,25,1,0 ! Define line divisions and mesh area

AMESH,1

EPLOT

NSEL,S,EXT ! Apply velocity b.c. on exterior nodes

D,ALL,,,,,,VX,VY

NSEL,S,NODE,,1 ! Apply thermal b.c. on left edge

NSEL,A,NODE,,52

NSEL,A,NODE,,77,100

D,ALL,TEMP,320

NSEL,S,NODE,,2 ! Apply thermal b.c. on right edge

NSEL,A,NODE,,27,51

D,ALL,TEMP,280

NSEL,ALL

ESEL,ALL

FLDATA1,SOLU,TEMP,1 ! Set solution option to thermal

FLDATA2,ITER,EXEC,200 ! Set FLOTRAN execution controls

FLDATA2,ITER,OVER,50

FLDATA5,OUTP,SUMF,50

FLDATA13,VARY,DENS,1 ! Set fluid properties

FLDATA7,PROT,DENS,AIR-SI

FLDATA7,PROT,VISC,AIR-SI

FLDATA7,PROT,COND,AIR-SI

FLDATA8,NOMI,COND,-1

FLDATA7,PROT,SPHT,AIR-SI

ACEL,0,9.81,0 ! Set flow environment gravity

FLDATA18,METH,PRES,1 ! Set FLOTRAN solver controls

FLDATA19,TDMA,PRES,100

FINISH

/SOLU

SOLVE ! Solve model

FINISH

/POST1

SET,LAST

PLNSOL,TEMP ! Plot temperature solution

PLNSOL,STRM ! Plot streamline contours

/DEVICE,VECTOR,1

PLVECT,V, , , ,VECT,ELEM ! Plot velocity vectors

wpstyle,0.0005,0.0001,-1,1,0.00005,0,2,,5

EPLOT

TRPOIN,P ! The P argument enables graphical picking

! of trace points via the GUI

PLTRAC,FLUID,TEMP ! Plot particle traces contoured by

PLTRAC,FLUID,V,SUM ! temperature and velocity magnitude

FINISH

4.9. Example of Radiation Analysis Using FLOTRAN (Command Method)

The following is an example of a laminar, thermal, steady-state FLOTRAN analysis with surface-to-surface radiation
using the radiosity solution method (command method). In this example a buoyancy-driven flow in a square
cavity with differentially heated vertical walls is considered. All walls of the cavity are radiating surfaces with an
emissivity of 0.9. The final temperature distribution in the cavity effected by the presence of the radiating walls
in the fluid domain.

To do the surface-to-surface radiation problem, you issue these ANSYS commands:

/prep7

et, 1, 141 ! 2-D Fluid element

rectng, , .027744, , .027744 ! Create square cavity

esize, , 20 ! Set number of elements

amesh, all ! Mesh area

nsel, s, ext ! Select external nodes

d, all,,,,,,vx,vy ! Set all external wall velocities to zero

allsel

lsel, s, loc, x, 0.0

Section 4.9: Example of Radiation Analysis Using FLOTRAN (Command Method)

4–17

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

nsll, s, 1

d, all, temp, 500 ! Set wall temperature at x = 0.0 to 500 K

lsel, s, loc, x, .027744

nsll, s, 1

d, all, temp, 200 ! Set wall temperature at x = 0.027744 to 200 K

nsel, all

esel, all

fldata1, solu, temp, 1 ! Set solution option to thermal

fldata2, iter, exec, 200 ! Set FLOTRAN execution control

fldata2, iter, over, 50

fldata5, outp, sumf, 50

fldata13, vary, dens, 1 ! Set fluid properties

fldata7, prot, dens, air-si

fldata7, prot, visc, air-si

fldata7, prot, cond, air-si

fldata8, nomi, cond, -1

fldata7, prot, spht, air-si

acel, 0, 9.81, 0 ! Set flow environment gravity

fldata18, meth, pres, 1

fldata19, tdma, pres, 100

fldata18, meth, temp, 6

stef,5.67e-8 ! Set Stefan-Boltzmann constant

toff,0 ! Set temperature offset to zero

radopt,.5,0.0001 ! Set radiosity solver options

finish

/solu

allsel

nsel,s,ext ! Select all external nodes

sf, all, rdsf, 0.9, -1 ! Apply radiation on external faces facing inwards

allsel

solve ! Solve

finish

/post1

set last

plnsol, temp ! Plot temperature solution

plnsol, strm ! Plot streamline contours

4.10. Where to Find Other FLOTRAN Analysis Examples

Another example of a FLOTRAN analysis is the CFD Tutorial. Also, the ANSYS Verification Manual contains several
additional examples of FLOTRAN analyses. The ANSYS Verification Manual examples include:

VM46 - Flow Between Rotating Concentric Cylinders
VM121 - Laminar Flow Through a Pipe with Uniform Heat Flux
VM178 - Plane Poiseuille Flow
VM209 - Multiple Species Flow Entering A Circular Pipe
VM219 - Non-Newtonian Pressure Driven Sector Flow

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

4–18

Chapter 4: FLOTRAN Thermal Analyses

Chapter 5: FLOTRAN Transient Analyses

You activate the transient algorithm by setting the solution option, using one of these methods:

Command(s): FLDATA1,SOLU,TRAN,TRUE
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Solution Options
Main Menu> Solution> FLOTRAN Set Up> Solution Options

You must make decisions regarding the time step, the method of converging the analysis during a time step,
the length of execution of the job and the frequency of output.

What you specify via one of the following methods determines the transient execution and output:

Command(s): FLDATA4,TIME and FLDATA4A,STEP
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Execution Ctrl
Main Menu> Solution> FLOTRAN Set Up> Execution Ctrl

The final section of this chapter explains how to apply transient boundary conditions for FLOTRAN.

5.1. Time Integration Method

There are two methods available for the time integration: Backward (the default) and Newmark. The Newmark
method is more accurate than the Backward method. To specify the Newmark method, use one of the following:

Command(s): FLDATA4,TIME,METH,NEWM
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Transient Contrl> Time Integration Meth
Main Menu> Solution> FLOTRAN Set Up> Transient Contrl> Time Integration Meth

When using the Newmark method, you can introduce numerical damping to stabilize the solution.

Command(s): FLDATA4,TIME,DELT,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Transient Contrl> Time Integration Meth
Main Menu> Solution> FLOTRAN Set Up> Transient Contrl> Time Integration Meth

The Newmark parameter must be

≥

0.5. It defaults to 0.5. The recommended range is 0.5 to 0.6. Higher values

are more stable because there is more damping. Lower values result in more accurate results with 0.5 correspond-
ing to second order accuracy. For more information on the Newmark method, see Section 17.2: Transient Ana-
lysis in the ANSYS, Inc. Theory Reference.

There are two mass types that you can set for the transient analysis: lumped (the default) and consistent. The
consistent type is more dissipative than the lumped type. To specify the consistent type, use one of the following:

Command(s): FLDATA38,MASS,

Label

,CONS MSMASS,SPNUM,CONS

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Transient Contrl> Mass Type
Main Menu> Solution> FLOTRAN Set Up> Transient Contrl> Mass Type
Main Menu> Solution> FLOTRAN Set Up> Multiple Species

5.2. Time Step Specification and Convergence

Because the algorithm is implicit in nature, no stability restrictions exist on the time step size. You specify a time
step or elect to have FLOTRAN calculate a time step. To do so, use either of the following:

Command(s): FLDATA4A,TIME,STEP,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Execution Ctrl
Main Menu> Solution> FLOTRAN Set Up> Execution Ctrl

The graphical user interface will require you to set the time step if you choose the User Defined option.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

The table below shows the values you can specify. A brief description of the FLOTRAN calculation follows the
table.

Table 5.1 Specifying Values for Time Steps

Meaning

Value to Specify

User Specified Time Step

Any value > 0

Advection Limit

-1

Pressure Wave Limit

-2

Smaller of Pressure wave and Advection

-3

Conduction Limit

-4

The advection limit prevents a particle of fluid from passing completely through a finite element during a time
step.

The pressure wave limit means the time step is chosen small enough to prevent a pressure wave from passing
all the way through a finite element during a single time step. This option is active only if you choose the com-
pressible solution algorithm.

The choice of -3 (again valid only for compressible analyses) means that the more restrictive (that is, smaller)
time step criterion will be imposed.

The conduction limit is calculated to prevent the conductive diffusion of a parcel of energy completely through
an element during a time step. The limit applies only to problems that include conduction, and is valid for
problems with both fluid and non-fluid elements.

FLOTRAN must execute global iterations to converge within a time step. The time step terminates when either
of the following happens:

•

The convergence criteria are met.

•

The maximum number of global iterations allowed per time step executes.

You set the maximum number of global iterations per time step using one of the following:

Command(s): FLDATA4A,TIME,GLOB,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Execution Ctrl
Main Menu> Solution> FLOTRAN Set Up> Execution Ctrl

The convergence criteria are values below which the convergence monitors for each active degree of freedom
must drop to cause the time step to terminate. You specify these values using the following commands or menu
paths:

Command(s): FLDATA4,TIME,Label,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Execution Ctrl
Main Menu> Solution> FLOTRAN Set Up> Execution Ctrl

As soon as all the convergence criteria are met, the time step terminates. The time step terminates on the number
of global iterations allowed if the convergence monitor criteria are not met.

If the problem is adiabatic, only the pressure equation monitor is checked. Both the pressure and temperature
equation monitors must be reduced below the convergence criteria values if the temperature equation also is
solved.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

5–2

Chapter 5: FLOTRAN Transient Analyses

As soon as the convergence monitor criteria are met, the time step terminates. The time step terminates on the
number of global iterations allowed if the convergence monitor criteria are not met.

5.3. Terminating and Getting Output from a Transient Analysis

You can either specify an end time for a transient FLOTRAN analysis or have it end after a specified number of
time steps. To specify an end time, use either method shown below.

Command(s): FLDATA4,TIME,TEND,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Execution Ctrl
Main Menu> Solution> FLOTRAN Set Up> Execution Ctrl

To specify a number of time steps, either use one of the menu paths listed above or issue the following command:

Command(s):

FLDATA4,TIME,NUMB,

Value

The event that occurs first (end time or reaching the time step threshold) terminates the analysis.

You determine how often ANSYS saves the analysis results for processing and how often it writes information
to the Jobname.PFL file. You do this by choosing from the following commands or menu paths:

Command(s): FLDATA4,TIME,

Label

Value

and FLDATA4A,STEP,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Execution Ctrl
Main Menu> Solution> FLOTRAN Set Up> Execution Ctrl

The table below shows you how the values you specify affect analysis output:

Table 5.2 Saving Analysis Results for Processing

Meaning of Value

Name, Label, Value

Output results to Jobname.RFL every

time steps

STEP,APPE,

Output results to Jobname.RFL every

seconds

TIME,APPE,

Add output summary to Jobname.PFL every

time steps

STEP,SUMF,

Add output summary to Jobname.PFL every

seconds

TIME,SUMF,

Overwrite the temporary results set every

time steps

STEP,OVER,

Overwrite the temporary results set every

seconds

TIME,OVER,

If you wish to control the output based on time, you must first defeat the default controls which set APPE and
SUMF to ten steps.

5.4. Applying Transient Boundary Conditions

When any boundary conditions are changed, FLOTRAN assumes either a step change (default) or a ramp change.
The ramp is chosen by setting the BC label in the TIME item to 1 via one in the following:

Command(s): FLDATA4,TIME,BC,1
GUI: Main Menu> Preprocessor> FLOTRAN Setup> Execution Control

The ramp will occur for the next execution over the period of time for execution specified by the user. This is the
difference between the current time (i.e., the beginning in the execution) and the end time as specified by the
following:

Command(s): FLDATA4,TIME,TEND,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Setup> Execution Control

Section 5.4: Applying Transient Boundary Conditions

5–3

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

The ramp is between the “old” boundary conditions and the “new” boundary conditions. A boundary condition
is considered old as soon as FLOTRAN has gone through the calculational loop. This means that to use a ramped
condition at the beginning of an analysis, a zero iteration execution (which may be accomplished with the
FLOCHECK command) should be done with the initial condition (applied as a boundary condition) and then the
boundary condition value(s) are changed to those at the end in the ramp.

Note that the ramp is calculated with the value of TEND as specified above, NOT the actual ending time in the
case. For this reason, it is recommended that the user terminate the case with the TIME controls rather than the
STEP controls. Ensure that the case will not terminate prematurely due to an insufficient number of time steps.
If the case terminates before the time specified by TEND, upon restart the boundary conditions will be immediately
changed from where they were when the run terminated to what the current boundary condition setting is. If
you use the STEP controls in the GUI to set the number of time steps, you need to set TEND in that same dialog
box. Otherwise, TEND defaults to 1.0 x 10

and the ramp is almost nonexistent.

Transient boundary conditions on velocity DOF (VX, VY, and VZ) must not be ramped from zero to a nonzero
value. A very small velocity must be used instead of zero so that FLOTRAN recognizes the face as an inlet or
outlet rather than a wall.

At any time, you can change the applied boundary conditions to the "old" state with one of the following:

Command(s): FLOCHECK,2
GUI: Main Menu> Preprocessor> FLOTRAN Setup> Flocheck

FLOCHECK,2 has no effect on the Jobname.RFL file.

Caution: FLOTRAN has no record of boundary conditions at earlier times. That is, if you want to restart
from an earlier point in time and simulate a ramped boundary condition it is necessary to apply the
boundary condition appropriate for the beginning of the ramp, make it an old condition via the FLOCHECK
command, and then apply the condition at the end of the ramp.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

5–4

Chapter 5: FLOTRAN Transient Analyses

Chapter 6: Volume of Fluid (VOF) Analyses

6.1. Overview

In a Volume of Fluid (VOF) analysis, FLOTRAN uses an advection algorithm for the volume fraction (VFRC) to track
the evolution of the free surface. The VFRC value for each element varies from zero to one, where zero denotes
an empty or void element and one denotes a full or fluid element. The values between zero and one indicate
that the corresponding elements are the partially full or surface elements (henceforth called partial elements),
and the free surface can thus be determined by the distribution of the VFRC field.

For the dynamic behavior at the interface between a gas and liquid, FLOTRAN uses a continuum surface force
(CSF) method to model the surface tension. Surface tension is an inherent characteristic of material interfaces.
It is a localized surface force acting on the interface. FLOTRAN reformulates this surface force into an equivalent
volumetric force in the momentum equation. This force consists of two components: a normal component to
the interface due to local curvature and a tangential component to the interface due to local variations of the
surface tension coefficient.

Currently, VOF capability is available only for quadrilateral elements for two dimensional planar or axisymmetric
analyses. For a VOF analysis, boundary conditions are required for boundary nodes that belong to at least one
non-empty (partial or full) element.

To activate a VOF analysis in FLOTRAN and model the surface tension effect, use the following commands or GUI
menu paths:

Command(s): FLDATA1,SOLU,VOF,

Value

FLDATA1,SOLU,SFTS,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Setup> Solution Options
Main Menu> Solution> FLOTRAN Setup> Solution Options

In FLOTRAN, the VOF algorithm first computes the motion of the polygon of fluid in a Lagrangian sense and then
utilizes the computational geometry of the intersection of two polygons to determine the VFRC fluxes. This
method is referred to as the Computational Lagrangian-Eulerian Advection Remap (CLEAR) method. See the
ANSYS, Inc. Theory Reference for information on the theoretical background. This CLEAR-VOF method tracks the
free surface explicitly in time, and it is therefore necessary to activate the transient solution option for a VOF
analysis. Refer to Chapter 5, “FLOTRAN Transient Analyses” for information on the selection of the transient
parameters, such as the time step, converging method, execution length and the output frequency. For accuracy,
you should use the Streamline Upwind Petrov-Galerkin (SUPG) approach described in Chapter 14, “Advection
Discretization Options”. If you encounter a convergence difficulty, the time increment may be reduced, and the
modified inertial relaxation (MIR) scheme may also be activated for robustness.

Caution: You should avoid using quadrilateral elements with only one node on the inflow or outflow
boundary.

6.2. VFRC Loads

When performing a VOF analysis, you need to apply both initial and boundary VFRC loads. In most cases, default
values are appropriate.

6.2.1. Initial VFRC Loads

You impose initial conditions for the velocity and other degrees of freedom in the usual manner. For the initial
VFRC field, you can define each element as initially full, partially full or empty. Take care when initially setting
partial elements. Each partial element must be adjacent to at least one full element and one empty element.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

During the analysis, if a partial element does not have any full elements as neighbors, it will be reset to empty.
You should also include at least one layer of empty elements above the free surface to allow the surface to evolve
in time.

To set the initial volume fraction field, use one of the following:

Command(s): ICE,ELEM,VFRC,

Value

GUI: Main Menu> Preprocessor> Loads> Define Loads> Apply> Fluid/CFD> Volume Fract> Init
Loads> On Elements
Main Menu> Solution> Define Loads> Apply> Fluid/CFD> Volume Fract> Init Loads> On Elements

By default, the volume fraction is zero. Therefore, if there is fluid initially inside the problem domain, you must
set the VFRC field accordingly.

To set the initial volume fraction for a given geometry, use one of the following:

Command(s): ICVFRC,

GEOM

VAL1

VAL2

VAL3

VAL4

GUI: Main Menu> Preprocessor> Loads> Define Loads> Apply> Volume Fract> Init Loads> By
Geom
Main Menu> Solution> Define Loads> Apply> Fluid/CFD> Volume Frac> Init Loads> By Geom

ICVFRC automatically calculates the volume fraction value for all selected elements that are either inside the
given geometry or intersect with it. The volume fraction is:

•

One for elements completely within the geometry

•

A fraction equal to the element area within the geometry for elements intersected by the boundary of
the geometry

Currently, there are two valid geometries: circle (CIRC) and ellipse (ELPT). For a circle or ellipse, VAL1 and VAL2
are the x and y coordinates of the center, respectively. For a circle, VAL3 is the radius and VAL4 is not used. For
an ellipse, VAL3 and VAL4 are the x and y semiaxes, respectively.

To display the initial volume fraction loads, use the following:

Command(s): /PICE,

VFRC

KEY

GUI: Utility Menu> PlotCtrls> Symbols

The /PBF and /PSF commands override the /PICE command.

6.2.2. Boundary VFRC Loads

You impose boundary conditions for the velocity and other degrees of freedom in the usual manner. Although
boundary conditions outside the fluid region have no physical meaning initially, these conditions will become
active if the fluid touches these boundaries. Accordingly, you should apply all appropriate boundary conditions
on all boundaries potentially touched by the fluid. FLOTRAN treats unspecified boundaries with natural conditions.

Boundary conditions for VFRC loads consist of the boundary VFRC value and the wetting status. FLOTRAN only
allows zero (empty) and one (full) values for the boundary VFRC values. By default, boundary VFRC values are
set to one (full). FLOTRAN uses the boundary VFRC values to determine the normal surface direction in the VOF
reconstruction stage, when the boundary is adjacent to the surface elements. The wetting status specifies
whether the fluid can be advected into the problem domain. A zero value indicates a non-wetting boundary,
whereas a unity value indicates a wetting boundary. By default, wetting status is set to zero (non-wetting
boundary). On a wetting boundary, fluid advection into the problem domain takes place. The corresponding
boundary VFRC value must be set to unity to be meaningful. On a non-wetting boundary, advection of the fluid
or void elements into the problem domain does not take place. The boundary VFRC value only acts passively to
help determine the normal surface direction.

To set boundary VFRC loads, use one of the following:

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

6–2

Chapter 6: Volume of Fluid (VOF) Analyses

Command(s): SFL,

LINE

,VFRC,

VALI

VALJ

VAL2I

VAL2J

SFE,

ELEM

LKEY

,VFRC,

KVAL

VAL1

VAL2

VAL3

VAL4

GUI: Main Menu> Preprocessor> Loads> Define Loads> Apply> Fluid/CFD> Volume Fract> Bound
Loads> On Lines
Main Menu> Preprocessor> Loads> Define Loads> Apply> Fluid/CFD> Volume Fract> Bound
Loads> On Elements
Main Menu> Solution> Define Loads> Apply> Fluid/CFD> Volume Fract> Bound Loads> On Lines
Main Menu> Solution> Define Loads> Apply> Fluid/CFD> Volume Fract> Bound Loads> On Elements

For the SFL command,

VALI

specifies the boundary VFRC value and (defaults to 1)

VAL2I

specifies the wetting

status (defaults to non-wetting). If

Lab

= VFRC, a

VAL2I

setting of 1 indicates a wetted boundary. For the SFE

command,

VAL1

specifies the boundary VFRC value (defaults to 1) when

KVAL

= 0 or 1, and

VAL1

specifies the

boundary wetting status (defaults to non-wetting) when

KVAL

= 2. If

Lab

= VFRC and

KVAL

= 2, a

VAL1

setting

of 1 indicates a wetted boundary. At a wetted boundary, the fluid upstream keeps the associated elements full.

6.3. Input Settings

When performing a VOF analysis, you may set the environmental conditions regarding the ambient conditions,
the VFRC tolerances, and the time stepping strategy.

When studying surface tension effects, you need set the proper values for the surface tension coefficient and
the wall static contact angle. Refer to Chapter 9, “Specifying Fluid Properties for FLOTRAN” for information on
these property types.

6.3.1. Ambient Conditions

Set the ambient nodal values outside the fluid region for the following variables:

VX - U velocity
VY - V velocity
VZ - W velocity
TEMP - Temperature
ENKE - Turbulent Kinetic Energy
ENDS - Turbulent Dissipation Rate

using one of the following:

Command(s): FLDATA36,AMBV,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Setup> VOF Environment> Ambient Condit'n
Main Menu> Solution> FLOTRAN Setup> VOF Environment> Ambient Condit'n

When a boundary node with Dirichlet Condition lies outside the fluid region, the assigned ambient values on
this node are ignored. The prescribed Dirichlet Condition will become active once its associate element becomes
partially full or full. Except for pressure, the ambient values are only set for postprocessing purposes. Pressure
acts as an actual boundary condition.

Unlike other FLOTRAN analyses, the pressure field for a VOF analysis will include both the dynamic pressure and
the static pressure and the static pressure will be in balance with the gravitational acceleration terms. For example,
in a VOF analysis, the pressure contours for a parallel uniform flow with gravity will consist of parallel lines with
a gradient balancing gravity, whereas they remain constant for other FLOTRAN analyses.

In a VOF analysis, an outlet can have specified pressures or it can have natural conditions. When outlet pressures
are specified, the values will differ from those in other FLOTRAN analyses by the offsets of the static pressure (or
elevation head). For natural boundary conditions the outlet pressures will adjust automatically. In that case, if a
steady state solution exists, the outlet pressures will converge to the correct values.

Section 6.3: Input Settings

6–3

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

6.3.2. VFRC Tolerances

Ideally, a VFRC value of one signifies a full or fluid element and a value of zero signifies an empty or void element.
In reality, however, exact values of one and zero are difficult to maintain in the VOF advection algorithm due to
various types of error accumulations. Hence, FLOTRAN introduces small cutoff values to determine the full and
empty elements. An element is considered full if its VFRC value is greater than or equal to 1 - VOFU, where VOFU
is the upper tolerance for the VOF advection algorithm. An element is considered empty if its VFRC value is less
than or equal to VOFL, where VOFL is the lower tolerance for the VOF advection algorithm. By default, VOFL and
VOFU are both set to 10

-5

In the FLOTRAN solution routines, a nearly empty element adjacent to a nearly full element may introduce an
abrupt change in the locally rescaled meshes. This can make the stiffness matrix more ill-conditioned and can
adversely affect the quality of the desired solution. To avoid this, FLOTRAN introduces another tolerance to not
assemble the finite element equations for those elements with VFRC values less than or equal to LAML for lam-
inar flows and TRBL for turbulent flows, where LAML and TRBL are the lower tolerances for laminar and turbulent
flows, respectively. Similarly, elements with VFRC values greater than or equal to 1 - LAMU for laminar flows and
1 - TRBU for turbulent flows are considered full when assembling the finite element equations. You can set any
of these tolerance values. By default, LAML and LAMU are set to 10

-2

and TRBL and TRBU are set to 10

-1

To set any of the tolerance values, use one of the following:

Command(s): FLDATA35,VFTOL,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Setup> VOF Environment> VFRC Tolerance
Main Menu> Solution> FLOTRAN Setup> VOF Environment> VFRC Tolerance

6.3.3. VOF Time Steps

Because the CLEAR-VOF is explicit in time, it must use a time step for the VOF advection algorithm that corresponds
to a CFL number less than one. On the other hand, selecting the time step based on the VOF constraint may be
too restrictive sometimes because the FLOTRAN transient solution algorithm is implicit in time, and there is no
stability restriction on the time step size. Accordingly, FLOTRAN allows multiple VOF advection steps per solution
step. The VOF advection time step is set equal to the solution time step divided by a factor that you specify. If
the VOF advection time step is still too large, FLOTRAN will automatically reduce the VOF time step by half. This
automatic reduction in the VOF time step continues until the local imbalance of the VFRC field during the VOF
advection computations is less than the VOFL tolerance. A good input parameter guess makes the calculation
more efficient by removing some checks on the time step.

To set the number of VOF advection time steps per solution time step, use one of the following:

Command(s): FLDATA4,TIME,NTVF,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Setup> VOF Environment> Time Stepping
Main Menu> Solution> FLOTRAN Setup> VOF Environment> Time Stepping

For a VOF analysis, the density is constant. Therefore, mass conservation is equivalent to the conservation of the
total fluid volume (or area in two dimensions). Ideally, the difference between the volume coming into the
problem domain and going out of the domain should be equal to the increase or decrease of the total volume
inside the domain. In an actual finite element analysis, however, continuity satisfaction is expressed in a Galerkin
weak form. Therefore, in general, each element has a small mass imbalance. The local mass imbalance is usually
of the order of the discretization error, and this error is a major source of the global VFRC imbalance introduced
in a VOF analysis. Even though this imbalance may be very small compared to the total volume, it can accumulate
exponentially as the number of time steps increases. Hence, FLOTRAN performs a global adjustment of the VFRC
field at each VOF time step. It proportionally increases or decreases the VFRC values of the partial elements to
guarantee the global VFRC balance. It prints the final VFRC imbalance in the Jobname.PFL file.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

6–4

Chapter 6: Volume of Fluid (VOF) Analyses

6.4. Postprocessing

The volume fraction is stored as a non-summable miscellaneous record in the element data section of the results
file. If you want to view the volume fraction, issue the command:

Command(s):

PLESOL,NMISC,1

Since the volume fraction is essentially an element based quantity, it is discontinuous across elements. If you
wish to see a smooth and continuous volume fraction, you should first store the results in an element table, using
one of the following:

Command(s): ETABLE,VFRC,NMISC,1
GUI: Main Menu> General Postproc> Element Table> Define Table

You can then plot the results with an averaging operation, using one of the following:

Command(s): PLETAB,VFRC,1
GUI: Main Menu> General Postproc> Element Table> Plot Elem Table

However, instead of using the foregoing commands, you can use one of the following:

Command(s): PLVFRC,

CONT

GUI: Main Menu> General Postproc> Plot Results> Contour Plot> Element Solu

The PLVFRC macro issues the ETABLE and PLETAB commands. When

CONT

= 0, PLVFRC uses contour levels of

0.5 and 1.0 to indicate the free surface and fluid regions. When

CONT

= 1, it uses the current contour settings.

You can also animate your results. To obtain an animation over a time sequence by interpolation between time
steps, use the PLVFRC command macro along with one of the following:

Command(s): PLVFRC,

CONT

ANTIME,

NFRAM

DELAY

NCYCL

AUTOCNTRKY

RSLTDAT

MIN

MAX

GUI: Utility Menu> PlotCtrls> Animate> Over Time

To produce an animation based on the time steps without interpolation, use the PLVFRC command macro along
with one of the following:

Command(s): PLVFRC,

CONT

ANDATA,

DELAY

NCYCL

RSCLDAT

MIN

MAX

INCR

FRCLST

AUTOCNTRKY

GUI: Utility Menu> PlotCtrls> Animate> Over Results

Note that if

CONT

= 0, the animation is based on two contour levels of 0.5 and 1.0. If

CONT

= 1, the animation is

based on AUTOCNTRKY setting.

6.5. VOF Analysis of a Dam

6.5.1. The Problem Described

In this example, two vertical walls confine a rectangular column of stationary water. When the right wall is removed,
the water flows out onto a rigid horizontal plane. The ICE command sets the initial volume fraction field.

6.5.2. Building and Solving the Model (Command Method)

The following command stream shows all the relevant parameters and solution strategy. All text prefaced with
an exclamation point (!) is a comment.

/BATCH,LIST

/title, broken dam problem by the VOF solution.

/com

/com ------------------------------------------------------------------

/com ** Reference: "Part IV: An Experimental Study of the Collapse of

Section 6.5: VOF Analysis of a Dam

6–5

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

/com ** Liquid Columns on a Rigid Horizontal Plane"

/com ** By Martin and Moyce, Phil. Trans. Roy. Soc.

/com ** (London,A244, pp. 312-324, 1952.

/com ** "Volume of Fluid (VOF) Method for the Dynamics of

/com ** Free Boundaries" By C.W. Hirt and B.D. Nichols,

/com ** J. Comput. Physics, Vol. 39, pp. 201-225, 1981.

/com **

/prep7

!!!!! Define some dimensions and gravity

LX = 5.0 ! X length

LY = 2.5 ! Y length

DELX = 0.2 ! X spacing

DELY = 0.05 ! Y spacing

grav = 9.81 ! Gravity

et,1,141

!!!! meshing

rect,0,LX,0,LY

lsel,s,,,2,4,2

lesize,all,DELY

lsel,s,,,1,3,2

lesize,all,DELX

amesh,all

nsel,s,loc,y,0.0 ! Wall boundary conditions

nsel,a,loc,x,0.0

d,all,vx,0.0

d,all,vy,0.0

nsel,s,loc,x,0.0,1.0 ! Setup initial VFRC

nsel,r,loc,y,0.0,2.0

esln,s,1

ice,all,vfrc,1.0

alls ! Initial conditions for vx & vy

ic,all,vx,0

ic,all,vy,0

save

fini

/solu

!!!! FLOTRAN input

acel,0.0,grav,0

FLDA,NOMI,DENS,1.0e3

FLDA,NOMI,VISC,1.0d-3

FLDA,SOLU,FLOW,T

FLDA,SOLU,TRAN,T

FLDA,SOLU,turb,F

flda,solu,vof,t

flda,time,glob,5

flda,time,numb,70

flda,time,step,0.01

flda,time,appe,0.1

flda,advm,mome,supg

flda,relx,vx,0.5

flda,relx,vy,0.5

flda,relx,pres,1.0

solve

fini

exit,nosa

6.6. VOF Analysis of Open Channel with an Obstruction

6.6.1. The Problem Described

In this example, water flows in an open channel with a semicircular obstruction on the bottom. The computation
uses the standard k-

ε turbulence model since the turbulence model is not very important for the prediction of

the free-surface shape. The solution domain extends five cylinder diameters upstream and five diameters

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

6–6

Chapter 6: Volume of Fluid (VOF) Analyses

downstream of the obstruction. The fluid starts to fill the domain at the beginning of the simulation. The SFE
and SFL commands set a wetting boundary on the left inlet.

6.6.2. Building and Solving the Model (Command Method)

The following command stream shows all the relevant parameters and solution strategy. All text prefaced with
an exclamation point (!) is a comment.

/BATCH,LIST

/title, initial development of flow over a bump.

/com

/com ------------------------------------------------------------------

/com ** Initial development of flow over a semicircular bump

/com ** Reference: "Critical Free-Surface Flow Over a Semi-Circular

/com ** Obstruction" By L.K. Forbes, J. Eng. Math.,

/com ** vol. 22, pp. 3-13, 1998.

/com ** "Computation of free-surface flows using the

/com ** finite-volume method and moving grids",

/com ** By S. Muzaferija and M. Peric, Numerical Heat

/com ** Transfer, Part B, 32:369-384, 1997.

/com ------------------------------------------------------------------

! Property and parameter input

rho = 1.0e0 ! Density

grav = 9.81 ! Gravity

mu = 1.0e-6 ! Viscosity

R = 0.03 ! Bump radius

L = 2*R

H = 0.075 ! Inlet height

H0 = R ! Height above the Inlet

outlen = 5.0*R ! Outlet length

inlen = 5.0*R ! Inlet length

ny1 = 8 ! Number of elements in line 1

ny2 = 2 ! Number of elements in line 2

ny3 = 4 ! Number of elements in line 3

ry2 = 1.0 ! Ratio of element size in line 2

ry3 = 1.0 ! Ratio of element size in line 3

nx1 = 15 ! Number of elements in line 13

nx2 = 15 ! Number of elements in line 21

nx3 = 20 ! Number of elements in line 17

rx1 = 0.5 ! Ratio of element size in line 13

rx2 = 1.0 ! Ratio of element size in line 25

rx3 = 1.5 ! Ratio of element size in line 17

nr1 = 10 ! Number of elements in radial direction near bump

/prep7

et,1,141

k,1,-inlen,0.0 ! KP 1 - 4 are at the inlet

k,2,-inlen,L

k,3,-inlen,H

k,4,-inlen,H+H0

l,1,2 ! Lines 1-3 are the inlet line

l,2,3

l,3,4

k,5,-L,0.0 ! KP 5 - 8 are before the bump

k,6,-L,L

k,7,-L,H

k,8,-L,H+H0

l,5,6 ! Lines 4-6 before the bump

l,6,7

l,7,8

k,9,L,0.0 ! KP 9 - 12 are after the bump

k,10,L,L

k,11,L,H

Section 6.6: VOF Analysis of Open Channel with an Obstruction

6–7

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

k,12,L,H+H0

l,9,10 ! Lines 7-9 after the bump

l,10,11

l,11,12

k,13,outlen,0.0 ! KP 13 - 16 are at the outlet

k,14,outlen,L

k,15,outlen,H

k,16,outlen,H+H0

l,13,14 ! Lines 10-12 at the outlet

l,14,15

l,15,16

l,1,5 ! Lines 13-16 are horizontal lines near inlet

l,2,6

l,3,7

l,4,8

l,9,13 ! Lines 17-20 are horizontal lines near outlet

l,10,14

l,11,15

l,12,16

l,6,10 ! Lines 21-23 are horizontal lines near the bump

l,7,11

l,8,12

k,17,R,0.0 ! KP 17 to 23 are for the semicircular bump

k,18,0.0,0.0

circle,18,R,,17,180,4

lcomb,25,26,0

l,19,9 ! Lines 26, 28-30 in radial direction near bump

l,20,10

l,22,6

l,23,5

! Select lines and establish line divisions

lsel,s,,,1,4,3

lesize,all,,,ny1

lsel,s,,,2,11,3

lesize,all,,,ny2,ry2

lsel,s,,,3,12,3

lesize,all,,,ny3,ry3

lsel,s,,,13,16

lesize,all,,,nx1,rx1

lsel,s,,,21,23

lesize,all,,,nx2,1.0/rx2

lsel,s,,,25

lesize,all,,,nx2,rx2

lsel,s,,,17,20

lesize,all,,,nx3,rx3

lsel,s,,,27

lesize,all,,,ny1

lsel,s,,,26

lsel,a,,,28,30

lesize,all,,,nr1

! define the y-direction mesh

lsel,s,,,24

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

6–8

Chapter 6: Volume of Fluid (VOF) Analyses

lsel,a,,,7

lsel,a,,,10

lesize,all,,,nx2,1.5

alls

! Create areas....

a,1,5,6,2 ! Inlet

a,2,6,7,3

a,3,7,8,4

a,9,13,14,10 ! Outlet

a,10,14,15,11

a,11,15,16,12

a,6,10,11,7 ! Bump

a,7,11,12,8

a,19,9,10,20

a,20,10,6,22

a,5,23,22,6

alls

amesh,all

! Inlet boundary condition

lsel,s,,,1,2

nsll,,1

d,all,vx,0.32

d,all,vy,0.0

nsel,s,loc,x,-inlen

nsel,r,loc,y,0.0

d,all,vx,0.001

! boundary volume fraction (SFL and SFE commands)

sfl,1,vfrc,1,,1

sfl,2,vfrc,1,,1

!!!! The walls

lsel,s,,,13

lsel,a,,,17

lsel,a,,,24,25

lsel,a,,,27

lsel,a,,,26

lsel,a,,,30

nsll,,1

d,all,vx,0

d,all,vy,0

alls

/solu

!!!! FLOTRAN Input

acel,0.0,grav,0.0

FLDA,SOLU,VOF,ON

FLDA,SOLU,FLOW,ON

FLDA,SOLU,TRAN,ON

FLDA,SOLU,TURB,ON

FLDA,TIME,GLOB,3

FLDA,TIME,NUMB,50

FLDA,TIME,STEP,1e-2

FLDA,TIME,APPE,0.1

FLDA,TIME,PRES,1.0E-6

FLDA,ADVM,MOME,SUPG

flda,relx,vx,0.5

flda,relx,vy,0.5

flda,relx,pres,1.0

flda,prot,dens,constant ! Constant density

flda,prot,visc,constant ! Constant viscosity

flda,nomi,dens,rho ! Density set earlier

flda,nomi,visc,mu ! Viscosity set earlier

solve

fini

exit,nosa

Section 6.6: VOF Analysis of Open Channel with an Obstruction

6–9

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

6.7. VOF Analysis of an Oscillating Droplet

6.7.1. The Problem Described

This example examines the interesting phenomenon of a liquid droplet oscillating in an dynamically inactive
gas. For small amplitudes, the angular frequency,

ω, is given by the following formula from A. Prosperetti, ("Free

Oscillations of Drops and Bubbles: The Initial-Value Problem," Journal of Fluid Mechanics, Vol. 100, p. 333, 1980):

= [8 - 5 / Re

]

(

)

where

ρ is the density, σ is the surface tension coefficient, and R

is the radius of the drop at its equilibrium state.

