Ansys 11 tutorial

ANSYS CFX
Tutorials

ANSYS CFX Release 11.0

December 2006

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
© 1996-2006 ANSYS Europe, Ltd. All rights reserved. Unauthorized use, distribution, or duplication is
prohibited.
ANSYS, ANSYS Workbench, AUTODYN, CFX, FLUENT and any and all ANSYS, Inc. brand, product, service
and feature names, logos and slogans are registered trademarks or trademarks of ANSYS, Inc. or its
subsidiaries located in the United States or other countries. ICEM CFD is a trademark used by ANSYS, Inc.
under license. CFX is a trademark of Sony Corporation in Japan. All other brand, product, service and
feature names or trademarks are the property of their respective owners.

Disclaimer Notice
THIS ANSYS SOFTWARE PRODUCT AND PROGRAM DOCUMENTATION INCLUDE TRADE SECRETS AND ARE
CONFIDENTIAL AND PROPRIETARY PRODUCTS OF ANSYS, INC., ITS SUBSIDIARIES, OR LICENSORS. The
software products and documentation are furnished by ANSYS, Inc., its subsidiaries, or affiliates under a
software license agreement that contains provisions concerning non-disclosure, copying, length and
nature of use, compliance with exporting laws, warranties, disclaimers, limitations of liability, and
remedies, and other provisions. The software products and documentation may be used, disclosed,
transferred, or copied only in accordance with the terms and conditions of that software license
agreement.
ANSYS, Inc. and ANSYS Europe, Ltd. are UL registered ISO 9001:2000 companies.

U.S. Government Rights
For U.S. Government users, except as specifically granted by the ANSYS, Inc. software license agreement,
the use, duplication, or disclosure by the United States Government is subject to restrictions stated in the
ANSYS, Inc. software license agreement and FAR 12.212 (for non DOD licenses).

Third-Party Software
See the online documentation in the product help files for the complete Legal Notice for ANSYS
proprietary software and third-party software. The ANSYS third-party software information is also
available via download from the Customer Portal on the ANSYS web page. If you are unable to access the
third-party legal notices, please contact ANSYS, Inc.
Published in the U.S.A.

Table of Contents
Copyright and Trademark Information

Disclaimer Notice

U.S. Government Rights

Third-Party Software

Introduction to the
ANSYS CFX Tutorials

Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1
Setting the Working Directory . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1
Changing the Display Colors. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2

Tutorial 1:
Simulating Flow in a Static Mixer Using CFX in Standalone Mode

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3
Before You Begin . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4
Tutorial 1 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4
Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5
Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6
Obtaining a Solution Using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .12
Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .15

Tutorial 1a:
Simulating Flow in a Static Mixer Using Workbench

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .31
Before You Begin . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .32
Tutorial 1a Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .32

ANSYS CFX Tutorials Page v

Table of Contents: Tutorial 2: Flow in a Static Mixer (Refined Mesh)
Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .33
Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .34

Tutorial 2:
Flow in a Static Mixer
(Refined Mesh)

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .59
Tutorial 2 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .60
Defining a Simulation using General Mode in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .61
Obtaining a Solution Using Interpolation with ANSYS CFX-Solver . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .66

Tutorial 3:
Flow in a Process Injection Mixing Pipe

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .77
Defining a Simulation using General Mode in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .79

Tutorial 4:
Flow from a Circular Vent

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .93
Defining a Steady-State Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .95
Obtaining a Solution to the Steady-State Problem . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .99
Defining a Transient Simulation in ANSYS CFX-Pre. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 100
Obtaining a Solution to the Transient Problem . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 104
Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 105

Tutorial 5:
Flow Around a Blunt Body

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 109
Tutorial 5 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 109
Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 111
Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 111

Page vi ANSYS CFX Tutorials

Table of Contents: Tutorial 6: Buoyant Flow in a Partitioned Cavity
Obtaining a Solution Using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 116

Tutorial 6:
Buoyant Flow in a Partitioned Cavity

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 127
Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 134

Tutorial 7:
Free Surface Flow Over a Bump

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 139
Using a Supercritical Outlet Condition . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 154

Tutorial 8:
Supersonic Flow Over a Wing

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 155

Tutorial 9:
Flow Through a Butterfly Valve

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 165

Tutorial 10:

ANSYS CFX Tutorials Page vii

Table of Contents: Tutorial 11: Non-Newtonian Fluid Flow in an Annulus
Flow in a Catalytic Converter

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 185
Tutorial 10 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 185

Tutorial 11:
Non-Newtonian Fluid Flow in an Annulus

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 199

Tutorial 12:
Flow in an Axial Rotor/Stator

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 207
Defining a Frozen Rotor Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 210
Obtaining a Solution to the Frozen Rotor Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 214
Viewing the Frozen Rotor Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 215
Setting up a Transient Rotor-Stator Calculation. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 216
Obtaining a Solution to the Transient Rotor-Stator Model. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 219
Viewing the Transient Rotor-Stator Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 220

Tutorial 13:
Reacting Flow in a Mixing Tube

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 223
Outline of the Process . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 224

Tutorial 14:

Page viii ANSYS CFX Tutorials

Table of Contents: Tutorial 15: Multiphase Flow in Mixing Vessel
Conjugate Heat Transfer in a Heating Coil

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 239
Exporting the Results to ANSYS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 247

Tutorial 15:
Multiphase Flow in Mixing Vessel

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 251

Tutorial 16:
Gas-Liquid Flow in an Airlift Reactor

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 269
Additional Fine Mesh Simulation Results . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 280

Tutorial 17:
Air Conditioning Simulation

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 283

Tutorial 18:
Combustion and Radiation in a Can Combustor

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 299

ANSYS CFX Tutorials Page ix

Table of Contents: Tutorial 19: Cavitation Around a Hydrofoil
Using Eddy Dissipation and P1 Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 301
Laminar Flamelet and Discrete Transfer Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 311
Further Postprocessing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 316

Tutorial 19:
Cavitation Around a Hydrofoil

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 317
Creating an Initial Simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 319
Obtaining an Initial Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 323
Viewing the Results of the Initial Simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 324
Preparing a Simulation with Cavitation. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 326
Obtaining a Cavitation Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 328
Viewing the Results of the Cavitation Simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 328

Tutorial 20:
Fluid Structure Interaction and Mesh Deformation

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 331
Using CEL Expressions to Govern Mesh Deformation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 334
Using a Junction Box Routine to Govern Mesh Deformation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 343

Tutorial 21:
Oscillating Plate with Two-Way Fluid-Structure Interaction

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 353
Setting up the Solid Physics in Simulation (ANSYS Workbench) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 355
Setting up the Fluid Physics and ANSYS Multi-field Settings in ANSYS CFX-Pre. . . . . . . . . . . . . . . . . . . . . . . . . 358
Viewing Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 365

Tutorial 22:

Page x ANSYS CFX Tutorials

Table of Contents: Tutorial 23: Aerodynamic & Structural Performance of a Centrifugal Compressor
Optimizing Flow in a Static Mixer

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 369
Creating the Project . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 371
Creating the Geometry . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 372
Creating the Mesh. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 377
Overview of ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 380
Setting the Output Parameter in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 386
Running Design Studies in DesignXplorer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 387

Tutorial 23:
Aerodynamic & Structural Performance of a Centrifugal Compressor

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 395
Reviewing the Centrifugal Compressor Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 397
Creating the Mesh in ANSYS TurboGrid . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 398
Defining the Aerodynamic Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 401
Importing Geometry into DesignModeler . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 405
Simulating Structural Stresses Due to Pressure Loads . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 406
Simulating Structural Stresses Due to Rotation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 407

ANSYS CFX Tutorials Page xi

Table of Contents: Tutorial 23: Aerodynamic & Structural Performance of a Centrifugal Compressor

Page xii ANSYS CFX Tutorials

Introduction to the
ANSYS CFX Tutorials

Overview
These tutorials are designed to introduce general techniques used in ANSYS CFX and
provide tips on advanced modeling.
Earlier tutorials introduce general principles used in ANSYS CFX, including setting up the
physical models, running ANSYS CFX-Solver and visualizing the results. The remaining
tutorials highlight specialized features of ANSYS CFX.
Files required to complete each tutorial is listed in the introduction to the tutorial, and
located in <CFXROOT>/examples, where <CFXROOT> is the installation directory.

Setting the Working Directory
One of the first things you must do when using ANSYS CFX is to set a working directory. The
working directory is the default location for loading and saving files for a particular session
or project.
The working directory is set according to how you run ANSYS CFX:
• Workbench
Set the working directory by saving a project file.
• Standalone
Set the working directory by entering it in CFX Launcher.

ANSYS CFX Tutorials Page 1
ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Introduction to the ANSYS CFX Tutorials: Changing the Display Colors

Changing the Display Colors
If viewing objects in ANSYS CFX becomes difficult due to contrast with the background, the
colors can be altered for improved viewing. The color options are set in different places,
depending on how you run ANSYS CFX, as follows:
• In standalone mode (i.e., after using CFX Launcher to launch ANSYS CFX-Pre or ANSYS
CFX-Post):
a. Select Edit > Options.
The Options dialog box appears.
b. Adjust the color settings under CFX-Pre > Viewer (for ANSYS CFX-Pre) or CFX-Post
> Viewer (for ANSYS CFX-Post).
c. Click OK.
• In ANSYS Workbench:
a. Select Tools > Options from the Project page.
b. Adjust the color settings under Common Settings > Graphics Style.
c. Click OK.

Page 2 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.

Tutorial 1:
Simulating Flow in a Static
Mixer Using CFX in Standalone
Mode

Introduction
This tutorial simulates a static mixer consisting of two inlet pipes delivering water into a
mixing vessel; the water exits through an outlet pipe. A general workflow is established for
analyzing the flow of fluid into and out of a mixer.
This tutorial includes:
• Before You Begin (p. 4)
• Tutorial 1 Features (p. 4)
• Overview of the Problem to Solve (p. 5)
• Defining a Simulation in ANSYS CFX-Pre (p. 6)
• Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 12)
• Viewing the Results in ANSYS CFX-Post (p. 15)

If this is the first tutorial you are working with, it is important to review the following topics
before beginning:
• Setting the Working Directory (p. 1)
• Changing the Display Colors (p. 2)
To learn how to perform these tasks in Workbench, see Tutorial 1a: Simulating Flow in a
Static Mixer Using Workbench (p. 31 in "ANSYS CFX Tutorials").


Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Before You Begin

Before You Begin
Create a working directory for your files. Once this is done, copy the sample files used in this
tutorial to your working directory from the installation folder for your software
(<CFXROOT>/examples/ (for example, C:Program FilesANSYS
Incv110CFXexamples)) to avoid overwriting source files provided with your
installation. If you plan to use a session file, please refer to Playing a Session File (p. 7).
Sample files used by this tutorial are:
• StaticMixerMesh.gtm
• StaticMixer.pre

Tutorial 1 Features
This tutorial addresses the following features of ANSYS CFX.

Component Feature Details
ANSYS CFX-Pre User Mode Quick Setup Wizard
Simulation Type Steady State
Fluid Type General Fluid
Domain Type Single Domain
Turbulence Model k-Epsilon
Heat Transfer Thermal Energy
Boundary Conditions Inlet (Subsonic)
Outlet (Subsonic)
Wall: No-Slip
Wall: Adiabatic
Timestep Physical Time Scale
ANSYS CFX-Post Plots Animation
Contour
Outline Plot (Wireframe)
Point
Slice Plane
Streamline

In this tutorial you will learn about:
• Using Quick Setup mode in ANSYS CFX-Pre to set up a problem.
• Modifying the outline plot in ANSYS CFX-Post.
• Using streamlines in ANSYS CFX-Post to trace the flow field from a point.
• Viewing temperature using colored planes and contours in ANSYS CFX-Post.
• Creating an animation and saving it to an MPEG file.


Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Overview of the Problem to Solve

Overview of the Problem to Solve
Water enters through both pipes at the same rate but at different temperatures. The first
entry is at a rate of 2 m/s and a temperature of 315 K and the second entry is at a rate of 2
m/s at a temperature of 285 K. The radius of the mixer is 2 m.
Your goal in this tutorial is to understand how to use ANSYS CFX to determine the speed and
temperature of the water when it exits the static mixer.
Figure 1 Static Mixer with 2 Inlet Pipes and 1 Outlet Pipe
2 m/s
r=2m 285 K

2 m/s
315 K

ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 5

Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Defining a Simulation in ANSYS CFX-Pre

Defining a Simulation in ANSYS CFX-Pre
Because you are starting with an existing mesh, you can immediately use ANSYS CFX-Pre to
define the simulation. This is how ANSYS CFX-Pre will look with the imported mesh:

In the image above, the left pane of ANSYS CFX-Pre displays the Outline . When you
double-click on items in the Outline, the Outline editor opens and can be used to create,
modify, and view objects.

Note: In this documentation, the details view can also be referenced by the name of the
object being edited, followed by the word “details view” (for example, if you double-click
the Wireframe object, the Wireframe details view appears).

Synopsis of Quick Setup Mode
Quick Setup mode provides a simple wizard–like interface for setting up simple cases. This
is useful for getting familiar with the basic elements of a CFD problem setup. This section
describes using Quick Setup mode to develop a simulation in ANSYS CFX-Pre.

Workflow Overview
This tutorial follows the general workflow for Quick Setup mode:
1. Creating a New Simulation (p. 7)
2. Setting the Physics Definition (p. 7)
3. Importing a Mesh (p. 7)
4. Defining Model Data (p. 9)
5. Defining Boundaries (p. 9)

6. Setting Boundary Data (p. 9)
7. Setting Flow Specification (p. 9)
8. Setting Temperature Specification (p. 10)
9. Reviewing the Boundary Condition Definitions (p. 10)
10. Creating the Second Inlet Boundary Definition (p. 10)
11. Creating the Outlet Boundary Definition (p. 10)
12. Moving to General Mode (p. 11)
13. Writing the Solver (.def) File (p. 11)

Playing a If you want to skip past these instructions and have ANSYS CFX-Pre set up the simulation
Session File automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre,
then run the appropriate session file. For details, see Playing the Session File and Starting
ANSYS CFX-Solver Manager (p. 12). After you have played the session file, proceed to
Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 12).

Creating a New Simulation
Before importing and working with a mesh, a simulation needs to be started using Quick
Setup mode.

Procedure 1. If required, launch ANSYS CFX-Pre.
2. Select File > New Simulation.
The New Simulation File dialog box is displayed.
3. Select Quick Setup and click OK.
Note: If this is the first time you are running this software, a message box will appear
notifying you that automatic generation of the default domain is active. To avoid seeing this
message again uncheck Show This Message Again.
4. Select File > Save Simulation As.
5. Under File name, type: StaticMixer
6. Click Save.

Setting the Physics Definition
You need to specify the fluids used in a simulation. A variety of fluids are already defined as
library materials. For this tutorial you will use a prepared fluid, Water, which is defined to be
water at 25°C.

Procedure 1. Ensure that Simulation Definition is displayed at the top of the details view.
2. Under Fluid select Water.

Importing a Mesh
At least one mesh must be imported before physics are applied.

Procedure 1. In Simulation Definition, under Mesh File, click Browse .
The Import Mesh dialog box appears.

2. Under File type, select CFX Mesh (*gtm *cfx).
3. From your working directory, select StaticMixerMesh.gtm.
4. Click Open.
The mesh loads.
5. Click Next.

Using the Viewer
Now that the mesh is loaded, take a moment to explore how you can use the viewer toolbar
to zoom in or out and to rotate the object in the viewer.

Using the Zoom There are several icons available for controlling the level of zoom in the viewer.
Tools
1. Click Zoom Box
2. Click and drag a rectangular box over the geometry.
3. Release the mouse button to zoom in on the selection.
The geometry zoom changes to display the selection at a greater resolution.

4. Click Fit View to re-center and re-scale the geometry.

Rotating the If you need to rotate an object or to view it from a new angle, you can use the viewer toolbar.
geometry
1. Click Rotate on the viewer toolbar.
2. Click and drag within the geometry repeatedly to test the rotation of the geometry.
The geometry rotates based on the direction of movement.
Notice how the mouse cursor changes depending on where you are in the viewer:

3. Right-click a blank area in the viewer and select Predefined Camera > View
Towards-X).
4. Right-click a blank area in the viewer and select Predefined Camera > Isometric View
(Z Up).
A clearer view of the mesh is displayed.



Defining Model Data
You need to define the type of flow and the physical models to use in the fluid domain.
You will specify the flow as steady state with turbulence and heat transfer. Turbulence is
modeled using the k - ε turbulence model and heat transfer using the thermal energy
model. The k - ε turbulence model is a commonly used model and is suitable for a wide
range of applications. The thermal energy model neglects high speed energy effects and is
therefore suitable for low speed flow applications.

Procedure 1. Ensure that Physics Definition is displayed.
2. Under Model Data, set Reference Pressure to 1 [atm].
All other pressure settings are relative to this reference pressure.
3. Set Heat Transfer to Thermal Energy.
4. Set Turbulence to k-Epsilon.
5. Click Next.

Defining Boundaries
The CFD model requires the definition of conditions on the boundaries of the domain.

Procedure 1. Ensure that Boundary Definition is displayed.
2. Delete Inlet and Outlet from the list by right-clicking each and selecting Delete.
3. Right-click in the blank area where Inlet and Outlet were listed, then select New.
4. Set Name to in1.
5. Click OK.
The boundary is created and, when selected, properties related to the boundary are
displayed.

Setting Boundary Data
Once boundaries are created, you need to create associated data. Based on Figure 1, you will
define the first inlet boundary condition’s velocity and temperature.

Procedure 1. Ensure that Boundary Data is displayed.
2. Set Boundary Type to Inlet.
3. Set Location to in1.

Setting Flow Specification
Once boundary data is defined, the boundary needs to have the flow specification assigned.

Procedure 1. Ensure that Flow Specification is displayed.
2. Set Option to Normal Speed.
3. Set Normal Speed to 2 [m s^-1].



Setting Temperature Specification
Once flow specification is defined, the boundary needs to have temperature assigned.

Procedure 1. Ensure that Temperature Specification is displayed.
2. Set Static Temperature to 315 [K].

Reviewing the Boundary Condition Definitions
Defining the boundary condition for in1 required several steps. Here the settings are
reviewed for accuracy.
Based on Figure 1, the first inlet boundary condition consists of a velocity of 2 m/s and a
temperature of 315 K at one of the side inlets.

Procedure 1. Review the boundary in1 settings for accuracy. They should be as follows:

Tab Setting Value
Boundary Data Boundary Type Inlet
Location in1
Flow Specification Option Normal Speed
Normal Speed 2 [m s^-1]
Temperature Specification Static Temperature 315 [K]

Creating the Second Inlet Boundary Definition
Based on Figure 1, you know the second inlet boundary condition consists of a velocity of 2
m/s and a temperature of 285 K at one of the side inlets. You will define that now.

Procedure 1. Under Boundary Definition, right-click in the selector area and select New.
2. Create a new boundary named in2 with these settings:

Tab Setting Value
Location in2

Creating the Outlet Boundary Definition
Now that the second inlet boundary has been created, the same concepts can be applied to
building the outlet boundary.
1. Create a new boundary named out with these settings:



Tab Setting Value
Boundary Data Boundary Type Outlet
Location out
Flow Specification Option Average Static Pressure
Relative Pressure 0 [Pa]

2. Click Next.

Moving to General Mode
There are no further boundary conditions that need to be set. All 2D exterior regions that
have not been assigned to a boundary condition are automatically assigned to the default
boundary condition.

Procedure 1. Set Operation to Enter General Mode and click Finish.
The three boundary conditions are displayed in the viewer as sets of arrows at the
boundary surfaces. Inlet boundary arrows are directed into the domain. Outlet
boundary arrows are directed out of the domain.

Setting Solver Control
Solver Control parameters control aspects of the numerical solution generation process.
While an upwind advection scheme is less accurate than other advection schemes, it is also
more robust. This advection scheme is suitable for obtaining an initial set of results, but in
general should not be used to obtain final accurate results.
The time scale can be calculated automatically by the solver or set manually. The Automatic
option tends to be conservative, leading to reliable, but often slow, convergence. It is often
possible to accelerate convergence by applying a time scale factor or by choosing a manual
value that is more aggressive than the Automatic option. In this tutorial, you will select a
physical time scale, leading to convergence that is twice as fast as the Automatic option.

Procedure 1. Click Solver Control .
2. On the Basic Settings tab, set Advection Scheme > Option to Upwind.
3. Set Convergence Control > Fluid Timescale Control > Timescale Control to
Physical Timescale and set the physical timescale value to 2 [s].
4. Click OK.

Writing the Solver (.def) File
The simulation file, StaticMixer.cfx, contains the simulation definition in a format that
can be loaded by ANSYS CFX-Pre, allowing you to complete (if applicable), restore, and
modify the simulation definition. The simulation file differs from the definition file in that it
can be saved at any time while defining the simulation.

Procedure 1. Click Write Solver File .


Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Obtaining a Solution Using ANSYS
The Write Solver File dialog box is displayed.
2. Set File name to StaticMixer.def.
3. Ensure that Start Solver Manager is selected from the drop down menu located in
the top-right corner of the dialog box.
4. Select Quit ANSYS CFX-Pre.
This forces standalone ANSYS CFX-Pre to close after the definition file has been written.
5. Click Save.
6. If you are notified the file already exists, click Overwrite.
This file is provided in the tutorial directory and may exist in your tutorial folder if you
have copied it there.
7. If prompted, click Yes or Save & Quit to save StaticMixer.cfx.
The definition file (StaticMixer.def) and the simulation file (StaticMixer.cfx) are
created. ANSYS CFX-Solver Manager automatically starts and the definition file is set in
the Define Run dialog box.
8. Proceed to Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 12).

Playing the Session File and Starting ANSYS CFX-Solver Manager
Note: This task is required only if you are starting here with the session file that was provided
in the examples directory. If you have performed all the tasks in the previous steps, proceed
directly to Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 12).
Events in ANSYS CFX-Pre can be recorded to a session file and then played back at a later
date to drive ANSYS CFX-Pre. Session files have been created for each tutorial so that the
problems can be set up rapidly in ANSYS CFX-Pre, if desired.

Procedure 1. If required, launch ANSYS CFX-Pre.
2. Select Session > Play Tutorial.
3. Select StaticMixer.pre.
4. Click Open.
A definition file is written.
5. Select File > Quit.
6. Launch the ANSYS CFX-Solver Manager from CFX Launcher.
7. After the ANSYS CFX-Solver starts, select File > Define Run.

8. Under Definition File, click Browse .
9. Select StaticMixer.def, located in the working directory.

Obtaining a Solution Using ANSYS CFX-Solver Manager
ANSYS CFX-Solver Manager has a visual interface that displays a variety of results and should
be used when plotted data needs to be viewed during problem solving.


Two windows are displayed when ANSYS CFX-Solver Manager runs. There is an adjustable
split between the windows, which is oriented either horizontally or vertically depending on
the aspect ratio of the entire ANSYS CFX-Solver Manager window (also adjustable).

One window shows the convergence history plots and the other displays text output from
ANSYS CFX-Solver.
The text lists physical properties, boundary conditions and various other parameters used
or calculated in creating the model. All the text is written to the output file automatically (in
this case, StaticMixer_001.out).

Start the Run
The Define Run dialog box allows configuration of a run for processing by ANSYS
CFX-Solver.
When ANSYS CFX-Solver Manager is launched automatically from ANSYS CFX-Pre, all of the
information required to perform a new serial run (on a single processor) is entered
automatically. You do not need to alter the information in the Define Run dialog box. This
is a very quick way to launch into ANSYS CFX-Solver without having to define settings and
values.

Procedure 1. Ensure that the Define Run dialog box is displayed.
2. Click Start Run.


ANSYS CFX-Solver launches and a split screen appears and displays the results of the run
graphically and as text. The panes continue to build as ANSYS CFX-Solver Manager
operates.
Note: Once the second iteration appears, data begins to plot. Plotting may take a long time
depending on the amount of data to process. Let the process run.