Here, Re is the Reynolds number given by:

Re =

ρσ

where µ is the dynamic viscosity of the liquid.

When the oscillation is fully damped by the viscosity, the droplet takes a spherical shape and the droplet pressure
is given by:

theory

The droplet analyzed here is initially elliptical with major and minor semiaxes of 24.69 mm and 18 mm, respectively.
This corresponds to a final radius of R

of 20 mm. The time increment,

∆t, is set to 2 x 10

-4

ms.

The material properties of the droplet are:

•

ρ = 10

mg/(µm)

•

µ = 10

mg/(µm)(ms)

•

σ = 0.073 mg/(ms)

The Prosperetti formula gives an oscillation frequency of 43.0 kHz.

6.7.2. Results

Figure 6.1: “Instantaneous Pressure Distributions at 0.001 ms” and Figure 6.2: “Instantaneous Pressure Distributions
at 0.012 ms” show the instantaneous pressure distributions at 0.001 ms and 0.012 ms, respectively. Rather than
a pressure jump across the interface, the pressure is observed to vary smoothly in a thin transition region near
the interface. Initially, the maximum pressure occurs at the top and bottom portion of the droplet due to a high
local curvature. The resulting pressure gradient forces the fluid inward and redirects it to the sides. As the droplet
moves, the pressure starts to rise at the sides due to the increasing local curvature. This slows down the movement
of the droplet and eventually forces the fluid back inward from the sides. The pressure distribution controls the
droplet oscillation by balancing the kinetic energy and the potential energy due to the surface tension. The
simulation produces a free surface profile every 5 time steps. The frequency is 42.6 kHz (two cycles occur in 0.047
ms). This agrees quite well with the 43.0 kHz predicted by the Prosperetti formula. The oscillation amplitude

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

6–10

Chapter 6: Volume of Fluid (VOF) Analyses

decreases with time and damps out at 0.2 ms due to viscosity. Averaging the pressure values on interior nodes
attached to only full elements gives the numerical droplet pressure. The difference between the numerical and
the analytical pressure is approximately 1%. There are some noises in the velocity field near the interface due to
the so-called parasitic currents inherent in the CSF formulation.

Figure 6.1 Instantaneous Pressure Distributions at 0.001 ms

Figure 6.2 Instantaneous Pressure Distributions at 0.012 ms

Section 6.7: VOF Analysis of an Oscillating Droplet

6–11

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

6.7.3. Building and Solving the Model (Command Method)

The following command stream shows all the relevant parameters and solution strategy. All text prefaced with
an exclamation point (!) is a comment.

/title, oscillating axisymmetric drop problem by the VOF/CSF solution.

/nopr

LX = 30 ! x length in micrometer (um)

LY = 30 ! y length in micrometer (um)

RadF = 20 ! radius of the final sphere in micrometer (um)

aRad = 18 ! x radius in micrometer (um)

bRad = RadF**3/aRad**2 ! y radius in micrometer (um)

DELX = 0.1*RadF ! x spacing in micrometer (um)

DELY = 0.1*RadF ! y spacing in micrometer (um)

DELT = 2.0e-4 ! time increment in millisecond (ms)

APPT = DELT*5 ! append time in millisecond (ms)

NDT = 1000 ! total number of time steps

Sigm = 0.073 ! SFTS coefficient in unit of (mg)/(ms)^2

rho = 1.0e-9 ! density in unit of (mg)/(um)^3

mu = 1.0e-6 ! viscosity in unit of (mg)/(um)(ms)

pexact=2*Sigm/RadF ! theoretical pressure in equilibrium

/prep7

et,1,141,,,1 ! RY geometry

rect,0,LX,-LY,LY

lsel,s,,,2,4,2

lesize,all,DELY

lsel,s,,,1,3,2

lesize,all,DELX

amesh,all

nsel,s,loc,x,0 ! symmetry condition

d,all,vx,0.0

alls

icvf,elpt,0.0,0.0,aRad,bRad ! initial VFRC

ic,all,vx,0 ! initial velocity

ic,all,vy,0

save

fini

/solu

flda,solu,tran,t

flda,solu,vof,t

flda,solu,sfts,t

flda,nomi,sfts,sigm

flda,nomi,dens,rho

flda,nomi,visc,mu

flda,time,glob,10

flda,time,numb,NDT

flda,time,step,DELT

flda,advm,mome,supg

flda,mir,mome,1.0

flda,relx,pres,1.0

flda,time,appe,APPT

solve

fini

/post1

set,last

PLVFRC,0

ANDATA,0.1, ,2,1,51,1,0.0,1

set,last

*GET,VFAdvU,FLDA,VFTO,VOFU

VFAdvU=1.0-VFAdvU

alls

*get,elmmax,elem,0,count ! Get the number of elements

*get,elmi,elem,0,num,min ! Get the lowest elem number in the set

*get,vfval,elem,elmi,nmis,1 ! Get the VFRC for the element

*IF,vfval,LE,VFAdvU,then

esel,u,,,elmi ! Remove elmi from the active set

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

6–12

Chapter 6: Volume of Fluid (VOF) Analyses

*ENDIF

*do,ilop,2,elmmax ! Loop over selected elements

*get,elmn,elem,elmi,nxth ! Get the next higher elem number in the set

*get,vfval,elem,elmn,nmis,1 ! Get the VFRC for the element

*IF,vfval,LE,VFAdvU,then

esel,u,,,elmn ! Remove elmn from the active set

*ELSE

elmi=elmn

*ENDIF

*enddo

nsle,s,all ! select all node attached to elements

nsel,u,ext ! unselect ext. nodes of prev. selected nodes

pavg=0.0

prms=0.0

*get,nodmax,node,0,count ! Get the number of selected nodes

*do,ilop,1,nodmax ! Loop over the number of nodes

*get,nodi,node,0,num,min ! Get the lowest node number in the set

*get,pval,node,nodi,pres ! Get the y

pavg=pavg+pval ! pressure sum

prms=prms+(pval-pexact)**2 ! pressure rms

nsel,u,,,nodi ! Remove node from the active set

*enddo

pavg=pavg/nodmax

prms=sqrt(prms/nodmax)/pexact

/go

*vwrite

(9x,'DelX/Rad ', 3x, 'PRES / Pexact ',3x,'Prms ')

*vwrite,DELX/RadF,pavg/pexact,prms

(3(4x,1pe12.5))

fini

exit,nosa

6.7.4. Where to Find Other Examples

For more examples on the VOF analysis of free surface problems with surface tension, refer to G. Wang, (“Finite
Element Simulations of Gas-Liquid Flows with Surface Tension,” International Mechanical Engineering Congress
& Exposition, November 5-10, 2000, Orlando, Florida).

Section 6.7: VOF Analysis of an Oscillating Droplet

6–13

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

6–14

Chapter 7: Arbitrary Lagrangian-Eulerian (ALE)
Formulation for Moving Domains

7.1. Introduction

Fluid flow problems often involve moving interfaces. The interfaces can be moving internal walls (for example,
a solid moving through a fluid), external walls, or free surfaces. In such problems, the fluid domain changes with
time and the finite element mesh must move to satisfy the boundary conditions at the moving interfaces. You
can use the Arbitrary Lagrangian-Eulerian (ALE) formulation to solve problems of this type.

Figure 7.1: “Torsional Mirror at t = 0 Seconds” illustrates a typical fluid flow problem requiring the ALE formulation.
It involves a micro-electromechanical system (MEMS) device with a viscous fluid between two rigid plates. Initially,
the plates are parallel and the fluid is at rest.

Figure 7.1 Torsional Mirror at t = 0 Seconds

The top plate begins to oscillate about its centerline setting the fluid in motion. The ALE formulation allows the
fluid domain to change with time and the finite element mesh to move to satisfy the boundary conditions at
the moving plate. Figure 7.2: “Torsional Mirror at t = 2.5 Seconds” and Figure 7.3: “Torsional Mirror at t = 7.5
Seconds” show the finite element mesh at later times.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Figure 7.2 Torsional Mirror at t = 2.5 Seconds

Figure 7.3 Torsional Mirror at t = 7.5 Seconds

To perform a transient analysis employing the ALE formulation, you must activate the ALE formulation and the
transient solution algorithm. To activate the ALE formulation, you use one of the following:

Command(s): FLDATA1,SOLU,ALE,TRUE
GUI: Main Menu> Preprocessor> FLOTRAN Setup> Solution Options
Main Menu> Solution> FLOTRAN Setup> Solution Options

To activate the transient algorithm, you use one of the following:

Command(s): FLDATA1,SOLU,TRAN,TRUE
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Solution Options
Main Menu> Solution> FLOTRAN Set Up> Solution Options

For more information on transient analyses and the transient algorithm, see Chapter 5, “FLOTRAN Transient
Analyses”.

To do an ALE analysis, you need to use one of the following elements:

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

7–2

Chapter 7: Arbitrary Lagrangian-Eulerian (ALE) Formulation for Moving Domains

FLUID141, KEYOPT(3) = 0 (Cartesian coordinates), 1 (axisymmetric about Y-axis), or 2 (axisymmetic about X-axis).

FLUID142, KEYOPT(3) = 0 (Cartesian coordinates). You cannot use a cylindrical coordinate system (KEYOPT(3) =
3) with ALE.

You will need to activate KEYOPT(4) to specify boundary motions (displacement DOFs). To define the element
type, use one of the following:

Command(s): ET,

ITYPE

Ename

KOP1

KOP2

KOP3

KOP4

KOP5

KOP6

KEYOPT,

ITYPE

KNUM

VALUE

GUI: Main Menu> Preprocessor> Element Type> Add/Edit/Delete

Currently, free surfaces are not a part of the ALE formulation. However, you can use the Volume of Fluid (VOF)
method in conjunction with the ALE formulation to simulate flows involving free surfaces and moving walls.
(Refer to Chapter 6, “Volume of Fluid (VOF) Analyses”.)

7.2. Boundary Conditions

Generally, either slip or stick boundary conditions apply for moving internal or external walls (See Fig-
ure 7.4: “Boundary Conditions for Moving Walls”.)

Figure 7.4 Boundary Conditions for Moving Walls

#"$"% & '("

)

./0

Table 7.1: “Interface Boundary Conditions” shows the required displacement and velocity specifications for slip
and stick boundary conditions.

Section 7.2: Boundary Conditions

7–3

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Table 7.1 Interface Boundary Conditions

Stick[1]

Slip[1]

Boundary Condi-
tion

Specify all displacement components for fluid nodes.

That is, specify the following:

Specify normal compon-
ent of displacement for
fluid nodes.

That is, specify the follow-
ing:

D = d n

⋅

Displacement

3-D

2-D

D = d n

⋅

= d

⋅

= d

⋅

or D

; D

D = d n

⋅

D = d

⋅

or D

; D

Viscous Flow

Specify all velocity components for fluid nodes.

That is, specify the following:

Inviscid Flow

Specify normal compon-
ent of velocity for fluid
nodes.

That is, specify the follow-
ing:

V =

⋅

Velocity

3-D

2-D

V =

⋅

υ τ

⋅

υ τ

⋅

or V

; V

V =

⋅

V =

υ τ

⋅

or V

; V

The time derivative of the normal displacement must be equal to the normal velocity, dD

/dt = V

Slip or stick boundary conditions can apply for displacement. For velocity, slip boundary conditions apply for
inviscid flow and stick boundary conditions apply for viscous flow. In all cases, the time derivative of the normal
displacement must be equal to the normal velocity. In FLOTRAN, only stick boundary conditions are currently
valid.

To set displacement or velocity boundary conditions at nodes, you can use either of the following:

Command(s): D
GUI: Main Menu> Preprocessor> Loads> Define Loads> Apply> Fluid/CFD> Displacement

(or

Velocity)

> On Nodes

Main Menu> Solution> Define Loads> Apply> Fluid/CFD> Displacement

(or Velocity)

> On

Nodes

To set boundary conditions on the solid model, you can use any of the following:

Command(s): DL and DA
GUI: Main Menu> Preprocessor> Loads> Define Loads> Apply> Fluid/CFD> Displacement

(or

Velocity)

> On Lines

Main Menu> Solution> Define Loads> Apply> Fluid/CFD> Displacement

(or Velocity)

> On Lines

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

7–4

Chapter 7: Arbitrary Lagrangian-Eulerian (ALE) Formulation for Moving Domains

Main Menu> Preprocessor> Loads> Define Loads> Apply> Fluid/CFD> Displacement

(or Velo-

city)

> On Areas

Main Menu> Solution> Define Loads> Apply> Fluid/CFD> Displacement

(or Velocity)

> On Areas

If a node is part of a distributed resistance or a fan model or part of a solid region composed of FLUID141 or
FLUID142 elements, homogenous displacement boundary conditions are automatically applied (that is,
D,ALL,UX,0.0 and D,ALL,UY,0.0 for 2-D and D,ALL,UX,0.0, D,ALL,UY,0.0, and D,ALL,UZ,0.0 for 3-D).

You can specify partial displacement boundary conditions to make external nodes move along a global axis. For
example, D,ALL,UX,0.0 will make a set of nodes slide along the y-axis in a 2-D model. Currently, normal and tan-
gential components of displacement can not be specified for an external boundary.

You can also specify generalized symmetry boundary conditions. If the ALE formulation is activated, velocity
components are then set equal to the mesh velocity. To do so, use one of the following commands or the GUI
equivalent:

NODE

,ENDS,-1

DL,

LINE

AREA

,ENDS,-1,

Value2

DA,

AREA

,ENDS,-1,

Value2

7.3. Mesh Updating

The ALE formulation uses the displacement boundary conditions applied by the D, DL, and DA commands to
update the finite element mesh. It determines the displacement at the beginning of each time step relative to
the previous time step. For each time step, an elasticity based morphing algorithm updates the mesh. The al-
gorithm ensures that boundary layers are retained (that is, nodes in a fine mesh area move less than nodes in a
coarse mesh area).

A transient analysis cannot proceed if morphing fails. If morphing is independent of the fluid flow solution, you
can step through the morphing algorithm before doing a fluid flow analysis to determine whether morphing
will fail. To do so, issue the following command sequence:

/solu

fldata,solu,turb,f

fldata,solu,temp,f

fldata,solu,spec,f

fldata,solu,ale,t

fldata,solu,flow,f

solve

You can not check for morphing failure in advance if the time step size depends on the fluid flow variables or
the problem involves a free surface.

Mesh morphing is currently available for the following element shapes:

•

Pure quadrilaterals, pure triangles, or a combination for FLUID141

•

Pure hexahedrals, pure tetrahedrals, pure pyramids, pure wedges, or any combination for FLUID142

Sometimes mesh morphing produces poor quality elements (for example, when a fluid domain is extremely
squeezed by a moving wall). The birth and death feature can then be useful. To implement this feature, you assign
a birth/death tolerance to the candidate elements using the real constant BDTOL. A node is automatically deac-
tivated if the distance from it to the center of any element face on the wall becomes less than the assigned
BDTOL. A element is deactivated if all of its nodes are deactivated. Conversely, a node is reactivated if the distance

Section 7.3: Mesh Updating

7–5

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

from it to the center of the closest element face on the wall becomes greater than or equal to the assigned
BDTOL. A element is reactivated if all of its nodes are reactivated.

7.4. Remeshing

Large fluid domain changes can produce poor quality elements and mesh morphing failure. To avoid element
failure, you must remesh.

To accomplish remeshing, issue one of the following:

Command(s): FLDATA39,REMESH
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Remesh Ctrl

FLDATA39,REMESH will automatically remesh the fluid elements and linearly interpolate the nodal solution
from the old mesh to the new mesh. Use it to specify one of the following three ways of remeshing:

•

Remesh all defined fluid elements if the quality of the worst defined element falls below any specified
quality requirement listed in Table 7.2: “Element Qualities”.

Whole domain remeshing is suitable when the moving boundary affects all of the fluid elements (all the
fluid elements may become distorted during solution).

•

Remesh defined fluid elements that have a quality below any specified quality requirement.

Partial domain remeshing is suitable when the distorted elements are locally distributed and the location
of the distorted elements is not known before solution or it changes during solution.

•

Remesh all grouped fluid elements with a specified component name if the quality of the worst selected
element falls below any specified quality requirement.

Selected component remeshing is suitable when the distorted elements are locally distributed, but the
location of the distorted elements is known before solution and it does not change during solution.

There are three maximum allowable element qualities that you need to specify for remeshing: aspect ratio,
change of element size, and change of element aspect ratio.

Table 7.2 Element Qualities

Tetrahedrons

Triangles

Element Quality

AR = ((l

avg

)

/ V) / 8.48

AR = ((l

avg

)

/ A) / 2.3

Generalized Aspect Ratio (AR)

VOCH = exp | log (V(t) / V(0)) |

VOCH = exp | log (A(t) / A(0)) |

Change of Element Size (VOCH)

ARCH = exp | log (AR(t) / AR(0)) |

Change of Aspect Ratio (ARCH)

where:

avg

= average length of the element edges

A = element area
V = element volume
A(t) and V(t) = element area and volume at time t
A(0) and V(0) = element area and volume at time 0

You may also specify the following remeshing inputs:

•

Elements Excluded

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

7–6

Chapter 7: Arbitrary Lagrangian-Eulerian (ALE) Formulation for Moving Domains

You can exclude all elements connected to boundary nodes from remeshing. For a fluid-structure interaction
analysis, you can exclude the elements connected to fluid-solid interfaces.

•

Element Size

The element remeshing size defaults to 0. The element size at the nearest boundary is then used for
remeshing.

•

Area Expansion or Contraction

You can size internal elements so that they are approximately the size of the boundary elements times
an expansion or contraction factor.

•

Checkpoints

You can specify element quality checkpoints in three ways: every time step, every Nth time step, or at a
single time point. The fluid elements will automatically remesh if any quality requirement is not met at a
checkpoint.

After each remesh, new databases and results files are written with the extensions .rfl0

and .db

, where

the remesh file number (Jobname.rfl01, Jobname.rfl02, ... and Jobname.db01, Jobname.db02,...). Use the
ANMRES command to create an animation across the results files.

Note — The original database file is Jobname.db0. The Jobname.db01, Jobname.db02, ... files have
elements that are detached from the solid model.

You can use the FLOTRAN remeshing capability in a pure fluid flow analysis or a fluid-solid interaction analysis.
For information on fluid-solid interaction analyses, see Chapter 3, “Fluid-Solid Interaction Solver” and Chapter 4,
“ANSYS Multi-field (TM) Solver” in the ANSYS Coupled-Field Analysis Guide.

Some important remeshing limitations are listed in the following table.

Table 7.3 Remeshing Limitations

Description

Limitation

Remeshing supports models meshed with triangular or tetrahedral elements. It only works
for element groups with one element type and one real constant.

Elements

Remeshing will not work for extreme area or volume changes.

Area/Volume Changes

2-D problems can have multiple domains; 3-D problems require a single domain. Do not allow
two separate domains without distance (e.g., when solving a FSI problem with a beam or shell
element, at least one side elements connected to the beam or shell elements must be excluded
from remeshing).

Domains

Remeshing can treat nodal loads on the boundary, but it cannot treat body loads applied to
interior nodes. Fluid-solid interaction is the only valid element based load.

Loads

Nodes on the boundary cannot be remeshed. Therefore, remeshing will not work if morphing
failed on surface nodes.

Boundary Nodes

See ALE Analysis of a Moving Cylinder for a problem using remeshing.

7.5. Postprocessing

For postprocessing, you can use the following contour and vector command sequence for the reference domain
or the current deformed domain:

Section 7.5: Postprocessing

7–7

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

set,load step,substep ! sets the set number for processing

/dscal,,1.0 ! sets the scaling for display

plns,pres,,0 ! display pressure contours on deformed domain

plve,v,,,,,,,1 ! display velocity vectors on the deformed domain

To view the deformed mesh , issue the following command sequence:

set,load step,substep ! sets the set number for processing

/dscal,,1.0 ! sets the scaling for display

pldi,2 ! display the deformed mesh overlayed with undeformed

! edges

To produce an animated sequence of the results, issue the ANTIME macro with the above commands.

Note — The displacements of non-structural elements are mesh (or grid) displacements to avoid mesh
distortion but have no physical meaning except at the interface between the fluid and the structure.

7.6. ALE Analysis of a Simplified Torsional Mirror

7.6.1. The Problem Described

This is an Arbitrary Lagrangian-Eulerian (ALE) analysis of a micro-electromechanical system (MEMS) device. The
device consists of a viscous fluid between two rigid plates. Initially, the plates are parallel and the fluid is at rest.
The top plate begins to oscillate about its centerline setting the fluid in motion. The top plate oscillates with a
very small angular amplitude.

You must determine the torque on the moving plate in order to develop a reduced order model for this device.

Figure 7.5 Torsional Mirror Problem Description

! "

$!%'&

(

-./

(

/-)"/0

%'&

(

132

7.6.2. Boundary Conditions

This section derives formulas for the displacement and velocity boundary conditions.

The angle of rotation is:

θ = θ

sin

ωt

Differentiating, the angular velocity is: &

ωθ

cos

ωt

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

7–8

Chapter 7: Arbitrary Lagrangian-Eulerian (ALE) Formulation for Moving Domains

The position of any point on the plate is given by:

x(t) = x

+ Rcos

y(t) = y

+ Rsin

where:

R = x

and x

is the x coordinate on the plate at time equals zero.

Therefore, the displacements of the plate are given by:

UX(t) = x(t) x(o) = x x

UY(t) = y(t) y(o) = y y

Substituting the expressions for x and y gives:

UX = R(cos

θ 1)

UY = Rsin

Note — As

θ approaches 0, UX approaches 0 and UY approaches Rθ.

Differentiating displacements gives the following velocity equations:

UX UX

VY UY R

= −

sin

cos

θθ

Note — As

θ approaches 0, VX approaches R θ &

∝

and VY approaches R &

∝

. Therefore, VX ap-

proaches 0 faster than VY.

The command listing in Section 7.6.4: Building and Solving the Model (Command Method) uses the above ex-
pressions for UX, UY, VX, and VY in the boundary condition tables.

7.6.3. Forces and Moments

This section derives formulas for the forces and moments acting on the torsional mirror.

Section 7.6: ALE Analysis of a Simplified Torsional Mirror

7–9

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Figure 7.6 Torsional Mirror Problem - Boundary Conditions

! "

#$%

'(*)

#$+

,-! "

#$%

!./!

12314

12312.7

Assuming the flow is 2-D and neglecting inertia terms, the Navier-Stokes equation reduces to the Reynolds
equation for incompressible flow:

∂

∂
∂







∂

= 6

hU + 12 V

(

)

where: h = h (x,t) is the gap height and U and V are the velocity components of the moving plate.

Assuming that the angular displacement of the mirror is small gives:

≈

R &

≈

Substituting these values in the Reynolds equation and assuming that U variations with x are small gives:

∂

∂
∂







= 12 V = 12 x

µ θ

Integrating gives:

∫

dx + C

µθ

where C

and C

are constants to be determined.

Substituting h

for h for small angular displacements and completing the integration gives:













C x

+ C

µθ

Substituting p = p

at x = ± L/2 gives:

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

7–10

Chapter 7: Arbitrary Lagrangian-Eulerian (ALE) Formulation for Moving Domains













+ C

µθ













+ C

µθ

Solving these two equations for C

and C

gives:

= p

= 2 µ &

(L/2)

Substituting the C

and C

values into the pressure equation gives:







µθ

(

)

p - p





















µθ

Thus, the force and moment on the torsional mirror are given by:

(p - p ) dx = 0

- L/2

L/2

∫

M =

p - p

xdx = -

- L/2

L/2

(

)

∫

µθ

The flow field at any x coordinate is given by:

U x,y,t =

y y -

(

)

(

)

∂
∂

Accordingly, the shear stress on the torsional mirror is:

µθ

∂

∂
∂



















3x -

y = h

Thus, the force and moment due to shearing stresses are:

F =

dx = 0

- L/2

L/2

y = h

∂

∫

Section 7.6: ALE Analysis of a Simplified Torsional Mirror

7–11

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

xdx = 0

- L/2

L/2

y = h

∂

∫

7.6.4. Building and Solving the Model (Command Method)

The following command stream shows all the relevant parameters and solution strategy. All text prefaced with
an exclamation point (!) is a comment. Please refer to Figure 7.5: “Torsional Mirror Problem Description”.

/BATCH,LIST

/tit,Torque Mirror Problem

/nopr

LX = 1.0 ! Plate Length in X direction

NDX = 40 ! Number of X divisions

H = 0.01 ! Gap in Y-direction

NDY = 10 ! Number of Y divisions

POUT = 0.0 ! Outlet relative pressure

RHO = 1.0000 ! Fluid density

MU = 1.00 ! Fluid viscosity

nts = 40 ! number of time steps

time = 10. ! total simulation time

delta = time/nts ! time step size

appf = delta ! append results every time step

*AFUN,RAD ! angles are in radians

AMAX = (2*H/LX)/8 ! adjust angular amplitude << 1

OMEGA = 2*3.14159/time ! complete 1 cycle in given time

X0 = LX/2 ! pivot point x-coord

Y0 = H ! pivot point y-coord

H0 = H

! use function builder/tables (refer to Section 2.6.15: Applying Loads Using Function Boundary
Conditions in the ANSYS Basic Analysis Guide)

! for displacements/velocities of oscillating plate

*DIM,UXTAB,TABLE,6,4,1

UXTAB(0,0,1) = 0.0,-999, 1, X0 ,AMAX, 0.0, 0.0

UXTAB(0,1,1) = 1.0,-1 , 0, 1.0 , 27 , 2 , 17 ! Radius = XR - X0

UXTAB(0,2,1) = 0.0,-2 , 9,OMEGA, 1 , 3 , 18 ! Angle=amax*sin(omega*t)

UXTAB(0,3,1) = 0.0,-3 , 10, 1.0 ,-2 , 3 ,-1 ! Radius*cos(Angle)

UXTAB(0,4,1) = 0.0,99 , 0, 1.0 ,-3 , 2 ,-1 ! Radius*cos(Angle)-Radius

*DIM,UYTAB,TABLE,6,3,1

UYTAB(0,0,1) = 0.0,-999, 1, X0 ,AMAX, 0.0, 0.0

UYTAB(0,1,1) = 1.0,-1 , 0, 1.0 , 27 , 2 , 17 ! Radius = XR - X0

UYTAB(0,2,1) = 0.0,-2 , 9,OMEGA, 1 , 3 , 18 ! Angle=amax*sin(omega*t)

UYTAB(0,3,1) = 0.0,99 , 9, 1.0 ,-2 , 3 ,-1 ! Radius*sin(Angle)

*DIM,VXTAB,TABLE,6,5,1

VXTAB(0,0,1) = 0.0,-999, 1, X0 ,AMAX,OMEGA*AMAX, 0.0

VXTAB(0,1,1) = 1.0,-1 , 0,-1.0 , 27 , 1 , 17 ! -Radius = -(XR-X0)

VXTAB(0,2,1) = 0.0,-2 , 9,OMEGA, 1 , 3 , 18 ! Angle=amax*sin(omega*t)

VXTAB(0,3,1) = 0.0,-3 , 10,OMEGA, 1, 3 , 19 ! Angle speed=

! amax*omega*cos(omega*t)

VXTAB(0,4,1) = 0.0,-4 , 9, 1.0 ,-2 , 3 , -1 ! -Radius*sin(angle)

VXTAB(0,5,1) = 0.0,99 , 0, 1.0 ,-4 , 3 , -3 !-Radius*sin(angle)*angle speed

*DIM,VYTAB,TABLE,6,5,1

VYTAB(0,0,1) = 0.0,-999, 1, X0 ,AMAX,OMEGA*AMAX, 0.0

VYTAB(0,1,1) = 1.0,-1 , 0, 1.0 , 27 , 2 , 17 !Radius = XR - X0

VYTAB(0,2,1) = 0.0,-2 , 9,OMEGA, 1 , 3 , 18 !Angle=amax*sin(omega*t)

VYTAB(0,3,1) = 0.0,-3 , 10,OMEGA, 1, 3 , 19 !Angle speed=

!amax*omega*cos(omega*t)

VYTAB(0,4,1) = 0.0,-4 , 10, 1.0 ,-2 , 3 , -1 !Radius*cos(angle)

VYTAB(0,5,1) = 0.0,99 , 0, 1.0 ,-4 , 3 , -3 !Radius*cos(angle)*angle speed

/PREP7 $smrt,off

et,1,141 ! 2-D XY system

keyopt,1,4,1 ! allow disp. DOFs

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

7–12

Chapter 7: Arbitrary Lagrangian-Eulerian (ALE) Formulation for Moving Domains

esha,2 ! Quad elements

rect,,LX,,H

lesize,1,,,NDX,

lesize,3,,,NDX,

lesize,2,,,NDY,-10

lesize,4,,,NDY,-10

alls

amesh,all

lsel,s,,,3 ! Moving top plate

nsll,s,1

d,all,VX,%VXTAB%

d,all,VY,%VYTAB%

d,all,enke,-1

d,all,ux,%UXTAB%

d,all,uy,%UYTAB%

lsel,s,,,2 ! Left & Right Outlets

lsel,a,,,4

nsll,s,1

d,all,pres,POUT

lsel,s,,,1 ! Stationary bottom plate

nsll,s,1

d,all,vx,

d,all,vy,

d,all,ux,0.0

d,all,uy,0.0

alls

fini

/SOLU

FLDA,NOMI,DENS,RHO ! Nominal density

FLDA,NOMI,VISC,MU ! Nominal viscosity

FLDA,OUTP,TAUW,T ! Output wall shear stress

flda,quad,momd,2 ! increased quadrature for deformed

flda,quad,moma,2 ! elements

flda,quad,moms,2

flda,quad,prsd,2

flda,quad,prss,2

flda,solu,tran,t

flda,time,step,delta

flda,time,numb,nts

flda,time,tend,time

flda,time,glob,25

flda,time,appe,appf

flda,solu,ale,t ! Turn ALE on

save

SOLVE

fini

!do the comparison with analytical solution here

/post1

!moving wall

*dim,RES1,,NDX+1,15

*do,j,1,nts,1 ! loop over the time steps

rsys,0

csys,0

set,1,j ! get the results of step j

*get,curtime,active,0,set,time ! get the time of this substep

theta = amax*sin(omega*curtime) ! get the plate angle

thetad = amax*omega*cos(omega*curtime) ! get plate angular speed

nsel,s,loc,y,H ! select moving wall nodes

*do,i,1,NDX+1 ! loop over these nodes

*get,XMAX,node,,mxloc,x

n = node(XMAX,H,0)

RES1(i,1) = n ! Node number

RES1(i,2) = NX(n) ! X-coordinate

RES1(i,3) = NY(n) ! Y-coordinate

RES1(i,4) = UX(n) ! UX

Rn = NX(n)-X0

Section 7.6: ALE Analysis of a Simplified Torsional Mirror

7–13

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

RES1(i,10) = Rn*(cos(theta)-1.0) ! UX exact

RES1(i,5) = UY(n) ! UY

RES1(i,11) = Rn*sin(theta) ! UY exact

RES1(i,6) = VX(n) ! VX

RES1(i,12) = -Rn*sin(theta)*thetad ! VX exact

RES1(i,7) = VY(n) ! VY

RES1(i,13) = Rn*cos(theta)*thetad ! VY exact

RES1(i,8) = PRES(n) ! Pressure

c1 = 2.0*MU*thetad/H0**3

c2 = NX(n) - X0

RES1(i,14) = c1*(c2**3 - c2*(LX/2)**2) ! Exact Pressure

*get,RES1(i,9),node,n,TAUW ! Shear stress

c0 = NX(n) - X0

c1 = H0 + theta*c0

c2 = 3*c0**2 - (LX/2)**2

RES1(i,15) = ABS(c1*mu*thetad*c2/H0**3) ! Exact shear stress

nsel,u,,,n

*enddo

/com Compare disps/velocities/pressures/shears on moving wall(X,H,0)

/com

*status,curtime

*status,theta

*vwrite

(4x,'NODE',7x,'X COOR',12x,'Y COOR',9x,'UX (FLOTRAN)',5x,'UX (Exact)')

*vwrite,RES1(1,1),RES1(1,2),RES1(1,3),RES1(1,4),RES1(1,10)

(3x,f5.0,4(1pe17.5))

/com

*vwrite

(4x,'NODE',7x,'X COOR',12x,'Y COOR',9x,'UY (FLOTRAN)',5x,'UY (Exact)')

*vwrite,RES1(1,1),RES1(1,2),RES1(1,3),RES1(1,5),RES1(1,11)

(3x,f5.0,4(1pe17.5))

/com

*vwrite

(4x,'NODE',7x,'X COOR',12x,'Y COOR',9x,'VX (FLOTRAN)',5x,'VX (Exact)')

*vwrite,RES1(1,1),RES1(1,2),RES1(1,3),RES1(1,6),RES1(1,12)

(3x,f5.0,4(1pe17.5))

/com

*vwrite

(4x,'NODE',7x,'X COOR',12x,'Y COOR',9x,'VY (FLOTRAN)',5x,'VY (Exact)')

*vwrite,RES1(1,1),RES1(1,2),RES1(1,3),RES1(1,7),RES1(1,13)

(3x,f5.0,4(1pe17.5))

/com

*vwrite

(4x,'NODE',7x,'X COOR',12x,'Y COOR',9x,'PRE (FLOTRAN)',5x,'PRE (Exact)')

*vwrite,RES1(1,1),RES1(1,2),RES1(1,3),RES1(1,8),RES1(1,14)

(3x,f5.0,4(1pe17.5))

/com

*vwrite

(4x,'NODE',7x,'X COOR',12x,'Y COOR',9x,'TAU (FLOTRAN)',5x,'TAU (Exact)')

*vwrite,RES1(1,1),RES1(1,2),RES1(1,3),RES1(1,9),RES1(1,15)

(3x,f5.0,4(1pe17.5))

/com

nsel,s,loc,y,H ! select nodes on moving plate

local,11,0,X0,Y0,0 ! setup local coord system for moment calcs

rsys,11

/com compute pressure force/moments on the wall

intsrf,pres

*get,forcex,intsrf,0,item,fx

*get,forcey,intsrf,0,item,fy

*get,forcez,intsrf,0,item,fz

*get,momx,intsrf,0,item,mx

*get,momy,intsrf,0,item,my

*get,momz,intsrf,0,item,mz

*status,forcex

*status,forcey ! should be zero

*status,forcez

*status,momx

*status,momy

*status,momz ! Flotran

Moment = -0.0166*mu*thetad*LX**5/H0**3 ! Exact

*status,moment

/com compute shear force/moments on the wall should be zero

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

7–14

Chapter 7: Arbitrary Lagrangian-Eulerian (ALE) Formulation for Moving Domains

intsrf,tauw

*get,forcex,intsrf,0,item,fx

*get,forcey,intsrf,0,item,fy

*get,forcez,intsrf,0,item,fz

*get,momx,intsrf,0,item,mx

*get,momy,intsrf,0,item,my

*get,momz,intsrf,0,item,mz

*status,forcex ! should be zero

*status,forcey

*status,forcez

*status,momx

*status,momy

*status,momz ! should be zero

*enddo

fini

/exit,nosa

7.7. ALE/VOF Analysis of a Vessel with a Moving Wall

7.7.1. The Problem Described

This problem involves a moving wall and a free surface. A square vessel is half filled with liquid and at t = 0 the
left wall begins to move to the right. The wall stops moving after a short time and the fluid comes to rest
gradually. The total analysis time is 2 seconds. The left wall comes to rest at 0.125 * (time) = 0.125*(2 seconds) =
0.25 seconds. The left wall displacement and velocity are input as tabular boundary conditions (see Figure 7.8: “Left
Wall Displacement and Velocity”). The simulation uses the Volume of Fluid (VOF) method in conjunction with
the ALE formulation.

Figure 7.7 Square Vessel with a Moving Wall

!#"

$&%

'()

$.-/

!#"0

$&%/

-1243657

!#"

;

$95

Section 7.7: ALE/VOF Analysis of a Vessel with a Moving Wall

7–15

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Figure 7.8 Left Wall Displacement and Velocity

"!$#

')(

7.7.2. Results

The initial fluid volume is 1/2 H times LX. Since H and LX are both equal to 1, the initial fluid volume is 0.500000000.
The calculated final fluid volume is 0.499999673.

7.7.3. Building and Solving the Model (Command Method)

The following command stream shows all the relevant parameters and solution strategy. All text prefaced with
an exclamation point (!) is a comment.

/BATCH,LIST

/title,ALE-VOF combination - container with moving wall & free surface

/nopr

LX = 1.0 ! Initial width in X direction

NDX = 10 ! Number of X divisions

H = 1.0 ! Height of container

NDY = 10 ! Number of Y divisions

RHO = 1.0000 ! Fluid density

MU = 1.00 ! Fluid viscosity

LXF = 0.750 ! Final X-Length

time = 2. ! Total simulation time

nts = 200 ! Total number of time steps

delta = time/nts ! Time step size

appf = delta ! Results append frequency

VEL = (LX-LXF)/(0.125*time) ! left wall moves for 12.5% of

! simulation time with velocity VEL

*dim,timutab,table,3,,,time ! left wall displacement history

timutab(1,0)=0,0.125*time,time

timutab(1,1)=0,(LX-LXF),(LX-LXF)

*dim,timvtab,table,4,,,time ! left wall fluid velocity history

timvtab(1,0)=0,0.125*time,0.125*time+0.000001,time

timvtab(1,1)=VEL,VEL,1.e-12,1.e-12

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

7–16

Chapter 7: Arbitrary Lagrangian-Eulerian (ALE) Formulation for Moving Domains

/PREP7 $smrt,off

et,1,141 ! 2-D XY system

keyopt,1,4,1 ! enable disp DOFs

esha,2 ! Quad elements

rect,,LX,,H

lesize,1,,,NDX,-10

lesize,3,,,NDX,-10

lesize,2,,,NDY,

lesize,4,,,NDY,

alls

amesh,all

lsel,s,,,4 ! Moving left wall

nsll,s,1

d,all,VX,%timvtab%

d,all,VY,

d,all,enke,-1

d,all,ux,%timutab%

d,all,uy,0.0

lsel,s,,,1 ! bottom wall

nsll,s,1

d,all,vx

d,all,vy

lsel,s,,,3 ! top wall

nsll,s,1

d,all,vx

d,all,vy

lsel,s,,,2 ! Stationary right wall

nsll,s,1

d,all,vx,

d,all,vy,

d,all,ux,0.0

d,all,uy,0.0

alls

nsel,s,loc,y,0,0.5*H ! select lower half elements

esln,s,1

ice,all,vfrc,1.0 ! apply vof initial conditions

allsel

fini

/SOLU

FLDA,NOMI,DENS,RHO ! Nominal density

FLDA,NOMI,VISC,MU ! Nominal viscosity

acel,,9.8 ! Apply gravity loading

flda,step,sumf,1

flda,solu,tran,t

flda,time,step,delta

flda,time,numb,nts

flda,time,tend,time

flda,time,glob,25

flda,time,appe,appf

flda,solu,ale,t ! Ale on

flda,solu,vof,t ! Vof on

save

SOLVE

fini

!do the comparison here for final fluid volume

/post1

set,last

fvol = 0. ! initialize volume to zero

*do,i,1,NDX*NDY ! loop over elements

n1 = nelem(i,1) ! 4 nodes of this element

n2 = nelem(i,2)

n3 = nelem(i,3)

n4 = nelem(i,4)

Section 7.7: ALE/VOF Analysis of a Vessel with a Moving Wall

7–17

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

x1 = nx(n1)+ux(n1) ! current coords of the 4 nodes

y1 = ny(n1)+uy(n1)

x2 = nx(n2)+ux(n2)

y2 = ny(n2)+uy(n2)

x3 = nx(n3)+ux(n3)

y3 = ny(n3)+uy(n3)

x4 = nx(n4)+ux(n4)

y4 = ny(n4)+uy(n4)

evol1 = x1*y2+y1*x3+y3*x2 ! compute volume of triangle 123

evol1 = evol1-y2*x3-y1*x2-x1*y3

evol1 = abs(0.5*evol1) ! first triangle volume

evol2 = x1*y4+y1*x3+y3*x4 ! compute volume of triangle 143

evol2 = evol2-y4*x3-y1*x4-x1*y3

evol2 = abs(0.5*evol2) ! second triangle volume

*get,frac,elem,i,nmisc,1 ! get VOF of this quad

fvol = fvol + (evol1+evol2)*frac!increment the total fluid volume

*enddo

*status,fvol ! print the final fluid volume

target = 0.5*H*LX

*status,target ! print the expected fluid volume

/com

fini

/exit,nosa

7.8. ALE Analysis of a Moving Cylinder

7.8.1. The Problem Described

This problem involves a cylinder passing through a channel with a constant velocity VX = 1.0. FLUID141 triangle
elements model the fluid. The simulation uses the ALE formulation and remeshing. FLDATA39,REMESH,Label,Value
specifies the quality requirements shown in the following table.

Table 7.4 Quality Requirements

FLDATA39,REMESH,Label,Value Command

Element Quality

FLDATA39,REMESH,ARMA,5.0

Aspect Ratio (AR)

FLDATA39,REMESH,VOCH,3.0

Change of Element Size (VOCH)

FLDATA39,REMESH,ARCH,3.0

Change of Aspect Ratio (ARCH)

FLDATA39,REMESH,ELEM,ALL sets the remeshing to all defined fluid elements if the quality of the worst defined
element falls below any quality requirement. The total analysis time is 44 seconds.

Figure 7.9 Moving Cylinder

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

7–18

Chapter 7: Arbitrary Lagrangian-Eulerian (ALE) Formulation for Moving Domains

7.8.2. Results

The ten results files are file.rfl01 through file.rfl10. They were created when one of the remeshing criteria were
met. The following figures display the remeshed elements at 0, 22, and 44 seconds.

Figure 7.10 Elements at 0 Seconds

Figure 7.11 Elements at 22 Seconds

Figure 7.12 Elements at 44 Seconds

7.8.3. Building and Solving the Model (Command Method)

The following command stream shows all the relevant parameters and solution strategy. All text prefaced with
an exclamation point (!) is a comment.

/batch,list

/verify,dv-1101c

/title, dv-1101c, Flotran Remeshing: Cylinder pass through a channel

/COM,****************************************************

/COM,* Cylinder pass through a channel (pure fluid flow)

/COM,* Verify partial domain re-meshing

/COM,****************************************************

r1 = 2.5

l1 = 5.0

l2= 20.0

l3=60.0

h = 10.0

rx0= l1+(l2-l1)/2.0

Section 7.8: ALE Analysis of a Moving Cylinder

7–19

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

ry0 = h/2.0

nl1 = 5

nl3 = 10

nr=8

nc=8

/PREP7

*DEL,_FNCNAME

*DEL,_FNCMTID

*DEL,_FNC_C1

*SET,_FNCNAME,'DIS'

*DIM,_FNC_C1,,1

*SET,_FNC_C1(1),1.0

! /INPUT,force.func

*DIM,%_FNCNAME%,TABLE,6,3,1

! Begin of equation: a*{TIME}

*SET,%_FNCNAME%(0,0,1), 0.0, -999

*SET,%_FNCNAME%(2,0,1), 0.0

*SET,%_FNCNAME%(3,0,1), %_FNC_C1(1)%

*SET,%_FNCNAME%(4,0,1), 0.0

*SET,%_FNCNAME%(5,0,1), 0.0

*SET,%_FNCNAME%(6,0,1), 0.0

*SET,%_FNCNAME%(0,1,1), 1.0, -1, 0, 1, 17, 3, 1

*SET,%_FNCNAME%(0,2,1), 0.0, 99, 0, 1, -1, 0, 0

*SET,%_FNCNAME%(0,3,1), 0

! End of equation: a*{TIME}

!-->

RECTNG,0,l1,0,h,

RECTNG,l1,l2,0,h,

RECTNG,l2,l3,0,h,

aglue,all

CYl4,rx0,ry0,0,45,r1,135

CYl4,rx0,ry0,0,135,r1,225

CYl4,rx0,ry0,0,225,r1,315

CYl4,rx0,ry0,0,315,r1,405

asel,s,,,2

asel,a,,,3

asel,a,,,6

asel,a,,,7

allsel,below,area

aglue,all

allsel

FLST,3,4,5,ORDE,3

FITEM,3,2

FITEM,3,8

FITEM,3,-10

ASBA, 4,P51X

aplot

et,1,141

KEYOPT,1,4,1

type,1

mat,1

asel,s,,,1

esize,.5

mshape,1,2d

mshkey,0

amesh,all

et,2,141

KEYOPT,2,4,1

type,2

mat,1

asel,s,,,3

esize,.5

mshape,1,2d

mshkey,0

amesh,all

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

7–20

Chapter 7: Arbitrary Lagrangian-Eulerian (ALE) Formulation for Moving Domains

et,3,141

KEYOPT,3,4,1

type,3

mat,1

asel,s,,,5

esize,2.0

mshape,1,2d

mshkey,0

amesh,all

nsel,s,loc,x,0

D,ALL,VX,0.0,

D,ALL,VY, 0.0

D,ALL,UX,0.0,

D,ALL,UY, 0.0

nsel,s,loc,x,l3

D,ALL,pres,0.0

D,ALL,UX,0.0,

D,ALL,UY, 0.0

nsel,s,loc,y,0

D,ALL,vy,0.0

D,ALL,UX,0.0,

D,ALL,UY, 0.0

nsel,s,loc,y,h

D,ALL,vy,0.0

D,ALL,UX,0.0,

D,ALL,UY,0.0,

lsel,s,,,5

lsel,a,,,23

lsel,a,,,25

lsel,a,,,27

nsll,s,1

d,all,UX,%DIS%

d,all,UY,0.0

d,all,VX,1.0

d,all,VY,0.0

allsel

cdwrite,db,fluid,cdb,

fini

! Flotran Setup

/solu

FLDATA30,QUAD,MOMD,2,

FLDATA30,QUAD,MOMS,2,

FLDATA30,QUAD,PRSD,2,

FLDATA30,QUAD,PRSS,2,

FLDATA30,QUAD,THRD,0,

FLDATA30,QUAD,THRS,0,

FLDATA30,QUAD,TRBD,0,

FLDATA30,QUAD,TRBS,2,

/solu

FLDATA4,TIME,NUMB,100000,

FLDATA4,TIME,TEND,44.0,

FLDA,SOLU,ALE,T ! ALE solution

FLDATA1,SOLU,FLOW,1

FLDATA1,SOLU,TRAN,1

!FLDATA1,SOLU,TURB,1

FLDATA2,TIME,GLOB,5

FLDATA7,PROT,DENS,CONSTANT

FLDATA8,NOMI,DENS,1.0

FLDATA7,PROT,VISC,CONSTANT

FLDATA8,NOMI,VISC,1.0

!FLDA,BULK,BETA,1.0e5

FLDA,TIME,STEP, 2.0

!!! Newmark method

FLDATA,OUTP,TAUW,T

FLDATA,TIME,METH,NEWM

FLDATA,TIME,DELT,0.5

Section 7.8: ALE Analysis of a Moving Cylinder

7–21

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

!! Set ANSYS-STRUCTURE commands

SAVE

/COM

/COM Re-meshing Commands

/COM

FLDATA,REMESH,ELEM,ALL ! all defined element re-meshing

FLDATA,REMESH,ARMA,10.0 ! maximum aspect ratio

FLDATA,REMESH,VOCH,5.0 ! maximum volume change

FLDATA,REMESH,ARCH,5.0 ! maximum aspect ratio change

SOLVE

SAVE

finish

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

7–22

Chapter 7: Arbitrary Lagrangian-Eulerian (ALE) Formulation for Moving Domains

Chapter 8: FLOTRAN Compressible Analyses

8.1. Requirements for Compressible Analysis

As is true with turbulence, activating the compressible algorithm is at your discretion. You should activate turbu-
lence for virtually all compressible analyses, (although in principle the Reynolds number can be in the laminar
range for high Mach numbers). Differences in results (pressure, density, velocity distributions) between the in-
compressible and compressible algorithms can exist at Mach numbers as low as 0.3, and are quite pronounced
when the Mach number is as high as 0.7.

The speed of sound is a function of the equation of state of the fluid and its absolute temperature. For a constant
density fluid, the speed of sound is infinite. For an ideal gas, regardless of whether the incompressible or com-
pressible solution algorithm is used, the relationship is:

= γ

In the preceding equation:

•

R is the Universal Gas Constant

•

γ is the ratio of specific heats (C

)

•

T is the absolute temperature

For 2-D compressible analyses, meshes using quadrilateral elements are highly recommended. Hexagonal elements
are recommended for 3-D cases. For more information, see Section 8.4: Structured vs. Unstructured Mesh.

8.2. Property Calculations

The compressible algorithm takes into account the kinetic energy changes of the fluid as it accelerates. The for-
mulation is in terms of the total temperature.

In an adiabatic analysis, the total temperature remains constant throughout the problem domain. You specify
the temperature using either of the following methods:

Command(s): FLDATA14,TEMP,TTOT,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Flow Environment> Ref Conditions
Main Menu> Solution> FLOTRAN Set Up> Flow Environment> Ref Conditions

The conservation of energy is then a balance between thermal storage (static temperature) and kinetic energy.

The total (stagnation) temperature is the temperature of the fluid after it has been brought isentropically to a
zero velocity. Typically, you choose the conditions at the inlet. Knowledge of the static temperature and the ve-
locity magnitude |V| at the inlet enables you to calculate the total temperature via the following equation,

static

This relationship is sometimes useful when cast in terms of the Mach number (M):

+ −

(

)

You must specify the specific heat and the ratio of specific heats

γ. (To enter this ratio, use one of the following:)

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Command(s): FLDATA17,GAMM,COMP,
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Flow Environment> Ref Conditions
Main Menu> Solution> FLOTRAN Set Up> Flow Environment> Ref Conditions

The ANSYS program uses the resulting static temperature and the absolute pressure to calculate the density
from the equation of state.

Note — Unlike incompressible analyses, where freezing the density calculation for the early global itera-
tions can be an advantage, compressible analyses automatically involve the variable density option.
Another difference between these types of analysis is that for compressible analyses, initial properties
are calculated from the calculated static temperature, not from the nominal temperature.

8.3. Boundary Conditions

Typically, you will know the Mach number or the velocity or the mass flow along with the static temperature for
the inlet. Knowing the velocity or Mach number enables you, using the above equations, to calculate of the ap-
propriate total temperature. If you know only the mass flow rate, you can approximate the pressure at the inlet
by the reference pressure and use it with the equation of state to approximate the inlet density and thus the
velocity.

For subsonic problems, the boundary condition strategy is similar to that used for incompressible flow problems,
that is, velocity or pressure at the inlet and pressure at the outlet. For supersonic problems, however, the nature
of the equations changes and the effects of downstream boundary conditions cannot propagate upstream. It is
common in such cases to apply both pressure and velocity to upstream locations. Leave the downstream
boundary unspecified.

Free stream conditions are often applied as far field boundary conditions for external flow problems. Often
specification of pressure at these boundaries helps. However, as the solution develops, phenomena such as
shock waves propagate to these boundaries. In this case, you should remove the boundary conditions. Failure
to do so could adversely affect the resultant mass balance. Also, if the boundary is too close to the region of interest
(e.g. the airfoil the flow is moving past), the velocity solution near the boundary will tend to be greater than the
free stream velocity. In such cases, a better choice for the velocity boundary conditions is the symmetry condition
(only specify the velocity normal to the boundary as zero).

If the problem is thermal, ANSYS takes all of the applied boundary conditions to be total temperature, not static
temperature. Conversely, if a problem is adiabatic, thermal boundary conditions are ignored.

If you use a thermal incompressible solution as a starting point for a thermal compressible problem, you must
change the boundary conditions so that they are specified in terms of total temperature.

8.4. Structured vs. Unstructured Mesh

As noted at the beginning of this chapter, for 2-D compressible flow problems, quadrilateral mesh is the best to
use. Consider Figure 8.1: “Three Types of Meshing”:

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

8–2

Chapter 8: FLOTRAN Compressible Analyses

Figure 8.1 Three Types of Meshing

(a) Quadrilateral mesh, (b) Triangular mesh with a random pattern, (c) Triangular mesh with a
symmetrical pattern

In 2-D compressible analyses, mesh (a), the quadrilateral mesh, produces the most accurate results. Mesh (b)
yields 2-D, not 1-D results, and mesh (c) yields 1-D results.

Similarly, in a 3-D compressible analysis, a hexagonal mesh (the equivalent of quadrilateral mesh in 2-D) produces
the best results. A tetrahedral mesh with a random pattern (the 3-D equivalent of mesh (b)) yields only 3-D results,
not 1-D. And a tetrahedral symmetric mesh, the 3-D equivalent of mesh (c), gives you 1-D results.

8.5. Solution Strategies

You must solve compressible analyses as pseudo-transient or transient problems. This is due to the non-elliptic
nature of supersonic problems. The pseudo-transient approach is quite adequate when the time-history of the
developing transient is not of interest. In that approach, you apply inertial relaxation to the pressure equation
(see Section 8.5.1: Inertial Relaxation).

For an ideal gas, the density is always calculated from an equation of state involving the absolute pressure and
the absolute temperature. Because of this, you must prevent negative values of absolute pressure and absolute
static temperature from being encountered during the iterative process, as these would lead to a negative
density. One way to do this is to use a converged incompressible solution as a starting point. Another way is to
use capping to specify a minimum FLOTRAN (relative) pressure. For example, to keep the absolute pressure at
a minimum of 1 psi, you would cap the relative pressure at -13.7 psi for a reference pressure of 14.7 psi. Capping
is not a stability control and by itself it will not control the solution progression. It only helps prevent negative
properties.

Artificial viscosity helps to prevent negative temperatures. You set it at the beginning of the analysis, and must
reduce it slowly for subsequent continuations of the analysis. You will probably encounter divergence if you in-
crease the viscosity between runs. The magnitude of the artificial viscosity required can vary greatly. The smaller
the starting value, the fewer the global iterations required. But if it is not large enough, you may encounter
negative static temperatures. You can use the laminar and effective viscosities to gauge a good starting value.
It is typically a couple orders of magnitude higher than the effective viscosity, which in turn is initialized as a

Section 8.5: Solution Strategies

8–3

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

multiple of the laminar value. Generally, a value 3 or 4 orders of magnitude higher than the laminar viscosity is
a good approximate starting point.

In a compressible problem, the final answer would be a function of the artificial viscosity if it were not removed.
Therefore, after stability has been achieved, gradually remove the artificial viscosity during repeated analysis
continuations.

8.5.1. Inertial Relaxation

Inertial relaxation helps to stabilize a solution by increasing the magnitude of the main diagonal of the matrix
equation along with a corresponding increase in the forcing function. Values used are generally between 1.0 x
10

-3

(less relaxation) and 1.0 x 10

-6

(more relaxation) for pressure. The smaller values provide more diagonal

dominance and thus equation stability. The cost of this is slower convergence since it de-emphasizes the influence
of the cross-coupling terms present in the equations.

Unlike artificial viscosity, the inertial relaxation does not affect the answer if the problem is converged and thus
does not have to be removed. It is best to reduce the magnitude to the range of 1 x 10

-4

later in the analysis. You

can measure the effectiveness of the relaxation by observing the performance of the parameter RTR in the Job-
name.DBG file.

All the techniques discussed so far involve the steady state algorithm. It is common for supersonic problems,
even if they are posed as steady state to be solved with the transient algorithm. An initial velocity field can be
imposed as a first guess. The inertial relaxation acts similarly to the transient algorithm and its use is considered
redundant in transient analyses. Do note that problems involving moving shocks may lead to inaccurate solutions
when using the transient algorithm. With the current set of governing partial differential equations and the dis-
cretization techniques used, the transient algorithm has demonstrated solutions that are qualitatively correct
but may yield quantitatively inaccurate results.

8.6. Example of a Compressible Flow Analysis

8.6.1. The Example Described

This example evaluates compressible flow in a converging-diverging nozzle. The nozzle is axisymmetric with
inlet, throat, and outlet radii of 2.432 cm, 0.5 cm and 0.80 cm, respectively. The nozzle inlet pressure is given as
6.13769e+6 dynes/cm

8.6.1.1. Fluid Properties

The analysis uses density, viscosity, thermal conductivity, and specific heat properties for air in units of cm-g-sec.

8.6.1.2. Approach and Assumptions

The compressible flow analysis is a turbulent analysis that uses the FLUID141 2-D Fluid-Thermal element.

The analysis assumes atmospheric pressure conditions at the outlet. It assumes a stagnation temperature of 550
K.

Inlet and outlet pressure boundary conditions are set to 6.13769e+6 dynes/cm

and 0, respectively. The VY velocity

component is set to 0 along the axis of symmetry and the VX and VY velocity components are set to 0 along the
outer surface.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

8–4

Chapter 8: FLOTRAN Compressible Analyses

The analysis starts with 20 iterations at an artificial viscosity of 10. It then continues for 20 iterations at artificial
viscosity values of 1, .1, .01, .001, .0001, and .00001 to give a total of 140 iterations. The analysis then continues
for another 160 iterations at an artificial viscosity of 0. After 300 iterations of slowly reducing the viscosity to 0,
the analysis continues for 100 iterations with increased momentum and pressure inertial relaxation factors. Finally,
the analysis converges to a final solution with the momentum and pressure inertial relaxation factors increased
to higher values for 400 iterations.

8.7. Doing the Example Compressible Flow Analysis (GUI Method)

You perform the following steps to analyze the converging diverging nozzle using the GUI Method.

Step 1: Establish an Analysis Title and Preferences

Choose Utility Menu> File> Change Title. The Change Title dialog box appears.

Enter the text "Compressible Flow in a Converging Diverging Nozzle."

Click on OK.

Choose Main Menu> Preferences. The Preferences for GUI Filtering dialog box appears.

Click the button for FLOTRAN CFD to "On."

Click on OK.

Step 2: Define Element Types

Choose Main Menu> Preprocessor> Element Type> Add/Edit/Delete. The Element Types dialog box
appears.

Click on Add. The Library of Element Types dialog box appears.

In the two scrollable lists, highlight (click on) "FLOTRAN CFD" and "2D FLOTRAN 141."

Click on OK. ANSYS returns you to the Element Types dialog box.

Click on Close.

Step 3: Create Keypoints

Choose Main Menu> Preprocessor> Modeling> Create> Keypoints> In Active CS. The Create Keypoints
in Active Coordinate System dialog box appears.

In the "Keypoint number (NPT)" field enter 1 and in the "Location in active CS (X and Y)" fields enter 0
and 2.432, respectively. Click on Apply.

Repeat the previous substep for the following sets of keypoint numbers and (X, Y) locations: 2 (0, 0), 3
(1, 2.432), 4 (1, 0), 5 (2, 2.232), 6 (2, 0), 7 (5, 0), 8 (5, 0.7), 9 (6, 0), 10 (6, 0.5), 11 (14, 0), 12 (14, 0.8). After en-
tering each set, click on Apply. After entering the last set, click on OK.

Click on SAVE_DB on the ANSYS Toolbar.

Step 4: Create Lines

Choose Utility Menu> PlotCtrls> Numbering. The Plot Numbering Controls dialog box appears.

Click the button for "Line Numbers (LINE)" to "On" and click OK.

Choose Main Menu> Preprocessor> Modeling> Create> Lines> Lines> In Active Coord. The Lines
in Active Coord picking menu appears.

Section 8.7: Doing the Example Compressible Flow Analysis (GUI Method)

8–5

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Pick the keypoint numbers 2 and 4 and click on Apply.

Repeat steps 3 and 4 for the following sets of keypoint numbers: 3 and 4; 1 and 3; 1 and 2; and 5 and 8.
After entering each set, click on Apply. After entering the last set, click on OK.

Choose Main Menu> Preprocessor> Modeling> Create> Lines> Lines> Tan to 2 Lines. The Line
Tangent to 2 Lines picking menu appears.

Pick line number 3 and click on Apply. The Line Tangent to 2 Lines picking menu reappears.

Pick keypoint number 3 and click on Apply. The Line Tangent to 2 Lines picking menu reappears.

Pick line number 5 and click on Apply. The Line Tangent to 2 Lines picking menu reappears.

10. Pick keypoint number 5 and click on OK.

11. Choose Main Menu> Preprocessor> Modeling> Create> Lines> Lines> In Active Coord. The Lines

in Active Coord picking menu appears.

12. Pick the keypoint numbers 10 and 12 and click on OK.

13. Choose Main Menu> Preprocessor> Modeling> Create> Lines> Lines> Tan to 2 Lines. The Line

Tangent to 2 Lines picking menu appears.

14. Pick line number 5 and click on Apply. The Line Tangent to 2 Lines picking menu reappears.

15. Pick keypoint number 8 and click on Apply. The Line Tangent to 2 Lines picking menu reappears.

16. Pick line number 7 and click on Apply. The Line Tangent to 2 Lines picking menu reappears.

17. Pick keypoint number 10 and click on OK.

18. Choose Main Menu> Preprocessor> Modeling> Create> Lines> Lines> In Active Coord. The Lines

in Active Coord picking menu appears.

19. Pick the keypoint numbers 4 and 6 and click on Apply.

20. Enter the following sets of keypoint number by repeating steps 18 and 19: 6 and 7; 7 and 9; and 9 and

11. After entering each set, click on Apply. After entering the last set, click on OK.

Step 5: Create Areas

Choose Main Menu> Preprocessor> Modeling> Create> Areas> Arbitrary> Through KPs. The Create
Area thru KPs picking menu appears.

Pick the keypoint numbers (2, 4, 3, 1) and click on Apply.

Repeat the previous substep for the following sets of keypoint numbers: (4, 6, 5, 3), (6, 7, 8, 5), (7, 9, 10,
8), and (9, 11, 12, 10). After entering each set, click on Apply. After entering the last set, click on OK.

Click on SAVE_DB on the ANSYS Toolbar.

Step 6: Define Scalar Parameters

Choose Utility Menu> Parameters> Scalar Parameters. The Scalar Parameters dialog box appears.

Type in the parameter values shown below. (Press ENTER after entering each value.)

ntran = 24
rtran = 10
na = 10
nb = 10
nc = 25
nd = 10

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

8–6

Chapter 8: FLOTRAN Compressible Analyses

ne = 100
re = -1.5

Click on Close to close the dialog box.

Step 7: Mesh the Model

Choose Main Menu> Preprocessor> Meshing> Size Cntrls> Lines> Picked Lines. The Element Size
on Picked Lines picking menu appears.

Pick line number 4 and click on Apply. The Element Sizes on Picked Lines dialog box appears.

In the "No. of element divisions (NDIV)" field, enter ntran, and in the "Spacing ratio (SPACE)" field enter
rtran. Click on Apply.

Repeat steps 2 and 3 for line number 2.

Pick line number 13 and click on Apply. The Element Sizes on Picked Lines dialog box appears.

In the "No. of element divisions (NDIV)" field, enter ntran, and in the "Spacing ratio (SPACE)" field enter
1/rtran. Click on Apply.

Repeat steps 5 and 6 for line numbers 14, 15, and 16.

Pick line number 1 and click on Apply. The Element Sizes on Picked Lines dialog box appears.

In the "No. of element divisions (NDIV)" field, enter na, and in the "Spacing ratio (SPACE)" field enter 1.
Click on Apply.

10. Repeat steps 8 and 9 for line number 3.

11. Pick line number 6 and click on Apply. The Element Sizes on Picked Lines dialog box appears.

12. In the "No. of element divisions (NDIV)" field, enter nb, and in the "Spacing ratio (SPACE)" field enter 1.

Click on Apply.

13. Repeat steps 11 and 12 for line number 9.

14. Pick line number 5 and click on Apply. The Element Sizes on Picked Lines dialog box appears.

15. In the "No. of element divisions (NDIV)" field, enter nc, and in the "Spacing ratio (SPACE)" field enter 1.

Click on Apply.

16. Repeat steps 14 and 15 for line number 10.

17. Pick line number 8 and click on Apply. The Element Sizes on Picked Lines dialog box appears.

18. In the "No. of element divisions (NDIV)" field, enter nd, and in the "Spacing ratio (SPACE)" field enter 1.

Click Apply.

19. Repeat steps 17 and 18 for line number 11.

20. Pick line number 7 and click on Apply. The Element Sizes on Picked Lines dialog box appears.

21. In the "No. of element divisions (NDIV)" field, enter ne, and in the "Spacing ratio (SPACE)" field enter re.

Click on Apply.

22. Repeat steps 20 and 21 for line number 12 but this time click OK.

23. Choose Main Menu> Preprocessor> Meshing> Mesh> Areas> Mapped> 3 or 4 sided. A picking menu

appears.

24. Click on Pick All. The meshed model appears.

Section 8.7: Doing the Example Compressible Flow Analysis (GUI Method)

8–7

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Step 8: Compress Numbers

Choose Main Menu> Preprocessor> Numbering Ctrls> Compress Numbers. The Compress Numbers
dialog box appears.

Select Nodes as the "Item to be compressed" and click on Apply.

Select Elements as the "Item to be compressed" and click on OK.

Step 9: Apply Boundary Conditions

Choose Utility Menu> Select> Entities. The Select Entities dialog box appears.

Choose "Lines" and "By Num/Pick," then click on OK. A Select Lines picking menu appears.

Choose Utility Menu> Plot>Lines.

Pick lines 1, 9, 10, 11, and 12 and click on OK.

Choose Utility Menu> Select> Entities. The Select Entities dialog box appears.

Choose "Nodes" and "Attached to," click on Lines, all, and then click on OK.

Choose Main Menu> Preprocessor> Loads> Define Loads> Apply> Fluid/CFD> Velocity> On Nodes.
The Apply V on Nodes picking menu appears.

Click on Pick All. The Velocity Constraints on Nodes dialog box appears.

In the "Velocity component (VY)" field, enter 0, and click on OK.

10. Choose Utility Menu> Select> Entities. The Select Entities dialog box appears.

11. Choose "Lines" and "By Num/Pick," then click on the Sele All button. Click on OK. The Select Lines picking

menu appears.

12. Pick line number 4 and click on OK.

13. Choose Utility Menu> Select> Entities. The Select Entities dialog box appears.

14. Choose "Nodes" and "Attached to," click on Lines, all, and then click on OK.

15. Choose Main Menu> Preprocessor> Loads> Define Loads> Apply> Fluid/CFD> Pressure DOF> On

Nodes. The Apply PRES on Nodes picking menu appears.

16. Click on Pick All. The Pressure Constraint on Nodes dialog box appears.

17. In the "Pressure value (PRES)" field, enter 6.13769e+6, and click on OK.

18. Choose Utility Menu> Select> Entities.

19. Choose "Lines" and "By Num/Pick," then click on the Sele All button. Click on OK. The Select Lines picking

menu appears.

20. Pick line numbers 3, 5, 6, 7, and 8 and click on OK.

21. Choose Utility Menu> Select> Entities.

22. Choose "Nodes" and "Attached to," click on Lines, all, and then click on OK.

23. Choose Main Menu> Preprocessor> Loads> Define Loads> Apply> Fluid/CFD> Velocity> On Nodes.

The Apply V on Nodes picking menu appears.

24. Click on Pick All. The Velocity Constraints on Nodes dialog box appears.

25. In the "Velocity component (VX)" field and in the "Velocity component (VY)" enter 0, and click on OK.

26. Choose Utility Menu> Select> Entities. The Select Entities dialog box appears.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

8–8

Chapter 8: FLOTRAN Compressible Analyses

27. Choose "Lines" and "By Num/Pick," click on the Sele All button, and then click on OK. The Select Lines

picking menu appears.

28. Pick line number 16 and click on OK.

29. Choose Utility Menu> Select> Entities. The Select Entities dialog box appears.

30. Choose "Nodes" and "Attached to," click on Lines, all, and then click on OK.

31. Choose Main Menu> Preprocessor> Loads> Define Loads> Apply> Fluid/CFD> Pressure DOF> On

Nodes. The Apply PRES on Nodes picking menu appears.

32. Click on Pick All. The Pressure Constraint on Nodes dialog box appears.

33. In the "Pressure value (PRES)" field, enter 0, and click on OK.

Step 10: Set Fluid Properties

Choose Utility Menu> Select> Everything.

Choose Main Menu> Preprocessor> FLOTRAN Set Up> Fluid Properties. The Fluid Properties dialog
box appears.

Set the "Density (DENS)," "Viscosity (VISC)," "Conductivity (COND)," and "Specific heat (SPHT)" fields to
AIR-CM.

Set the "Allow density variations?" field to yes.

Click on Apply. The CFD Flow Properties dialog box appears.

Read the information about how coefficients will be calculated, and click on OK.

Step 11: Set Flow Environment Parameters

Choose Main Menu> Preprocessor> FLOTRAN Set Up> Flow Environment> Ref Conditions. The
Reference Conditions dialog box appears.

Set the "Reference pressure (REFE)" field to 1.01325e+6 and the "Nominal temperature (NOMI)" and
"Stagnation (total) temperature (TTOT)" fields to 550, and then click on OK.

Step 12: Set Solution Options and CFD Solver Controls

Choose Main Menu> Preprocessor> FLOTRAN Set Up> Solution Options. The FLOTRAN Solution
Options dialog box appears.

Set the "Laminar or turbulent (TURB)" field to Turbulent and the "Incompress or compress (COMP)" field
to Compressible. Click OK.

Choose Main Menu> Preprocessor> FLOTRAN Set Up> CFD Solver Contr> PRES Solver CFD. The
PRES Solver CFD dialog box appears.

Choose Precond conj res.

Click on OK. The Semi Direct Solver Options for Pressure dialog box appears.

In the "Convergence criterion" field, enter 1.e-12, and click on OK.

Step 13: Solve

Choose Main Menu> Solution> FLOTRAN Set Up> Relax/Stab/Cap> Prop Relaxation. The Property
Relaxation dialog box appears.