Move from ANSYS CFX-Solver to ANSYS CFX-Post
Once ANSYS CFX-Solver has finished, you can use ANSYS CFX-Post to review the finished
results.

Procedure 1. When ANSYS CFX-Solver is finished, click Yes to post-process the results.

After a short pause, ANSYS CFX-Post starts and ANSYS CFX-Solver Manager closes.


Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-Post

Viewing the Results in ANSYS CFX-Post
When ANSYS CFX-Post starts, the viewer and Outline workspace are displayed.

The viewer displays an outline of the geometry and other graphic objects. You can use the
mouse or the toolbar icons to manipulate the view, exactly as in ANSYS CFX-Pre.

Workflow Overview
This tutorial describes the following workflow for viewing results in ANSYS CFX-Post:
1. Setting the Edge Angle for a Wireframe Object (p. 16)
2. Creating a Point for the Origin of the Streamline (p. 17)
3. Creating a Streamline Originating from a Point (p. 18)
4. Rearranging the Point (p. 19)
5. Configuring a Default Legend (p. 19)
6. Creating a Slice Plane (p. 20)
7. Defining Slice Plane Geometry (p. 21)
8. Configuring Slice Plane Views (p. 21)
9. Rendering Slice Planes (p. 22)
10. Coloring the Slice Plane (p. 23)
11. Moving the Slice Plane (p. 23)
12. Adding Contours (p. 24)
13. Working with Animations (p. 25)
14. Showing the Animation Dialog Box (p. 25)


15. Creating the First Keyframe (p. 26)
16. Creating the Second Keyframe (p. 26)
17. Viewing the Animation (p. 27)
18. Modifying the Animation (p. 28)
19. Saving to MPEG (p. 29)

Setting the Edge Angle for a Wireframe Object
The outline of the geometry is called the wireframe or outline plot.
By default, ANSYS CFX-Post displays only some of the surface mesh. This sometimes means
that when you first load your results file, the geometry outline is not displayed clearly. You
can control the amount of the surface mesh shown by editing the Wireframe object listed
in the Outline.
The check boxes next to each object name in the Outline control the visibility of each
object. Currently only the Wireframe and Default Legend objects have visibility selected.
The edge angle determines how much of the surface mesh is visible. If the angle between
two adjacent faces is greater than the edge angle, then that edge is drawn. If the edge angle
is set to 0°, the entire surface mesh is drawn. If the edge angle is large, then only the most
significant corner edges of the geometry are drawn.
For this geometry, a setting of approximately 15° lets you view the model location without
displaying an excessive amount of the surface mesh.
In this module you can also modify the zoom settings and view of the wireframe.

Procedure 1. In the Outline, under User Locations and Plots, double-click Wireframe.
Tip: While it is not necessary to change the view to set the angle, do so to explore the
practical uses of this feature.
2. Right-click on a blank area anywhere in the viewer, select Predefined Camera from the
shortcut menu and select Isometric View (Z up).
3. In the Wireframe details view, under Definition, click in the Edge Angle box.
An embedded slider is displayed.
4. Type a value of 10 [degree].
5. Click Apply to update the object with the new setting.


Notice that more surface mesh is displayed.

6. Drag the embedded slider to set the Edge Angle value to approximately 45 [degree].
Less of the outline of the geometry is displayed.
shortcut menu and select View Towards -X.

Creating a Point for the Origin of the Streamline
A streamline is the path that a particle of zero mass would follow through the domain.

Procedure 1. Select Insert > Location > Point from the main menu.
You can also use the toolbars to create a variety of objects. Later modules and tutorials
explore this further.
2. Click OK.
This accepts the default name.
3. Under Definition, ensure that Method is set to XYZ.
4. Under Point, enter the following coordinates: -1, -1, 1.
This is a point near the first inlet.
5. Click Apply.
The point appears as a symbol in the viewer as a crosshair symbol.



Creating a Streamline Originating from a Point
Where applicable, streamlines can trace the flow direction forwards (downstream) and/or
backwards (upstream).

Procedure 1. From the main menu, select Insert > Streamline.
will explore this further.
2. Click OK.
3. Under Definition, in Start From, ensure that Point 1 is set.
Tip: To create streamlines originating from more than one location, click the ellipsis icon
to the right of the Start From box. This displays the Location Selector dialog box,
where you can use the <Ctrl> and <Shift> keys to pick multiple locators.
4. Click the Color tab.
5. Set Mode to Variable.
6. Set Variable to Total Temperature.
7. Set Range to Local.
8. Click Apply.
The streamline shows the path of a zero mass particle from Point 1. The temperature
is initially high near the hot inlet, but as the fluid mixes the temperature drops.



Rearranging the Point
Once created, a point can be rearranged manually or by setting specific coordinates.
Tip: In this module, you may choose to display various views and zooms from the
Predefined Camera option in the shortcut menu (such as Isometric View (Z up) or
View Towards -X) and by using Zoom Box if you prefer to change the display.

Procedure 1. In Outline, under User Locations and Plots double-click Point 1.
Properties for the selected user location are displayed.
2. Under Point, set these coordinates: -1, -2.9, 1.
3. Click Apply.
The point is moved and the streamline redrawn.
4. In the selection tools, click Single Select.

While in this mode, the normal behavior of the left mouse button is disabled.
5. In the viewer, drag Point 1 (appears as a yellow addition sign) to a new location within
the mixer.
The point position is updated in the details view and the streamline is redrawn at the
new location. The point moves normal in relation to the viewing direction.

6. Click Rotate .
Tip: You can also click in the viewer area, and press the space bar to toggle between
Select and Viewing Mode. A way to pick objects from Viewing Mode is to hold down
<Ctrl> + <Shift> while clicking on an object with the left mouse button.
7. Under Point, reset these coordinates: -1, -1, 1.
8. Click Apply.
The point appears at its original location.
9. Right-click a blank area in the viewer and select Predefined Camera > View Towards
-X.

Configuring a Default Legend
You can modify the appearance of the default legend.
The default legend appears whenever a plot is created that is colored by a variable. The
streamline color is based on temperature; therefore, the legend shows the temperature
range. The color pattern on the legend’s color bar is banded in accordance with the bands
in the plot1.

1. An exception occurs when one or more bands in a contour plot represent values beyond the
legend’s range. In this case, such bands are colored using a color that is extrapolated slightly
past the range of colors shown in the legend. This can happen only when a user-specified
range is used for the legend.


The default legend displays values for the last eligible plot that was opened in the details
view. To maintain a legend definition during an ANSYS CFX-Post session, you can create a
new legend by clicking Legend .
Because there are many settings that can be customized for the legend, this module allows
you the freedom to experiment with them. In the last steps you will set up a legend, based
on the default legend, with a minor modification to the position.
Tip: When editing values, you can restore the values that were present when you began
editing by clicking Reset. To restore the factory-default values, click Default.

Procedure 1. Double click Default Legend View 1.
The Definition tab of the default legend is displayed.
2. Apply the following settings

Tab Setting Value
Definition Title Mode User Specified
Title Streamline Temp.
Horizontal (Selected)
Location > Y Justification Bottom

3. Click Apply.
The appearance and position of the legend changes based on the settings specified.
4. Modify various settings in Definition and click Apply after each change.
5. Select Appearance.
6. Modify a variety of settings in the Appearance and click Apply after each change.
7. Click Defaults.
8. Click Apply.
9. Under Outline, in User Locations and Plots, clear the check boxes for Point 1 and
Streamline 1.
Since both are no longer visible, the associated legend no longer appears.

Creating a Slice Plane
Defining a slice plane allows you to obtain a cross–section of the geometry.
In ANSYS CFX-Post you often view results by coloring a graphic object. The graphic object
could be an isosurface, a vector plot, or in this case, a plane. The object can be a fixed color
or it can vary based on the value of a variable.
You already have some objects defined by default (listed in the Outline). You can view
results on the boundaries of the static mixer by coloring each boundary object by a variable.
To view results within the geometry (that is, on non-default locators), you will create new
objects.
You can use the following methods to define a plane:
• Three Points: creates a plane from three specified points.


• Point and Normal: defines a plane from one point on the plane and a normal vector
to the plane.
• YZ Plane, ZX Plane, and XY Plane: similar to Point and Normal, except that the
normal is defined to be normal to the indicated plane.

Procedure 1. From the main menu, select Insert > Location > Plane or click Location > Plane.
2. In the New Plane window, type: Slice
3. Click OK.
The Geometry, Color, Render and View tabs let you switch between settings.
4. Click the Geometry tab.

Defining Slice Plane Geometry
You need to choose the vector normal to the plane. You want the plane to lie in the x-y
plane, hence its normal vector points along the z-axis. You can specify any vector that points
in the z-direction, but you will choose the most obvious (0,0,1).

Procedure 1. If required, under Geometry, expand Definition.
2. Under Method select Point and Normal.
3. Under Point enter 0,0,1.
4. Under Normal enter 0, 0,1.
5. Click Apply.
Slice appears under User Locations and Plots. Rotate the view to see the plane.

Configuring Slice Plane Views
Depending on the view of the geometry, various objects may not appear because they fall
in a 2D space that cannot be seen.

Procedure 1. Right-click a blank area in the viewer and select Predefined Camera > Isometric View
(Z up).


The slice is now visible in the viewer.

2. Click Zoom Box .
3. Click and drag a rectangular selection over the geometry.

5. Click Rotate .
6. Click and drag the mouse pointer down slightly to rotate the geometry towards you.
7. Select Isometric View (Z up) as described earlier.

Rendering Slice Planes
Render settings determine how the plane is drawn.

Procedure 1. Select the Render tab.
2. Clear Draw Faces.
3. Select Draw Lines.
4. Under Draw Lines change Color Mode to User Specified.
5. Click the current color in Line Color to change to a different color.
For a greater selection of colors, click the ellipsis to use the Select color dialog box.
6. Click Apply.

7. Click Zoom Box .
8. Zoom in on the geometry to view it in greater detail.


The line segments show where the slice plane intersects with mesh element faces. The
end points of each line segment are located where the plane intersects mesh element
edges.
-Z.
The image shown below can be used for comparison with tutorial 2 (in the section
Creating a Slice Plane (p. 68)), where a refined mesh is used.

Coloring the Slice Plane
The Color panel is used to determine how the object faces are colored.

Procedure 1. Apply the following settings to Slice

Tab Setting Value
Color Mode Variable*
Variable Temperature
Render Draw Faces (Selected)
Draw Lines (Cleared)
*. You can specify the variable (in this case, temperature) used to color the graphic
element. The Constant mode allows you to color the plane with a fixed color.

2. Click Apply.
Hot water (red) enters from one inlet and cold water (blue) from the other.

Moving the Slice Plane
The plane can be moved to different locations.


(Z up) from the shortcut menu.
Review the settings in Definition under Point and under Normal.
3. Click Single Select .
4. Click and drag the plane to a new location that intersects the domain.
As you drag the mouse, the viewer updates automatically. Note that Point updates with
new settings.
5. Set Point settings to 0,0,1.
6. Click Apply.

7. Click Rotate .
8. Turn off visibility for Slice by clearing the check box next to Slice in the Outline.

Adding Contours
Contours connect all points of equal value for a scalar variable (for example, Temperature)
and help to visualize variable values and gradients. Colored bands fill the spaces between
contour lines. Each band is colored by the average color of its two bounding contour lines
(even if the latter are not displayed).

Procedure 1. Select Insert > Contour from the main menu or click Contour .
The New Contour dialog box is displayed.
2. Set Name to Slice Contour.
3. Click OK.

Tab Setting Value
Geometry Locations Slice

5. Click Apply.
Important: The colors of 3D graphics object faces are slightly altered when lighting is on. To
view colors with highest accuracy, clear Lighting under Draw Faces on the Render tab and
click Apply.


The graphic element faces are visible, producing a contour plot as shown.

Note: Make sure that the checkbox next to Slice in the Outline is cleared.

Working with Animations
Animations build transitions between views for development of video files.