Set the "Density relaxation" field to 1.0 and click on OK.

Section 8.7: Doing the Example Compressible Flow Analysis (GUI Method)

8–9

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Choose Main Menu> Solution> FLOTRAN Set Up> Relax/Stab/Cap> MIR Stabilization. The Modified
Inertial Relaxation (MIR) dialog box appears.

Set the MIR values for the momentum and turbulence equations to 0.2

Choose Main Menu> Solution> FLOTRAN Set Up> Relax/Stab/Cap> Stability Parms. The Stability
Parameters dialog box appears.

Set the "Momentum inertia" field to 1.0, the "Pressure inertia" field to 1.e-4, and the "Artificial viscosity"
field to 10, and then click on OK.

Choose Main Menu> Solution> FLOTRAN Set Up> Execution Ctrl. The Steady State Control Settings
dialog box appears.

Set the "Global iterations (EXEC) field to 20 and click on OK.

Choose Main Menu> Solution> Run FLOTRAN.

10. After 20 iterations finish, the Solution is done message appears. Close it. Choose Main Menu> Solution>

FLOTRAN Set Up> Relax/Stab/Cap> Stability Parms. The Stability Parameters dialog box appears.

11. Set the "Artificial viscosity" field to 1 and click on OK.

12. Choose Main Menu> Solution> Run FLOTRAN.

13. Repeat the previous 3 substeps and continue to reduce the "Artificial viscosity" to .1, .01, .001, .0001, and

.00001.

14. After 140 total iterations finish, the Solution is done message appears. Close it. Choose Main Menu>

Solution> FLOTRAN Set Up> Relax/Stab/Cap> Stability Parms. The Stability Parameters dialog box
appears.

15. Set the "Artificial viscosity" field to 0 and click on OK.

16. Choose Main Menu> Solution> FLOTRAN Set Up> Execution Ctrl. The Steady State Control Settings

dialog box appears.

17. Set the "Global iterations (EXEC) field to 160 and click on OK.

18. Choose Main Menu> Solution> Run FLOTRAN.

19. After 300 total iterations finish, the Solution is done message appears. Close it. Choose Main Menu>

Solution> FLOTRAN Set Up> Relax/Stab/Cap> Stability Parms. The Stability Parameters dialog box
appears.

20. Set the "Momentum inertia" field to 10, the "Pressure inertia" field to 1.e-2, and then click on OK.

21. Choose Main Menu> Solution> FLOTRAN Set Up> Execution Ctrl. The Steady State Control Settings

dialog box appears.

22. Set the "Global iterations (EXEC) field to 100 and click on OK.

23. Choose Main Menu> Solution> Run FLOTRAN.

24. After 400 total iterations finish, the Solution is done message appears. Close it. Choose Main Menu>

Solution> FLOTRAN Set Up> Relax/Stab/Cap> Stability Parms. The Stability Parameters dialog box
appears.

25. Set the "Momentum inertia" field to 1e+15, the "Pressure inertia" field to 1.e+15, and then click on OK.

26. Choose Main Menu> Solution> FLOTRAN Set Up> Execution Ctrl. The Steady State Control Settings

dialog box appears.

27. Set the "Global iterations (EXEC) field to 400 and click on OK.

28. Choose Main Menu> Solution> Run FLOTRAN. When the Solution is done message appears, close it.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

8–10

Chapter 8: FLOTRAN Compressible Analyses

29. Click QUIT on the ANSYS Toolbar. Choose an exit option and click OK.

8.8. Doing the Example Compressible Flow Analysis (Command Method)

You issue the following ANSYS commands to perform a compressible flow analysis of the converging diverging
nozzle. Text preceded by an exclamation point (!) is a comment.

/title, Compressible Flow in a Converging Diverging Nozzle

/prep7

! Assign Element Type

et,1,141

! Create the Model Geometry

/pnum,line,1

k,1,0,2.432

k,2,0,0

k,3,1,2.432

k,4,1,0

k,5,2,2.232

k,6,2,0

k,7,5,0

k,8,5,.7

k,9,6,0

k,10,6,.5

k,11,14,0

k,12,14,.8

l,2,4

l,3,4

l,1,3

l,1,2

l,5,8

l2tan,3,5

l,10,12

l2tan,5,7

l,4,6

l,6,7

l,7,9

l,9,11

a,2,4,3,1

a,4,6,5,3

a,6,7,8,5

a,7,9,10,8

a,9,11,12,10

! !Mesh the Model and Compress Numbers

ntran=24

rtran=10

na=10

nb=10

nc=25

nd=10

ne=100

re=-1.5

lesize,4,,,ntran,rtran

lesize,2,,,ntran,rtran

lesize,13,,,ntran,1/rtran

lesize,14,,,ntran,1/rtran

lesize,15,,,ntran,1/rtran

lesize,16,,,ntran,1/rtran

lesize,1,,,na

lesize,3,,,na

lesize,6,,,nb

lesize,9,,,nb

lesize,5,,,nc

lesize,10,,,nc

lesize,8,,,nd

Section 8.8: Doing the Example Compressible Flow Analysis (Command Method)

8–11

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

lesize,11,,,nd

lesize,7,,,ne,re

lesize,12,,,ne,re

amesh,all

numcmp,node

numcmp,elem

! Apply Boundary Conditions

lsel,s,,,1

lsel,a,,,9,12,1

nsll,,1

d,all,vy,0

lsel,all

lsel,s,,,4

nsll,,1

d,all,pres,6.13769e+6

lsel,all

lsel,s,,,3

lsel,a,,,5,8,1

nsll,,1

d,all,vx,0

d,all,vy,0

lsel,all

lsel,s,,,16

nsll,,1

d,all,pres,0

! Set Fluid Properties

alls

/solu

flda,prot,dens,air-cm

flda,prot,visc,air-cm

flda,prot,cond,air-cm

flda,prot,spht,air-cm

flda,vary,dens,t

! Set Flow Environment Parameters

flda,pres,refe,1.01325e+6

flda,temp,ttot,550

flda,temp,nomi,550

! Set Solution Options and CFD Solver Controls

flda,solu,turb,t

flda,solu,comp,t

flda,meth,pres,3

flda,conv,pres,1e-12

! Solve

flda,relx,dens,1

flda,mir,mome,0.2

flda,mir,turb,0.2

flda,stab,mome,1

flda,stab,pres,1e-4

flda,stab,visc,10

flda,iter,exec,20

solve

flda,stab,visc,1

solve

flda,stab,visc,.1

solve

flda,stab,visc,.01

solve

flda,stab,visc,.001

solve

flda,stab,visc,.0001

solve

flda,stab,visc,.00001

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

8–12

Chapter 8: FLOTRAN Compressible Analyses

solve

flda,stab,visc,0

flda,iter,exec,160

solve

flda,stab,mome,10

flda,stab,pres,1e-2

flda,iter,exec,100

solve

flda,stab,mome,1e+15

flda,stab,pres,1e+15

flda,iter,exec,400

solve

Section 8.8: Doing the Example Compressible Flow Analysis (Command Method)

8–13

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

8–14

Chapter 9: Specifying Fluid Properties for
FLOTRAN

9.1. Guidelines for Specifying Properties

Every flow analysis requires the fluid properties density and viscosity. Thermal analyses, in addition, require the
fluid's thermal conductivity as well as specific heat. Volume of Fluid (VOF) analyses, in addition, might require
the fluid properties surface tension coefficient and wall static contact angle. You specify fluid properties using
one of the following:

Command(s): FLDATA7,PROT,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Fluid Properties
Main Menu> Solution> FLOTRAN Set Up> Fluid Properties

The command shown above simply sets the fluid property type. After choosing the property type, you may have
to set values.

To specify non-fluid properties (density, specific heat, and thermal conductivity), use one of the following:

Command(s): MP
GUI: Main Menu> Preprocessor> Loads> Other> Change Mat Props> Polynomial
Main Menu> Preprocessor> Material Props> Material Models> Thermal> Density
Main Menu> Preprocessor> Material Props> Material Models> Thermal> Specific Heat
Main Menu> Preprocessor> Material Props> Material Models> Thermal> Conductivity> Isotropic
Main Menu> Solution> Other> Change Mat Props> Polynomial

Non-fluid thermal conductivities can vary with temperature. Orthotropic variation of non-fluid thermal conduct-
ivity also is supported. For further information, see the descriptions of the MP and MPDATA commands, and
related commands.

ANSYS provides no default values for density or viscosity properties. This prevents default properties from putting
the analysis into an unexpected flow regime.

A value of -1 will appear in the user interface for properties that must be set. If you submit an analysis without
setting these properties, an error message results and you will be reminded that you must specify properties.

9.2. Fluid Property Types

A "fluid property type" defines how the particular fluid property will vary with temperature (and pressure, in the
case of density for a gas). You choose the fluid property type separately for density, viscosity, thermal conduct-
ivity, specific heat, surface tension coefficient, and wall static contact angle.

You must use a consistent set of units for all the data that you enter. All thermal quantities must have the same
energy unit as shown in the following table:

Table 9.1 Units for Thermal Quantities

Units

Thermal Quantity

energy/length-temperature-time

Thermal Conductivity

energy/mass-temperature

Specific Heat

energy/length

-time

Heat Flux

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Units

Thermal Quantity

energy/length

-time

Volumetric Heat Source

energy/length

-temperature-time

Heat Transfer Coefficient

Except for incompressible flow analyses including viscous heating, you can use any energy unit as long as you
use the same unit for all thermal quantities. The metric and English property types defined below use joules and
BTUs, respectively, as the energy unit for thermal conductivity and specific heat. For an incompressible analysis
including viscous heating, you must use the energy unit for the system as shown in the following table:

Table 9.2 Energy Units for Incompressible Analyses with Viscous Heating

Energy Unit[1]

System

Joule

SI (meter-kg-sec)

Erg

CGS (cm-g-sec)

Centi-erg

mm-g-sec

lbf-ft

British (ft-slug-sec)

lbf-in

PSI

1 Joule = 1.0E9 Centi-ergs; 1 BTU = 778.26 lbf-ft.

9.2.1. Property Types for Specific Heat

For specific heat, you can choose among the following property types: CONSTANT, CMIX, TABLE, user-defined
through a file (floprp.ans), user-programmable subroutine (USER), and the variations of AIR shown below in
Table 9.3: “Units for the AIR Property Type”.

9.2.2. Property Types for Density and Thermal Conductivity

For density and thermal conductivity, the property types you can choose are CONSTANT, CMIX, TABLE, GAS, LIQUID,
user-defined through a file (floprp.ans), and the variations of AIR shown below. (To learn how to add more, see
Section 9.4: Modifying the Fluid Property Database.) A user-programmable subroutine (USER) also is available.
For density only, you have one other property type option: CGAS.

Table 9.3 Units for the AIR Property Type

Viscosity Units

Density Units

Pressure Units

Units

PROT

kg/m-sec

kg/m

Pascals

meter-kg-sec

AIR

kg/m-sec

kg/m

Pascals

meter-kg-sec

AIR-SI

g/cm-sec (poise)

g/cm

dynes/cm

cm-g-sec

AIR-CM

g/mm-sec

g/mm

Pascals

mm-g-sec

AIR-MM

slug/ft-sec

slugs/ft

lbf/ft

ft-slug-sec

AIR-FT

lbf-s/in

lbf-sec

/in

psi

in-(lbf-s

/in)-sec

AIR-IN

ANSYS automatically supplies for you, in the property database, the relevant input for the AIR property types.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

9–2

Chapter 9: Specifying Fluid Properties for FLOTRAN

9.2.3. Property Types for Viscosity

For viscosity, you can choose the property types CMIX, TABLE, CONSTANT, LIQUID, GAS, Power Law (POWL),
Bingham (BING), Carreau (CARR), user-defined through a file (floprp.ans), and a user-programmable subroutine
(USER or USRV). The AIR and GAS property types assume that the fluid is an ideal gas with constant specific heat.
The viscosity and thermal conductivity variations with temperature are assumed to follow Sutherland's laws for
gases, the form of which is shown below. A LIQUID assumes up to a second order polynomial for the variation
of density with temperature, a constant value for specific heat, and Sutherland's laws for a liquid for viscosity
and thermal conductivity.

Viscosity as a function of the velocity gradient is represented by the non-Newtonian viscosity types: Power Law,
Bingham, and Carreau. Refer to Section 9.6: Using the ANSYS Non-Newtonian Flow Capabilities for more inform-
ation.

9.2.4. Property Types for Surface Tension Coefficient

For surface tension coefficient, you can choose among the following property types: CONSTANT, LIQUID, and
user-programmable subroutine (USER).

9.2.5. Property Types for Wall Static Contact Angle

For wall static contact angle, CONSTANT is the only valid property type.

9.2.6. General Guidelines for Setting Property Types

You must use a consistent set of units (the gravitational constant g

must be unity.) Of course, the proper length

unit must be assumed when building the finite element model. Additional choices are available for air as per the
table shown below. Units for density are simply mass/volume; the table omits them.

Set the property type using the following:

Command(s): FLDATA7,PROT,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Fluid Properties
Main Menu> Solution> FLOTRAN Set Up> Fluid Properties

For

Label

, you specify one of the following: DENS (density), VISC (viscosity), COND (thermal conductivity), SPHT

(specific heat), or SFTS (surface tension coefficient).

For

Value

, you specify any of the property types listed in Table 9.4: “Property types for Value”, or you can specify

a table of fluid properties. To specify a table, enclose the table name in percent signs (%) (for example,
FLDATA7,PROT,DENS,%Table%).

9.2.6.1. Using a Fluid Property Table

If working interactively, you define a new table prior to using the table to apply loads. You can define a table
interactively via the Utility Menu> Parameters> Array Parameters> Define/Edit menu path, or in batch mode
via the *DIM command. If working interactively, you will be asked to define the table through a series of dialog
boxes. If working in batch mode, you need to define the table before issuing any of the loading commands.

For more information on defining tables, see the discussion of table array parameters in the ANSYS APDL Program-
mer's Guide.

When you define the table, you can define the following primary variables:

Section 9.2: Fluid Property Types

9–3

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

•

Temperature (TEMP)

•

Pressure (PRESSURE)

•

Time (TIME)

•

X-coordinate (X)

•

Y-coordinate (Y)

•

Z-coordinate (Z)

•

Velocity (VELOCITY)

•

Reference X-coordinate (Xr) (ALE formulation only)

•

Reference Y-coordinate (Yr) (ALE formulation only)

•

Reference Z-coordinate (Zr) (ALE formulation only)

The valid labels used by the *DIM command are shown in parentheses.

If you need to specify a variable other than one of the primary variables listed, you can do so by defining an in-
dependent variable. To specify an independent variable, define an additional table for the independent variable.
That table must have the same name as the independent variable and can be a function of either a primary
variable or another independent variable.

9.2.6.2. Specifying Property Types

The following table describes the property types that you can specify.

Table 9.4 Property types for

Value

Argument

Property Type

CONSTANT

Constant properties

GAS

Gas properties

LIQUID

Liquid properties

TABLE

Table of property values and corresponding temperature values (which you enter using the
MPDATAand MPTEMP commands)

AIR or AIR-SI

Air properties in units of meter-kg-sec

AIR_B or AIR-SI_B

Air properties in units of meter-kg-sec, with pressure set to the reference pressure for the
evaluation of density

AIR-CM

Air properties in units of cm-g-sec

AIR-CM_B

Air properties in units of cm-g-sec, with pressure set to the reference pressure for the evalu-
ation of density

AIR-MM

Air properties in units of mm-g-sec

AIR-MM_B

Air properties in units of mm-g-sec, with pressure set to the reference pressure for the
evaluation of density

AIR-FT

Air properties in units of fl-slug-sec

AIR-FT_B

Air properties in unites of fl-slug-sec, with pressure set to the reference pressure for the
evaluation of density

AIR-IN

Air properties in units of in-(lbf-s**2/in)-sec (results in units of psi for pressure)

AIR-IN_B

Air properties in units of in-(lbf-s**2/in)-sec (results in units of psi for pressure), with pressure
set to the reference pressure for the evaluation of density

POWL

Power Law non-Newtonian viscosity type

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

9–4

Chapter 9: Specifying Fluid Properties for FLOTRAN

Argument

Property Type

CARR

Carreau non-Newtonian viscosity type

BING

Bingham non-Newtonian viscosity type

CMIX

Property is mass fraction average of the species component

USER

User-programmable via subroutines:UserVisLaw for viscosityUserSpht for specific
heatUserDens for densityUserCond for conductivityUserSfts for surface tension

CGAS

A variation of ideal gas law based on species mass fractions. Available for density only.

Once you choose property types, you do not need to specify any coefficients for the properties. If the characters
_B are added to these property types (as in the AIR types listed above), the pressure in the ideal gas law calculation
is at a constant density corresponding to atmospheric pressure. The length and time units of conductivity and
specific heat must be consistent with the rest of the properties. The energy units in these quantities are unres-
tricted.

If using property types CONSTANT, GAS, or LIQUID, you must specify property coefficients. To do so, either issue
the commands shown below or choose one of the following menu paths:

Command(s): FLDATA8,NOMI,

Label

Value

FLDATA9,COF1,

Label

Value

FLDATA10,COF2,

La-

bel

Value

FLDATA11,COF3,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Fluid Properties
Main Menu> Solution> FLOTRAN Set Up> Fluid Properties

If you use the commands, you enter the property in the

Label

field of each command and enter the value itself

in each command's

Value

field.

The format of the equations for GAS and LIQUID input is oriented towards calculating constants based on chosen
data points. All cases take COF1 to be the absolute temperature at which the chosen property has the value set
by NOMI. (Section 9.5: Using Reference Properties discusses the use of relative temperatures and an offset tem-
perature to calculate absolute temperatures.) This is not used in the COF1 specification; COF1 should always be
an absolute temperature.

Once values are inserted into the relationships below for NOMI and COF1, the values of COF2 and COF3, if neces-
sary, follow from knowledge of one or two additional data points, respectively. When calculating COF2 and COF3
for GAS and LIQUID property types, you must use absolute temperatures and pressures in these relationships.
If COF1 is set to zero, the property will become constant at the value set by NOMI. For GAS and LIQUID property
types, the specific heat is constant and therefore the parameters COF1, COF2 and COF3 are not needed. For vis-
cosity types Power Law, Bingham, and Carreau, NOMI, COF1, COF2, and COF3 have different interpretations. This
is discussed in the ANSYS, Inc. Theory Reference and in Section 9.2.8: Viscosity.

9.2.7. Density

If the property type choice is CONSTANT, then set the constant value of the property using the FLDATA8,NOMI
command or the equivalent menu path. For example, you set the density to 1.205 via:

Command(s):

FLDATA8,NOMI,DENS,1.205

If the property type is GAS, the ideal gas law is used for the density. You specify density for this choice as:

Density = NOMI * (P/COF2) / (T/COF1)

If the choice is LIQUID, then a second order polynomial as a function of temperature is used for density.

Section 9.2: Fluid Property Types

9–5

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Density = NOMI + COF2*(T - COF1) + COF3*(T - COF1)

If the property type is CMIX, then:

Density

∑

i i

In the equation shown above, N is the defined number of species, Y

is the mass fraction of the ith species, and

is the density of the ith species.

If the property is CGAS, then:

Density

∑

Y M

(

)

In the CGAS equation shown above, N is the defined number of species, Y

is the mass fraction of the ith species,

is the molecular weight of the ith species, R is the universal gas constant, and P is the absolute pressure.

If the property type is TABLE, the density is interpolated linearly between the data points provided via the
MPTEMP or MPDATA commands (or their GUI equivalents).

If the choice is USER, the density is computed in the user-programmable subroutine UserDens. The four coefficients
NOMI, COF1, COF2, and COF3 are available in this routine.

9.2.8. Viscosity

If the property type choice is CONSTANT, then set the constant value of the property using the FLDATA8,NOMI
command or the equivalent menu path. For example, you set the viscosity to 1.205 via:

Command(s):

FLDATA8,NOMI,VISC,1.205

If the choice is GAS, Sutherland's law for gases is used for viscosity. You can enter the parameters NOMI, COF1,
and COF2.

The ideal gas constant R is defined as (COF2/NOMI*COF1)

Viscosity ("Property"):

Property/NOMI = (T/COF1)

1.5

* (COF1 + COF2)/(T + COF2)

As an example of using this relationship, suppose that there are two data points available for the calculation of
viscosity as a function of temperature:

Viscosity = 4.18 x 10

-5

at T = 760

Viscosity = 5.76 x 10

-5

at T = 1010

Consider the first data point as the nominal value. This means that NOMI = 4.18 x 10

-5

and COF1 = 760. Using

these in the Sutherland relationship yields:

Property/4.18 x 10

-5

= (T/760)

1.5

(760 + COF2)/(T + COF2)

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

9–6

Chapter 9: Specifying Fluid Properties for FLOTRAN

Use the remaining data point to calculate COF2 by setting "Property" to 5.76 x 10

-5

and T = 1010. Thus, the con-

stants are calculated from the data points.

If the choice is LIQUID, then Sutherland's liquid law is used for the viscosity.

Viscosity ("Property"):

Property/NOMI = EXP{COF2*(1/T - 1/COF1) + COF3(1/T - 1/COF1)

}

If the choice is POWL, then the non-Newtonian Power Law model is used for the viscosity:

Viscosity =

NOMI*COF2*D

,D>COF1

NOMI*COF2*COF1

(COF3-1)

,,D COF1

≤








If the choice is BING, then the non-Newtonian Bingham model is used for the viscosity:

Viscosity =

NOMI+

COF1

COF2 NOMI

COF2

,D<

COF1

COV2 -NOMI

≥

−











If the choice is CARR, the non-Newtonian Carreau model is used for the viscosity:

Viscosity =COF1+(NOMI - COF1)*(1+(COF2*D) )

COF3-1









If the property type is CMIX, then:

Viscosity

∑

i i

In the equation shown above, N is the defined number of species, Y

is the mass fraction of the ith species, and

is the viscosity of the ith species.

If the property type is TABLE, the density is interpolated linearly between the data points provided via the
MPTEMP or MPDATA commands (or their GUI equivalents).

If the choice is USRV or USER, then the viscosity is computed in the user programmable subroutine UserVisLaw.
The four coefficients NOMI, COF1, COF2, and COF3 are available in this routine.

9.2.9. Specific Heat

If the property type choice is CONSTANT, then set the constant value of the property using the FLDATA8,NOMI
command or the equivalent menu path. For example, you set the specific heat to 1.205 via:

Command(s):

FLDATA8,NOMI,SPHT,1.205

If the choice is USER, specify specific heat via user-programmable subroutine UserSpht. For specific heat, NOMI,
COF1, COF2, and COF3 are available in the user-programmable subroutine UserSpht.

If the property type is CMIX, then:

Section 9.2: Fluid Property Types

9–7

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Specific Heat

∑

Y C

In the equation shown above, N is the defined number of species, Y

is the mass fraction of the ith species, and

is the specific heat of the ith species.

If the property type is TABLE, the specific heat is interpolated linearly between the data points provided via the
MPTEMP or MPDATA commands (or their GUI equivalents).

9.2.10. Thermal Conductivity

If the property type choice is CONSTANT, then set the constant value of the property using the FLDATA8,NOMI
command or the equivalent menu path. For example, you set the thermal conductivity to 1.205 via:

Command(s):

FLDATA8,NOMI,COND,1.205

If the choice is GAS, Sutherland's law for gases is used for conductivity. You can enter the parameters NOMI,
COF1, and COF2.

The ideal gas constant R is defined as (COF2/NOMI*COF1)

Thermal Conductivity ("Property"):

Property/NOMI = (T/COF1)

1.5

* (COF1 + COF2)/(T + COF2)

If the choice is LIQUID, then Sutherland's liquid law is used for conductivity.

Thermal Conductivity ("Property"):

Property/NOMI = EXP{COF2*(1/T - 1/COF1) + COF3(1/T - 1/COF1)

}

If the property type is CMIX, then:

Conductivity

∑

Y K

i i

In the equation shown above, N is the defined number of species, Y

is the mass fraction of the ith species, and

is the conductivity of the ith species.

If the property type is TABLE, the density is interpolated linearly between the data points provided via the
MPTEMP or MPDATA commands (or their GUI equivalents).

If the choice is USER, then the thermal conductivity is computed in the user programmable subroutine UserCond.
The four coefficients NOMI, COF1, COF2, and COF3 are available in this routine.

9.2.11. Surface Tension Coefficient

If the property type choice is CONSTANT, then set the constant value of the property using the FLDATA8,NOMI
command or the equivalent menu path. For example, you set the surface tension coefficient to 73.0 via:

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

9–8

Chapter 9: Specifying Fluid Properties for FLOTRAN

Command(s):

FLDATA8,NOMI,SFTS,73.0

If the choice is LIQUID, then a second order polynomial as a function of temperature is used for surface tension
coefficient.

Surface tension coefficient = NOMI + COF2*(T - COF1) + COF3*(T - COF1)

If the choice is USER, the surface tension coefficient is computed in the user-programmable subroutine UserSfts.
The four coefficients NOMI, COF1, COF2, and COF3 are available in this routine.

9.2.12. Wall Static Contact Angle

To set the constant value use the FLDATA8,NOMI command or the equivalent menu path. For example, set the
wall static contact angle to 120.0 degrees via:

Command(s):

FLDATA8,NOMI,WSCA,120.0

The wall static contact angle defaults to 90 degrees. Angles less than 90 degrees describe an adhesive wall con-
dition and angles between 90 and 180 degrees describe a nonadhesive wall condition. In reality, the angle is not
only a material property of the fluid, but also depends on the local fluid and wall conditions. FLOTRAN treats it
as a single input constant for simplicity.

9.3. Initializing and Varying Properties

When an analysis begins, ANSYS calculates properties based on the specified property type and the appropriate
constants. To set the initial temperature, choose one of the following:

Command(s): FLDATA14,TEMP,NOMI,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Flow Environment> Ref Conditions
Main Menu> Solution> FLOTRAN Set Up> Flow Environment> Ref Conditions

You can choose to treat this temperature as an absolute or a relative temperature. If it is a relative temperature,
the difference between the relative and the absolute temperature is the offset from absolute zero set by one of
the following:

Command(s): TOFFST,Value
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Flow Environment> Ref Conditions
Main Menu> Solution> FLOTRAN Set Up> Flow Environment> Ref Conditions

Either way, FLOTRAN initializes the absolute nominal temperature as the sum of the values set by the
FLDATA,TEMP,NOMI and TOFFST commands or their equivalent menu paths.

Unless otherwise specified through boundary or initial condition commands, the initial relative pressure is zero.
In the absence of gravity and rotation the absolute pressure is the sum of the reference and relative pressures.
Therefore, the initial absolute pressure is the reference pressure.

For specific heat, density, surface tension coefficient, and thermal conductivity, the ANSYS program uses initial
values of absolute nominal temperature and absolute pressure to calculate the initial properties. However, for
non-Newtonian viscosity, you specify initial properties using either the command FLDATA12,PROP,IVISC,

Value

(Main Menu> Preprocessor> FLOTRAN Set Up> Fluid Properties). If you specify a value less than or equal to
zero, the NOMI coefficient described in the previous section is used to initialize the viscosity.

Section 9.3: Initializing and Varying Properties

9–9

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

9.3.1. Activating Variable Properties

Once the analysis begins, the properties will vary only between global iterations as the temperature and pressure
change if the property variations are activated. This is accomplished with the FLDATA13,VARY,

Label

Value

command with the labels SPHT, DENS, VISC, SFTS, and COND. Allowable

Value

s are TRUE and FALSE (T or F). The

VARY setting has no effect if the property type are set to CONSTANT or COF1 is zero for a GAS or LIQUID.

9.4. Modifying the Fluid Property Database

Choices other than CGAS, CMIX, TABLE, USER, GAS, LIQUID, CONSTANT or AIR for density, thermal conductivity,
viscosity, and specific heat imply that all the properties will be obtained from the information in the floprp.ans
file (a text file), where the data for AIR resides. This file is provided with ANSYS, and you should make a local copy
if you plan additions to it. You can make the copy at the system level with a text editor. The procedure for making
additions requires you to:

Choose a property name.

Specify functional form and constants.

id Integer equation identifier (two digit number)
n Number of coefficients
C

Equation coefficients

You can access the following forms through the property database by specifying the appropriate ID. The variable
"y" refers to the value of the property of interest, T is the absolute temperature, and P is the absolute pressure.

Polynomial ID: 01

y = C

+ C

T + C

+ ... + C

n-1

Inverse Polynomial ID: 02

+ +

−

3
2

…

Exponential Polynomial ID: 03

In(y) = C

+ C

T + C

+ ... + C

n-1

Exponential Inverse Polynomial ID: 04

In y

( )

+ +

−

3
2

…

Power Law ID: 05

y = C

Ideal Gas Law ID: 11

C T

Sutherland's Formula ID: 12

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

9–10

Chapter 9: Specifying Fluid Properties for FLOTRAN

C T

T C

Pressure based variation ID: 15

C P

Non-Newtonian Power Law ID: 16 (applies to viscosity only)

y C C D

D C

y C C C

D C

≤

−

1 3

1 3 2

(

)

(

)

where

, I

is the second invariant of the strain rate tensor.

Non-Newtonian Bingham Model ID: 17 (applies to viscosity only)

y C

≥

−

Carreau Model ID: 18 (applies to viscosity only)

y C

C D

−







4 1

(

) * (

(

) )

User-programmable subroutine: 19

y = y (C

, C

)

Because you can use the subroutine to describe property variations, you can use the four coefficients in any way
within the subroutine.

The format of the property database file floprp.ans is provided in the table below:

Table 9.5 Property Database Format

Description

Line

Fluid Name [A8] and optional comments

nLines [I6]

Proplab, tProp, nProp

(PropCF(i)=1,nProp)

[A4, 1x, 2I6, 5E12.5/6E 12.5]

nLines

Section 9.4: Modifying the Fluid Property Database

9–11

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Description

Line

Fluid Name=Fluid property type

nLines=Number of properties to be read

Proplab=Property label (one of the following):

SPHT - Specific heat
DENS - Density
VISC - Viscosity
COND - Conductivity
GAMM - Gamma
tProp - Equation identifier for property
nProp - Number of coefficients for property
PropCF - Coefficients for property calculation

9.5. Using Reference Properties

The following properties are part of the flow environment:

•

The ratio of specific heats, C

, known as gamma, is a reference property that applies only to compressible

problems. Currently it is a constant. Specify this property using one of these methods:

Command(s): FLDATA17,GAMM,COMP,VALUE
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Flow Environment> Ref Conditions

File:

Edit the file floprp.ans and set the value of GAMM.

•

The pressures FLOTRAN calculates are relative pressures. A reference pressure is added to the relative
pressure to calculate the absolute pressure. Rotational and gravitational terms also are added as needed.
For more information, see Chapter 10, “FLOTRAN Special Features”.

To specify the reference pressure, use one of the following:

Command(s): FLDATA15,PRES,REFE,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Flow Environment> Ref Conditions
Main Menu> Solution> FLOTRAN Set Up> Flow Environment> Ref Conditions

•

You can use a relative temperature (for example, degrees Fahrenheit rather than degrees Rankine). In this
case, an offset temperature is set so that property calculations include absolute temperatures. This is ne-
cessary, for instance, for calculating densities from the ideal gas law. ANSYS automatically adds the offset
temperature to all of the boundary condition temperatures applied.

To set the offset temperature, use one of the following

Command(s): TOFFST,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Flow Environment> Ref Conditions
Main Menu> Solution> FLOTRAN Set Up> Flow Environment> Ref Conditions

•

The nominal temperature is that at which the properties initialize. It may be a relative temperature if you
use the TOFFST command or an equivalent menu path. If the viscosity is not stored in the results file (the
default condition) and is now allowed to vary, ANSYS recalculates it when the analysis continues at the
nominal temperature.

To specify the nominal temperature, use one of the following:

Command(s): FLDATA14,TEMP,NOMI,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Flow Environment> Ref Conditions

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

9–12

Chapter 9: Specifying Fluid Properties for FLOTRAN

Main Menu> Solution> FLOTRAN Set Up> Flow Environment> Ref Conditions

•

You can specify gravitational accelerations using one of the following:

Command(s): ACEL,

ACELX

ACELY

ACELZ

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Flow Environment> Gravity
Main Menu> Solution> FLOTRAN Set Up> Flow Environment> Gravity

The sign convention of the gravitational acceleration denotes as positive the direction of the reaction force.

9.6. Using the ANSYS Non-Newtonian Flow Capabilities

The ANSYS program enables you to specify viscosity for non-Newtonian fluid flows. (You can use this capability
only with FLUID141 and FLUID142 elements.) You can choose among four types of models:

•

The Power Law model, useful for modeling polymers, blood, rubber solutions, etc.

•

The Carreau model, which removes some of the deficiencies associated with the Power Law model. Use
this model when fluid has intermediate values of shear rate but remains bounded for zero/infinite shear
rates.

•

The Bingham model, useful for modeling slurries and pastes.

•

A user-programmable subroutine UserVisLaw, which gives you greater flexibility in choosing viscosity
models.

Typically, you select one of these models after you have built and meshed the model for your problem and after
you have applied the boundary conditions.

9.6.1. Activating the Power Law Model

To activate the Power Law viscosity model, issue the command or use one of the menu paths shown below:

Command(s): FLDATA7,PROT,VISC,POWL
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Fluid Properties
Main Menu> Solution> FLOTRAN Set Up> Fluid Properties

Choosing any of the above automatically issues other commands which set output and storage controls and the
property variation flag. For details, see the descriptions of the FLDATA commands in the ANSYS Commands
Reference.

To specify the four coefficients associated with the Power Law model, choose either of the menu paths shown
above (and specify the appropriate coefficients), or issue the following commands:

Command(s):

FLDATA8,NOMI,VISC,

Value

(specifies nominal viscosity)

FLDATA9,COF1,VISC,

Value

(specifies the cutoff shear rate)

FLDATA10,COF2,VISC,

Value

(specifies the consistency coefficient)

FLDATA11,COF3,VISC,

Value

(specifies the power)

The ANSYS, Inc. Theory Reference describes these coefficients.

Once you have specified the coefficients, you can issue the SOLVE command or choose menu path Main Menu>
Solution> Run FLOTRAN.

Section 9.6: Using the ANSYS Non-Newtonian Flow Capabilities

9–13

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

9.6.2. Activating the Carreau Model

To activate the Carreau viscosity model, issue the command or use one of the menu paths shown below:

Command(s): FLDATA7,PROT,VISC,CARR
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Fluid Properties
Main Menu> Solution> FLOTRAN Set Up> Fluid Properties

Choosing one of the above automatically issues commands which set output and storage controls and the
property variation flag. For more information about the FLDATA commands, see the ANSYS Commands Reference.

You need to specify the four coefficients associated with the Carreau model, using either of the menu paths
shown above or the following commands:

Command(s):

FLDATA8,NOMI,VISC,

Value

(specifies the zero shear viscosity)

FLDATA9,COF1,VISC,

Value

(specifies the infinite shear viscosity)

FLDATA10,COF2,VISC,

Value

(specifies the time constant)

FLDATA11,COF3,VISC,

Value

(specifies the power)

The ANSYS, Inc. Theory Reference describes these coefficients. Once you have specified them, you can issue the
SOLVE command or choose menu path Main Menu> Solution> Run FLOTRAN.

9.6.3. Activating the Bingham Model

To activate the Bingham viscosity model, issue the command or choose one of the menu paths shown below:

Command(s): FLDATA7,PROT,VISC,BING
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Fluid Properties
Main Menu> Solution> FLOTRAN Set Up> Fluid Properties

Choosing one of the items shown above automatically issues commands that set output and storage controls
and the property variation flag.

To set the coefficients associated with the Bingham model, either use one of the menu paths shown above or
issue the following commands:

FLDATA8,NOMI,VISC,

Value

(specifies the plastic viscosity)

FLDATA9,COF1,VISC,

Value

(specifies the plastic/yield stress)

FLDATA10,COF2,VISC,

Value

(specifies the Newtonian viscosity)

The ANSYS, Inc. Theory Reference describes these coefficients.

You can also specify an initial viscosity to accelerate convergence. Typically, you can set this to be the Newtonian
viscosity (that is, COF2) via one of the following:

Command(s): FLDATA12,PROP,VISC,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Fluid Properties
Main Menu> Solution> FLOTRAN Set Up> Fluid Properties

9.7. Using User-Programmable Subroutines

User-programmable subroutines are available for specific heat, density, viscosity, surface tension coefficient,
and thermal conductivity of fluid regions. Since the procedures are quite similar, only one property will be de-
scribed in depth here.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

9–14

Chapter 9: Specifying Fluid Properties for FLOTRAN

If you wish to use the user-programmable viscosity subroutine, USERVISLAW, you will need to customize it for
the particular model you are analyzing. You compile the subroutine, link it with the ANSYS libraries, and make
an executable copy available. Then, you can resume the model to be analyzed and activate the viscosity model
you have defined. To do so, use one of the following:

Command(s): FLDATA7,PROT,VISC,USRV (or USER)
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Fluid Properties
Main Menu> Solution> FLOTRAN Set Up> Fluid Properties

At this point, you may want to specify that properties are updated every iteration and that you want viscosity
output to go to the results file. To do so, issue the following commands or use the following menu paths:

Command(s): FLDATA12,PROP,UFRQ,1 and FLDATA5,OUTP,VISC,T
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Fluid Properties
Main Menu> Solution> FLOTRAN Set Up> Fluid Properties

Next, you need to specify the four coefficients associated with the user-defined viscosity model. To do so, use
either of the menu paths shown above or issue the following commands:

Command(s):

FLDATA7,NOMI,VISC,

Value

(specifies coefficient 1)

FLDATA6,COF1,VISC,

Value

(specifies coefficient 2)

FLDATA9,COF2,VISC,

Value

(specifies coefficient 3)

FLDATA10,COF3,VISC,

Value

(specifies coefficient 4)

These coefficients are available within the UserVisLaw subroutine. By default, this subroutine produces a Power
Law viscosity model using the coefficients you define. To see a copy of the subroutine, see the Guide to ANSYS
User Programmable Features.

You can also specify an initial viscosity to accelerate convergence, via one of the following:

Command(s): FLDATA12,PROP,IVISC,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Fluid Properties
Main Menu> Preprocessor> FLOTRAN Set Up> Fluid Properties

Once you have specified the coefficients, and, optionally, an initial viscosity, you can solve your model by issuing
the SOLVE command or choosing Main Menu> Solution> Run FLOTRAN.

Section 9.7: Using User-Programmable Subroutines

9–15

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

9–16

Chapter 10: FLOTRAN Special Features

10.1. Coordinate Systems

You set the coordinate system via one of the following:

Command(s): KEYOPT
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Flow Environment> FLOTRAN Coor Sys
Main Menu> Solution> FLOTRAN Set Up> Flow Environment> FLOTRAN Coor Sys

The table below shows you how to select various coordinate systems and describes the velocities represented
by DOFs VX, VY, and VZ in these systems. The default value of the KEYOPT is zero, which selects Cartesian coordin-
ates.

Figure 10.1 Direction of Positive Swirl Velocity VZ for Axisymmetric Models

Table 10.1 Coordinate System Specification

KEYOPT(3)

Coordinate System

Cartesian

swirl

axial

radial

2-D - Axisymmetric about Y axis

swirl

radial

axial

2-D - Axisymmetric about X axis

N/A

theta

radial

2-D - Polar Coordinates

axial

theta

radial

3-D - Cylindrical Coordinates

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

For axisymmetric problems, the sign convention for the swirl (VZ) component conforms to positive rotation
about the axis of symmetry, as defined by the right hand rule. Thus, for a model that is axisymmetric about the
Y axis, a nonnegative swirl velocity VZ is considered to be pointing "into the page." Similarly, for a model that is
axisymmetric about the X axis, a nonnegative swirl velocity VZ is considered to be pointing "out of the page."
This should be accounted for when you apply boundary conditions in rotating coordinates.

Note — Based on the definition of directions for the cylindrical coordinate system, gravity is only appro-
priate for the Z direction when KEYOPT(3) is set to 3.

10.2. Rotating Frames of Reference

You can choose to solve your problem in a rotating reference frame. In this case, the velocities are calculated
and specified with respect to a coordinate system which is rotating at constant angular velocity. Such an approach
is useful for pump blade passage analysis. Figure 10.2: “Rotating Flow Problem” shows a schematic of a rotating
problem which requires moving coordinate systems. Figure 10.3: “Problem Schematic with Rotating Coordinate”
shows the problem schematic in the rotating coordinate system.

The pressures specified by boundary conditions are in terms of the static pressure observable by the stationary
analyst, not in terms of the rotating coordinate system. The transformations necessary to solve the equations in
the rotating coordinate frame are done internally.

You can set rotational speeds using any of the following:

Command(s): CGOMGA
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Flow Environment> Rotating Coords
Main Menu> Solution> FLOTRAN Set Up> Flow Environment> Rotating Coords

For all but 3-D Cartesian coordinate systems, you must specify the axis of rotation as being about the Z axis. For
2-D axisymmetric systems, the ANSYS program automatically interprets the specified Z-axis rotation as actually
acting about the correct axis of symmetry (that is, about either the X or Y axis). For 3-D Cartesian geometries, the
rotational axis need not be in the same direction as one of the principal axes of the global coordinate system,
and may be offset from the origin of the global coordinate system.

To specify offsets for the axis of rotation, use one of the following:

Command(s): CGLOC
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Flow Environment> Rotating Coords
Main Menu> Solution> FLOTRAN Set Up> Flow Environment> Rotating Coords

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

10–2

Chapter 10: FLOTRAN Special Features

Figure 10.2 Rotating Flow Problem

Figure 10.3 Problem Schematic with Rotating Coordinate

10.3. Swirl

Swirl applies only to axisymmetric problems and refers to motion perpendicular to the X-Y plane. To activate
swirl, choose one of the following:

Section 10.3: Swirl

10–3

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Command(s): FLDATA1,SOLU,SWIRL,TRUE
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Solution Options
Main Menu> Solution> FLOTRAN Set Up> Solution Options

Either a moving wall (for instance, a rotating shaft) or a component of swirl at an inlet can cause the motion in
the swirl direction (with velocity component VZ).

In a swirl problem, there are no changes in the "theta" direction since it is axisymmetric.

The swirl component is calculated through solution of the momentum equation in the swirl direction. With no
pressure gradient in the swirl direction, nothing contributes to the swirl velocity directly from the velocity update
step in the segregated solution algorithm. It is thus sometimes useful to accelerate the convergence of swirl
problems by solving the momentum in the swirl direction equation with a relaxation factor of 1.0 for a few
global iterations.

10.4. Distributed Resistance/Source

Distributed resistances are macroscopic representations of geometric features not directly concerned with the
region of interest and considered too detailed for exact representation. A typical example is pipe flow which
encounters a screen.

You apply distributed resistance on an element basis through the use of real constants. See the ANSYS Elements
Reference for the formulation and the list and meaning of the real constants.

Since the distributed resistance parameters will describe the known behavior of the flow in the region, the use
of the turbulence model is redundant. You should deactivate it in the distributed resistance region by setting
ENKE to 0.0 and ENDS to 1.0.

To do so, choose one of the following:

Command(s): D
GUI: Main Menu> Preprocessor> Loads> Define Loads> Apply> Fluid/CFD> Turbulence> On Nodes
Main Menu> Solution> Define Loads> Apply> Fluid/CFD> Turbulence> On Nodes

The distributed resistances referred to above are used to describe losses to the system. You can model momentum
sources in similar fashion. Such sources can be used to represent fans or pumps in a system. Typical characteriz-
ation of these components is a "Head-Capacity Curve," representing the pressure rise as a function of flow for a
constant speed pump. The fan or pump model is not intended to describe the details of the flow in the pump
region, but rather to approximate its effects on the rest of the system. You can use any coordinate system or
FLOTRAN element shape, but Cartesian coordinate systems with hex shaped elements in three dimensions and
quadrilateral elements in two dimensions tend to give more stable results.

The fan model input takes the form of element real constants, and is described in detail in the ANSYS Elements
Reference.

The ANSYS program supports two types of fan model. A "Type Four" fan model acts only along a specific coordinate
direction, while a "Type Five" model enables the user to align the fan or pump in an arbitrary direction. Coefficients
are assigned for each coordinate direction.

The equation for the fan model is in terms of a pressure gradient applied in the direction of flow. You therefore
must know over what length the fan model is to be applied in order to achieve the correct total pressure rise.
The relationship defining the momentum source for an arbitrary direction "s" is as follows:

C V

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

10–4

Chapter 10: FLOTRAN Special Features

In the above equation, V is the velocity through the fan. If the given data is in terms of volumetric flow, you must
know the area of the actual pump. The actual velocity at the outlet of the pump as well as the volumetric flow
rate should be preserved. Consistent units must be used, that is, the gravitational conversion constant must be
1.0. If, for example, the pressure drop is in psi, the velocity units are in/sec.

Generally, you determine the fan or pump coefficients by taking three pairs of pressure-velocity points on the
"fan curve" and solving for the coefficients. If the flow is to be in the negative direction, the signs of all the coef-
ficients change.

The type 5 model is used for pumps not aligned with one of the coordinate directions. Given V as the velocity
in the S arbitrary direction and the pump constants C

, C

, and C

; the directional coefficients can be calculated.

is the angle between the arbitrary direction S and the x coordinate direction, the directional constants are:

cos

Similarly, if

and

are defined as the angles between the fan direction and the y and z coordinate direction

respectively:

cos

Section 10.4: Distributed Resistance/Source

10–5

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

10–6

Chapter 11: FLOTRAN CFD Solvers and the
Matrix Equation

11.1. Which Solver Should You Use?

In the sequential solution algorithm, you have three options for solving equations sets for degrees of freedom:

A fast, approximate solver

This solver, the Tri-Diagonal Matrix Algorithm (TDMA), performs a user-specified number of iterations
through the problem domain.

"Exact" solvers

The "exact" methods are semi-direct conjugate direction methods that iterate to a specified convergence
criterion.

These methods are:

•

The Conjugate Residual (CR), Preconditioned Conjugate Residual (PCCR), Preconditioned Generalized
Minimum Residual (PGMR), and Preconditioned BiCGStab (PBCGM) methods for non-symmetric
matrix equations.

•

The preconditioned conjugate gradient method for the incompressible pressure equation.

Sparse Direct solver

This solver uses Gaussian elimination to factorize the matrix and then uses backward/forward substitution
to solve for the unknowns.

You choose the method for each DOF via one of the following:

Command(s): FLDATA18,METH,

Label

Value

(

Label

= DOF)

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> CFD Solver Controls> PRES Solver CFD
Main Menu> Solution> FLOTRAN Set Up> CFD Solver Controls> PRES Solver CFD

Valid choices are: 1 (TDMA), 2 (conjugate residual), 3 (preconditioned conjugate residual or gradient), 4 (precon-
ditioned generalized minimum residual), 5 (sparse direct), or 6 (preconditioned BiCGStab). A choice of 0 indicates
that the equation set is not to be solved. The preconditioned conjugate gradient method automatically applies
to the incompressible pressure equation for choices 2 or 3.

The default solver (TDMA) for the velocities and the turbulence equations is adequate for virtually every problem
encountered. The number of sweeps (iterations) for the velocity is 1. Do not change this value. Experience has
shown that the default number of 10 sweeps for the turbulence equations is most efficient although you can
increase this number to see if better convergence is attained for a particular application.

In general, the solution of the pressure equation must be accurate and conjugate direction methods are used.
However, the TDMA method can be successful for natural convection flows. The sections for the various types
of analyses discuss where to use solvers other than the default choices.

11.2. Tri-Diagonal Matrix Algorithm

You set the number of sweeps for the TDMA solver using one of the following:

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

Command(s): FLDATA19,TDMA,

Label

Value

(

Label

= DOF)

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> CFD Solver Controls>

desired DOF solver

Main Menu> Solution> FLOTRAN Set Up> CFD Solver Controls>

desired DOF solver

In the GUI, you do not have access to this command unless the TDMA method has been requested for that DOF.
It is not available in the GUI at all for velocities.

11.3. Semi-Direct Solvers

You can gauge the performance of the semi-direct solvers by the behavior during the solution process of the
inner product of the residuals, referred to as RTR (or ZTR for the incompressible pressure equation.) RTR should
be reduced during the global iteration to a fraction, typically 1.0 x 10

-7

of its initial value.

The fraction is the convergence criterion for the semi-direct methods, set with one of the following:

Command(s): FLDATA21,CONV,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> CFD Solver Controls>

desired DOF solver

Main Menu> Solution> FLOTRAN Set Up> CFD Solver Controls>

desired DOF solver

To set the maximum number of iterations allowed during a global iteration, choose one of the following:

Command(s): FLDATA22,MAXI,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> CFD Solver Controls>

desired DOF solver

Main Menu> Solution> FLOTRAN Set Up> CFD Solver Controls>

desired DOF solver

Data concerning how the semi-direct solvers are performing appears in the text file Jobname.DBG for every
DOF for which they are used, generally PRES, TEMP, or both.

The semi-direct algorithms may conclude in three different ways: convergence is achieved, the maximum number
of iterations has been reached without convergence, or the solution has stalled.

If the maximum number has been reached without convergence, more iterations may be required (for example,
in a large or ill-conditioned problem). If so, increase the maximum number of iterations. The maximum number
also may be reached if the convergence criterion has been set to a very small value (for example, less than 1.0 x
10

-15

), in which case the convergence criterion should be eased. It may also, however, mean that the solution is

diverging. If so, large values of RTR or ZTR (perhaps above 1.0 x 10

) will appear in the debug file; but increasing

the number of iterations will not help.

Stall occurs when the new iteration makes no progress towards the solution but the convergence criterion has
not been achieved. If the rate of change is small enough the solution process stops.

Note — You specify the rate of change which leads to termination of the solver by using one of the fol-
lowing:

Command(s): FLDATA23,DELT,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> CFD Solver Controls>

desired DOF solver

Main Menu> Solution> FLOTRAN Set Up> CFD Solver Controls>

desired DOF solver

The label refers to the DOF being solved. Stall can occur in the solution of the compressible pressure equation
or in the solution of the temperature equation of some conjugate heat transfer problems. The value of RTR does
not decrease significantly and at the last iteration the value of DelMax is less than the value you specified. This
means that the solution is essentially not changing, and further computational effort is wasted.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

11–2

Chapter 11: FLOTRAN CFD Solvers and the Matrix Equation

You can resolve a stall situation by increasing the number of search directions or using inertial relaxation. To in-
crease search directions, either use one of the menu paths described above (with the FLDATA23,DELT command),
or issue the following command:

Command(s):

FLDATA20,SRCH,

Label

Value

The default value is 2, appropriate for well conditioned problems. The number of search directions required may
vary widely among problems. Values of 20 may be required, but be aware that each search direction specified
requires

compute storage locations in memory. (

is the number of finite element nodes in the problem). The

computer storage required for large values of SRCH could exceed the computational resources available, in
which case inertial relaxation should be used.

Figure 11.1: “Typical Debug Files” shows typical debug files.

Figure 11.1 Typical Debug Files

11.3.1. Preconditioned Generalized Minimum Residual (PGMR) Solver

The PGMR method uses fill-in when constructing the L and U decomposition matrices. The PGMR method is a
version of the generalized minimum residual method that uses an LU preconditioning to transform the system
of equations into a set easier to solve. As with the PCCR method, the coefficient matrix is decomposed into an
approximate LU product. In the PCCR method, the sparsity pattern of the original matrix is preserved in the L
and U matrices.

Accordingly, when you are using the Preconditioned Generalized Minimum Residual (PGMR) solver, you need
to specify the amount of fill-in. You must also specify the number of search vectors.

The fill-in value represents the number of extra elements allowed in each row of the L and U decomposition
matrices. An extra element is defined as being in addition to the number of nonzero elements in the row of the
original matrix.

There are two PGMR algorithms available for FLOTRAN. The choice is automatically made by the program. The
difference lies in the "fill-in". It is only required and only available for the PRES and TEMP degrees of freedom.

Section 11.3: Semi-Direct Solvers

11–3

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

To specify the amount of fill-in, use either of these methods:

Command(s): FLDATA20A,PGMR,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> CFD Solver Controls>

desired DOF solver

Main Menu> Solution> FLOTRAN Set Up> CFD Solver Controls>

desired DOF solver

The allowable range for fill-in is 1 to 10. The default value is 6. A single fill-in value is input for all applicable DOF.

For some problems, it is unnecessary to obtain an exact solution to the energy equation every global iteration.
To save some time, you can then employ the foregoing command with a Label of MODP. You use it to specify a
number of global iterations performed using the TDMA method between global iterations performed using the
PGMR method for the temperature DOF.

The number of search directions required may vary widely among problems. If large values of SRCH result in the
required computer storage exceeding the computational resources, inertial relaxation should be used. To specify
the number of search vectors, use either of these methods:

Command(s): FLDATA20,SRCH,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> CFD Solver Controls>

desired DOF solver

Main Menu> Solution> FLOTRAN Set Up> CFD Solver Controls>

desired DOF solver

For the PGMR solver, the allowable range of search vectors is 12 to 20. The default value is 12.

The PGMR method is not recommended for velocity DOF.

The output associated with the solver is recorded in the Jobname.OUT file for non-FLOTRAN analyses. The
FLOTRAN iterative solver output is recorded in the jobname.dbg file.

The fact that the PGMR solver is being used is indicated in the Jobname.DBG file. The file shows if convergence
is reached, the maximum number of iterations is reached without convergence, or the solution is stalled.

The PGMR method output is in the same form as that provided in the jobname.out file for non-FLOTRAN analyses.
The NORM referred to in the Jobname.OUT file is the square root of the convergence criterion specified in the
FLOTRAN input. For example, a EQSLV command solver tolerance value of 1.E-5 corresponds to the FLOTRAN
default convergence criterion value of 1.E-10.

The PGMR method can fail for the following reasons:

•

The problem is ill-conditioned.

•

The problem is improperly formulated.

•

The specified convergence criterion is too tight.

•

An insufficient number of iterations is specified.

If the PGMR method stalls, it may be because the problem is ill-conditioned or improperly formulated. If the
problem is ill-conditioned, you can control several parameters to enhance performance. You can increase the
amount of fill-in or the number of search vectors. You can also use inertial relaxation. If the problem is improperly
formulated, there may be an input error or the boundary conditions may be applied incorrectly. You need to
check the input parameters and boundary conditions to ensure that they are accurate.

FLOTRAN does not allow a convergence criterion less restrictive than the default value. You can enter a higher
value, but FLOTRAN issues a warning message and changes it to the default value.

If the maximum number of iterations has been reached without convergence, it may mean more iterations are
required. This could be the case if you see that the Norm has been lowered, but it is not quite to the target. If so,
you can try increasing the maximum number of iterations.

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

11–4

Chapter 11: FLOTRAN CFD Solvers and the Matrix Equation

If the PGMR method converges and the results are questionable, reduce the convergence criterion below the
default value of 1.E-10. A convergence criterion as low as 1.E-20 may be necessary for some problems.

11.3.2. Preconditioned BiCGStab (PBCGM) Solver

The PBCGM method is a version of the generalized bi-conjugate gradient method that uses two sets of vectors
constructed from both the coefficient matrix and its real transpose matrix by making them orthogonal to each
other. At each iteration, a new vector is first generated orthogonal to some user-specified number of previous
vectors (search directions) from the basis of the real transpose matrix. A minimization procedure is then used to
stabilize the numerical procedure. Similar to PGMR, the PBCGM method uses fill-in when constructing the L and
U decomposition matrices. This preconditioning procedure transforms the system of equations into a set easier
to solve by decomposing the coefficient into an approximate LU product.

Accordingly, when you are using the Preconditioned BiCGStab (PBCGM) solver, you need to specify the amount
of fill-in. You must also specify the number of search vectors.

There are two PBCGM algorithms available for FLOTRAN. The difference lies in the fill-in value. When it is specified
to be zero, the algorithm is parallelized except the LU preconditioning part. For other fill-in values, the algorithm
is not parallelized at all.

To specify the amount of fill-in, use the following command or menu path:

Command(s): FLDATA20B,PBCGM,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> CFD Solver Controls>

desired DOF solver

Main Menu> Solution> FLOTRAN Set Up> CFD Solver Controls>

desired DOF solver

The allowable range for fill-in is 0 to 10. The default value is 6. A single fill-in value is input for all applicable DOF.

The number of search directions required may vary widely among problems. If large values of SRCH result in the
required computer storage exceeding the computational resources, use inertial relaxation. In practice, you should
usually use a value of 1 or 2 in order to save the memory storage. To specify the number of search vectors, use
the following command or menu path:

Command(s): FLDATA20,SRCH,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> CFD Solver Controls>

desired DOF solver

Main Menu> Solution> FLOTRAN Set Up> CFD Solver Controls>

desired DOF solver

For the PBCGM solver, the allowable range of search vectors is 1 to 8. The default value is 2.

11.4. Sparse Direct Method

The Sparse Direct method is memory intensive and you should only use it if all other methods have failed. This
method produces intermediate files during matrix factorization and it is difficult to predict the memory required.
Ensure enough hard disk space exists for intermediate files.

If you choose the Sparse Direct method for the VX, VY, or VZ DOFs, FLOTRAN will reset the method to Precondi-
tioned Conjugate Residual (PCCR). The Sparse Direct method is not suitable for the velocity degrees of freedom.

Section 11.4: Sparse Direct Method

11–5

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

11–6

Chapter 12: Coupling Algorithms

12.1. Overview

Chapter 11, “FLOTRAN CFD Solvers and the Matrix Equation” describes the linear solvers available to solve each
individual equation. To obtain a final solution, you must usually account for the coupling between the individual
equations. In FLOTRAN, this nonlinear coupling is handled in a segregated or decoupled manner. The coupling
algorithms belong to a general class referred to as the Semi-Implicit Method for Pressure Linked Equations
(SIMPLE). For more information on this general class of algorithms, see S.V. Patankar, D.B. Spalding, ("A calculation
procedure for heat, mass and momentum transfer in 3-D parabolic flows," International Journal of Heat and Mass
Transfer, Vol 15, pp. 1787-1806, 1972).

To handle the coupling between the pressure and momentum equations, there are two segregated solution al-
gorithms: SIMPLEF and SIMPLEN. For many years, SIMPLEF was the sole pressure-velocity coupling algorithm. It
was developed by R.J. Schnipke and J.G. Rice ("Application of a new finite element method to convection heat
transfer," Fourth International Conference on Numerical Methods in Thermal Problems, Swansea, U.K., July 1985).
The SIMPLEF algorithm has been improved by utilizing some ideas from the SIMPLEC algorithm developed by
J.P. Van Doormaal and G.D. Raithby ("Enhancements of the SIMPLE method for predicting incompressible fluid
flows," Numerical Heat Transfer, Vol. 7, pp. 147-163, 1984). To improve the rate of convergence, the SIMPLEN al-
gorithm has been added to FLOTRAN. It was developed by G. Wang ("A fast and robust variant of the SIMPLE al-
gorithm for finite-element simulations of incompressible flows," Computational Fluid and Solid Mechanics, Vol.
2, pp. 1014-1016, Elsevier, 2001).

SIMPLEF is the default algorithm. To activate the SIMPLEN algorithm, use one of the following:

Command(s): FLDATA37
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Algorithm Control
Main Menu> Solution> FLOTRAN Set Up> Algorithm Control

12.2. Algorithm Settings

In general, FLOTRAN automatically set defaults suited for the two segregated algorithms. However, for some
problems, you may need to reset the advection scheme, solver choice, or relaxation factors.

12.2.1. Advection Scheme

You can discretize the advection term using three approaches: Monotone Streamline Upwind (MSU), Streamline
Upwind/Petrov-Galerkin (SUPG), or Collocated Galerkin (COLG). Refer to Chapter 14, “Advection Discretization
Options” for information on how to select a proper advection scheme.

Refer to the following table for a list of the defaults.

Table 12.1 Advection Scheme Defaults

SIMPLEN Algorithm

SIMPLEF Algorithm

Transport Equation

SUPG

Momentum

MSU

SUPG

Turbulence

MSU

Pressure

SUPG

Energy

SUPG

Species

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

12.2.2. Solver

For the SIMPLEF algorithm, the TDMA solver is the default for the momentum and turbulence equations. None
of the other solvers will improve the overall rate of convergence. Even when exact solutions are obtained on
those individual equations, the overall rate of convergence will not improve. This is due to weak coupling between
the pressure and momentum equations.

For the SIMPLEN algorithm, the overall rate of convergence can be improved considerably when more exact
solutions are obtained for each individual equation. Therefore, when SIMPLEN is activated, FLOTRAN automatically
resets the solver option to the preconditioned BiCGStab method (PBCGM) for the momentum, turbulence and
energy equations. Furthermore, it will reset the fill-in parameter for PBCGM to zero for computational efficiency.

12.2.3. Relaxation Factors

Due to the nonlinear coupling between equations, in order to stabilize the overall solution procedure, relaxation
is usually necessary to moderate changes from one global iteration to the next. Experience indicates that relax-
ation factors greater than 0.5 for the velocity and pressure degrees of freedom will generally cause instability
and divergence for the SIMPLEF algorithm. On the other hand, the SIMPLEN algorithm provides more consistent
coupling between the pressure and velocity degrees of freedom. For incompressible flow problems, SIMPLEN
removes the need for relaxation for the pressure equation and allows a relaxation factor close to 1.0 for the mo-
mentum equations. For compressible flow problems, relaxation is usually needed for the pressure equation in
order to obtain a convergent solution. The default for SIMPLEF is 0.5 for the pressure and velocity degrees of
freedom. When SIMPLEN is activated, FLOTRAN automatically resets the relaxation factor to 1.0 for the incom-
pressible pressure equation, 0.5 for the compressible pressure equation, and 0.8 for the momentum equations.

12.3. Performance

Table 12.2: “SIMPLEF and SIMPLEN Performance Results” presents results for laminar flow in a 2-D square cavity.
The Reynolds number is 100 based on the length of the cavity side and the velocity at the top. The uniform grid
consists of 32

= 1024 elements.

Table 12.2 SIMPLEF and SIMPLEN Performance Results

SIMPLEN

SIMPLEF

0.99

0.98

0.95

0.9

0.8

0.5

RELX

176

114

153

325

Iter. No.

8.9

5.7

3.3

4.0

7.2

12.9

CPU (sec)

For the SIMPLEN algorithm , the total number of global iterations and the computational time decrease as the
relaxation factor (RELX) increases from 0.8 to 0.95. As RELX increases above 0.95, the iteration number and
computational time increase. The optimal RELX value is 0.95. At this value, the SIMPLEN convergence rate is
about 4 times faster than SIMPLEF. The SIMPLEN computational time is about 1/4 of the SIMPLEF computational
time.

Results for a finer mesh of 128

= 16,384 elements show an even better SIMPLEN performance. At an optimal

RELX value of 0.99, the SIMPLEN computational time is about 1/40 of the SIMPLEF computational time.

SIMPLEN significantly improves the rate of convergence if pressure-velocity coupling dominates the convergence.
If other factors affect the overall rate of convergence, SIMPLEN will not increase the rate of convergence as sig-
nificantly. However, for those problems, SIMPLEN will generally be more robust than SIMPLEF, and it will usually
give a better convergence behavior. For more comparisons, see Wang G., "A fast and robust variant of the SIMPLE

ANSYS Fluids Analysis Guide . ANSYS Release 9.0 . 002114 . © SAS IP, Inc.

12–2

Chapter 12: Coupling Algorithms

algorithm for finite-element simulations of incompressible flows," Computational Fluid and Solid Mechanics,
vol. 2, pp. 1014-1016, Elsevier, 2001.

Below is the command input listing used to perform this analysis. All text preceded by an exclamation point (!)
is a comment.

/title, Lid driven cavity flow analysis using SIMPLEF/SIMPLEN algorithms

NDL = 32 ! Number of line divisions

MU = 0.010 ! Fluid viscosity

RHO = 1.0

L = 1.0

sL = 1.0e-8

Vel = 1.000

niter = 10000

/PREP7

et,1,141 ! 2-D XY system

esha,2 ! Quad elements

rect,,L,,L

lesi,all,,,NDL

amesh,1

alls

! Apply Boundary Conditions

nsel,s,ext ! Wall boundary conditions

d,all,vx

d,all,vy

nsel,r,loc,y,L-sL,L+sL !top

d,all,vx,vel

d,all,vy

d,all,enke,-1

alls

d,1,PRES

fini

save

/SOLU ! SIMPLEF algorithm

flda,iter,exec,niter ! No. of global iterations

flda,nomi,visc,MU

flda,nomi,dens,RHO

flda,term,pres,1.e-6

solve

fini

/delete,,rfl

/SOLU ! SIMPLEN algorithm

flda,algr,segr,simplen

solve

fini

/delete,,rfl

/SOLU

flda,relx,vx,0.9

flda,relx,vy,0.9

solve

fini

/delete,,rfl

/SOLU

flda,relx,vx,0.95

flda,relx,vy,0.95

solve

fini

/delete,,rfl

/SOLU

flda,relx,vx,0.98

flda,relx,vy,0.98

solve

fini

/delete,,rfl

Section 12.3: Performance

12–3

/SOLU

flda,relx,vx,0.99

flda,relx,vy,0.99

solve

fini

12–4

Chapter 12: Coupling Algorithms

Chapter 13: Multiple Species Transport

13.1. Overview of Multiple Species Transport

The multiple species transport capability enables you to track several different fluids at once, subject to the
limitation that a single momentum equation is solved for the flow field. Transport equations are solved for each
species. The properties used in the momentum equation can be those of a "main" fluid, a "bulk" fluid (dilute
mixture analysis), or a combination of component fluids. Momentum effects such as advection and diffusion
cause the fluid transport.

The following restrictions apply to this type of analysis:

•

Currently, no reactions are modeled among the species.

•

Solid model boundary /initial conditions are not supported for species mass fractions.

•

Also, you must postprocess multiple species results by issuing commands instead of via the GUI.

13.2. Mixture Types

In terms of property variations, the strategies for solving multiple species problems parallel those for thermal
problems. The key issue is determining how large a mass fraction of the overall flow field the species to be traced
represents. You can choose among three mixture types for analysis: dilute mixture, composite mixture, and
composite gas. For each mixture type, the properties may be a function of temperature.

13.2.1. Dilute Mixture Analysis

In a dilute mixture analysis, small mass fractions of species fluids are tracked in a flow field, and the species
properties do not significantly influence the flow field. The fluid properties are set and the bulk fluid analysis
proceeds as in any other FLOTRAN analysis. You solve the transport equations for species using the bulk density
and the velocities from the bulk fluid analysis.

If the analysis problem is isothermal or the properties are assumed not to vary with temperature, you can converge
the flow field completely before the species transport option is activated. The number of species to be solved is
a feature of the element and is controlled via a key option on the element. The appropriate KEYOPT setting must
be defined during the PREP7 phase of the analysis. Once the element type and number of species has been set,
the multiple species input commands (e.g., MSSPEC) can be issued from either PREP7 or SOLUTION phases.
However, the multiple species menus are accessible only from PREP7.

To activate multiple species transport, use one of the following:

Command(s): FLDATA1,SOLU,SPEC,T
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Solution Options
Main Menu> Solution> FLOTRAN Set Up> Solution Options

13.2.2. Composite Mixture Analysis

A composite mixture analysis calculates the properties used in the solution from a linear combination of the
species, weighted by mass fraction as a function of space. The solution of the momentum equation depends on
the species distribution, so the momentum and transport equations are strongly coupled.

You initialize the species mass fractions using either the MSNOMF command (which has no GUI menu equivalent)
or (typically for a transient analysis) one of the following:

Command(s): IC,

Label

Value

GUI: Main Menu> Preprocessor> Loads> Analysis Type> Analysis Options
Main Menu> Solution> Define Loads> Apply> Initial Condit'n> Define

The mass fractions specified must add up to 1.0. To activate the composite mixture option for an individual
property, use one of the following:

Command(s): FLDATA7,PROT,

Label

,CMIX

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Fluid Properties
Main Menu> Solution> FLOTRAN Set Up> Fluid Properties

13.2.3. Composite Gas Analysis

In a composite gas analysis, at each node the fluid density is calculated as a function of the mass fractions and
molecular weights of the gases:

ρ =

∑

In the equation above:

•

R is the Universal Gas constant. You can set it using one of the following:

Command(s): MSDATA
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Multiple Species

•

is the molecular weight of the ith species. You set this weight using one of the following:

Command(s): MSSPEC
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Multiple Species

•

N is the total number of species defined.

•

P is pressure degree of freedom (PRES).

•

T is the absolute temperature (TEMP).

To invoke the composite gas option for the bulk fluid, use one of the following:

Command(s): FLDATA7,PROT,DENS,CGAS
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Fluid Properties
Main Menu> Solution> FLOTRAN Set Up> Fluid Properties

13.3. Doing a Multiple Species Analysis

The procedure for a multiple species analysis has six steps:

Establish the number of species to model and assign species names.

Designate an algebraic species.

Adjust output format if desired.

Set properties.

Specify boundary conditions and nominal mass fractions.

Set relaxation and solution parameters for the solution of the transport equations (if necessary).

13.3.1. Establish the Species

To set the number of species, use one of these methods:

13–2

Chapter 13: Multiple Species Transport

Command(s): KEYOPT,1,1,

(

= number of species (at least 2, but no more than 6))

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Multiple Species

To name each species, use the menu paths shown above or the following command:

Command(s):

MSSPEC

FLOTRAN uses these names for assigning boundary conditions and in postprocessing listings and plots. The
default names for species are SP01, SP02, and so on.

13.3.2. Choose an Algebraic Species

The transport equations solve for the mass fractions of each species. You must choose one as the algebraic species,
using the value set by the ALGEB argument or one of the following:

Command(s): MSDATA
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Multiple Species

The transport equation for the algebraic species is not solved, but its concentration as a function of space is
calculated by ensuring that the mass fractions of all the species add up to 1.0 everywhere.

Note — The MSDATA command also sets the universal gas constant. Every issuance of the command
sets both numbers.

13.3.3. Adjust Output Format

You can set the format of the convergence monitors on the file Jobname.PFL to list columns of values for all
the degrees of freedom for a single iteration. (This also affects the ANSYS output file.) To adjust output, use one
of the following:

Command(s): FLDATA6
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Additional Out> Print Controls
Main Menu> Solution> FLOTRAN Set Up> Additional Out> Print Controls

13.3.4. Set Properties

For a dilute mixture analysis, set the bulk property type as appropriate (CONSTANT, Liquid, etc.).

If the bulk properties are to be a linear combination of the species properties, set the bulk property type to CMIX.
For example, you would use the following command:

Command(s):

FLDATA7,PROT,

Label

Type

In the preceding command,

Label

can be DENS, VISC, COND, or SPHT, and

Type

is CMIX. If

Label

= DENSE,

Type

may be CGAS. Using CGAS requires you to enter a molecular weight for the gas via the MSSPEC command or its
equivalent GUI path.

You handle individual species property variations the same way, and with the same options as, the bulk fluid.
The CONSTANT, LIQUID, and GAS fluid types are available. Specify them, along with coefficients, using one of
the following:

Command(s): MSPROP
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Multiple Species

Section 13.3: Doing a Multiple Species Analysis

13–3

For all analyses, you must enter the mass diffusion coefficient data for each species. For a dilute mixture, the
density is the only other relevant property because the bulk or main fluid properties govern the solution of the
momentum equation. For the CMIX and CGAS options, you need to specify density and viscosity using MSPROP
or an equivalent menu path. Also specify conductivity if the energy equation is to be solved.