Workflow This tutorial follows the general workflow for creating a keyframe animation:
Overview

Showing the Animation Dialog Box
The Animation dialog box is used to define keyframes and to export to a video file.

Procedure 1. Select Tools > Animation or click Animation .
The Animation dialog box can be repositioned as required.



Creating the First Keyframe
Keyframes are required in order to produce an animation. You need to define the first viewer
state, a second (and final) viewer state, and set the number of interpolated intermediate
frames.

(Z up).
2. In the Outline, under User Locations and Plots, clear the visibility of Slice
Contour and select the visibility of Slice.

3. In the Animation dialog box, click New .
A new keyframe named KeyframeNo1 is created. This represents the current image
displayed in the viewer.

Creating the Second Keyframe
Keyframes are required in order to produce an animation.

Procedure 1. In the Outline, under User Locations and Plots, double-click Slice.
2. On the Geometry tab, set Point coordinate values to (0,0,-1.99).
3. Click Apply.
The slice plane moves to the bottom of the mixer.

KeyframeNo2 is created and represents the image displayed in the Viewer.


5. Select KeyframeNo1.
6. Set # of Frames (located below the list of keyframes) to 20.
This is the number of intermediate frames used when going from KeyframeNo1 to
KeyframeNo2. This number is displayed in the Frames column for KeyframeNo1.
7. Press Enter.
The Frame # column shows the frame in which each keyframe appears. KeyframeNo1
appears at frame 1 since it defines the start of the animation. KeyframeNo2 is at frame
22 since you have 20 intermediate frames (frames 2 to 21) in between KeyframeNo1 and
KeyframeNo2.

Viewing the Animation
More keyframes could be added, but this animation has only two keyframes (which is the
minimum possible).

Synopsis The controls previously greyed-out in the Animation dialog box are now available. The
number of intermediate frames between keyframes is listed beside the keyframe having the
lowest number of the pair. The number of keyframes listed beside the last keyframe is
ignored.

Procedure 1. Click Play the animation .
The animation plays from frame 1 to frame 22. It plays relatively slowly because the slice
plane must be updated for each frame.



Modifying the Animation
To make the plane sweep through the whole geometry, you will set the starting position of
the plane to be at the top of the mixer. You will also modify the Range properties of the
plane so that it shows the temperature variation better. As the animation is played, you can
see the hot and cold water entering the mixer. Near the bottom of the mixer (where the
water flows out) you can see that the temperature is quite uniform. The new temperature
range lets you view the mixing process more accurately than the global range used in the
first animation.


Tab Setting Value
Geometry Point 0, 0, 1.99
Color Variable Temperature
Range User Specified
Min 295 [K]
Max 305 [K]

2. Click Apply.
The slice plane moves to the top of the static mixer.

Note: Do not double click in the next step.
3. In the Animation dialog box, single click (do not double-click) KeyframeNo1 to select it.
If you had double-clicked KeyFrameNo1, the plane and viewer states would have been
redefined according to the stored settings for KeyFrameNo1. If this happens, click
Undo and try again to select the keyframe.

4. Click Set Keyframe .
The image in the Viewer replaces the one previously associated with KeyframeNo1.
5. Double-click KeyframeNo2.
The object properties for the slice plane are updated according to the settings in
KeyFrameNo2.
6. Apply the following settings to Slice

Tab Setting Value
Color Variable Temperature
Min 295 [K]
Max 305 [K]

7. Click Apply.
8. In the Animation dialog box, single-click KeyframeNo2.

9. Click Set Keyframe to save the new settings to KeyframeNo2.



Saving to MPEG
By defining the geometry and then saving to MPEG, the results can be saved to a video file.

Procedure 1. Click More Animation Options to view the additional options.
The Loop and Bounce radio buttons determine what happens when the animation
reaches the last keyframe. When Loop is selected, the animation repeats itself the
number of times defined by Repeat. When Bounce is selected, every other cycle is
played in reverse order, starting with the second.
2. Click Save MPEG.

3. Click Browse next to Save MPEG.
4. Under File name type: StaticMixer.mpg
5. If required, set the path location to a different folder.
6. Click Save.
The MPEG file name (including path) is set. At this point, the animation has not yet been
produced.
7. Click Previous Keyframe .
Wait a moment as the display updates the keyframe display.

8. Click Play the animation .
9. If prompted to overwrite an existing movie click Overwrite.
The animation plays and builds an MPEG file.
10. Click the Options button at the bottom of the Animation dialog box.
In Advanced, you can see that a Frame Rate of 24 frames per second was used to create
the animation. The animation you produced contains a total of 22 frames, so it takes just
under 1 second to play in a media player.
11. Click Cancel to close the dialog box.
12. Close the Animation dialog box.
13. Review the animation in third–party software as required.

Exiting ANSYS CFX-Post
When finished with ANSYS CFX-Post exit the current window:
1. When you are finished, select File > Quit to exit ANSYS CFX-Post.
2. Click Quit if prompted to save.


Tutorial 1a:
Simulating Flow in a Static
Mixer Using Workbench

Introduction
This tutorial comprises:
• Before You Begin (p. 32)
• Tutorial 1a Features (p. 32)

before beginning:
To learn how to perform these tasks using CFX in Standalone mode, see Tutorial 1:
Simulating Flow in a Static Mixer Using CFX in Standalone Mode (p. 3 in "ANSYS CFX
Tutorials").


Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Before You Begin

Before You Begin
Create a working directory for your files. Once this is done, copy the sample files used in this
tutorial to your working directory from the installation folder for your software
(<CFXROOT>/examples/ (for example, C:Program FilesANSYS
Incv110CFXexamples)) to avoid overwriting source files provided with your
• StaticMixerMesh.gtm
• StaticMixer.pre

Tutorial 1a Features

ANSYS CFX-Pre User Mode Quick Setup Wizard
Outlet (Subsonic)
Wall: No-Slip
Wall: Adiabatic
Contour
Point
Slice Plane
Streamline

• Using Quick Setup mode in ANSYS CFX-Pre to set up a problem.
• Modifying the outline plot in ANSYS CFX-Post.
• Using streamlines in ANSYS CFX-Post to trace the flow field from a point.
• Viewing temperature using colored planes and contours in ANSYS CFX-Post.
• Creating an animation and saving it to an MPEG file.


Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Overview of the Problem to Solve

Water enters through both pipes at the same rate but at different temperatures. The first
entry is at a rate of 2 m/s and a temperature of 315 K and the second entry is at a rate of 2
m/s at a temperature of 285 K. The radius of the mixer is 2 m.
Your goal in this tutorial is to understand how to use ANSYS CFX to determine the speed and
temperature of the water when it exits the static mixer.
Figure 1 Static Mixer with 2 Inlet Pipes and 1 Outlet Pipe
2 m/s
r=2m 285 K

2 m/s
315 K


Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Defining a Simulation in ANSYS CFX-Pre

Because you are starting with an existing mesh, you can immediately use ANSYS CFX-Pre to
define the simulation. This is how ANSYS CFX-Pre will look with the imported mesh:

In the image above, the left pane of ANSYS CFX-Pre displays the Outline. When you
double-click on items in the Outline, the Outline editor opens and can be used to create,
modify, and view objects.

Note: In this documentation, the details view can also be referenced by the name of the
object being edited, followed by the word “details view” (for example, if you double-click
the Wireframe object, the Wireframe details view appears).

Synopsis of Quick Setup Mode
Quick Setup mode provides a simple wizard–like interface for setting up simple cases. This
is useful for getting familiar with the basic elements of a CFD problem setup. This section
describes using Quick Setup mode to develop a simulation in ANSYS CFX-Pre.

Workflow Overview
This tutorial follows the general workflow for Quick Setup mode:
2. Setting the Physics Definition (p. 35)
4. Defining Model Data (p. 37)
5. Defining Boundaries (p. 37)

6. Setting Boundary Data (p. 37)
7. Setting Flow Specification (p. 37)
8. Setting Temperature Specification (p. 38)
9. Reviewing the Boundary Condition Definitions (p. 38)
10. Creating the Second Inlet Boundary Definition (p. 38)
11. Creating the Outlet Boundary Definition (p. 39)
12. Moving to General Mode (p. 39)

Playing a If you want to skip past these instructions and have ANSYS CFX-Pre set up the simulation
Session File automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre,

Before importing and working with a mesh, a simulation needs to be started using Quick
Setup mode.

Procedure 1. If required, launch ANSYS Workbench.
2. Click Empty Project.
The Project page appears displaying an unsaved project.

3. Select File > Save or click Save .
4. If required, set the path location to the working folder you created for this tutorial.
6. Click Save.
7. On the left-hand task bar under Advanced CFD, click Start CFX-Pre.
9. Select Quick Setup in the New Simulation File dialog box and click OK.
12. Click Save.

Setting the Physics Definition
You need to specify the fluids used in a simulation. A variety of fluids are already defined as
library materials. For this tutorial you will use a prepared fluid, Water, which is defined to be
water at 25°C.

Procedure 1. Ensure that Simulation Definition is displayed at the top of the Details view.
2. Under Fluid select Water.



Importing a Mesh

Procedure 1. In Simulation Definition, under Mesh File, click Browse .
The Import Mesh dialog box appears.
2. Under File type, select CFX Mesh (*gtm).
3. From your working directory, select StaticMixerMesh.gtm.
4. Click Open.
The mesh loads.
5. Click Next.

Using the Viewer
Now that the mesh is loaded, take a moment to explore how you can use the viewer toolbar
to zoom in or out and to rotate the object in the viewer.

Using the Zoom There are several icons available for controlling the level of zoom in the viewer.
Tools
1. Click Zoom Box
2. Click and drag a rectangular box over the geometry.
The geometry zoom changes to display the selection at a greater resolution.

4. Click Fit View to re-center and re-scale the geometry.

Rotating the If you need to rotate an object or to view it from a new angle, you can use the viewer toolbar.
geometry
1. Click Rotate on the viewer toolbar.
2. Click and drag within the geometry repeatedly to test the rotation of the geometry.
The geometry rotates based on the direction of movement.
Notice how the mouse cursor changes depending on where you are in the viewer:

3. Right-click a blank area in the viewer and select Predefined Camera > View
Towards-X).


(Z Up).
A clearer view of the mesh is displayed.

Defining Model Data
You need to define the type of flow and the physical models to use in the fluid domain.
You will specify the flow as steady state with turbulence and heat transfer. Turbulence is
modelled using the k - ε turbulence model and heat transfer using the thermal energy
model. The k - ε turbulence model is a commonly used model and is suitable for a wide
range of applications. The thermal energy model neglects high speed energy effects and is
therefore suitable for low speed flow applications.

Procedure 1. Ensure that Physics Definition is displayed.
2. Under Model Data, set Reference Pressure to 1 [atm].
All other pressure settings are relative to this reference pressure.
3. Set Heat Transfer to Thermal Energy.
4. Set Turbulence to k-Epsilon.
5. Click Next.

Defining Boundaries
The CFD model requires the definition of conditions on the boundaries of the domain.

Procedure 1. Ensure that Boundary Definition is displayed.
2. Delete Inlet and Outlet from the list by right-clicking each and selecting Delete.
3. Right-click in the blank area where Inlet and Outlet were listed, then select New.
4. Set Name to: in1
5. Click OK.
The boundary is created and, when selected, properties related to the boundary are
displayed.

Setting Boundary Data
Once boundaries are created, you need to create associated data. Based on Figure 1, you will
define the first inlet boundary condition to have a velocity of 2 m/s and a temperature of 315
K at one of the side inlets.

Procedure 1. Ensure that Boundary Data is displayed.
2. Set Boundary Type to Inlet.
3. Set Location to in1.

Setting Flow Specification
Once boundary data is defined, the boundary needs to have the flow specification assigned.


Procedure 1. Ensure that Flow Specification is displayed.
2. Set Option to Normal Speed.
3. Set Normal Speed to 2 [m s^-1].

Setting Temperature Specification
Once flow specification is defined, the boundary needs to have temperature assigned.

Procedure 1. Ensure that Temperature Specification is displayed.
2. Set Static Temperature to 315 [K].