The form of the diffusion term is:

∇⋅

∇

(

)

The value D

is the diffusion coefficient, and Y

is the mass fraction being solved.

Sometimes, the available data is expressed as a Schmidt number. The following equality enables expression of
the diffusion portion of transport in terms of laminar viscosity µ, the density

ρ, and the Schmidt number:

∇ =

∇

Note — The input must be in terms of the mass diffusion coefficient, not the Schmidt number. The Schmidt
number relating the diffusion coefficient to the density and viscosity differs from the turbulent Schmidt
number discussed below.

In addition, the flow field may be turbulent. Another representation of the diffusion term, this time including
the effect of the turbulent viscosity µ, is:

∇⋅









∇

The quantity SC

is the turbulent Schmidt number, which you specify via one of the following:

Command(s): MSSPEC
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Multiple Species

The normal default value of 1.0 is sufficient unless you want to regulate explicitly the effect of turbulence on the
transport.

13.3.5. Specify Boundary Conditions

The default boundary condition is zero gradient of the mass fraction at the boundaries. You can specify the mass
fraction at a boundary, such as the inlet, by entering the species name in the

LAB

field of one of the following:

Command(s): D
GUI: Main Menu> Preprocessor> Loads> Define Loads> Apply> Fluid/CFD> Displacement> On
Nodes
Main Menu> Solution> Define Loads> Apply> Fluid/CFD> Displacement> On Nodes

Initialize the mass fractions for every species, including the algebraic species. The fractions must sum to 1.0.

13.3.6. Set Relaxation and Solution Parameters

Relaxation factors for the property calculations and the mass fraction update default to 0.5. To change the factors,
use one of the following:

Command(s): MSRELAX
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Multiple Species

You can set modified inertial relaxation factors for multiple species. To do so, use one of the following:

Command(s): MSMIR,

SPNUM

Value

13–4

Chapter 13: Multiple Species Transport

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Multiple Species

A larger modified inertial relaxation factor gives a more robust scheme, but it may yield a slower convergence.
The recommended range is 0.1 to 1.0.

You can change parameters for the algebraic solvers for the transport equation and choose a solver by using
one of the following commands or menu paths:

Command(s): MSSOLU, MSMETH
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Multiple Species

Activating mass fraction capping is recommended to prevent intermediate calculations from producing unreal-
istic results. Use either of the following for each species:

Command(s): MSCAP
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Multiple Species

Finally, you activate the multiple species option using one of the following:

Command(s): FLDATA1,SOLU,

Spec

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Solution Options
Main Menu> Preprocessor> FLOTRAN Set Up> Solution Options

13.4. Doing a Heat Exchanger Analysis Using Two Species

Although FLOTRAN permits only one fluid region to correspond to material number 1 (using the command
MAT,1 or an equivalent GUI path), you can simulate multiple fluids within this restriction. To do so, you set all
fluid property types to CMIX, then set the appropriate species mass fraction to 1.0 in a particular region. These
settings enable all properties in that region to correspond to that of species with mass fraction 1.0. For such
multiple fluid simulations, the mass fractions must remain constant throughout the analysis; that is, the analysis
should not turn on the species solution.

A typical heat exchanger analysis consists of two fluids flowing in opposite directions, separated by a wall as
shown in Figure 13.1: “Environment for a Typical Heat Exchanger Analysis”:

Figure 13.1 Environment for a Typical Heat Exchanger Analysis

The sample command stream that follows shows you how to set up the model shown in Figure 13.1: “Environment
for a Typical Heat Exchanger Analysis”, apply boundary conditions, set up appropriate properties, etc. It is important

Section 13.4: Doing a Heat Exchanger Analysis Using Two Species

13–5

to note that, although two species are defined, the species transport has not been activated. In addition, all fluid
properties must be declared variable so that the initial value (the same in regions 1 and 2) is reset based on the
mass fraction.

/BATCH,LIST

/tit,heat exchanger problem

!two different fluids separated by a solid wall

!cartesian geometry, pressure-driven flow

!solve by 2 species

LX = 10 ! Length in X direction

NDX = 10 ! Number of X divisions

LY1 = 2 ! fluid 1 width

LY2 = 0.1 ! solid width

LY3 = 1.0 ! fluid 2 width

NDY1 = 10

NDY2 = 3

NDY3 = 10

YOFFSET = 0 !offset from X-axis

/prep7 $smrt,off

et,1,141 ! 2-D XY system

!species

keyopt,1,1,2 ! 2 species

!axisymm

!keyopt,1,3,2 !use for axisymm RY system only

esha,2 !Quad elements

rect,,LX,YOFFSET,YOFFSET+LY1 !fluid 1 area

rect,,LX,YOFFSET+LY1,YOFFSET+LY1+LY2 !solid area

rect,,LX,YOFFSET+LY1+LY2,YOFFSET+LY1+LY2+LY3` !fluid 2 area

nummrg,all

numcmp,all

lsel,s,,,3,9,3

lsel,a,,,1

lesi,all,,,NDX,

lsel,s,,,2,4,2

lesi,all,,,NDY1,-5.0

lsel,s,,,5,7,2

lesi,all,,,NDY2,-5.0

lsel,s,,,8,10,2

lesi,all,,,NDY3,-5.0

allsel

mat,1 !for fluids material must be 1

amesh,1 !mesh fluid 1 region

amesh,3 !mesh fluid 2 region

mat,2 !for solid set material to 2

amesh,2 !mesh solid region

!inner region 1

!bc inlet

lsel,s,,,4

nsll,s,1

d,all,pres,10 !inlet pressure & temp specified for fluid 1

d,all,temp,100

!bc outlet

lsel,s,,,2

nsll,s,1

d,all,pres,0. !outlet pressure specified for fluid 1

!symm

lsel,s,,,1

nsll,s,1

d,all,vy,0 !symmetry surface for fluid 1 only

!region 2

!bc inlet

lsel,s,,,8

nsll,s,1

d,all,pres,10. !inlet pressure & temp specified for fluid 2

d,all,temp,400

!bc outlet

lsel,s,,,10

nsll,s,1

d,all,pres,0. !outlet pressure specified for fluid 2

!top wall

13–6

Chapter 13: Multiple Species Transport

lsel,s,,,9

nsll,s,1

d,all,vx,0 !wall boundary conditions

d,all,vy,0

allsel

!solid properties

mp,dens,2,5. !specify solid region 3 properties

mp,kxx,2,100

mp,c,2,13

/SOLU

!ic for species

nsel,s,loc,x,,lx !select nodes for fluid 1

nsel,s,loc,y,o,ly1

ic,all,sp01,1.0 !set mass fraction for fluid 1

ic,all,sp02,0.0

nsel,s,loc,x,,lx

nsel,s,loc,y,ly1+ly2,ly1+ly2+ly3 !select nodes for fluid 2

ic,all,sp01,0.0 !set mass fraction for fluid 2

ic,all,sp02,1.0

allsel

FLDA,ITER,EXEC,200

FLDA,PROT,DENS,CMIX ! Fluid density

FLDA,PROT,VISC,CMIX ! Fluid viscosity

FLDA,PROT,COND,CMIX ! Fluid conductivity

FLDA,PROT,SPHT,CMIX ! Fluid specific heat

flda,vary,dens,t !all properties MUST be variable

flda,vary,visc,t

flda,vary,cond,t

flda,vary,spht,t

FLDA,NOMI,DENS,1.0 ! initial density for all fluid region

FLDA,NOMI,VISC,2.0 ! initial viscosity for all fluid region

FLDA,NOMI,COND,3.0 ! initial conductivity for all fluid region

FLDA,NOMI,SPHT,4.0 ! initial specific heat for all fluid region

msprop,1,spht,constant,1 !sp heat for fluid 1

msprop,2,spht,constant,2 !sp heat for fluid 2

msprop,1,dens,constant,1 !density for fluid 1

msprop,2,dens,constant,2 !density for fluid 2

msprop,1,visc,constant,1.0 !viscosity for fluid 1

msprop,2,visc,constant,2.0 !viscosity for fluid 2

msprop,1,cond,constant,.1 !conductivity for fluid 1

msprop,2,cond,constant,.2 !conductivity for fluid 2

FLDA,CONV,PRES,1.0E-10 ! PCCR convergence criterion

FLDA,TERM,PRES,1.E-09

FLDA,OUTP,SP01,T

FLDA,OUTP,SP02,T

save

SOLVE !solve for flow only

FLDA,SOLU,ENRG,T

FLDA,SOLU,FLOW,F

FLDA,METH,ENRG,3

FLDA,ITER,EXEC,50

FLDA,RELX,TEMP,1.

SOLVE !solve for temperature only

fini

/exit,nosa

13.5. Example Analysis Mixing Three Gases

The following example analysis mixes three gases: oxygen (O

), nitrogen (N

), and hydrogen (H

). The mass

fractions of the gases are set at each inlet along with the velocity. For the three inlets:

Section 13.5: Example Analysis Mixing Three Gases

13–7

Bottom:

Left:

Top:

VX = 0

VY = 0.1

TEMP = 300

= 0.0

=0.0

= 1.0

VX = 0.1

VY = 0

TEMP = 400

= 0.0

= 1.0

= 0.0

VX = 0

VY = -0.1

TEMP = 300

= 1.0

= 0.0

The command stream for the example (shown below) shows all the relevant properties and the solution strategy.

/batch,list

/filename,spec

/com ** Analysis Types Laminar and Turbulent, Incompressible

/com 2-D - quadrilateral and triangular elements

/com ** Features Thermal, Multiple Species Transport

/com ** Options Dilute mixtures, composite property types (CGAS, CMIX)

/com ** Variable laminar properties

/com ** Turbulence

/com ** Construction of geometry

/prep7

!!!!!!! Define some dimensions - SI units are used

lenin=.3

half=lenin/2.

width=.1

hfwid=width/2.

outlen=1.2

!!!!!!! Define inlet and outlet rectangles

rect,-lenin,0,-hfwid,hfwid

rect,.2,.3,.25,.25+lenin

rect,.2,.3,-.25,-.25-lenin

rect,.4,.4+outlen,-.15,.15

!!!!!!! Lines that border the mixing area

l2tan,-3,-8

l2tan,-6,-15

l2tan,-13,-10

l2tan,-12,-1

!!!!!!! Parameters defined for meshing

nlcurv=16

rlcurv=1

nscurv=9

rscurv=1

nispan=8

rispan=-1.5

nospan=13

rospan=-2

nilen=10

rilen=-2

nolen=24

rolen=4

!!!!!!!

!flst,2,2,4,orde,2

!fitem,2,17

!fitem,2,20

lsel,s,,,17,20,3

lesize,all,,,nlcurv,rlcurv

lsel,s,,,18,19

!fitem,2,18

!fitem,2,-19

lesize,19,,,nscurv,rscurv

!flst,2,3,4,orde,3

!fitem,2,2

!fitem,2,5

!fitem,2,11

lsel,s,,,2,5,3

13–8

Chapter 13: Multiple Species Transport

lsel,a,,,11

lesize,all,,,nispan,1

!flst,2,3,4,orde,3

!fitem,2,4

!fitem,2,7

!fitem,2,9

lsel,s,,,4,7,3

lsel,a,,,9

lesize,all,,,nispan,rispan

!flst,2,6,4,orde,6

!fitem,2,1

!fitem,2,3

!fitem,2,6

!fitem,2,8

!fitem,2,10

!fitem,2,12

lsel,s,,,1,3,2

lsel,a,,,6,12,2

lesize,all,,,nilen,rilen

lsel,s,,,13,16

lesize,13,,,nolen,rolen

lesize,15,,,nolen,1./rolen

lesize,16,,,nospan,rospan

lesize,14,,,nospan,rospan

alls

!!!!!!! Define the mixing area...

!flst,2,8,3

!fitem,2,2

!fitem,2,12

!fitem,2,11

!fitem,2,13

!fitem,2,16

!fitem,2,6

!fitem,2,5

!fitem,2,3

a,2,12,11,13,16,6,5,3

alls

/com ** CONSTRUCTION OF THE MESH

!!!!!!! Put triangles in the mixing area (5)

asel,s,,,5

et,1,141

mshape,1,2d

amesh,5

!!!!!!! Put a mapped mesh in the rectangles (quads)

asel,s,,,1,4

mshape,0,2d

mshkey,1

amesh,all

/com ** BOUNDARY CONDITIONS

!!!!!!! Wall boundary conditions

lsel,s,,,1,3,2

lsel,a,,,6,12,2

lsel,a,,,13,17,2

lsel,a,,,18,20

nsll,,1

d,all,vx,0

d,all,vy,0

!!!!!!! Define velocities, temperature at top, bottom, left

vtop=.1

vbot=.1

vlef=.1

lsel,s,,,7

nsll

d,all,vx,0

d,all,vy,-vtop

nsll,,1

d,all,temp,300

lsel,s,,,4

nsll

d,all,vx,vlef

d,all,vy,0

nsll,,1

Section 13.5: Example Analysis Mixing Three Gases

13–9

d,all,temp,400

lsel,s,,,9

nsll

d,all,vx,0

d,all,vy,vbot

nsll,,1

d,all,temp,300

lsel,s,,,14

nsll,,1

d,all,pres,0

flda,conv,iter,5

save

finish

alls

/solu

/com ** FLOTRAN INPUT

flda,iter,exec,40

flda,temp,nomi,300 ! Initial temperature field is 300K

flda,prot,dens,air-si ! Initial solution will be for AIR

flda,vary,dens,true

flda,prot,visc,air-si

flda,vary,visc,true

flda,prot,cond,air-si

flda,vary,cond,true

flda,prot,spht,air-si

save

solve ! Solve 40 iterations with air at 300K

finish ! Prepare for species transport ...

/prep7

flda,prot,dens,cmix ! Composite mixture for density

flda,prot,visc,cmix ! Composite mixture for viscosity

keyopt,1,1,3 ! Specify that there are 3 species

flda,solu,spec,t ! Turn on solution for multiple species transport

msdata,2 ! Specify species 2 (N2) as the algebraic species

!!!!!!! Species Property Input

msspec,1,o2,31.999

msprop,1,DENS,GAS,1.2998,300,1.01325E+5

msvary,1,dens,t

msnomf,1,.3

msprop,1,VISC,CONSTANT,1.2067E-5

msprop,1,mdif,CONSTANT,2.149E-5

msprop,1,cond,CONSTANT,.02674

mscap,1,1

msspec,2,n2,28.018

msprop,2,DENS,GAS,1.1381,300,1.01325E+5

msvary,2,dens,t

msnomf,2,.3

msprop,2,VISC,CONSTANT,1.786E-5

msprop,2,mdif,CONSTANT,1.601E-5

msprop,2,cond,CONSTANT,.02598

mscap,2,1

msspec,3,h2,2.016

msprop,3,DENS,GAS,0.0819,300,1.01325E+5

msvary,3,dens,t

msnomf,3,.4

msprop,3,VISC,CONSTANT,8.94E-6

msprop,3,mdif,CONSTANT,4.964E-5

msprop,3,cond,CONSTANT,.1815

mscap,3,1

msrelx,1,1.0

msrelx,3,1.0

msmeth,1,3

mssolu,1,,,2,1.e-8

msmeth,3,3

mssolu,3,,,2,1.e-8

alls

!!!!!!! Species boundary conditions

13–10

Chapter 13: Multiple Species Transport

lsel,s,,,7

nsll,,1

d,all,o2,1.0

d,all,n2,0.0

d,all,h2,0.0

lsel,s,,,4

nsll,,1

d,all,o2,0.0

d,all,n2,1.0

d,all,h2,0.0

lsel,s,,,9

nsll,,1

d,all,o2,0.0

d,all,n2,0.0

d,all,h2,1.0

alls

!!!!!!! End of species boundary conditions

flda,iter,exec,20 ! Ask for 20 global iterations

flda,conv,outp,land ! Adjust convergence monitor output style

save

finish

/solu

solve ! 20 iterations with species activated

!Prepare for energy solution

flda,solu,temp,t ! Achieve a constant flow temperature solution

flda,solu,flow,f ! Freeze the flow field

flda,meth,temp,3 ! Activate PCCR solver

flda,conv,temp,1.e-10 ! Convergence criterion for PCCR

flda,iter,exec,5 ! Need only a few iterations for solution...

flda,relx,temp,1.0 ! no relaxation on temperature

save

solve

!! Prepare for coupled solution

flda,iter,exec,35 ! Achieve a flow and thermal solution

flda,solu,flow,t

solve

flda,iter,exec,50 ! Run 50 more iterations to refine solution

save

solve

Section 13.5: Example Analysis Mixing Three Gases

13–11

13–12

Chapter 14: Advection Discretization Options

14.1. Introduction

When momentum, energy, species transport, turbulence or the compressible pressure equations are solved, the
advection term plays a significant role in the solution. When the advection term dominates over other terms in
the governing equations, it can lead to numerical instabilities. Accordingly, you must be careful with the discret-
ization of this particular term.

You can discretize the advection term using three approaches: monotone streamline upwind (MSU), streamline
upwind/Petrov-Galerkin (SUPG), or collocated Galerkin (COLG). For the momentum, energy, turbulence or
compressible pressure equations, you specify the approach using one of the following:

Command(s): FLDATA33,ADVM,

Label

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Advection
Main Menu> Solution> FLOTRAN Set Up> Advection

For the species transport equation, you specify the approach using one of the following:

Command(s): MSADV,

SPNUM

MTHA

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Multiple Species
Main Menu> Solution> FLOTRAN Set Up> Multiple Species

MSU tends to be first order accurate while SUPG and COLG are second order accurate. MSU produces diagonally
dominant matrices and is generally quite robust. SUPG and COLG provide less diagonal dominance, but are
generally more accurate. COLG provides an exact energy balance for incompressible flows, even with a coarse
mesh. Special techniques may be required to achieve convergence using SUPG or COLG.

For more information on the approaches, consult the ANSYS, Inc. Theory Reference.

14.2. Using SUPG and COLG

For simple geometries and simple flows, the SUPG or COLG approach provides a convergent solution in a straight
forward fashion.

For laminar flow past obstacles, which generally produce regions of recirculation in the wake, you may need to
turn on modified inertial relaxation in the momentum equation using one of the following:

Command(s): FLDATA34,MIR,MOME,

Value

GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Relax/Stab/Cap> MIR Stabilization
Main Menu> Solution> FLOTRAN Set Up> Relax/Stab/Cap> MIR Stabilization

For turbulent problems, FLOTRAN will sometimes display a message stating that the coefficient matrix has a
negative diagonal and the solution is probably divergent. You should then try turning on modified inertial relax-
ation in the momentum equation or turbulence equation.

Command(s):

FLDATA34,MIR,MOME,

Value

or FLDATA34,MIR,TURB,

Value

The modified inertial relaxation

Value

should be between 0.1 and 1.0. A larger

Value

leads to more relaxation.

To achieve a faster convergence rate, use the smallest

Value

possible.

For complex geometries with turbulence and complex flow fields, you can employ the following techniques to
achieve a convergent solution with SUPG or COLG.

•

Set the turbulence ratio to a high value of 1 x 10

and the effective viscosity relaxation factor to a low value

of 0.1 using the following commands. These conditions provide the necessary diagonal dominance until
the solution enters the radius of convergence.

Command(s): FLDATA24,TURB,RATI,1.0E6
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Turbulence> Turbulence Model
Main Menu> Preprocessor> FLOTRAN Set Up> Turbulence> Turbulence Param
Main Menu> Solution> FLOTRAN Set Up> Turbulence Model
Main Menu> Solution> FLOTRAN Set Up> Turbulence Param
Command(s): FLDATA25,RELX,EVIS,0.1
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Relax/Stab/Cap> Prop Relaxation
Main Menu> Solution> FLOTRAN Set Up> Relax/Stab/Cap> Prop Relaxation

•

Achieve a convergent solution using MSU on all variables. Then, using the following command, perform
a restart employing SUPG or COLG on the momentum variables only. After achieving a convergent solution,
you can perform a restart again employing SUPG or COLG on the turbulence, pressure, temperature and
species variables.

Command(s): FLDATA33,ADVM,MOME,SUPG FLDATA33,ADVM,MOME,COLG
GUI: Main Menu> Preprocessor> FLOTRAN Set Up> Advection
Main Menu> Solution> FLOTRAN Set Up> Advection

•

Although the foregoing techniques might work on a coarse mesh, both may fail on a fine mesh. In this
case, you may have to resort to a transient algorithm which has the necessary diagonal dominance due
to the inertia term.

14.3. Strategies for Difficult Solutions

Although SUPG and COLG are more accurate than MSU, they may lead to spurious oscillations in the solution.
This may lead to nonphysical solutions or convergence difficulties. You may encounter negative temperatures
in the energy equation solution. In this case, you should refine the mesh in that region. You may also encounter
negative turbulence values. Internally, FLOTRAN tries to reset these values to some realistic numbers, but this
may lead to a situation where the solution stalls. In this situation, you should try using MSU on turbulence variables
while retaining SUPG or COLG on momentum variables. The solution to the species transport equation must be
bounded between 0 and 1.0, and oscillations in the SUPG or COLG solution may make this difficult to achieve
even though capping has been turned on. If convergence is not achieved, you should then refine the mesh.

A poor mesh, recirculating regions, or a strong swirl might cause the SUPG technique to have strong oscillations
in an axisymmetric analysis. Temperatures (or species concentrations) could be higher or lower than any applied
boundary conditions. The mesh should be refined or another advection discretization method should be used.

14–2

Chapter 14: Advection Discretization Options

Part II. Acoustics

Chapter 15: Acoustics

15.1. What Is Acoustics?

Acoustics is the study of the generation, propagation, absorption, and reflection of sound pressure waves in a
fluid medium. Applications for acoustics include the following:

•

Sonar - the acoustic counterpart of radar

•

Design of concert halls, where an even distribution of sound pressure is desired

•

Noise minimization in machine shops

•

Noise cancellation in automobiles

•

Underwater acoustics

•

Design of speakers, speaker housings, acoustic filters, mufflers, and many other similar devices.

•

Geophysical exploration

15.1.1. Types of Acoustic Analysis

An acoustic analysis, available in the ANSYS Multiphysics and ANSYS Mechanical programs only, usually involves
modeling the fluid medium and the surrounding structure. Typical quantities of interest are the pressure distri-
bution in the fluid at different frequencies, pressure gradient, particle velocity, the sound pressure level, as well
as, scattering, diffraction, transmission, radiation, attenuation, and dispersion of acoustic waves. A coupled
acoustic analysis takes the fluid-structure interaction into account. An uncoupled acoustic analysis models only the
fluid and ignores any fluid-structure interaction.

The ANSYS program assumes that the fluid is compressible, but allows only relatively small pressure changes
with respect to the mean pressure. Also, the fluid is assumed to be non-flowing and inviscid (that is, viscosity
causes no dissipative effects). Uniform mean density and mean pressure are assumed, with the pressure solution
being the deviation from the mean pressure, not the absolute pressure.

15.2. Solving Acoustics Problems

You can solve many acoustics problems by performing a harmonic response analysis. The analysis calculates the
pressure distribution in the fluid due to a harmonic (sinusoidally varying) load at the fluid-structure interface. By
specifying a frequency range for the load, you can observe the pressure distribution at various frequencies. You
can also perform modal and transient acoustic analyses. (See the ANSYS Structural Analysis Guide for more inform-
ation on these types of analyses.)

The procedure for a harmonic acoustic analysis consists of three main steps:

•

Build the model.

•

Apply boundary conditions and loads and obtain the solution.

•

Review the results.

15.3. Building the Model

In this step, you specify the jobname and analysis title and then use the PREP7 preprocessor to define the element
types, element real constants, material properties, and the model geometry. These tasks, common to most analyses,
are described in the ANSYS Basic Analysis Guide.

15.3.1. Harmonic Acoustic Analysis Guidelines

For a harmonic acoustic analysis, consider the following points:

Element Types - Four ANSYS element types are specifically designed for acoustic analyses: FLUID29 and FLUID30
are used to model the fluid portion of 2-D and 3-D models respectively. FLUID129 and FLUID130, companion
elements to FLUID29 and FLUID30, are used to model an infinite envelope around the FLUID29 and FLUID30
elements. Use these element types to model the fluid portion, and then use a corresponding structural element
(PLANE42, SOLID45, etc.) for the solid. Only FLUID29 and FLUID30 elements can be in contact with structural
elements (either on the inside or outside of the structure); FLUID129 and FLUID130 can contact only the FLUID29
and FLUID30 elements, and not the structural elements directly.

15.3.1.1. FLUID29 and FLUID30

For acoustic elements that are in contact with the solid, be sure to use KEYOPT(2) = 0, the default setting that allows
for fluid-structure interaction. This results in unsymmetric element matrices with UX, UY, UZ, and PRES as the
degrees of freedom. For all other acoustic elements, set KEYOPT(2) = 1, which results in symmetric element
matrices with the PRES degree of freedom. (See Figure 15.1: “Example of a 2-D Acoustic Model (Fluid Within a
Structure)”.) Symmetric matrices require much less storage and computer time, so use them wherever possible.
For more information on fluid-structure interaction, see the ANSYS, Inc. Theory Reference.

Figure 15.1 Example of a 2-D Acoustic Model (Fluid Within a Structure)

15.3.1.2. FLUID129 and FLUID130

These infinite acoustic elements absorb the pressure waves, simulating the outgoing effects of a domain that
extends to infinity beyond the FLUID29 and FLUID30 elements. FLUID129 and FLUID130 provide a second-order
absorbing boundary condition so that an outgoing pressure wave reaching the boundary of the model is absorbed
with minimal reflections back into the fluid domain.

FLUID129 is used to model the boundary of 2-D fluid regions and as such is a line element. FLUID130 is used to
model the boundary of 3-D fluid regions and as such is a plane surface element.

Material Properties - The acoustic elements require density (DENS) and speed of sound (SONC) as material prop-
erties (FLUID129 and FLUID130 require only SONC). If sound absorption at the fluid-structure interface exists,
use the label MU to specify boundary admittance

β (absorption coefficient). Values of β are usually determined

from experimental measurements. For the structural elements, specify the Young's modulus (EX), density (DENS),
and Poisson's ratio (PRXY or NUXY).

Real Constants - When using FLUID129 and FLUID130, the boundary of the underlying finite element mesh must
be circular (2-D and axisymmetric) or spherical (3-D), and the radius of the circular or spherical boundary of the

15–2

Chapter 15: Acoustics

finite domain must be specified as real constant RAD. (See Figure 15.2: “Example of Absorption Element Applic-
ation”.) The center of the circle or sphere is also specified using real constants:

R,3,RAD,X0,Y0!REAL set 3 for FLUID129

R,3,RAD,X0,Y0,Z0!REAL set 3 for FLUID130

If the coordinates (X0, Y0) for the 2-D and axisymmetric cases or (X0, Y0, Z0) for the 3-D case of the center of the
circle or sphere are not specified via real constants, ANSYS assumes the center to be the origin of the global co-
ordinate system.

Figure 15.2 Example of Absorption Element Application

Figure 15.3 Submerged Cylindrical Shell

Section 15.3: Building the Model

15–3

15.4. Meshing the Model

A typical meshing procedure using the 2-D infinite acoustic elements follows. The procedure is the same with
3-D elements. If you have a structural component as well, the structural elements must lie next to the FLUID29
elements, and cannot lie next to the infinite fluid elements (FLUID129).

This process automatically adds the FLUID129 elements on the boundary of the finite domain. Here an annular
structural ring is meshed with PLANE42 structural elements. The layer of fluid elements in touch with PLANE42
elements is modeled using FLUID29 with UX and UY DOFs and with the fluid-structure interface turned on. The
outer layers of fluid are modeled using FLUID29 without the UX and UY DOFs. The radius for placing FLUID129
is 0.31242 (see Section 15.4.2: Step 2: Generate the Infinite Acoustic Elements) with X0 = Y0 = 0. You define the
FLUID129 elements using:

Command(s): ESURF
GUI: Main Menu> Preprocessor> Modeling> Create> Elements> Inf Acoustic

15.4.1. Step 1: Mesh the Interior Fluid Domain

Mesh the interior fluid domain that is bounded by a circular or spherical boundary (PLANE42) with FLUID29
elements.

Figure 15.4 Mesh the Fluid Domain

15.4.2. Step 2: Generate the Infinite Acoustic Elements

Follow these steps:

Select the nodes on the circular or spherical boundary.

Command(s): NSEL
GUI: Utility Menu> Select> Entities

15–4

Chapter 15: Acoustics

Specify FLUID129 as the infinite fluid element type associated with the FLUID29 element.

Command(s): TYPE, REAL
GUI: Main Menu> Preprocessor> Meshing> Mesh Attributes> Default Attribs
Main Menu> Preprocessor> Real Constants> Add/Edit/Delete

The infinite elements perform well for low as well as high frequency excitations. Numerical experiments
have determined that the placement of the absorbing elements at a distance of approximately 0.2

beyond the region occupied by the structure or source of vibration can produce accurate solutions.
Here

λ = c/f is the dominant wavelength of the pressure waves. c is the speed of sound (SONC) in the

fluid and f is the dominant frequency of the pressure wave. For example, in the case of a submerged
circular or spherical shell of diameter D, the radius of the enclosing boundary, RAD, should be at least
(D/2) + 0.2

λ. Also, for acoustic analysis in general, the mesh must be fine enough to resolve the smallest

dominant frequency.

Generate the absorption elements (FLUID129) on the boundary.

Command(s): ESURF
GUI: Main Menu> Preprocessor> Modeling> Create> Elements> Inf Acoustic

Figure 15.5 Add the Absorption Element on the Boundary

15.4.3. Step 3: Specify the Fluid-Structure Interface

Specify the fluid-structure interface:

Select all nodes on the interface.

Command(s): NSEL
GUI: Utility Menu> Select Entities

Select the fluid elements attached to this set of nodes.

Command(s): ESEL
GUI: Utility Menu> Select> Entities

Specify the selected nodes as fluid-structure interface nodes.

Command(s): SF

Section 15.4: Meshing the Model

15–5

GUI: Main Menu> Preprocessor> Loads> Define Loads> Apply> Fluid-Struct Intr> On Nodes

Note — Be sure to reselect all nodes before solving your analysis.

Figure 15.6 Specify Fluid-Structure Interface

15.5. Applying Loads and Obtaining the Solution

In this step, you define the analysis type and options, apply loads, specify load step options, and initiate the finite
element solution. The next few sections explain how to do these tasks.

15.5.1. Step 1: Enter the SOLUTION Processor

Enter the SOLUTION processor by choosing GUI path Main Menu> Solution or by executing the /SOLU command.

15.5.2. Step 2: Define the Analysis Type

Using either the GUI or a set of commands, define the analysis type and analysis options.

To define the analysis type, use one of the following:

Command(s): ANTYPE,HARMIC
GUI: Main Menu> Solution> Analysis Type> New Analysis

You must choose New Analysis because restarts are not valid in a harmonic response analysis. If you need to
apply additional harmonic loads, do a new analysis each time (or use the "partial solution" procedure described
in the ANSYS Basic Analysis Guide).

15.5.3. Step 3: Define Analysis Options

To specify the solution method, use one of the following:

15–6

Chapter 15: Acoustics

Command(s): HROPT
GUI: Main Menu> Solution> Analysis Options

Although full, reduced, or mode superposition methods are options, choose the full method because it alone
can handle unsymmetric matrices.

To define the solution listing format, use one of the following:

Command(s): HROUT
GUI: Main Menu> Solution> Analysis Options

This option determines how ANSYS lists the harmonic degree-of-freedom solution in the printed output (Job-
name.OUT).

To specify the equation solver to be used, use one of the following:

Command(s): EQSLV
GUI: Main Menu> Solution> Analysis Options

You can choose the frontal solver (default), the sparse direct solver (SPARSE), the Jacobi Conjugate Gradient
(JCG) solver, or the Incomplete Cholesky Conjugate Gradient (ICCG) solver. The JCG solver is recommended for
most models.

15.5.4. Step 4: Apply Loads on the Model

A harmonic analysis, by definition, assumes that any applied load varies harmonically (sinusoidally) with time.
To completely specify a harmonic load in an acoustic analysis, two pieces of information are usually required:
the amplitude and the forcing frequency. The amplitude is the maximum value of the load, which you specify using
the commands shown in Table 15.2: “Commands for Applying Loads in Acoustic Analysis”. The forcing frequency
is the frequency of the harmonic load (in cycles/time). You specify it later as a load step option with the HARFRQ
command (Main Menu> Solution> Time/Frequenc> Freq & Substeps). Section 15.5.5: Step 5: Specify Load
Step Options describes this task.

Table 15.1: “Loads Applicable in an Acoustic Analysis” shows all possible loads for a harmonic acoustic analysis
and the commands to define, list, and delete them. Notice that except for inertia loads, you can define loads
either on the solid model (keypoints, lines, and areas) or on the finite element model (nodes and elements). For
a general discussion of solid-model loads versus finite-element loads, see Chapter 2, “Loading” and Chapter 3,
“Solution” in the ANSYS Basic Analysis Guide.

Table 15.1 Loads Applicable in an Acoustic Analysis

GUI Path

Cmd Family

Category

Load Type

Main Menu> Preprocessor> Define Loads>
Apply> Structural> Displacement or Potential
Main Menu> Solution> Define Loads> Apply>
Structural> Displacement

Constraints

Displacement
(UX,UY,UZ),

Pressure (PRES)

Main Menu> Preprocessor> Define Loads>
Apply> Force/Moment
Main Menu> Solution> Define Loads> Apply>
Force/Moment

Forces

Force (FX,FX,FZ),

Moment
(MX,MY,MZ),

Flow loading

Section 15.5: Applying Loads and Obtaining the Solution

15–7

GUI Path

Cmd Family

Category

Load Type

Main Menu> Preprocessor> Define Loads>
Apply>

load type

Main Menu> Solution> Define Loads> Apply>

load type

Surface Loads

Pressure (PRES)

Impedance (IMPD)

Fluid-structure inter-
action flag (FSI)

Main Menu> Preprocessor> Define Loads>
Apply>

load type

Main Menu> Solution> Define Loads> Apply>

load type

ACEL, OMEGA,
DOMEGA, CG-
LOC, CGOMGA,
DCGOMG, IRLF

Inertia Loads

Gravity, Spinning,
etc.

In an analysis, you can apply, remove, operate on, or list loads.

15.5.4.1. Applying Loads Using the GUI

You access all loading operations except List (see below) through a series of cascading menus. From the Solution
menu, you choose the operation (apply, etc.), then the load type (displacement, force, etc.), and then the object
(keypoint, etc.) to which you are applying the load.

For example, to apply a displacement load to a line, follow this GUI path: Main Menu> Solution> Define Loads>
Apply> Displacement> On Lines

To list loads, use this GUI path: Utility Menu> List> Loads>

load type

15.5.4.2. Applying Loads Using Commands

Table 15.2: “Commands for Applying Loads in Acoustic Analysis” lists all the commands you can use to apply
loads in an acoustic analysis.

Table 15.2 Commands for Applying Loads in Acoustic Analysis

Apply Settings

Operate

List

Delete

Apply

Entity

Solid

Model or

Load Type

DTRAN

DKLIST

DKDELE

Keypoints

Solid
Model

Displace-
ment, Pres-
sure

DTRAN

DLLIST

DLDELE

Lines

Solid
Model

DTRAN

DALIST

DADELE

Areas

Solid
Model

DCUM

DSCALE

DLIST

DDELE

Nodes

Finite
Elem

FTRAN

FKLIST

FKDELE

Keypoints

Solid
Model

Force, Mo-
ment

FCUM

FSCALE

FLIST

FDELE

Nodes

Finite
Elem

SFGRAD

SFTRAN

SFLLIST

SFLDELE

SFL

Lines

Solid
Model

Pressure,
Impedance,
Fluid- Struc-
ture Interac-
tion Flag

SFGRAD

SFTRAN

SFALIST

SFADELE

SFA

Areas

Solid
Model

15–8

Chapter 15: Acoustics

SFCUM , SFGRAD

SFSCALE

SFLIST

SFDELE

Nodes

Finite
Elem

SFBEAM, SFCUM,
SFFUN, SFGRAD

SFSCALE

SFELIST

SFEDELE

SFE

Elements

Finite
Elem

Apply Settings

Operate

List

Delete

Apply

Entity

Solid

Model or

Load Type

ACEL, CGLOC,
CGOMGA,
DCGOMG,
OMEGA, DO-
MEGA, IRLF

Inertia

15.5.4.3. Load Types

Displacements (UX, UY, UZ) and pressures (PRES)

These are DOF (degree-of-freedom) constraints. For example, you specify zero displacements at a rigid fluid-
structure interface. You may also specify nonzero displacements, but remember that they are assumed to be
harmonic. You usually specify zero pressures at free fluid boundaries (where the fluid is not enclosed, such as at
an opening).