Reviewing the Boundary Condition Definitions
Defining the boundary condition for in1 required several steps. Here the settings are
reviewed for accuracy.
Based on Figure 1, the first inlet boundary condition consists of a velocity of 2 m/s and a
temperature of 315 K at one of the side inlets.

Procedure 1. Review the boundary in1 settings for accuracy. They should be as follows:

Tab Setting Value
Location in1

Creating the Second Inlet Boundary Definition
Based on Figure 1, you know the second inlet boundary condition consists of a velocity of 2
m/s and a temperature of 285 K at one of the side inlets. You will define that now.

Procedure 1. Under Boundary Definition, right-click in the selector area and select New.
2. Create a new boundary named in2 with these settings:

Tab Setting Value
Location in2



Creating the Outlet Boundary Definition
Now that the second inlet boundary has been created, the same concepts can be applied to
building the outlet boundary.
1. Create a new boundary named out with these settings:

Tab Setting Value
Boundary Data Boundary Type Outlet
Location out
Flow Specification Option Average Static Pressure

2. Click Next.

Moving to General Mode
There are no further boundary conditions that need to be set. All 2D exterior regions that
have not been assigned to a boundary condition are automatically assigned to the default
boundary condition.

Procedure 1. Set Operation to Enter General Mode and click Finish.
The three boundary conditions are displayed in the viewer as sets of arrows at the
boundary surfaces. Inlet boundary arrows are directed into the domain. Outlet
boundary arrows are directed out of the domain.

Solver Control parameters control aspects of the numerical solution generation process.
While an upwind advection scheme is less accurate than other advection schemes, it is also
more robust. This advection scheme is suitable for obtaining an initial set of results, but in
general should not be used to obtain final accurate results.
The time scale can be calculated automatically by the solver or set manually. The Automatic
option tends to be conservative, leading to reliable, but often slow, convergence. It is often
possible to accelerate convergence by applying a time scale factor or by choosing a manual
value that is more aggressive than the Automatic option. In this tutorial, you will select a
physical time scale, leading to convergence that is twice as fast as the Automatic option.

2. On the Basic Settings tab, set Advection Scheme > Option to Upwind.
3. Set Convergence Control > Fluid Timescale Control > Timescale Control to
Physical Timescale and set the physical timescale value to 2 [s].
4. Click OK.



The simulation file, StaticMixer.cfx, contains the simulation definition in a format that
can be loaded by ANSYS CFX-Pre, allowing you to complete (if applicable), restore, and
modify the simulation definition. The simulation file differs from the definition file in that it
can be saved at any time while defining the simulation.

2. Set File name to StaticMixer.def.
3. Ensure that Start Solver Manager is selected from the drop down menu located in
the top-right corner of the dialog box.
4. Click Save.
This file is provided in the tutorial directory and may exist in your tutorial folder if you
6. If prompted, click Yes or Save & Quit to save StaticMixer.cfx.
The definition file (StaticMixer.def) and the simulation file (StaticMixer.cfx) are
created. ANSYS CFX-Solver Manager automatically starts and the definition file is set in

Note: This task is required only if you are starting here with the session file that was provided
in the examples directory. If you have performed all the tasks in the previous steps, proceed
directly to Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 41).
Events in ANSYS CFX-Pre can be recorded to a session file and then played back at a later
date to drive ANSYS CFX-Pre. Session files have been created for each tutorial so that the
problems can be set up rapidly in ANSYS CFX-Pre, if desired.

Procedure 1. If required, launch ANSYS Workbench.
2. Click Empty Project.

5. Click Save.
6. Click Start CFX-Pre.
8. Select StaticMixer.pre.
9. Click Open.
10. Click the CFX-Solver tab.
11. Select File > Define Run.



Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Obtaining a Solution Using ANSYS CFX-Solver
13. Select StaticMixer.def, located in the working directory.

ANSYS CFX-Solver Manager has a visual interface that displays a variety of results and should
be used when plotted data needs to be viewed during problem solving.
split between the windows, which is oriented either horizontally or vertically depending on

One window shows the convergence history plots and the other displays text output from
ANSYS CFX-Solver.
The text lists physical properties, boundary conditions and various other parameters used
or calculated in creating the model. All the text is written to the output file automatically (in
this case, StaticMixer_001.out).

Start the Run
The Define Run dialog box allows configuration of a run for processing by ANSYS
CFX-Solver.


Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Obtaining a Solution Using ANSYS CFX-Solver
When ANSYS CFX-Solver Manager is launched automatically from ANSYS CFX-Pre, all of the
information required to perform a new serial run (on a single processor) is entered
automatically. You do not need to alter the information in the Define Run dialog box. This
is a very quick way to launch into ANSYS CFX-Solver without having to define settings and
values.

Procedure 1. Ensure that the Define Run dialog box is displayed.
2. Click Start Run.
ANSYS CFX-Solver launches and a split screen appears and displays the results of the run
graphically and as text. The panes continue to build as ANSYS CFX-Solver Manager
operates.
Note: Once the second iteration appears, data begins to plot. Plotting may take a long time
depending on the amount of data to process. Let the process run.

Move from ANSYS CFX-Solver to ANSYS CFX-Post
results.

Procedure 1. When ANSYS CFX-Solver is finished, click Yes to post-process the results.

After a short pause, ANSYS CFX-Post starts and ANSYS CFX-Solver Manager closes.


Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-Post

When ANSYS CFX-Post starts, the viewer and Outline workspace are displayed.

The viewer displays an outline of the geometry and other graphic objects. You can use the
mouse or the toolbar icons to manipulate the view, exactly as in ANSYS CFX-Pre.

Workflow Overview
This tutorial describes the following workflow for viewing results in ANSYS CFX-Post:
1. Setting the Edge Angle for a Wireframe Object (p. 44)
2. Creating a Point for the Origin of the Streamline (p. 45)
3. Creating a Streamline Originating from a Point (p. 46)
4. Rearranging the Point (p. 47)
5. Configuring a Default Legend (p. 47)
6. Creating a Slice Plane (p. 48)
7. Defining Slice Plane Geometry (p. 49)
8. Configuring Slice Plane Views (p. 49)
9. Rendering Slice Planes (p. 50)
10. Coloring the Slice Plane (p. 51)
11. Moving the Slice Plane (p. 51)
12. Adding Contours (p. 52)
13. Working with Animations (p. 53)



Setting the Edge Angle for a Wireframe Object
The outline of the geometry is called the wireframe or outline plot.
By default, ANSYS CFX-Post displays only some of the surface mesh. This sometimes means
that when you first load your results file, the geometry outline is not displayed clearly. You
can control the amount of the surface mesh shown by editing the Wireframe object listed
in the Outline.
The check boxes next to each object name in the Outline control the visibility of each
object. Currently only the Wireframe and Default Legend objects have visibility selected.
The edge angle determines how much of the surface mesh is visible. If the angle between
two adjacent faces is greater than the edge angle, then that edge is drawn. If the edge angle
is set to 0°, the entire surface mesh is drawn. If the edge angle is large, then only the most
significant corner edges of the geometry are drawn.
For this geometry, a setting of approximately 15° lets you view the model location without
displaying an excessive amount of the surface mesh.
In this module you can also modify the zoom settings and view of the wireframe.

Procedure 1. In the Outline, under User Locations and Plots, double-click Wireframe.
Tip: While it is not necessary to change the view to set the angle, do so to explore the
practical uses of this feature.
shortcut menu and select Isometric View (Z up).
3. In the Wireframe details view, under Definition, click in the Edge Angle box.
An embedded slider is displayed.


Notice that more surface mesh is displayed.

6. Drag the embedded slider to set the Edge Angle value to approximately 45 [degree].
Less of the outline of the geometry is displayed.
shortcut menu and select View Towards -X.

Creating a Point for the Origin of the Streamline
A streamline is the path that a particle of zero mass would follow through the domain.

Procedure 1. Select Insert > Location > Point from the main menu.
explore this further.
2. Click OK.
3. Under Definition, ensure that Method is set to XYZ.
4. Under Point, enter the following coordinates: -1, -1, 1.
This is a point near the first inlet.
5. Click Apply.
The point appears as a symbol in the viewer as a crosshair symbol.



Creating a Streamline Originating from a Point
Where applicable, streamlines can trace the flow direction forwards (downstream) and/or
backwards (upstream).

Procedure 1. From the main menu, select Insert > Streamline.
will explore this further.
2. Click OK.
3. Under Definition, in Start From, ensure that Point 1 is set.
Tip: To create streamlines originating from more than one location, click the ellipsis icon
to the right of the Start From box. This displays the Location Selector dialog box,
where you can use the <Ctrl> and <Shift> keys to pick multiple locators.
4. Click the Color tab.
5. Set Mode to Variable.
6. Set Variable to Total Temperature.
7. Set Range to Local.
8. Click Apply.
The streamline shows the path of a zero mass particle from Point 1. The temperature
is initially high near the hot inlet, but as the fluid mixes the temperature drops.



Rearranging the Point
Once created, a point can be rearranged manually or by setting specific coordinates.
Tip: In this module, you may choose to display various views and zooms from the
Predefined Camera option in the shortcut menu (such as Isometric View (Z up) or
View Towards -X) and by using Zoom Box if you prefer to change the display.

Procedure 1. In Outline, under User Locations and Plots double-click Point 1.
Properties for the selected user location are displayed.
2. Under Point, set these coordinates: -1, -2.9, 1.
3. Click Apply.
The point is moved and the streamline redrawn.
4. In the selection tools, click Single Select.

While in this mode, the normal behavior of the left mouse button is disabled.
5. In the viewer, drag Point 1 (appears as a yellow addition sign) to a new location within
the mixer.
The point position is updated in the details view and the streamline is redrawn at the
new location. The point moves normal in relation to the viewing direction.

6. Click Rotate .
Tip: You can also click in the viewer area, and press the space bar to toggle between
Select and Viewing Mode. A way to pick objects from Viewing Mode is to hold down
<Ctrl> + <Shift> while clicking on an object with the left mouse button.
7. Under Point, reset these coordinates: -1, -1, 1.
8. Click Apply.
The point appears at its original location.
-X.

Configuring a Default Legend
You can modify the appearance of the default legend.
The default legend appears whenever a plot is created that is colored by a variable. The
streamline color is based on temperature; therefore, the legend shows the temperature
range. The color pattern on the legend’s color bar is banded in accordance with the bands
in the plot1.

1. An exception occurs when one or more bands in a contour plot represent values beyond the
legend’s range. In this case, such bands are colored using a color that is extrapolated slightly
past the range of colors shown in the legend. This can happen only when a user-specified
range is used for the legend.


The default legend displays values for the last eligible plot that was opened in the details
view. To maintain a legend definition during an ANSYS CFX-Post session, you can create a
new legend by clicking Legend .
Because there are many settings that can be customized for the legend, this module allows
you the freedom to experiment with them. In the last steps you will set up a legend, based
on the default legend, with a minor modification to the position.
Tip: When editing values, you can restore the values that were present when you began
editing by clicking Reset. To restore the factory-default values, click Default.

Procedure 1. Double click Default Legend View 1.
The Definition tab of the default legend is displayed.

Tab Setting Value
Definition Title Mode User Specified
Title Streamline Temp.
Horizontal (Selected)
Location > Y Justification Bottom

3. Click Apply.
The appearance and position of the legend changes based on the settings specified.
4. Modify various settings in Definition and click Apply after each change.
5. Select Appearance.
6. Modify a variety of settings in the Appearance and click Apply after each change.
7. Click Defaults.
8. Click Apply.
9. Under Outline, in User Locations and Plots, clear the check boxes for Point 1 and
Streamline 1.
Since both are no longer visible, the associated legend no longer appears.

Defining a slice plane allows you to obtain a cross–section of the geometry.
In ANSYS CFX-Post you often view results by coloring a graphic object. The graphic object
could be an isosurface, a vector plot, or in this case, a plane. The object can be a fixed color
or it can vary based on the value of a variable.
You already have some objects defined by default (listed in the Outline). You can view
results on the boundaries of the static mixer by coloring each boundary object by a variable.
To view results within the geometry (that is, on non-default locators), you will create new
objects.
You can use the following methods to define a plane:
• Three Points: creates a plane from three specified points.