Forces (FX, FY, FZ) and moments (MX, MY, MZ)

Usually, you specify these loads on the solid portion of the model to "excite" the fluid.

Flow Load

This is a mass flow rate per unit time (for example, kg/sec/sec in SI units). It represents a pulsating mass flow rate
at a node. Specify it using the FLOW force label:

Command(s): F,,FLOW
GUI: Main Menu> Solution> Define Loads> Apply> Structural> Force/Moment> On Nodes

Pressure (PRES)

You can specify surface loads on the solid portion instead of forces and moments.

Impedance (IMPD)

These are not really loads but indicate surfaces that absorb sound. Specify the degree of sound absorption as
the material property MU (boundary admittance or absorption coefficient).

Fluid-structure interaction flag (FSI)

This denotes an interface surface between the fluid and structure part of the model.

For problems with fluid-structure interaction on both sides of a structure (e.g., a submerged plate), mesh the
structure with solid elements to provide two distinct fluid-interaction surfaces. For problems with fluid-structure
interaction on only one side of a structure, mesh the structure with shell or solid elements.

15.5.5. Step 5: Specify Load Step Options

You have the following options for a harmonic acoustic analysis:

Section 15.5: Applying Loads and Obtaining the Solution

15–9

Table 15.3 Load Step Options for a Harmonic Acoustic Analysis

GUI Path

Com-

mand

Option

Dynamics Options

Main Menu> Solution> Load Step Opts> Time/Frequenc> Freq
& Substeps

HARFRQ

Forcing frequency range

General Options

Main Menu> Solution> Load Step Opts> Time/Frequenc> Freq
& Substeps

NSUBST

Number of harmonic solu-
tions

Main Menu> Solution> Load Step Opts> Time/Frequenc> Freq
& Substeps

KBC

Stepped or ramped loads

Output Controls

Main Menu> Solution> Output Ctrls> Solu Printout

OUTPR

Control of printed output

Main Menu> Solution> Output Ctrls> DB/Results File

OUTRES

Database and results file
output

Main Menu> Solution> Output Ctrls> Integration Pt

ERESX

Extrapolation of results

15.5.5.1. Dynamics Options

The only valid option in this category is the forcing frequency range, which must be defined (in cycles/time) for
a harmonic analysis. Within this range, you then specify the number of solutions to be calculated. (See "General
Options.")

15.5.5.2. General Options

You can request any number of harmonic solutions (via the NSUBST command or its equivalent GUI path) to be
calculated. The solutions (or substeps) will be evenly spaced within the previously specified frequency range.
For example, if you specify 10 solutions in the range 30 to 40 Hz, the program will calculate the response at 31,
32, 33, ..., 39, and 40 Hz. No response is calculated at the lower end of the frequency range.

The loads may be stepped or ramped (via KBC or its GUI counterpart). By default, they are ramped; that is, the
load value increases gradually with each substep. By stepping the loads, you maintain the same load value for
all substeps in the frequency range.

15.5.5.3. Output Controls

Use OUTPR or its GUI equivalent if you want to include any results data on the printed output file (Jobname.OUT).
OUTRES and its GUI counterpart control the data on the results file (Jobname.RST). ERESX and its GUI path allow
you to review element integration point results by copying them to the nodes instead of extrapolating them
(default).

Note — By default, the program writes only the last substep of each load step to the results file. If you
want all substeps (the solution at all frequencies) on the results file, be sure to set the

FREQ

field on

OUTRES to ALL (or 1).

15.5.6. Step 6: Back Up Your Database

Save a backup copy of the database on a named file using Utility Menu> File> Save as or the SAVE command.
Doing so enables you to retrieve your model should your computer abort during the solution. (To retrieve a
model, reenter ANSYS and then issue the RESUME command or choose Utility Menu> File> Resume.)

15–10

Chapter 15: Acoustics

15.5.7. Step 7: Apply Additional Load Steps (Optional)

If you wish to apply additional load steps, repeat steps 5 and 6.

15.5.8. Step 8: Finish the Solution

Solve the analysis and then finish.

Command(s): SOLVE
GUI: Main Menu> Solution> Solve> Current LS
Command(s): FINISH
GUI: Main Menu> Finish

15.6. Reviewing Results

The ANSYS program writes results from a harmonic acoustic analysis to the structural results file, Jobname.RST.
Results consist of the following data, all of which vary harmonically at each forcing frequency for which the
solution was calculated:

•

Primary data

– Nodal pressures

– Nodal displacements

•

Derived data

– Nodal and element pressure gradients

– Nodal and element stresses

– Element forces

– Nodal reaction forces

You can review this information using POST1 or POST26.

15.7. Fluid-Structure Interaction

The interaction of the fluid and the structure at a mesh interface causes the acoustic pressure to exert a force
applied to the structure and the structural motions produce an effective "fluid load." The governing finite element
matrix equations then become:

[

] { } [

] { } {

} [ ] { }

[

] { } [

] { } { }

[ ]

R P

−ρ

{{ }

[R] is a "coupling" matrix that represents the effective surface area associated with each node on the fluid-
structure interface (FSI). The coupling matrix [R] also takes into account the direction of the normal vector defined
for each pair of coincident fluid and structural element faces that comprises the interface surface. The positive
direction of the normal vector, as the ANSYS program uses it, is defined to be outward from the fluid mesh and
in towards the structure. Both the structural and fluid load quantities that are produced at the fluid-structure
interface are functions of unknown nodal degrees of freedom. Placing these unknown "load" quantities on the
left hand side of the equations and combining the two equations into a single equation produces the following:

Section 15.7: Fluid-Structure Interaction

15–11

























−



























&&
&&









Equation 3 implies that nodes on a fluid-structure interface have both displacement and pressure degrees of
freedom.

15.8. Sample Applications

The two example problems presented here illustrate the application of the acoustic elements. The first example
shows the use of the acoustic absorption elements in modeling far-field problems. The second example is a near-
field problem showing the use of standing wave prediction in an enclosed space.

15.9. Example 1: Fluid-Structure Coupled Acoustic Analysis (Command
Method)

In this problem you will determine the first flexural mode (egg mode) frequency of an annular ring submerged
in water which extends to infinity. You will perform a harmonic analysis using a frequency sweep between 34
and 38 Hz. The distance from the center of the ring to the infinite elements will at least be equal to (D/2) + 0.2

where D is the outer diameter of the ring and

λ = c/f is the dominant wavelength of the pressure waves. Using

0.26035 for the outer radius of the ring, 1460 for the speed of sound (c), and 36 for the estimated dominant fre-
quency (f), gives (D/2) + 0.2

λ = 0.26035 + (0.2)(1460)/36 = 8.37146. However, this is much greater than the distance

required when using the acoustic infinite element and a distance of 2 times the outer radius of the ring will be
used ( 2 x .26035 = .5207), as shown in the command listing.

/BATCH,LIST

/VERIFY,EV129-1S

/PREP7

/TITLE,AMA,EV129-1S,FLUID129,HARMONIC ANALYSIS

ET,1,PLANE42 ! structural element

ET,2,FLUID29 ! acoustic fluid element with ux & uy

et,3,129 ! acoustic infinite line element

r,3,0.5207,0,0

ET,4,FLUID29,,1,0 ! acoustic fluid element without ux & uy

! material properties

MP,EX,1,2.068e11

MP,DENS,1,7929

MP,NUXY,1,0MP,DENS,2,1030

MP,SONC,2,1460

! create inner and outer quarter circles

CYL4,0,0,0.254,0,0.26035,90

CYL4,0,0,0.26035,0,0.5207,90

! select, assign attribute to and mesh area 1

ASEL,S,AREA,,1

AATT,1,1,1,0

LESIZE,1,,,16,1

LESIZE,3,,,16,1

LESIZE,2,,,1,1

LESIZE,4,,,1,1

MSHKEY,1

MSHAPE,0,2D ! mapped quad mesh

AMESH,1

! select, assign attribute to and mesh area 2

ASEL,S,AREA,,2

AATT,2,1,2,0

LESIZE,5,,,16,1

LESIZE,7,,,16,1

LESIZE,6,,,5

LESIZE,8,,,5

MSHKEY,0

MSHAPE,0,2D ! mapped quad mesh

AMESH,2

15–12

Chapter 15: Acoustics

! reflect quarter circle into semicircle about x-axis

nsym,x,1000,all ! offset node number by 1000

esym,,1000,all

! reflect semicircle into full circle about y-axis

nsym,y,2000,all ! offset node number by 2000

esym,,2000,all

NUMMRG,ALL ! merge all quantities

! modify outer 2 layers of el29 into type 4

esel,s,type,,1

nsle,s

esln,s,0

nsle,s

esel,inve

nsle,s

emodif,all,type,4

esel,all

nsel,all

! define el129 line element

csys,1

nsel,s,loc,x,0.5207

type,3

real,3

mat,2

esurf

esel,all

nsel,all

! flag interface as fluid-structure interface

nsel,s,loc,x,0.26035

esel,s,type,,2

sf,all,fsi,1

nsel,all

esel,all

FINISH

! enter solution module

/SOLU

ANTYPE,harmic ! select harmonic analysis

hropt,full

f,19,fx,1000.

f,1019,fx,-1000.

harfrq,34.,38.

nsubst,100

kbc,1

SOLVE

FINISH

! postprocess

/post26

plcplx,0

nsol,2,1,u,x,d1ux

store

conjug,3,2

prod,4,2,3

sqrt,5,4

*get,uxmx,vari,5,extrem,tmax

/COM -------------------------------------------------------------

/COM Expected Result:

/COM

/COM The following "uxmx" should equal 35.24 Hz.

/COM -------------------------------------------------------------

*status,uxmx

finish

15.10. Example 2: Room Acoustic Analysis (Command Method)

This sample problem demonstrates the use of FLUID30 to predict the acoustic standing wave pattern of a typical
enclosure representing a room. A sound-absorption material is located at the bottom surface of the enclosure
and a vibrating structure with a cylindrical surface is located at the top right hand corner of the enclosure. This
problem will determine the acoustic pressure wave pattern when the structure vibrates at an excitation frequency
of 80 HZ.

Section 15.10: Example 2: Room Acoustic Analysis (Command Method)

15–13

/batch,list

/com, Harmonic Analysis - Room Acoustics

/PREP7

/TITLE,Room Acoustic Analysis

ANTYPE,HARM

ET,1,30 ! Acoustic elements in contact with walls and vibrating surface

ET,2,30,,1 ! Acoustic elements in interior (not in contact with walls)

! Set parameters for mesh generation

XDIV=29 ! Number of divisions along x-axis

YDIV=19 ! Number of divisions along y-axis

ZDIV=1 ! Number of divisions along z-axis

CDIV=2 ! Number of divisions along radius

! Dimensions of the room

LEN=27

HGT=20

RAD=0.9

! Mesh generation

K,1

K,2,LEN

K,3,LEN,HGT

K,4,,HGT

K,5,,,-1

K,6,LEN,,-1

K,7,LEN,HGT,-1

K,8,,HGT,-1

L,1,5,1

L,2,6,1

L,3,7,1

L,4,8,1

CIRC,3,RAD,7,2,90,2

ADRAG,5,6,,,,, 3

PIO4=ATAN(1)

LENC=COS(PIO4)

LENC=LENC*RAD

HGTC=HGT-LENC

LENC=LEN-LENC

K,15,,HGTC

K,16,,HGTC,-1

K,17,LENC

K,18,LENC,,-1

L,1 ,17,XDIV

L,10,15,XDIV

L,11,4 ,XDIV

L,17,10,YDIV

L,15, 1,YDIV

L,2 ,9 ,YDIV

L,5 ,18,XDIV

L,13,16,XDIV

L,14,8 ,XDIV

L,18,13,YDIV

L,16,5 ,YDIV

L,6 ,12,YDIV

ESIZE,,CDIV

V,1 ,17,10,15, 5,18,13,16

V,15,10,11,4 ,16,13,14,8

V,17,2 ,9 ,10,18,6 ,12,13

VMESH,ALL

! Material properties

MP,DENS,1,2.35E-3 ! (Rho) density of air (lb/ft**3)

MP,SONC,1,1100.0 ! (C) speed of sound in air (ft/sec)

MP,MU,1,0.04 ! (Beta) absorption coefficient of the walls

! ('Beta' should be between 0 - 1)

MP,DENS,2,2.35E-3

15–14

Chapter 15: Acoustics

MP,SONC,2,1100.0

MP,MU,2,0.70 ! (Beta) absorption coefficient of

! the absorbing material on the floor

! ('Beta' should be between 0 -1)

MP,DENS,3,2.35E-3

MP,SONC,3,1100.0

MP,MU,3,0.0 ! (Beta) zero absorption coefficient for interior elements

NSEL,S,LOC,Y,0.0

NSEL,R,LOC,X,12,15

ESLN

MAT,2

EMODIF,ALL ! Elements which have the absorbing material on the floor

! Boundary conditions

ALLS

NSEL,S,LOC,X,0.0

NSEL,A,LOC,Y,0.0

NSEL,A,LOC,X,LEN

NSEL,A,LOC,Y,HGT

D,ALL,UX,,,,,UY,UZ! Constrain all displacements to zero at the walls

LOCAL,11,1,27,20

NSEL,A,LOC,X,RAD

ESLN

ESEL,INVE

TYPE,2

MAT,3

EMODIF,ALL ! Interior elements are specified as Type=2 & material=3

ALLS

! Fluid-Structure Interface (FSI)

NSEL,S,LOC,X,RAD ! Select interface (FSI) surface nodes

ESLN ! Select elements attached to interface surface

SF,ALL,FSI ! Specify vibrating surface as Fluid-structure interface

NROTAT,ALL

D,ALL,UX,.01 ! Radial vibration amplitude of Vibrating surface

D,ALL,UY,,,,,UZ

! Impedance Surface (IMPD)

CSYS,0

ALLS

NSEL,S,LOC,X,0.0

NSEL,A,LOC,X,LEN

NSEL,A,LOC,Y,0.0

NSEL,A,LOC,Y,HGT

SF,ALL,IMPD,1 ! Specify the walls as Impedance Surface flag

! to activate absorption

ALLS

FINISH

/SOLU

! Excitation Frequency for Harmonic Analysis

HARF,80,80 ! Frequency of excitation = 80 Hz

SOLVE

FINISH

! Plot the Standing Wave Pattern (f = 80 Hz)

/POST1

/SHOW,ENCL1,GRPH,1

SET,1,1 ! plot the real part of pressure response

EPLOT

/EDGE,1

/TITLE,-ROOM ACOUSTICS- * REAL PART OF PRESSURE

PLNS,PRES

SET,1,1,,1 ! plot the imag. part of pressure response

/TITLE,-ROOM ACOUSTICS- * IMAG. PART OF PRESSURE

PLNS,PRES

FINISH

Section 15.10: Example 2: Room Acoustic Analysis (Command Method)

15–15

15–16

Part III. Thin Film

Chapter 16: Thin Film Analysis

A thin film is a small gap of fluid between moving surfaces. This thin layer of fluid can alter the structural response
of the structure by adding stiffness and/or damping to the system. Movement normal to the gap produces a
squeeze film effect. Movement tangential to the gap produces a slide film effect.

Thin film effects are important in macrostructures, but they are particularly critical in microstructures where the
damping and stiffening effects of thin layers of air can significantly affect the behavior of devices used in micro-
electromechanical systems (MEMS). Squeeze film effects are important in devices such as accelerometers and
micromirrors. Slide film effects are important in devices such as comb drives.

One method for assessing the effect of thin films is to use thin film fluid elements based on the Reynolds number
(which is known from lubrication technology and rarified gas physics) to calculate the stiffening and damping
effects. These effects can then be added to the overall system model. Separate element types are used to assess
squeeze and slide film effects.

The governing Reynolds equation limits the application of thin film analyses to structures with lateral dimensions
much greater than the gap separation. In addition, the pressure change across the gap must be much smaller
than the ambient (i.e., surrounding) pressure, and any viscous heating effects must be ignored. If these three
conditions are not satisfied, then the effects of the thin film cannot be assessed using thin film elements. For
those situations, the Navier Stokes equations must be solved using FLOTRAN to assess the effect of the fluid.

16.1. Elements for Modeling Thin Films

The ANSYS program has three elements for modeling thin film effects. FLUID136 and FLUID138 are used to
model squeeze film effects. FLUID139 is used to model slide film effects.

Table 16.1 Thin Film Fluid Elements

DOF

Shape or Characteristic

Dimens.

Element

PRES

Quadrilateral, 4 or 8-node

3-D

FLUID136

PRES

Line, 2-node

3-D

FLUID138

UX or UY or UZ

Line, 2-node

1-D

FLUID139

16.2. Squeeze Film Analysis

Squeeze film analysis simulates the effects of fluid in small gaps between fixed surfaces and structures moving
perpendicular to the surfaces. Depending on the operating frequencies, the fluid can add stiffening and/or
damping to the system. At low frequencies, the fluid can escape before it compresses. Therefore, the fluid only
adds damping to the system. At high frequencies, the fluid compresses before it can escape. Therefore, the fluid
adds both stiffening and damping to the system.

A static analysis is used to determine the damping effects at low frequencies. A harmonic analysis is used to de-
termine the stiffening and damping effects at high frequencies.

The FLUID136 element is used to model the fluid domain between a fixed surface and a structure moving normally
to that surface. The fluid domain is modeled by overlaying FLUID136 elements on the moving surface of the
structure (i.e., lower surface of the structure adjacent to the fixed wall).

Figure 16.1 Moving Plate above a Fixed Wall

The FLUID138 element is used to model the pressure drop through holes in a moving structure. Microstructures
are commonly perforated to reduce the damping effects of the fluid layer. FLUID138 elements are used in con-
junction with FLUID136 elements to obtain a consistent pressure distribution, including the effects of holes.

Figure 16.2 Perforated Plate Structure

A squeeze film analysis can be performed on structures with known velocities or unknown velocities. If the velocity
profile is known, you can apply it directly to the fluid elements. If the velocity profile is not known (or is too
complicated), it can be determined from the mode-frequency response of the structure (model projection
method). This section deals with directly applying the velocities. Section 16.3: Modal Projection Method for
Squeeze Film Analysis covers the modal projection method.

16.2.1. Static Analysis Overview

Use a static analysis to calculate the pressure distribution for low operating frequencies, where the compression
of the fluid (and thus the stiffening effect) is negligible. The resulting pressure distribution can then be used to
extract a damping coefficient that reflects the damping effect of the fluid.

16–2

Chapter 16: Thin Film Analysis

F is the total pressure force at the fluid structure interface and v

is the normal velocity component of the moving

structure. A typical pressure distribution on a rectangular plate is shown in Figure 16.3: “Pressure Distribution
on a Plate at a Low Driving Frequency”.

Figure 16.3 Pressure Distribution on a Plate at a Low Driving Frequency

16.2.2. Harmonic Response Analysis Overview

Use a harmonic analysis to calculate the complex pressure distribution for high operating frequencies. The
complex pressure distribution can be used to extract a damping coefficient and a stiffness coefficient. The phase
shift between the pressure and the velocity is caused by compression of the fluid. The real pressure component
contributes to the damping of the system. The imaginary pressure component contributes to the stiffening of
the system.

is the real component of the pressure force. F

is the imaginary component of the pressure force. Omega

(

ω) is the frequency (rad/sec). The damping and stiffness coefficients are frequency-dependent. Figure 16.4: “Damp-

ing and Squeeze Stiffness Coefficients vs. Frequency” illustrates the frequency dependency for a typical microsys-
tem application.

Figure 16.4 Damping and Squeeze Stiffness Coefficients vs. Frequency

The DMPEXT command is used to extract frequency-dependent damping parameters for use with the MDAMP,
DMPRAT, ALPHAD, and BETAD command inputs.

Section 16.2: Squeeze Film Analysis

16–3

16.2.3. Flow Regime Considerations

The Reynolds squeeze film approach assumes a continuous fluid flow regime. To ensure a continuous flow regime,
the characteristic length (i.e., gap thickness) must be more than one hundred times larger than the mean free
path of the fluid particles.

L P

(

)

0 0

m(po)

is the mean free path of the fluid at the operating pressure P

, and L

is the mean path at reference pressure

. If the fluid is air at atmospheric pressure (1.01325*10

), then by definition L

is approximately 64*10

-9

meters

(64 µm). So, for continuum theory to be directly applicable (without modification) to air at atmospheric pressure,
the gap should be greater than 6.4 µm (64*10

-9

meters * 100).

The applicability of the continuum theory is generally assessed using the Knudsen number, which is equal to
the mean free fluid path divided by the gap. For continuum theory to be valid, the Knudsen number should be
less than 0.01.

L P

p d

0 0

For high Knudsen numbers, the continuum theory is not valid. However, the dynamic viscosity can be adjusted
to simulate the high Knudsen number flow regime. The default flow regime for FLUID136 and FLUID138 is con-
tinuum theory (KEYOPT(1) = 0). Set KEYOPT (1) = 1 to specify the high Knudsen number flow regime.

The type of reflection of the gas molecules at the wall interface is specified using accommodation factors. Squeeze
film models assume diffuse reflection of the gas molecules at the wall interface (accommodation factor = 1). This
assumption is valid for most metals, but is less accurate for micromachined surfaces, particularly those fabricated
from silicon. Materials such as silicon cause specular reflection. Typical accommodation factors for silicon are
between 0.80 and 0.90.

16.2.4. Modeling and Meshing Considerations

The methods used to model and mesh the fluid domain depend on the squeeze film analysis method. If the ve-
locities are directly applied to the fluid elements, the fluid elements can be independent of the structure. If the
velocities are determined from the mode-frequency response of the structure (modal projection method), the
fluid elements cannot be independent of the structure.

In the modal projection method, the FLUID136 elements must lie on the surface of the structural mesh. Use the
ESURF command to overlay FLUID136 elements on the surface of an existing structural mesh. FLUID136 supports
4-node and 8-node options, along with degenerative triangles.

The FLUID138 element is used to model the pressure drop in the channels (holes) in a structure as shown in
Figure 16.2: “Perforated Plate Structure”. The element supports a circular hole configuration and a rectangular
hole configuration (KEYOPT(3)). The element works in conjunction with FLUID136 to correctly compute the
pressure distribution on the structure's surface and through the channels. To correctly model the FLUID138
element:

Use a single FLUID138 element for each hole.

Align the FLUID138 element at the center of the hole. The element should extend through the depth of
the hole and have a length equal to the depth of the hole.

16–4

Chapter 16: Thin Film Analysis

Assume the pressure at the center of the hole (flush with the plate surface in the thin film region) is at
the same pressure as the nodes modeled at the periphery of the hole. Couple the nodes of the FLUID136
element at the whole periphery with the node of the FLUID138 element as shown in Figure 16.5: “Coupling
of Nodes at the Hole Periphery with the Center Node of a FLUID138 Element”.

Figure 16.5 Coupling of Nodes at the Hole Periphery with the Center Node of a FLUID138
Element

#"%$#

&('

&*)

&* ,

&1023

4! 5 6

* 7

#&(#0/

;

16.2.5. Analysis Settings and Options

A thin film analysis using FLUID136 and FLUID138 is a linear solution for both a static and a harmonic response
analysis. No special analysis options or load step options are required. See the ANSYS Basic Analysis Guide for
general guidelines on solving a static analysis.

For a harmonic response analysis, you must use the full method.

16.2.6. Loads and Solution

The fluid elements support pressure loads at the nodal PRES degrees of freedom and velocity body loads (FLUE)
at the node or element as shown in Table 16.2: “Load Options for Thin Film Fluid Elements”. Pressure loads are
applied using the D family of commands. The velocity load is applied using the BF family of commands. For the
velocity load, a positive velocity load will cause a positive pressure. For a harmonic response analysis, a positive
velocity load will cause a positive in-phase pressure load. See Section 2.6.8: Body Loads for details on applying
body loads.

Note — Velocity body loads (FLUE) are the velocities of the moving wall in a direction normal to the wall.
They are not in-plane velocities of the fluid.

Table 16.2 Load Options for Thin Film Fluid Elements

ANSYS Label

Type

Load

PRES

Nodal DOF

Pressure

FLUE

Body Load

Normal Velocity

The recommended equation solvers for the fluid elements are the Sparse Direct Solver (SPARSE), the Jacobi
Conjugate Gradient Solver (JCG) and the Incomplete Cholesky Conjugate Gradient Solver (ICCG).

Section 16.2: Squeeze Film Analysis

16–5

16.2.7. Review Results

Results from a thin film fluid analysis are stored on the Jobname.RST file. The primary result from the fluid ana-
lysis is the nodal pressures. For a harmonic response analysis, the pressures are stored as complex values (Real
and Imaginary components). Chapter 5, “The General Postprocessor (POST1)” discusses reading results into the
database and viewing the nodal degree of freedom (pressure) results.

Each fluid element computes and stores results for the mid-plane fluid velocity (PG) and effective viscosity. Use
the element table to retrieve and view these results.

To compute the damping and squeeze stiffness coefficients from the resulting pressure distribution on the surface
of a structure, use the element table tools to compute the force on a per-element basis, then sum over all elements
to compute the coefficients. The following command sequence demonstrates how to do this task. This example
assumes parameters “omega” and “velo” exist (frequency and normal velocity (FLUE loading), respectively).

set,1,1 ! store Real solution

etable,presR,temp ! extract "Real" pressure

etable,earea,volu ! extract element area

smult,forR,presR,earea ! compute "Real" force

ssum ! sum over all elements

*get,Fre,ssum,,item,forR ! get the total "real" force

set,1,1,,1 ! store Imaginary solution

etable,presI,temp ! extract "Imaginary" pressure

smult,forI,presI,earea ! compute "Imaginary" force

ssum ! sum over all elements

*get,Fim,ssum,,item,forI ! get the total "imaginary" force

K=abs(Fim*omega/velo) ! Compute squeeze stiffness coefficient

C=abs(Fre/velo) ! Compute damping coefficient

/com, ** Equivalent squeeze stiffness coefficient **

*stat,K

/com, ** Equivalent damping coefficient **

*stat,C

16.2.8. Example Problem

A rectangular beam with perforated holes under transverse motion is modeled to compute the effective damping
and squeeze stiffness coefficients. The thin film surface of the structure is modeled with FLUID136 elements.
FLUID138 elements are used to model the hole regions. By altering the boundary condition of the free FLUID138
node, we can simulate different pressure boundary conditions of the hole region. The purpose of the analysis is
to compute the equivalent squeeze stiffness and damping coefficient for an assumed uniform plate velocity. A
harmonic response analysis is performed at 150 kHz. A previous modal analysis indicated that the pertinent ei-
genfrequency was 150 kHz. Since the analysis is linear, the magnitude of the velocity can be arbitrary for com-
puting the coefficients.

Three cases were considered:

Holes modeled with no resistance (pressure = 0 at hole location, no FLUID138 elements ).

Holes modeled with finite resistance (FLUID138 elements modeled, pressure set to zero on fluid node
at top of plate).

Holes modeled with infinite resistance (no pressure specification at hole location, no FLUID138 elements).

Case 1 is typical for large diameter holes compared to the hole depth. Case 3 is typical for very high flow resistance,
which happens in the case of narrow and long holes. Case 2 is the most accurate case where the fluid pressure
drop is taken into account by the FLUID138 elements.

16–6

Chapter 16: Thin Film Analysis

Table 16.3: “Beam Model Results Considering Perforated Holes” lists the damping and squeeze coefficient results.
Figure 16.6: “Pressure Distribution (Real Component)” and Figure 16.7: “Pressure Distribution (Imaginary Com-
ponent)” illustrate the real and imaginary pressure distribution. The input file for case 2 is listed.

Table 16.3 Beam Model Results Considering Perforated Holes

Squeeze stiffness coefficient

Damping Coefficient

Hole option

Frequency (kHz.)

1.201

2.016e-5

Infinite resistance

150

.5465

1.325e-5

Finite resistance

150

.4607

1.165e-5

No resistance

150

Figure 16.6 Pressure Distribution (Real Component)

Section 16.2: Squeeze Film Analysis

16–7

Figure 16.7 Pressure Distribution (Imaginary Component)

The input file for this example is shown below for the finite-resistance Case 2

/batch,list

/PREP7

/title, Damping and Squeeze film stiffness calculations for a rigid

/com, plate with holes

/com uMKS units

ET, 1,136,1 ! 4-node option, High Knudsen Number

ET, 2,138,1 ! Circular hole option, Hugh Knudsen Number

s_l=100 ! Half Plate length (um)

s_l1=60 ! Plate hole location

s_w=20 ! Plate width

s_t=1 ! Plate thickness

c_r=3 ! Hole radius

d_el=2 ! Gap

pamb=.1 ! ambient pressure (MPa)

visc=18.3e-12 ! viscosity kg/(um)(s)

velo=2000 ! arbitrary velocity (um/s)

freq=150000 ! Frequency (Hz.)

pi=3.14159

omega=2*pi*freq ! Frequency (rad/sec)

pref=.1 ! Reference pressure (MPa)

mfp=64e-3 ! mean free path (um)

Knud=mfp/d_el ! Knudsen number

mp,visc,1,visc ! Dynamic viscosity gap

mp,visc,2,visc ! Dynamic viscosity holes

r,1,d_el,,,pamb ! Real constants - gap

rmore,pref,mfp

r,2,c_r,,,pamb ! Real constants - hole

rmore,pref,mfp

! Build the model

rectng,-s_l,s_l,-s_w,s_w ! Plate domain

pcirc,c_r ! Hole domain

16–8

Chapter 16: Thin Film Analysis

agen,3,2,,,-s_l1/3

agen,3,2,,,s_l1/3

ASBA, 1, all

TYPE, 1

MAT, 1

smrtsize,4

AMESH, all ! Mesh plate domain

! Begin Hole generation

*do,i,1,5

nsel,all

*GET, numb, node, , num, max ! Create nodes for link elements

N, numb+1,-s_l1+i*s_l1/3,,

N, numb+2,-s_l1+i*s_l1/3,, s_t

TYPE,2

MAT, 2

REAL,2

NSEL, all

E, numb+1, numb+2 ! Define 2-D link element

ESEL, s, type,,1

NSLE,s,1

local,11,1,-s_l1+i*s_l1/3

csys,11

NSEL,r, loc, x, c_r ! Select all nodes on the hole circumference

NSEL,a, node, ,numb+1

*GET, next, node, , num, min

CP, i, pres, numb+1, next

nsel,u,node, ,numb+1

nsel,u,node, ,next

CP, i, pres,all !Coupled DOF set for constant pressure

csys,0

*enddo

! End hole generation

nsel,s,loc,x,-s_l

nsel,a,loc,x,s_l

nsel,a,loc,y,-s_w

nsel,a,loc,y,s_w

nsel,r,loc,z,-1e-9,1e-9

d,all,pres ! Fix pressure at outer plate boundary

nsel,all

esel,s,type,,2

nsle,s,1

nsel,r,loc,z,s_t

d,all,pres,0 ! P=0 at top of plate

dlist,all

allsel

bfe,all,flue,,velo ! Apply arbitrary velocity

fini

finish

/solu

antyp,harm ! Full Harmonic analysis

harfrq,freq

solve

finish

/post1

esel,s,type,,1

set,1,1

etable,presR,pres ! extract "Real" pressure

etable,earea,volu

smult,forR,presR,earea ! compute "Real" force

ssum

*get,Fre,ssum,,item,forR

set,1,1,,1

etable,presI,pres ! extract "Imaginary" pressure

smult,forI,presI,earea ! compute "Imaginary" pressure

Section 16.2: Squeeze Film Analysis

16–9

ssum

*get,Fim,ssum,,item,forI

K=abs(Fim*omega/velo) ! Compute equivalent stiffness

C=abs(Fre/velo) ! Compute equivalent damping

/com, ******* Equivalent stiffness ************************

*stat,K

/com, ******* Equivalent damping **************************

*stat,C

finish

16.3. Modal Projection Method for Squeeze Film Analysis

Modal projection techniques provide an efficient method for computing damping parameters for flexible bodies.
The Modal Projection Technique is the process of calculating the squeeze stiffness and damping coefficients of
the fluid using the eigenvectors of the structure. In the modal projection method, the velocity profiles are de-
termined from the mode-frequency response of the structure.

16.3.1. Modal Projection Method Overview

For a structure undergoing flexible body dynamics, the displacement and velocity vary along the structure. For
a thin-film fluid adjacent to the structure, there is a true dependency between the structural velocity and the
fluid pressure. A modal analysis of a structure provides information on the fundamental eigenfrequencies and
mode shapes (eigenvectors). For each mode, i, we can impress the distributed eigenvector values as velocity
loads and compute the resulting pressure distribution and hence the fluid force acting on mode j. Therefore, we
can compute a matrix of modal squeeze stiffness coefficients, K

, and modal damping coefficients, C

. The diag-

onal terms of these matrices are the coefficients of each mode, the off-diagonal terms represent the "cross-talk"
coefficients between modes. Figure 16.8: “Modal Projection Technique for Damping Characterization” illustrates
the modal projection technique.

Figure 16.8 Modal Projection Technique for Damping Characterization

16–10

Chapter 16: Thin Film Analysis

From the modal squeeze and stiffness coefficients for the main diagonal terms (source mode = target mode),
other useful damping parameters can be calculated. For example, the modal damping ratio,

ξ , and the modal

squeeze to stiffness ratio, kr

, can be computed by:

)

Where m

is the modal mass and

the eigenfrequency. The damping ratio can be used to compute ALPHAD

and BETAD parameters for Rayleigh damping (see ABEXTRACT command), or to specify constant and modal
damping by means of the DMPRAT or MDAMP commands.

The squeeze to stiffness ratio represents the relative stiffening of the mechanical system due to fluid compression
and resonance shift. If the squeeze-to-stiffness ratio is small (e.g., <.02), then the squeeze stiffness affects the
structural stiffness by less than 2%, which may be negligible. At higher frequencies, the ratio can be much larger,
indicating a significant stiffening of the structure.

The stiffness and damping coefficients may be strongly frequency-dependent. Figure 16.9: “Damping and Squeeze
Stiffness Parameters for a Rectangular Plate” shows a typical frequency dependency of the squeeze and damping
forces on a flat plate, and the resulting stiffness and damping constant. The frequency where the forces intersect
is known as the cut-off frequency. Below this frequency, structures may be accurately characterized by a constant
damping coefficient, and stiffness effects can be ignored. Structures which operate far above the cut-off can be
described by a constant stiffness coefficient, and damping effects can be ignored.

Figure 16.9 Damping and Squeeze Stiffness Parameters for a Rectangular Plate

16.3.2. Steps in Computing the Damping Parameter Using the Modal Projection
Technique

The basic steps in performing the analysis are as follows:

Build a structural and thin-film fluid model and mesh.

Perform a modal analysis on the structure.

Extract the desired mode eigenvectors.

Select the desired modes for damping parameter calculations.

Perform a harmonic analysis on the thin-film elements.

Compute the modal squeeze stiffness and damping parameters.

Compute modal damping ratio and squeeze stiffness coefficient.

Display the results.

Section 16.3: Modal Projection Method for Squeeze Film Analysis

16–11

Steps 4-7 have been automated using the DMPEXT command macro. Step 8 is available through the MDPLOT
command macro.