• Point and Normal: defines a plane from one point on the plane and a normal vector
to the plane.
• YZ Plane, ZX Plane, and XY Plane: similar to Point and Normal, except that the
normal is defined to be normal to the indicated plane.

Procedure 1. From the main menu, select Insert > Location > Plane or click Location > Plane.
2. In the New Plane window, type: Slice
3. Click OK.
The Geometry, Color, Render, and View tabs let you switch between settings.

Defining Slice Plane Geometry
You need to choose the vector normal to the plane. You want the plane to lie in the x-y
plane, hence its normal vector points along the z-axis. You can specify any vector that points
in the z-direction, but you will choose the most obvious (0,0,1).

Procedure 1. If required, under Geometry, expand Definition.
2. Under Method select Point and Normal.
3. Under Point enter 0,0,1.
4. Under Normal enter 0, 0,1.
5. Click Apply.
Slice displays under User Locations and Plots. Rotate the view to see the plane.

Configuring Slice Plane Views
Depending on the view of the geometry, various objects may not appear because they fall
in a 2D space that cannot be seen.

(Z up).


The slice is now visible in the viewer.

2. Click Zoom Box .
3. Click and drag a rectangular selection over the geometry.

5. Click Rotate .
6. Click and drag the mouse pointer down slightly to rotate the geometry towards you.
7. Select Isometric View (Z up) as described earlier.

Rendering Slice Planes
Render settings determine how the plane is drawn.

Procedure 1. In the Details pane for Slice, select the Render tab.
2. Clear Draw Faces.
3. Select Draw Lines.
4. Under Draw Lines change Color Mode to User Specified.
5. Click the current color in Line Color to change to a different color.
For a greater selection of colors, click the ellipsis to use the Select color dialog box.
6. Click Apply.

7. Click Zoom Box .


The line segments show where the slice plane intersects with mesh element faces. The
end points of each line segment are located where the plane intersects mesh element
edges.
-Z.
The image shown below can be used for comparison with tutorial 2 (in the section
Creating a Slice Plane (p. 68)), where a refined mesh is used.

The Color panel is used to determine how the object faces are colored.


Tab Setting Value
Color Mode Variable*
*. You can specify the variable (in this case, temperature) used to color the graphic
element. The Constant mode allows you to color the plane with a fixed color.

2. Click Apply.
Hot water (red) enters from one inlet and cold water (blue) from the other.

Moving the Slice Plane
The plane can be moved to different locations.


Review the settings in Definition under Point and under Normal.
3. Click Single Select .
4. Click and drag the plane to a new location that intersects the domain.
As you drag the mouse, the viewer updates automatically. Note that Point updates with
new settings.
5. Set Point settings to 0,0,1.
6. Click Apply.

7. Click Rotate .
8. Turn off visibility for Slice by clearing the check box next to Slice in the Outline.

Adding Contours
Contours connect all points of equal value for a scalar variable (for example, Temperature)
and help to visualize variable values and gradients. Colored bands fill the spaces between
contour lines. Each band is colored by the average color of its two bounding contour lines
(even if the latter are not displayed).


2. Select Insert > Contour from the main menu or click Contour .
The New Contour dialog box is displayed.
3. Set Name to Slice Contour.
4. Click OK.

Tab Setting Value
Geometry Locations Slice

6. Click Apply.

Important: The colors of 3D graphics object faces are slightly altered when lighting is on. To
view colors with highest accuracy, on the Render tab under Draw Faces clear Lighting and
click Apply.


The graphic element faces are visible, producing a contour plot as shown.

Working with Animations
Animations build transitions between views for development of video files.

Workflow This tutorial follows the general workflow for creating a keyframe animation:
Overview

Showing the Animation Dialog Box
The Animation dialog box is used to define keyframes and to export to a video file.

Procedure 1. Select Tools > Animation or click Animation .

Creating the First Keyframe
Keyframes are required in order to produce an animation. You need to define the first viewer
state, a second (and final) viewer state, and set the number of interpolated intermediate
frames.

(Z up).
2. In the Outline, under User Locations and Plots, clear the visibility of Slice
Contour and select the visibility of Slice.

3. Select Tools > Animation or click Animation .

A new keyframe named KeyframeNo1 is created. This represents the current image
displayed in the viewer.

Creating the Second Keyframe
Keyframes are required in order to produce an animation.

Procedure 1. In the Outline, under User Locations and Plots, double-click Slice.
2. On the Geometry tab, set Point coordinate values to (0,0,-1.99).
3. Click Apply.
The slice plane moves to the bottom of the mixer.

KeyframeNo2 is created and represents the image displayed in the Viewer.
5. Select KeyframeNo1.
6. Set # of Frames (located below the list of keyframes) to 20.


This is the number of intermediate frames used when going from KeyframeNo1 to
KeyframeNo2. This number is displayed in the Frames column for KeyframeNo1.
7. Press Enter.
The Frame # column shows the frame in which each keyframe appears. KeyframeNo1
appears at frame 1 since it defines the start of the animation. KeyframeNo2 is at frame
22 since you have 20 intermediate frames (frames 2 to 21) in between KeyframeNo1 and
KeyframeNo2.

Viewing the Animation
More keyframes could be added, but this animation has only two keyframes (which is the
minimum possible).
The controls previously greyed-out in the Animation dialog box are now available. The
number of intermediate frames between keyframes is listed beside the keyframe having the
lowest number of the pair. The number of keyframes listed beside the last keyframe is
ignored.

Procedure 1. Click Play the animation .
The animation plays from frame 1 to frame 22. It plays relatively slowly because the slice
plane must be updated for each frame.



Modifying the Animation
To make the plane sweep through the whole geometry, you will set the starting position of
the plane to be at the top of the mixer. You will also modify the Range properties of the
plane so that it shows the temperature variation better. As the animation is played, you can
see the hot and cold water entering the mixer. Near the bottom of the mixer (where the
water flows out) you can see that the temperature is quite uniform. The new temperature
range lets you view the mixing process more accurately than the global range used in the
first animation.


Tab Setting Value
Geometry Point 0, 0, 1.99
Color Mode Variable
Min 295 [K]
Max 305 [K]

2. Click Apply.
The slice plane moves to the top of the static mixer.

Note: Do not double click in the next step.
3. In the Animation dialog box, single click (do not double-click) KeyframeNo1 to select it.
If you had double-clicked KeyFrameNo1, the plane and viewer states would have been
redefined according to the stored settings for KeyFrameNo1. If this happens, click
Undo and try again to select the keyframe.

4. Click Set Keyframe .
The image in the Viewer replaces the one previously associated with KeyframeNo1.
5. Double-click KeyframeNo2.
The object properties for the slice plane are updated according to the settings in
KeyFrameNo2.
6. Apply the following settings to Slice

Tab Setting Value
Color Mode Variable
Min 295 [K]
Max 305 [K]

7. Click Apply.
8. In the Animation dialog box, single-click KeyframeNo2.

9. Click Set Keyframe to save the new settings to KeyframeNo2.



Saving to MPEG
By defining the geometry and then saving to MPEG, the results can be saved to a video file.

Procedure 1. Click More Animation Options to view the additional options.
The Loop and Bounce radio buttons determine what happens when the animation
reaches the last keyframe. When Loop is selected, the animation repeats itself the
number of times defined by Repeat. When Bounce is selected, every other cycle is
played in reverse order, starting with the second.
2. Click Save MPEG.

4. Under File name type: StaticMixer.mpg
6. Click Save.
produced.
7. Click Previous Keyframe .
Wait a moment as the display updates the keyframe display.

9. If prompted to overwrite an existing movie click Overwrite.
The animation plays and builds an MPEG file.
10. Click the Options button at the bottom of the Animation dialog box.
In Advanced, you can see that a Frame Rate of 24 frames per second was used to create
the animation. The animation you produced contains a total of 22 frames, so it takes just
under 1 second to play in a media player.
11. Click Cancel to close the dialog box.
13. Review the animation in third–party software as required.

When finished with ANSYS CFX-Post, exit the current window:
1. Select File > Close to close the current file.
2. If prompted to save, click Close.
3. Return to the Project page. Select File > Close Project.
4. Select No, then close Workbench.


Tutorial 2:
Flow in a Static Mixer
(Refined Mesh)

Introduction
• Defining a Simulation using General Mode in ANSYS CFX-Pre (p. 61)
• Obtaining a Solution Using Interpolation with ANSYS CFX-Solver (p. 66)

before beginning:
Unless you plan on running a session file, you should copy the sample files used in this
tutorial from the installation folder for your software (<CFXROOT>/examples/) to your
working directory. This prevents you from overwriting source files provided with your
• StaticMixerRefMesh.gtm
• StaticMixerRef.pre
• StaticMixer.def
• StaticMixer_001.res


Tutorial 2: Flow in a Static Mixer (Refined Mesh): Tutorial 2 Features

Tutorial 2 Features

ANSYS CFX-Pre User Mode General Mode
Outlet (Subsonic)
Wall: No-Slip
Wall: Adiabatic
ANSYS CFX-Post Plots Planevolume
Slice Plane
Spherevolume
Other Viewing the Mesh

• Using the General Mode of ANSYS CFX-Pre (this mode is used for more complex cases).
• Rerunning a problem with a refined mesh.
• Importing CCL to copy the definition of a different simulation into the current
simulation.
• Viewing the mesh with a Sphere volume locator and a Surface Plot.
• Using a Plane Volume locator and the Mesh Calculator to analyze mesh quality.

In this tutorial, you use a refined mesh to obtain a better solution to the Static Mixer problem
created in Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode (p. 3).
You establish a general workflow for analyzing the flow of fluid into and out of a mixer. This
tutorial uses a specific problem to teach the general approach taken when working with an
existing mesh.
You start a new simulation in ANSYS CFX-Pre and import the refined mesh. This tutorial
introduces General Mode—the mode used for most tutorials—in ANSYS CFX-Pre. The
physics for this tutorial are the same as for Tutorial 1: Simulating Flow in a Static Mixer Using
CFX in Standalone Mode (p. 3); therefore, you can import the physics settings used in that
tutorial to save time.


Tutorial 2: Flow in a Static Mixer (Refined Mesh): Defining a Simulation using General Mode in ANSYS CFX-Pre

Defining a Simulation using General Mode in ANSYS CFX-Pre
After having completed meshing, ANSYS CFX-Pre is used as a consistent and intuitive
interface for the definition of complex CFD problems.

Playing a Session File
If you want to skip past these instructions, and have ANSYS CFX-Pre set up the simulation
automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre,
Obtaining a Solution Using Interpolation with ANSYS CFX-Solver (p. 66).

Workflow Overview
This section provides a brief summary of the topics so that you can see the workflow:
3. Importing CCL (p. 62)
4. Viewing Domain Settings (p. 63)
5. Viewing the Boundary Condition Setting (p. 64)
6. Defining Solver Parameters (p. 64)
As an alternative to these steps, you can also review Playing the Session File and Starting
ANSYS CFX-Solver Manager (p. 65)
To begin this tutorial and create a new simulation in ANSYS CFX-Pre, continue from Creating
a New Simulation (p. 61).

Before importing and working with a mesh, a simulation needs to be developed using
General mode.

Note: Two procedures are documented. Depending on your installation of ANSYS CFX,
follow either the Standalone procedure or the Workbench procedure.

Procedure in 1. If required, launch ANSYS CFX-Pre.
Standalone 2. Select File > New Simulation.
3. Select General in the New Simulation File dialog box and click OK.
5. Under File name, type StaticMixerRef and click Save.
6. Proceed to Importing a Mesh (p. 62).

Procedure in 1. If required, launch ANSYS Workbench.
Workbench 2. Click Empty Project.


The Project page appears displaying an unsaved project.

4. If required, set the path location to your working folder.
6. Click Start CFX-Pre under Advanced CFD on the left hand task bar.
8. Click General in the New Simulation File window, and then click OK.

Importing a Mesh
An assembly is a group of mesh regions that are topologically connected. Each assembly
can contain only one mesh, but multiple assemblies are permitted. The Mesh tree shows the
regions in Assembly in a tree structure. The level below Assembly displays 3D regions and
the level below each 3D region shows the 2D regions associated with it. The check box next
to each item in the Mesh tree indicates the visibility status of the object in the viewer; you
can click these to toggle visibility.

Procedure 1. Select File > Import Mesh or right-click Mesh and select Import Mesh.
2. In the Import Mesh dialog box, select StaticMixerRefMesh.gtm from your working
directory.
This is a mesh that is more refined than the one used in Tutorial 1.
3. Click Open.

Importing CCL
Since the physics for this simulation is very similar to that for Tutorial 1, you can save time
by importing the settings used there.
The CCL contains settings that reference mesh regions. For example, the outlet boundary
condition references the mesh region named out. In this tutorial, the name of the mesh
regions are the same as in Tutorial 1, so you can import the CCL without error.
The physics for a simulation can be saved to a CCL (CFX Command Language) file at any time
by selecting File > Export CCL. However, a number of other files can also be used as sources
to import CCL including:
• Simulation files (*.cfx)
• Results files (*.res)
• Definition files(*.def)
Note: If you import CCL that references non-existent mesh regions, you will get errors.


Procedure 1. Select File > Import CCL.
The Import CCL dialog box appears.
2. Under Import Method, select Append.
Replace is useful if you have defined physics and want to update or replace them with
newly imported physics.
3. Under File type, select CFX-Solver Files (*def *res).
4. Select StaticMixer.def created in Tutorial 1. If you did not work through Tutorial 1,
you can copy this file from the examples directory.
5. Click Open.
6. Select the Outline tab.
Tip: To select Outline you may need to click the navigation icons next to the tabs to
move ‘forward’ or ‘backward’ through the various tabs.
The tree view displays a summary of the current simulation in a tree structure. Some
items may be recognized from Tutorial 1—for example the boundary condition objects
in1, in2, and out.

Viewing Domain Settings
It is useful to review the options available in General Mode.
Various domain settings can be set. These include:
• General Options
Specifies the location of the domain, coordinate frame settings and the fluids/solids that
are present in the domain. You also reference pressure, buoyancy and whether the
domain is stationary or rotating. Mesh motion can also be set.
• Fluid Models
Sets models that apply to the fluid(s) in the domain, such as heat transfer, turbulence,
combustion, and radiation models. An option absent in Tutorial 1 is Turbulent Wall
Functions, which is set to Scalable. Wall functions model the flow in the near-wall
region. For the k-epsilon turbulence model, you should always use scalable wall
functions.
• Initialization
Sets the initial conditions for the current domain only. This is generally used when
multiple domains exist to allow setting different initial conditions in each domain, but
can also be used to initialize single-domain simulations. Global initialization allows the
specification of initial conditions for all domains that do not have domain-specific
initialization.

Procedure 1. On the Outline tree view, under Simulation, double-click Default Domain.
The domain Default Domain is opened for editing.
2. Click General Options and review, but do not change, the current settings.
3. Click Fluid Models and review, but do not change, the current settings.
4. Click Initialization and review, but do not change, the current settings.
5. Click Close.



Viewing the Boundary Condition Setting
For the k-epsilon turbulence model, you must specify the turbulent nature of the flow
entering through the inlet boundary. For this simulation, the default setting of Medium
(Intensity = 5%) is used. This is a sensible setting if you do not know the turbulence
properties of the incoming flow.

Procedure 1. Under Default Domain, double-click in1.
2. Click the Boundary Details tab and review the settings for Flow Regime, Mass and
Momentum, Turbulence and Heat Transfer.
3. Click Close.

Defining Solver Parameters
Solver Control parameters control aspects of the numerical-solution generation process.
In Tutorial 1 you set some solver control parameters, such as Advection Scheme and
Timescale Control, while other parameters were set automatically by ANSYS CFX-Pre.
In this tutorial, High Resolution is used for the advection scheme. This is more accurate
than the Upwind Scheme used in Tutorial 1. You usually require a smaller timestep when
using this model. You can also expect the solution to take a higher number of iterations to
converge when using this model.

Procedure 1. Select Insert > Solver > Solver Control from the main menu or click Solver Control .
2. Apply the following Basic Settings

Setting Value
Advection Scheme > Option High Resolution
Convergence Control > Max. Iterations* 150
Convergence Control > Fluid Timescale Control > Physical Timescale
Timescale Control
Convergence Control > Fluid Timescale Control > Physical 0.5 [s]
Timescale
*. If your solution does not meet the convergence criteria after this number of
timesteps, the ANSYS CFX-Solver will stop.

3. Click Apply.
4. Click the Advanced Options tab.
5. Ensure that Global Dynamic Model Control is selected.
6. Click OK.

Once all boundaries are created you move from ANSYS CFX-Pre into ANSYS CFX-Solver.


The simulation file—StaticMixerRef.cfx—contains the simulation definition in a format
that can be loaded by ANSYS CFX-Pre, allowing you to complete (if applicable), restore, and
modify the simulation definition. The simulation file differs from the definition file in two
important ways:
• The simulation file can be saved at any time while defining the simulation.
• The definition file is an encapsulated set of meshes and CCL defining a solver run, and is
a subset of the data in the simulation file.

2. If required, set the path to your working directory.
3. Apply the following settings:

Setting Value
File name StaticMixerRef.def
Quit CFX–Pre* (Selected)

*. If using ANSYS CFX-Pre in Standalone Mode.

4. Ensure Start Solver Manager is selected and click Save.
5. If you are notified that the file already exists, click Overwrite.
6. If prompted, click Yes or Save & Quit to save StaticMixerRef.cfx.
The definition file (StaticMixerRef.def) and the simulation file
(StaticMixerRef.cfx) are created. ANSYS CFX-Solver Manager automatically starts
and the definition file is set in the Definition File box of Define Run.
7. Proceed to Obtaining a Solution Using Interpolation with ANSYS CFX-Solver (p. 66).

If you have performed all the tasks in the previous steps, proceed directly to Obtaining a
Solution Using Interpolation with ANSYS CFX-Solver (p. 66).
Two procedures are documented. Depending on your installation of ANSYS CFX follow
either the standalone procedure or the ANSYS Workbench procedure.

Standalone 2. Select Session > Play Tutorial.
3. Select StaticMixerRef.pre.
4. Click Open.
6. Launch ANSYS CFX-Solver Manager from CFX Launcher.
7. After ANSYS CFX-Solver starts, select File > Define Run.

9. Select StaticMixerRef.def, located in the working directory.


Tutorial 2: Flow in a Static Mixer (Refined Mesh): Obtaining a Solution Using Interpolation with ANSYS CFX-Solver
10. Proceed to Obtaining a Solution Using Interpolation with ANSYS CFX-Solver (p. 66).

ANSYS 2. Click Empty Project.
Workbench

7. Select StaticMixerRef.pre.
8. Click Open.

12. Select StaticMixerRef.def, located in the working directory.

Obtaining a Solution Using Interpolation with ANSYS
CFX-Solver
split between the windows which is oriented either horizontally or vertically, depending on

Workflow Overview
This section provides a brief summary of the topics to follow as a general workflow:
1. Interpolating the Results and Starting the Run (p. 66)
2. Confirming Results (p. 67)
3. Moving from ANSYS CFX-Solver to ANSYS CFX-Post (p. 67)

Interpolating the Results and Starting the Run
In the ANSYS CFX-Solver Manager, Define Run is visible and Definition File has
automatically been set to the definition file from ANSYS CFX-Pre: StaticMixerRef.def.
You want to make use of the results from Tutorial 1, but the two meshes are not identical.
The initial values file needs to have its data interpolated onto the new mesh associated with
the definition file.
The ANSYS CFX-Solver supports automatic interpolation that will be used in the following
steps:


Tutorial 2: Flow in a Static Mixer (Refined Mesh): Obtaining a Solution Using Interpolation with ANSYS CFX-Solver
The values from StaticMixer_001.res will be interpolated onto the definition file’s mesh
when the run is started. The results from StaticMixer_001.res will be used as the initial
guess for this simulation (rather than Solver defaults) because you have set the initialization
for all variables in ANSYS CFX-Pre to Automatic or Automatic with Value.

Procedure 1. Under Initial Values File, click Browse .
2. Select the results file from Tutorial 1: StaticMixer_001.res
If you did not complete the first tutorial, you can use StaticMixer_001.res from your
working directory.
3. Click Open.
4. Select Interpolate Initial Values onto Def File Mesh.
5. Click Start Run.
Note: The message Finished interpolation successfully appears relatively quickly.
Convergence information is plotted once the second outer loop iteration is complete.

Confirming Results
When interpolation is successful, specific information appears in the text screen of ANSYS
CFX-Solver.
To confirm that the interpolation was successful, look in the text pane in ANSYS CFX-Solver
Manager. The following text appears before the convergence history begins:
+---------------------------------------------------------+
| Initial Conditions Supplied by Fields in the Input Files
+---------------------------------------------------------+
This lists the variables that were interpolated from the results file. After the final iteration, a
message similar to the following content appears:
CFD Solver finished: Tue Oct 19 08:06:45 2004
CFD Solver wall clock seconds: 1.7100E+02
Execution terminating:
all residual
are below their target criteria
This indicates that ANSYS CFX-Solver has successfully calculated the solution for the
problem to the specified accuracy or has run out of coefficient loops.

Procedure 1. When the run finishes and asks if you want to post-process the results, click No to keep
ANSYS CFX-Solver open. Review the results on the Out File tab for details on the run
results.

Moving from ANSYS CFX-Solver to ANSYS CFX-Post
results.

Procedure 1. Select Tools > Post–Process Results or click Post–Process Results in the toolbar.
2. If using ANSYS CFX-Solver in Standalone Mode, select Shut down Solver Manager.
This forces Standalone ANSYS CFX-Solver to close when finished. This option is not
required in Workbench.
3. Click OK.


Tutorial 2: Flow in a Static Mixer (Refined Mesh): Viewing the Results in ANSYS CFX-Post
After a short pause, ANSYS CFX-Post starts.

In the following sections, you will explore the differences between the mesh and the results
from this tutorial and tutorial 1.

More information exists for use by ANSYS CFX-Post in this tutorial than in Tutorial 1 because
the slice plane is more detailed.
Once a new slice plane is created it can be compared with Tutorial 1. There are three
noticeable differences between the two slice planes.
• Around the edges of the mixer geometry there are several layers of narrow rectangles.
This is the region where the mesh contains prismatic elements (which are created as
inflation layers). The bulk of the geometry contains tetrahedral elements.
• There are more lines on the plane than there were in Tutorial 1. This is because the slice
plane intersects with more mesh elements.
• The curves of the mixer are smoother than in Tutorial 1 because the finer mesh better
represents the true geometry.

(Z up).
2. From the main menu, select Insert > Location > Plane or under Location, click Plane.
3. In the Insert Plane dialog box, type Slice and click OK.
The Geometry, Color, Render and View tabs let you switch between settings.

Tab Setting Value
Geometry Domains Default Domain
Definition > Method XY Plane
Definition > Z 1 [m]
Render Draw Faces (Cleared)
Draw Lines (Selected)

5. Click Apply.
-Z.

7. Click Zoom Box .


Compare the on-screen image with the equivalent picture from tutorial 1 (in the section
Rendering Slice Planes (p. 22)).

Here, you will color the plane by temperature.

Procedure 1. Apply the following settings

Tab Setting Value
Color Mode * Variable
Range Global
*. A mode setting of Constant would allow you to color the plane with a fixed color.

2. Click Apply.

Loading Results from Tutorial 1 for Comparison
In ANSYS CFX-Post, you may load multiple results files into the same instance for
comparison.

Procedure 1. To load the results file from Tutorial 1, select File > Load Results or click
Load Results .
2. Be careful not to click Open until instructed to do so. In the Load Results File dialog
box, select StaticMixer_001.res in the <CFXROOT>examples directory or from your
working directory if it has been copied.