16.3.2.1. Modeling and Meshing

Model preparation for the modal projection method for damping parameter extraction follows very closely to
the method outlined in Section 16.2.4: Modeling and Meshing Considerations. Both the structural model and
the thin-film fluid model need to be defined simultaneously. Group the fluid nodes on the structure surface into
a node component named "FLUN". This component should only include nodes attached to FLUID136 elements.
This component defines the nodes for which the eigenvector values will be extracted from the mode-frequency
analysis.

16.3.2.2. Perform Modal Analysis

A modal analysis of the structure is required to obtain the eigenvectors of the desired modes. The modal analysis
should be set up with the following options:

Use the Block Lanczos method (MODOPT command).

Extract the eigenmodes of interest (MODOPT command).

Expand the eigenmodes of interest (MXPAND command).

The expanded eigenmodes will compute the necessary eigenvectors required for the modal projection technique.
Note: The thin-film fluid elements may be left active in the model when performing the modal analysis. These
elements will not contribute to the modal solution.

16.3.2.3. Extracting Eigenvectors

The eigenvectors from the modal analysis must be retrieved and stored in a format appropriate for use by the
thin-film fluid elements for a subsequent harmonic fluid analysis. Use the RMFLVEC command in POST1 to retrieve
the eigenvectors. The data is stored in the file Jobname.EFL.

16.3.2.4. Performing a Harmonic Response Analysis and Extracting Damping
Parameters

The command macro DMPEXT performs a harmonic response analysis with the thin-film fluid elements using
the eigenvector information for the desired mode(s). The macro also extracts damping parameter information
for use in subsequent dynamic structural analysis. Damping parameters extracted include the modal damping
coefficient, modal squeeze stiffness coefficient, damping ratio, and the squeeze-to-stiffness ratio.

DMPEXT requires a "source" mode number and a "target" mode number. The source mode is the mode for which
the eigenvectors are used to impart a velocity field on the fluid elements. The target mode is the mode which is
acted on by the pressure solution (fluid forces). For transverse oscillations and a uniform gap, there is little mode
interaction and hence only diagonal terms are required (source mode (i) = target mode (j)). For transverse motion
with nonuniform gaps, or asymmetric plate motion, mode interaction effects (cross-talk) can be significant and
should be computed (source mode .ne. target mode). Typical cross-talk scenarios are shown in Figure 16.10: “Flu-
idic Cross-Talk between Transverse and Rotational Motion”.

16–12

Chapter 16: Thin Film Analysis

Figure 16.10 Fluidic Cross-Talk between Transverse and Rotational Motion

Damping parameter extraction can be selected over a desired frequency range or at the eigenfrequencies of the
structure. Damping results are computed and stored in an array parameter.

Computed damping ratios may be used in subsequent dynamic structural analyses. A constant damping ratio
can be applied using DMPRAT for a subsequent harmonic or mode-superposition transient analysis. Mode
damping ratios may be applied using the MDAMP command for use in mode-superposition harmonic and
transient analyses. Note: Subsequent structural analysis using these damping parameters do not require the
thin-film fluid elements in the model.

The command macro ABEXTRACT (like DMPEXT) extracts alpha and beta damping parameters for use in the
ALPHAD and BETAD commands. These commands define Rayleigh damping and can be used in time-transient
structural analysis to model damping effects. The damping parameters are computed from two modes defined
by the user.

The command macro MDPLOT may be used to display the frequency-dependent damping parameters.

16.3.3. Example Problem Using the Modal Projection Method

A rectangular beam with perforated holes is modeled to compute the effective damping coefficient, stiffness
coefficient, and damping ratio. The surface of the structure is modeled with FLUID136 elements to represent the
thin film. The structure is modeled with SOLID45 elements. This example computes the Rayleigh damping
coefficients (

α and β) and modal damping ratios ξ

for use in a transient dynamic analysis.

The problem is defined as an extension to the earlier squeeze film example. After modeling the fluid domain,
the structure of the beam is modeled and meshed with SOLID45 elements. A modal analysis is performed on
the structure and the first two eigenvalues and eigenvectors are computed. RMFLVEC is used to extract the ei-
genvectors for use in the modal projection method to compute the thin-film damping parameters. The command

Section 16.3: Modal Projection Method for Squeeze Film Analysis

16–13

macro ABEXTRACT is used to compute the Rayleigh parameters from the lowest two eigenmodes . Modal
damping ratios are also provided by the ABEXTRACT macro for the two eigenmodes.

Table 16.4: “Modal Damping Parameters for First Two Eigenfrequencies” lists the results from the damping
parameter extraction. Computed Rayleigh parameters are: ALPHAD=65212, BETAD=1.829e-8. The input file for
this example is shown below.

Table 16.4 Modal Damping Parameters for First Two Eigenfrequencies

Stiffness Ratio

Damping Ratio

Modal Squeeze Stiffness
Coefficient

Modal Damping Coeffi-
cient

Frequency (Hz.)

.2285e-2

.9703e-1

.2758e9

67419

55294

.3644e-2

.4200e-1

.3568e10

83123

157497

The input file for this example is shown below.

/batch,list

/PREP7

/title, Damping Ratio and Rayleigh Damping Calculations for a Perforated Plate

/com uMKS units

ET, 1,136,1 ! 4-node option, High Knudsen Number

ET, 2,138,1 ! Circular hole option, Hugh Knudsen Number

ET,3,45 ! Structural element

s_l=100 ! Half Plate length (um)

s_l1=60 ! Plate hole location

s_w=20 ! Plate width

s_t=1 ! Plate thickness

c_r=3 ! Hole radius

d_el=2 ! Gap

pamb=.1 ! ambient pressure (MPa)

visc=18.3e-12 ! viscosity kg/(um)(s)

pref=.1 ! Reference pressure (MPa)

mfp=64e-3 ! mean free path (um)

Knud=mfp/d_el ! Knudsen number

mp,visc,1,visc ! Dynamic viscosity gap

mp,visc,2,visc ! Dynamic viscosity holes

mp,ex,3,79e3 ! Gold

mp,dens,3,19300e-18

mp,nuxy,3,.1

r,1,d_el,,,pamb ! Real constants - gap

rmore,pref,mfp

r,2,c_r,,,pamb ! Real constants - hole

rmore,pref,mfp

! Build the model

rectng,-s_l,s_l,-s_w,s_w ! Plate domain

pcirc,c_r ! Hole domain

agen,3,2,,,-s_l1/3

agen,3,2,,,s_l1/3

ASBA, 1, all

TYPE, 1

MAT, 1

smrtsize,4

AMESH, all ! Mesh plate domain

! Begin Hole generation

*do,i,1,5

16–14

Chapter 16: Thin Film Analysis

nsel,all

*GET, numb, node, , num, max ! Create nodes for link elements

N, numb+1,-s_l1+i*s_l1/3,,

N, numb+2,-s_l1+i*s_l1/3,, s_t

TYPE,2

MAT, 2

REAL,2

NSEL, all

E, numb+1, numb+2 ! Define 2-D link element

ESEL, s, type,,1

NSLE,s,1

local,11,1,-s_l1+i*s_l1/3

csys,11

NSEL,r, loc, x, c_r ! Select all nodes on the hole circumference

NSEL,a, node, ,numb+1

*GET, next, node, , num, min

CP, i, pres, numb+1, next

nsel,u,node, ,numb+1

nsel,u,node, ,next

CP, i, pres,all !Coupled DOF set for constant pressure

csys,0

*enddo

! End hole generation

esize,,2

type,3

mat,3

real,3

vext,all,,,,,s_t ! Extrude structural domain

nsel,s,loc,x,-s_l

nsel,a,loc,x,s_l

nsel,a,loc,y,-s_w

nsel,a,loc,y,s_w

nsel,r,loc,z,-1e-9,1e-9

d,all,pres ! Fix pressure at outer plate boundary

nsel,all

esel,s,type,,2

nsle,s,1

nsel,r,loc,z,s_t

d,all,pres,0 ! P=0 at top of plate

dlist,all

esel,s,type,,1

nsle,s,1

nsel,u,cp,,1,5

cm,FLUN,node

allsel

nsel,s,loc,x,-s_l

nsel,a,loc,x,s_l

d,all,ux

d,all,uy

d,all,uz

allsel

fini

/solu

antype,modal ! Modal analysis

modopt,lanb,2 ! Extract lowest two eigenmodes

eqslv,sparse

mxpand,2 ! Expand lowest two eigenmodes

solve

fini

/post1

RMFLVEC ! Extract eigenvectors

Section 16.3: Modal Projection Method for Squeeze Film Analysis

16–15

fini

/solu

abextract,1,2 ! Extract damping ratios and Rayleigh constants

finish

A transient dynamic analysis on the switch can be performed using the extracted damping parameters. The fol-
lowing input illustrates a coupled electrostatic-structural time-transient solution. The electrostatic field is assumed
to be normal to the plate in the gap, and fringing effects are ignored. TRANS126 elements are used to model the
coupled electrostatic-structural interaction with the switch. The EMTGEN command is used to generate the
transducer elements. A step voltage pulse is applied over a short duration (65 micro-seconds) then released.
Rayleigh damping parameters, when used, are applied to the global mass (ALPHAD parameter) and stiffness
(BETAD parameter) matrices. We want to apply these only to the mass and stiffness matrix of the SOLID45 elements,
and not the TRANS126 elements, because doing so may overdamp the system. The TRANS126 elements produce
a damping matrix and a stiffness matrix only. Hence, we can use the ALPHAD parameter for the global mass
matrix since there is no contribution from the TRANS126 elements. To isolate the SOLID45 elements for beta
damping, we can apply the beta damping via a material damping option (MP,DAMP). Figure 16.11: “Time-Tran-
sient Response from Voltage Pulse” illustrates the displacement of a node near the center of the plate over time.
The maximum amplitude of displacement (0.11 microns) is small enough to ignore large deflection damping
effects.

/batch,list

/PREP7

/title, Damped Transient Dynamic Response of an RF MEMS switch

/com uMKS units

/com, Small deflection assumption

et,1,200,6

ET,3,45 ! Structural element

s_l=100 ! Plate length (um)

s_l1=60 ! Plate hole location

s_w=20 ! Plate width

s_t=1 ! Plate thickness

c_r=3 ! Hole radius

d_el=2 ! Gap

pamb=.1 ! ambient pressure (MPa)

visc=18.3e-12 ! viscosity kg/(um)(s)

pref=.1 ! Reference pressure (MPa)

mfp=64e-3 ! mean free path (um)

Knud=mfp/d_el ! Knudsen number

mp,ex,3,79e3 ! Gold

mp,dens,3,19300e-18

mp,nuxy,3,.1

mp,damp,1,1.829e-8 ! Material damping (from squeeze film results)

! Build the model

rectng,-s_l,s_l,-s_w,s_w ! Plate domain

pcirc,c_r ! Hole domain

agen,3,2,,,-s_l1/3

agen,3,2,,,s_l1/3

ASBA, 1, all

TYPE, 1

MAT, 1

smrtsize,4

AMESH, all ! Mesh plate domain

esize,,2

type,3

mat,3

real,3

vext,all,,,,,s_t ! Extrude structural domain

nsel,s,loc,x,-s_l

nsel,a,loc,x,s_l

16–16

Chapter 16: Thin Film Analysis

d,all,ux

d,all,uy

d,all,uz

allsel

aclear,all

save

nsel,s,loc,z

cm,base,nodes

emtgen,'base',,,'uz',-d_el ! generate Transducer elements

allsel,all

nsel,s,loc,z,-d_el

d,all,uz,0

d,all,volt,0

cmsel,s,base

d,all,volt,10

allsel,all

fini

/solu

antyp,trans

alphad,65211 ! alpha damping computed from Squeeze-film theory

kbc,1

time,.000065

deltime,2.0e-6

outres,all,none

outres,nsol,all

solve

time,.0002

cmsel,s,base

d,all,volt,0

allsel,all

solve

fini

n1=node(0,2,0)

/post26

nsol,2,n1,uz

prvar,2

plvar,2

finish

Figure 16.11 Time-Transient Response from Voltage Pulse

Section 16.3: Modal Projection Method for Squeeze Film Analysis

16–17

16.3.4. Damping Extraction for Large Signal Cases

If a structure does not undergo significant deformation, the gap between the structure and the fixed wall may
be assumed to be constant (small signal case). If the structural deformation in the gap is significant, the change
in the gap may effect the damping of the structure (large signal case). The gap is defined as a real constant in
the thin-film fluid elements. Use SETFGAP to automatically define and/or update the gap real constants for the
thin-film FLUID136 elements. The command can be used to:

•

Create real constant table entries for every selected FLUID136 element (large signal case).

•

Update an existing real constant table according to structural displacements for every FLUID136 element
(large signal case).

This option allows you to check the dependence of the damping parameters over the deflection range of the
structure.

16.4. Slide Film Damping

Slide film damping occurs if two surfaces separated by a thin fluid film move tangentially with respect to each
other, because energy is dissipated due to viscous flow. Typical applications are damping between the fingers
of comb drives and horizontally-moving seismic masses.

FLUID139 is used to model slide film damping. FLUID139 can model Couette and Stokes flow (Figure 16.12: “Slide
Film Damping at Low and High Frequencies”). Couette flow assumes a constant velocity gradient across the
fluid gap. Tangentially moving surfaces at low frequencies produce a nearly constant velocity gradient in the
fluid, so Couette flow is applicable to low frequencies.

Stokes flow assumes that the velocity gradient is not constant across the fluid gap. Tangentially moving surfaces
at high frequencies do not produce a constant velocity gradient, so the Stokes flow is applicable to high frequen-
cies. The transition from Couette to Stokes flow occurs near the cut-off frequency.

πρ

where

ρ is the fluid density, η the dynamic viscosity and d the gap separation.

Couette flow does not occur at high frequencies, because inertial effects are important and viscous friction is
only able to accelerate a thin fluid layer near the moving surface. The penetration depth is given by

Ω

16–18

Chapter 16: Thin Film Analysis

Figure 16.12 Slide Film Damping at Low and High Frequencies

"!$#%

'()*)+(-, %

/.0

)234(56,7%

/.0

:<;" =

>!$#%

?=@BA

F<%

#)+(/(%

)*H

F<%

#)+(/(%

)*H

@NMPO

GU5Q

VWR

Ω

ηρ

( ) ( )

FLUID139 models the effect of viscous flow in the thin film with a series of mass-damper elements, as shown in
Figure 16.13: “Viscous Slide Film Element FLUID139”. Couette flow is modeled using a two-node option. Stokes
flow is modeled using a 32-node option. In the 32-node option, the end nodes (node 1 and 32) are connected
to the structural portion of the model with structural degrees of freedom, and the series of mass-damper elements
are contained within "auxiliary" nodes (nodes 2-31).

The gap separation distance (GAP) and the overlap area of the surfaces (AREA) are specified as real constants for
FLUID139. If the overlap area changes during the analysis, the area change rate (DADU) must also be specified
as a real constant. A changing overlap area is typical in lateral comb drives.

d A

new

initial

−

(

)

AREA is the initial overlap area, DADU is the change in the overlap area with respect to the surface displacement,
and u

and u

are the location of the interface nodes (1 and 32). Note: For a constant surface area, DADU is the

width of the overlap surface.

FLUID139 may be used for a prestress static analysis in conjunction with a prestress harmonic analysis, as well
as a full transient analysis. Prestress analysis is required if the plate area changes due to the structural displacement.
A typical command sequence for a prestress harmonic analysis would include the following:

/solu

antyp,static

pstress,on

solve

fini

Section 16.4: Slide Film Damping

16–19

/solu

antyp,harmonic

pstress,on

solve

finish

KEYOPT(3) specifies the continuous flow options. For a no-slip assumption at the wall, use the continuum theory
(KEYOPT(3) = 0). For slip flow where the Knudsen number is much less or much greater than 1.0, use the first order
slip flow condition (KEYOPT(3) = 1). For slip flow with a Knudsen number of approximately 1.0, use the extended
slip flow option (KEYOPT(3) = 2).

Figure 16.13 Viscous Slide Film Element FLUID139

!#"%$&'

!("%$)'

+*&

+*& +*

,.-//021

,.-/031

,.-//04

,5-//04

,.-//04

0/78-9$&'

:+*

:/ ;

:/<*

=%>

0/78-?$)'

:% 4

:<*

:/ ;

:/<*

:/%

@BA

16.4.1. Slide Film Damping Example

Comb drive resonators are a common application for slide film damping. Figure 16.14: “Comb Drive Resonator”
illustrates a typical comb drive assembly consisting of fixed and moving comb drives, springs, and a central mass.

16–20

Chapter 16: Thin Film Analysis

Figure 16.14 Comb Drive Resonator

Details on the comb drive geometry are given in the input file listed below. The electrostatic behavior of the
moving comb drives are represented by two TRANS126 transducer elements with prescribed Stroke vs. Capacitance
data obtained from finite element runs. The structural behavior of the crab legs is modeled by a spring element.
The inertial effects of the central mass are modeled with a mass element. Damping occurs between the comb
teeth (lateral dimension), and between the comb teeth and the substrate (vertical dimension). Four FLUID139
elements are used to model the lateral and vertical damping (two per comb drive). The cut-off frequency is well
below the frequency range for the analysis; therefore, Couette flow is assumed. Since the comb drive effective
surface area changes with displacement, the DADU real constant is used (equal to the width of the plate area).

A static prestress analysis is run using a DC bias voltage on the input and output fixed comb drives. A harmonic
analysis sweep is then performed using a small AC voltage. The displacement (magnitude and phase angle) of
the central mass is shown in Figure 16.15: “Displacement of Central Mass”. Figure 16.16: “Real and Imaginary
Current” shows the current.

Figure 16.15 Displacement of Central Mass

Section 16.4: Slide Film Damping

16–21

Figure 16.16 Real and Imaginary Current

/prep7

/title Comb drive resonator with FLUID139 Couette damping

! DRIVE COMB

! |

! CRAB LEG SPRING --- CENTRAL MASS --- CRAB LEG SPRING

! |

! PICK-UP COMB

! Reference:

! "Microelectromechanical Filters for Signal Processing",

! Lin, L., Howe, R.T., J. Microelectromechanical Systems,

! VOL 7, No. 3, Sept 1998

! beam parameters (uMKS units)

E = 190e3 !Young modulus

d = 2.33e-15 ! density

hb = 2 ! beam thickness

wb = 2 ! beam width

Lb = 100 ! beam length

k = 5.699 ! mechanical stiffness

16–22

Chapter 16: Thin Film Analysis

! comb parameter

n= 9 ! number of finger

np=n*2 ! number of finger pairs

x0= 10 ! initial finger overlap

L0= 26 ! finger length (stator comb)

L=20 ! finger length (moving comb)

gi= L0-x0 ! initial gap

w= 4 ! finger width

h= hb ! finger thickness

gp=3 ! finger gap (lateral)

g= 3 ! comb gap (vertical)

Mr = 1.96563e-11 ! mass

! Lateral gap area

areal=np*h*x0

! Vertical gap area

areav=n*w*x0

! Stroke vs. Capacitance data

x1 = 14

cx1 = 0.97857e-2

x2 = 15

cx2 = 0.96669e-2

x3 = 16

cx3 = 0.95445e-2

x4 = 17

cx4 = 0.94185e-2

x5 = 18

cx5 = 0.93384e-2

! Voltage conditions

Vi = 40 ! input dc bias

Vo = 60 ! output dc bias

Vac = 10 ! input ac bias

! Damping parmeters

nu=18.3e-12 ! dynamic viscosity

po=0.1 ! reference pressure

dens=1.17e-18 ! density

fc=nu/(2*3.14159*dens*(g**2)) ! cutoff frequency

daduv=w*n ! change in plate area - vertical

dadul=h*np ! change in plate area - lateral

! Model

n,1,0

n,2,0

n,3,0

n,4,0

et,1,126,,0,1 !Trans126, UX-Volt DOF

r,1,,,gi,,

rmore,x1,cx1,x2,cx2,x3,cx3

rmore,x4,cx4,x5,cx5

e,1,2

e,2,3

et,2,21,,,4 ! Mass element

r,2,Mr

type,2

real,2

e,2

et,3,14,,1 ! linear spring, UX DOF

r,3,k

type,3

real,3

Section 16.4: Slide Film Damping

16–23

e,2,4

! Lateral dampers

et,4,139 ! Slide-film damper, Couette flow, Continuum theory

mp,visc,4,nu

mp,dens,4,dens

r,4,g,areal,-dadul,po

type,4

mat,4

real,4

e,1,2

e,2,3

! Vertical dampers

r,5,g,areav,-daduv,po

real,5

e,1,2

e,2,3

d,1,ux,0

d,3,ux,0

d,4,ux,0

d,2,uy,0

d,2,volt,0

! Prestress static analysis

/solu

d,1,volt,Vi

d,3,volt,Vo

pstres,on

solve

fini

! Harmonic Frequency Sweep

fr0=60000

fr1=120000

/solu

antyp,harm

d,1,volt,Vac ! AC voltage component on capacitor

d,3,volt,0

pstres,on ! prestress

harfrq,fr0,fr1

nsubs,60

outres,all,all

kbc,1

solve

/post26

nsol,2,2,u,x,ux2

esol,3,2,,nmisc,24,ir

esol,4,2,,nmisc,25,ii

/axlab,x,Frequency (Hz) ! label of x axis

plcplx,0

/axlab,y, Displacement (um)

plvar,2 ! plot displacement versus time (frequency)

plcplx,1

/axlab,y, Phase angle

plvar,2

plcplx,2

/axlab,y, Current (pA)

plvar,3,4

fini

16–24

Chapter 16: Thin Film Analysis

Index

acceleration, 9–12
ACEL command, 4–5, 9–12
acoustic analysis, 15–1

load step options, 15–9
loads for, 15–7
reviewing results from, 15–11

acoustics, 15–1

absolute pressure, 15–1
absorbing boundary condition, 15–2
amplitude, 15–7
applications of, 15–1
axisymmetric cases, 15–2
boundary admittance, 15–2
circular or spherical boundary (RAD), 15–2
compressible fluid, 15–1
coupled acoustic analysis, 15–1
coupling matrix, 15–11
definition of, 15–1
density, 15–2
far-field problems, 15–12
fluid load, 15–11
fluid-structure interaction, 15–1 , 15–11
fluid-structure interface, 15–5
forcing frequency, 15–7
harmonic acoustic analysis, 15–2
infinite acoustic elements, 15–2
inviscid fluid, 15–1
mean pressure, 15–1
meshing the model, 15–4
modal analysis, 15–1
outgoing pressure wave, 15–2
particle velocity, 15–1
pressure changes, 15–1
pressure gradient, 15–1
sample fluid-structure acoustic analysis (batch),
15–12
sample room acoustic analysis, 15–13
solving acoustics problems, 15–1
sound-absorption material, 15–13
speed of sound (SONC), 15–2
standing wave pattern, 15–13
transient acoustic analysis, 15–1
uncoupled acoustic analysis, 15–1
unsymmetric matrices, 15–6
wavelength, 15–4

ADAPT command, 2–2
adiabatic boundaries, 4–1
advection limit, 5–1

advection term, 14–1
ambient radiation, 4–1
amplitude, 15–7
analysis options

acoustics, 15–6

analysis type

acoustics, 15–1

angular acceleration vectors, 2–2
ANTYPE command, 2–2
Arbitrary Lagrangian-Eulerian analysis, 7–1

boundary conditions, 7–3
mesh updating, 7–5
remeshing, 7–6

arbitrary Lagrangian-Eulerian analysis

example problems, 7–8

artificial viscosity, 2–9 , 8–3
axis of rotation, 10–2

backward time integration method, 5–1
BFCUM command, 2–2
BFDELE command, 2–2
BFE command, 2–2
BFUNIF command, 2–2
Bingham viscosity model, 9–3, 9–6, 9–14
boundary conditions, 2–5, 8–2

laminar and turbulent flow, 3–11
thermal analysis, 4–1
transient analysis, 5–3

bulk temperature, 4–3
buoyancy, 4–5

Carreau viscosity model, 9–3 , 9–6 , 9–14
CE command, 2–2
CECMOD command, 2–2
CEDELE command, 2–2
CGLOC command, 10–2
CGOMEGA command, 10–2
/CLEAR command, 2–2
CNVTOL command, 2–2
collocated Galerkin approach, 4–7 , 14–1
compressible flow analysis, 1–2 , 2–4 , 3–1 , 8–1
compressible fluid, 15–1
conduction limit, 5–1
conductivity matrix algorithm, 4–5
conjugate heat transfer, 1–2, 4–5
convergence, 2–6, 2–8, 2–11 , 5–1 , 11–2
coordinate systems, 2–1 , 2–2 , 10–1
Couette flow, 16–18
coupled acoustic analysis, 15–1
coupling algorithms, 12–1

CP command, 2–2
cross-talk, 16–12

D command, 3–11 , 7–3, 10–4, 13–4
DA command, 3–11, 7–3
database

backing up, 15–10

DELTIM command, 2–2
density, 4–1 , 9–2
DESOL command, 2–2
displacements, 15–9
distributed resistance, 10–4
divergence, 2–14, 8–3
DK command, 2–2
DL command, 3–11 , 7–3
DOF capping, 2–9
domain file, 2–7
drag, 3–16
DSYM command, 2–2

effective viscosity, 2–5 , 3–2
elements, 2–1
ERESX command, 2–2
example problems

arbitrary Lagrangian-Eulerian analysis, 7–8
compressible flow, 8–4
incompressible flow, 3–16
modal projection method, 16–13
multiple species, 13–5
slide film, 16–20
squeeze film, 16–6
thermal analysis, 4–8
volume of fluid analysis, 6–5

files

Jobname.RST, 15–11

FLDATA1 command, 3–3, 4–1, 5–1
FLDATA10 command, 9–4
FLDATA11 command, 9–4
FLDATA12 command, 9–9 , 9–14
FLDATA13 command, 4–5 , 9–10
FLDATA14 command, 4–3 , 8–1 , 9–9
FLDATA15 command, 9–12
FLDATA17 command, 8–1 , 9–12
FLDATA18 command, 4–5 , 11–1
FLDATA19 command, 11–1
FLDATA2 command, 2–2, 2–6, 2–10
FLDATA20 command, 11–2, 11–3
FLDATA21 command, 11–2

FLDATA22 command, 11–2
FLDATA23 command, 11–2
FLDATA24 command, 3–3 , 3–11, 3–14 , 14–1
FLDATA25 command, 2–8 , 4–4 , 14–1
FLDATA26 command, 2–8 , 2–9
FLDATA29 command, 2–14
FLDATA3 command, 2–13
FLDATA30 command, 2–10
FLDATA31 command, 2–9 , 3–14
FLDATA32 command, 2–2 , 2–7
FLDATA33 command, 14–1
FLDATA34 command, 2–9 , 3–14, 14–1
FLDATA35 command, 6–4
FLDATA36 command, 6–3
FLDATA37 command, 4–5 , 12–1
FLDATA38 command, 5–1
FLDATA4 command, 2–2, 5–3, 6–4
FLDATA4A command, 5–1, 5–1
FLDATA5 command, 2–6, 2–6, 2–14
FLDATA7 command, 9–1, 9–3, 9–13 , 13–1
FLDATA8 command, 9–4
FLDATA9 command, 9–4
FLOCHECK command, 5–3
FLOTRAN analysis

applications, 1–1
characterizing flow, 3–3
compressible flow, 1–2 , 8–1
evaluating, 2–14
files , 2–5
fluid properties, 9–1
free surface, 1–2
incompressible flow, 1–2
laminar flow, 1–1
multiple species transport, 1–2
non-Newtonian fluid flow, 1–2
overview, 2–3
restarting, 2–7
setting parameters, 2–5
solvers, 11–1
special features, 10–1
stopping, 2–13
thermal analysis, 1–2, 4–1
transient analysis, 5–1
turbulent flow, 1–2
types, 1–1
verifying results, 2–14

FLOTRAN elements, 2–1
flow regime, 2–4

thin film, 16–4

FLREAD command, 2–6
fluid analyses

acoustics (see acoustics)

Index–2

Index

slide film, 16–18
squeeze film, 16–1
thin film, 16–1

fluid properties

initializing and varying, 9–9
specifying, 9–1
tables, 9–3
user-defined file, 9–2, 9–10
user-programmable subroutines, 9–2 , 9–14

fluid property types, 9–1
fluid-structure interaction, 15–1 , 15–9, 15–11
fluid-structure interface, 15–5
forced convection, 1–2, 4–4
forces, 15–9
forcing frequency, 15–7
free convection, 4–5
free surface analysis, 1–2

generalized symmetry boundary conditions, 3–11, 7–3
global iterations, 2–10 , 5–1, 11–2
graphical solution tracking, 2–11
gravitational acceleration, 9–12

harmonic acoustic analysis, 15–2
harmonic acoustic analysis guidelines, 15–2
heat balance, 4–7 , 4–8
heat fluxes, 4–1
heat transfer (film) coefficients, 4–1
hydraulic diameter, 3–2

IC command, 13–1
ICE command, 6–1
ICVFRC command, 6–1
impedance, 15–9
incompressible flow analysis, 1–2 , 3–1

boundary conditions, 3–11
difficult problems, 3–14
example problem, 3–16
meshing requirements, 3–9

inertial relaxation, 2–8, 8–4
infinite acoustic elements, 15–2
inlet parameters, 3–3
inlet values, 3–11
intersections, 3–11
INTSRF command, 3–16

KBC command, 2–2
KEYOPT command, 10–1, 13–2

kinetic energy, 2–5
Knudsen number, 16–4

laminar flow, 1–1 , 3–1, 3–3
large signal cases, 16–18
LCCALC command, 2–2
LCDEF command, 2–2
LCFACT command, 2–2
LCFILE command, 2–2
lift, 3–16
load step options

acoustics, 15–9

loads, 4–2, 15–6

mass imbalances, 3–11
mass types, 5–1
material model interface, 1–2
meshing, 2–4, 3–9 , 4–1
mixture types, 13–1
modal projection method, 16–10
modified inertial relaxation, 2–9, 13–4
moments, 15–9
monotone Streamline Upwind approach, 4–7
monotone streamline upwind approach, 14–1
moving wall, 3–11
MP command, 4–1, 9–1
MSADV command, 14–1
MSCAP command, 13–4
MSDATA command, 13–2 , 13–3
MSMETH command, 13–4
MSNOMF command, 13–1
MSPROP command, 13–3
MSRELAX command, 13–4
MSSOLU command, 13–4
MSSPEC command, 13–1 , 13–2, 13–3
multiple species transport, 1–2, 13–1

N command, 2–2
natural convection, 1–2
NCNV command, 2–2
NEQIT command, 2–2
Newmark time integration method, 5–1
NMODIF command, 2–2
nodal residuals file, 2–6
non-fluid properties, 4–1, 9–1
non-Newtonian fluid flow analysis, 1–2 , 9–13
non-Newtonian viscosity models, 9–3, 9–6
NROTAT command, 2–2
NSVR command, 2–2

Index

Index–3

overwrite frequency option, 2–6

particle velocity, 15–1
PERI command, 3–11
periodic boundaries, 3–11
/PICE command, 6–1
PLVFRC command, 6–5
power law viscosity model, 9–3 , 9–6, 9–13
preconditioned bicgstab solver, 11–5
preconditioned generalized minimum residual solver,
11–3
PRESOL command, 2–2
pressure gradient, 15–1
pressure surface loads, 15–9
pressure wave limit, 5–1
print file, 2–6
PRNLD command, 2–2
problem domain, 2–4
property calculations, 8–1
property types, 9–1 , 9–4
PRRSOL command, 2–2
PSOLVE command, 2–2

quadrature order, 2–10

radiosity solver method, 4–8
ratio of specific heats, 8–1, 9–12
reference pressure, 9–12
reference properties, 9–12
relaxation factors, 2–8, 4–4, 13–4
RESCONTROL command, 2–2
residuals, 2–6
restart file, 2–7
results file, 2–6
reviewing results

acoustics, 15–11

Reynolds number, 3–2
rotating reference frames, 10–2
rotational speeds, 10–2

sample acoustic analysis

batch method, 15–12

search directions, 11–2
semi-direct solvers, 11–2
SFE command, 6–2
SFL command, 6–2
SIMPLEF algorithm, 12–1

SIMPLEN algorithm, 12–1
slide film, 16–1 , 16–18
solution, 15–6
Solvers, 11–1, 15–6
sparse direct solver, 11–5 , 15–6
species mass fractions, 13–1
specific heat, 4–1, 8–1, 9–2 , 9–7
specified flow, 3–11
specified pressure, 3–11
squeeze film, 16–1
squeeze stiffness effect, 16–1
stationary wall, 3–11
stepped or ramped loads, 15–10
Stokes flow, 16–18
streamline upwind/Petrov-Galerkin approach, 4–7,
14–1
surface tension coefficient, 6–1 , 9–1 , 9–3, 9–8
surface-to-surface radiation, 4–1 , 4–8
Sutherland's law, 9–6
swirl, 10–3
symmetry boundary, 3–11

temperature equation, 4–1
temperature field algorithm, 4–5
temperature load, 4–1
temperature offset, 9–9
thermal analysis, 1–2

example problems, 4–8
loads and boundary conditions, 4–1
property specifications, 4–1

thermal boundary conditions, 4–1
thermal conductivity, 4–1 , 9–2 , 9–8
thin film analysis, 16–1

Couette vs. Stokes flow, 16–18
cross-talk, 16–12
flow regime, 16–4
harmonic response analysis, 16–3
large signal cases, 16–18
modal projection method, 16–10
slide film, 16–18
squeeze film, 16–1
static analysis, 16–2

TIME command, 2–2
time steps, 5–1
TIMINT command, 2–2
TOFFST command, 9–9, 9–12
total temperature, 8–1
transient analysis, 5–1

boundary conditions, 5–3
settings, 5–1
terminating, 5–3

Index–4

Index

tri-diagonal matrix algorithm, 11–1
TRNOPT command, 2–2
turbulence model, 2–4 , 2–10, 3–2, 3–3
turbulence ratio, 3–3, 3–14
turbulent flow, 1–2, 3–1
turbulent kinetic energy, 3–3, 3–11

uncoupled acoustic analysis, 15–1
units, 9–1
unspecified boundary, 3–11

variable density option, 4–5
velocity capping, 3–14
viscosity, 4–1

artificial, 2–9
Bingham model, 9–3, 9–6, 9–14
Carreau model, 9–3 , 9–6, 9–14
effective, 2–5 , 3–2
power law model, 9–3, 9–6, 9–13

viscous heating, 4–4
volume of fluid analysis, 6–1

boundary conditions, 6–2
example problems, 6–5
input settings, 6–3
loads, 6–1
postprocessing, 6–5

wall roughness, 3–11
wall static contact angle, 9–1 , 9–3 , 9–9

Index

Index–5

Document Outline

ANSYS Fluids Analysis Guide
Table of Contents
Part I. CFD
Part II. Acoustics
- Chapter 15: Acoustics
Part III. Thin Film
- Chapter 16: Thin Film Analysis
Index

Wyszukiwarka

Podobne podstrony:
Ansys Thermal Analysis Guide id Nieznany (2)
performance analysis guide
ANSYS LS Dyna User's Guide
Finite Element Analysis with ANSYS
Chizzola GC analysis of essential oils in the rumen fluid after incubation of Thuja orientalis tw
Analysis of Reinforced Concrete Structures Using ANSYS Nonlinear Concrete Model
Chizzola GC analysis of essential oils in the rumen fluid after incubation of Thuja orientalis tw
Forex, Foreign Exchange, Currency, Technical Analysis, Elliot Wave Theory, Trading Guide
16 0 ANSYS Quick Start Licensing Guide
Great Burgundy Wines A Principal Components Analysis of La Cote vineyards guide
Finite Element Analysis with ANSYS
16 0 ANSYS Quick Start Installation Guide
Analysing Power in Language A Practical Guide (T Bartlett)
GbpUsd analysis for July 06 Part 1

więcej podobnych podstron

ANSYS Fluid Analysis Guide

Document Outline