3. On the right side of the dialog box, there are two frames. Under Results file option,
select Add to current results.
4. Select the Offset in Y direction check box.
5. Under Additional actions, ensure that the Clear user state before loading check box
is cleared.
6. Click Open to load the results.
In the tree view, there is now a second group of domains, meshes and boundary
conditions with the heading StaticMixer_001.
7. Double-click the Wireframe object under User Locations and Plots.
8. In the Definition tab, set Edge Angle to 5 [degree].
9. Click Apply.
(Z up).
Both meshes are now displayed in a line along the Y axis. Notice that one mesh is of a
higher resolution than the other.
11. Set Edge Angle to 30 [degree].
12. Click Apply.

Creating a Second Slice Plane
Procedure 1. In the tree view, right-click the plane named Slice and select Duplicate.
2. Click OK to accept the default name Slice 1.
3. In the tree view, double-click the plane named Slice 1.
4. On the Geometry tab, set Domains to Default Domain 1.
5. On the Color tab, ensure that Range is set to Global.
6. Click Apply.
7. Double-click Slice and make sure that Range is set to Global.

Comparing Slice Planes using Multiple Views
Procedure 1. Select the option with the two vertical rectangles. Notice that the Viewer now has two
separate views.

The visibility status of each object is maintained separately for each view or figure that
can be displayed in a given viewport. This allows some planes to be shown while others
are hidden.


2. Click in the viewport that is set to show View 1, then clear the visibility check box for
Slice in the Outline tree view and ensure that the visibility check box for Slice 1 is
selected.
3. Click in the viewport that is set to show View 2, then select the visibility check box for
Slice and ensure that the visibility check box for Slice 1 is cleared.
4. In the tree view, double-click StaticMixer_001 and clear Apply Translation.
5. Click Apply.

6. In the viewer toolbar, click Synchronise Active Views .
Notice that both views move in the same way and are zoomed in at the same level.
7. Right-click in the viewer and select Predefined Camera > View Towards -Z.
Note the difference in temperature distribution.
8. To return to a single viewport, select the option with a single rectangle.

9. Right-click Slice 1 in the tree view and select Delete.
10. Ensure that the visibility check box for Slice is cleared.
11. Right-click StaticMixer_001 in the tree view and select Unload.

Viewing the Surface Mesh on the Outlet
In this part of the tutorial, you will view the mesh on the outlet. You will see five layers of
inflated elements against the wall. You will also see the triangular faces of the tetrahedral
elements closer to the center of the outlet.

(Z up).
2. In the tree view, ensure that the visibility check box for StaticMixerRef_001 >
Default Domain > out is selected, then double-click out to open it for editing.
Since the boundary location geometry was defined in ANSYS CFX-Pre, the details view
does not display a Geometry tab as it did for the planes.

Tab Setting Value
Color Mode User Specified
Line Color (Select any light color)
4. Click Apply.



5. Click Zoom Box .
6. Zoom in on the geometry to view out in greater detail.

7. Click Rotate on the Viewing Tools toolbar.
8. Rotate the image as required to clearly see the mesh.

Looking at the Inflated Elements in Three Dimensions
To show more clearly what effect inflation has on the shape of the elements, you will use
volume objects to show two individual elements. The first element that will be shown is a
normal tetrahedral element; the second is a prismatic element from an inflation layer of the
mesh.
Leave the surface mesh on the outlet visible to help see how surface and volume meshes are
related.

Procedure 1. From the main menu, select Insert > Location > Volume or, under Location click
Volume.
2. In the Insert Volume dialog box, type Tet Volume and click OK.

Tab Setting Value
Geometry Definition > Method Sphere
Definition > Point * 0.08, 0, -2
Definition > Radius 0.14 [m]
Definition > Mode Below Intersection
Inclusive† (Cleared)
Color Color Red
Render Draw Faces > Transparency 0.3
Draw Lines > Line Width 1
Draw Lines > Color Mode User Specified
Draw Lines > Line Color Grey
*. The z slider’s minimum value corresponds to the minimum z value of the entire
geometry, which, in this case, occurs at the outlet.
†. Only elements that are entirely contained within the sphere volume will be
included.

4. Click Apply to create the volume object.
5. Right-click Tet Volume and choose Duplicate.
6. In the Duplicate Tet Volume dialog box, type Prism Volume and click OK.
7. Double-click Prism Volume.



Tab Setting Value
Geometry Definition > Point -0.22, 0.4, -1.85
Definition > Radius 0.206 [m]
Color Color Orange

9. Click Apply.

Viewing the Surface Mesh on the Mixer Body
Procedure 1. Double-click the Default Domain Default object.

Tab Setting Value
Line Width 2

3. Click Apply.

Viewing the Layers of Inflated Elements on a Plane
You will see the layers of inflated elements on the wall of the main body of the mixer. Within
the body of the mixer, there will be many lines that are drawn wherever the face of a mesh
element intersects the slice plane.

Procedure 1. From the main menu, select Insert > Location > Plane or under Location, click Plane.
2. In the Insert Plane dialog box, type Slice 2 and click OK.

Tab Setting Value
Geometry Definition > Method YZ Plane
Definition > X 0 [m]

4. Click Apply.
5. Turn off the visibility of all objects except Slice 2.
6. To see the plane clearly, right-click in the viewer and select Predefined Camera > View
Towards -X.

Viewing the Mesh Statistics
You can use the Report Viewer to check the quality of your mesh. For example, you can load
a .def file into ANSYS CFX-Post and check the mesh quality before running the .def file in
the solver.


Procedure 1. Click the Report Viewer tab (located below the viewer window).
A report appears. Look at the table shown in the “Mesh Report” section.
2. Double-click Report > Mesh Report in the Outline tree view.
3. In the Mesh Report details view, select Statistics > Maximum Face Angle.
4. Click Refresh Preview.
Note that a new table, showing the maximum face angle for all elements in the mesh,
has been added to the “Mesh Report” section of the report. The maximum face angle is
reported as 148.95°.
As a result of generating this mesh statistic for the report, a new variable, Maximum Face
Angle, has been created and stored at every node. This variable will be used in the next
section.

Viewing the Mesh Elements with Largest Face Angle
In this section, you will visualize the mesh elements that have a Maximum Face Angle value
greater than 140°.

Procedure 1. Click the 3D Viewer tab (located below the viewer window).
(Z up).
3. In the Outline tree view, select the visibility check box of Wireframe.
4. From the main menu, select Insert > Location > Volume or under Location, click
Volume.
5. In the Insert Volume dialog box, type Max Face Angle Volume and click OK.

Tab Setting Value
Geometry Definition > Method Isovolume
Definition > Variable Maximum Face Angle*
Definition > Mode Above Value
Definition > Value 140 [degree]
Inclusive† (Selected)

*. Select Maximum Face Angle from the larger list of variables available by clicking

to the right of the Variable box.
†. This includes any elements that have at least one node with a variable value greater
than or equal to the given value.

7. Click Apply.
The volume object appears in the viewer.



Viewing the Mesh Elements with Largest Face Angle Using a Point
Next, you will create a point object to show a node that has the maximum value of Maximum
Face Angle. The point object will be represented by a 3D yellow crosshair symbol. In order
to avoid obscuring the point object with the volume object, you may want to turn off the
visibility of the latter.

Procedure 1. From the main menu, select Insert > Location > Point or under Location, click Point.
2. Click OK to use the default name.

Tab Setting Value
Geometry Definition > Method Variable Maximum
Definition > Location Default Domain
Definition > Variable Maximum Face Angle
Symbol Symbol Size 2

4. Click Apply.

Quitting ANSYS CFX-Post
Two procedures are documented. Depending on your installation of ANSYS CFX, follow

Procedure in 1. When you are finished, select File > Quit to exit ANSYS CFX-Post.
Standalone 2. Click Quit if prompted to save.

Procedure in 1. When you are finished, select File > Close to close the current file.
Workbench 2. Click Close if prompted to save.


Tutorial 3:
Flow in a Process Injection
Mixing Pipe

Introduction
• Defining a Simulation using General Mode in ANSYS CFX-Pre (p. 79)

before beginning:
Sample files referenced by this tutorial include:
• InjectMixer.pre
• InjectMixer_velocity_profile.csv
• InjectMixerMesh.gtm


Tutorial 3: Flow in a Process Injection Mixing Pipe: Tutorial 3 Features

Tutorial 3 Features

Boundary Conditions Boundary Profile visualization
Inlet (Profile)
Inlet (Subsonic)
Outlet (Subsonic)
Wall: No-Slip
Wall: Adiabatic
CEL (CFX Expression Language)
ANSYS CFX-Post Plots default Locators
Slice Plane
Streamline
Other Changing the Color Range
Expression Details View
Legend
Viewing the Mesh

• Applying a profile boundary condition using data stored in a file.
• Visualizing the velocity on a boundary in ANSYS CFX-Pre.
• Using the CFX Expression Language (CEL) to describe temperature dependent fluid
properties in ANSYS CFX-Pre.
• Using the k-epsilon turbulence model.
• Using streamlines in ANSYS CFX-Post to track flow through the domain.

In this tutorial, you establish a general workflow for analyzing the flow of fluid into and out
of an injection pipe. This tutorial is important because it uses a specific problem to teach the
general approach taken when working with an existing mesh.


Tutorial 3: Flow in a Process Injection Mixing Pipe: Defining a Simulation using General Mode in ANSYS CFX-Pre
The injection mixing pipe, common in the process industry, is composed of two pipes: one
with a larger diameter than the other. Analyzing and optimizing the mixing process is often
critical for many chemical processes. CFD is useful not only in identifying problem areas
(where mixing is poor), but also in testing new designs before they are implemented.
The geometry for this example consists of a circular pipe of diameter 1.0 m with a 90° bend,
and a smaller pipe of diameter 0.3 m which joins with the main pipe at an oblique angle.
Figure 1 Injection Mixing Pipe

0.5 m/s
φ=1.0 m 285.0 K

φ=0.3 m

5.0 m/s
315.0 K

Defining a Simulation using General Mode in ANSYS CFX-Pre
After having completed meshing, ANSYS CFX-Pre is used as a consistent and intuitive
interface for the definition of complex CFD problems.

If you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulation

Workflow Overview
3. Setting Temperature-Dependent Material Properties (p. 81)
4. Plotting an Expression (p. 82)


5. Evaluating an Expression (p. 82)
6. Modify Material Properties (p. 82)
7. Creating the Domain (p. 82)
8. Creating the Side Inlet Boundary Conditions (p. 83)
9. Creating the Main Inlet Boundary Conditions (p. 84)
10. Creating the Main Outlet Boundary Condition (p. 85)
11. Setting Initial Values (p. 85)
12. Setting Solver Control (p. 85)

Before importing and working with a mesh, a simulation needs to be started using General
Mode.

Note: Two procedures are documented. Depending on your installation of ANSYS CFX
follow either the Standalone procedure or the Workbench procedure.

Standalone 2. Select File > New Simulation.
3. Ensure General is selected and click OK.
5. Under File name, type InjectMixer.
6. Click Save.
7. Proceed to Importing a Mesh (p. 80).

Workbench 2. Click Empty Project.
The Project page will appear displaying an unsaved project.

4. If required, set the path location to your working folder.
6. Click Save.
7. Click Start CFX-Pre under Advanced CFD on the left hand task bar.
9. Click General in the New Simulation File window and then click OK.
12. Click Save.

Importing a Mesh
An assembly is a group of mesh regions that are topologically connected. Each assembly
can contain only one mesh, but multiple assemblies are permitted.


Procedure 1. Select File > Import Mesh.
2. From your tutorial directory, select InjectMixerMesh.gtm.
3. Click Open.
(Y up) from the shortcut menu.

Setting Temperature-Dependent Material Properties
You will create an expression for viscosity as a function of temperature and then use this
expression to modify the properties of the library material: Water.
Viscosity will be made to vary linearly with temperature between the following conditions:
• µ =1.8E-03 N s m-2 at T=275.0 K
• µ =5.45E-04 N s m-2 at T=325.0 K
The variable T (Temperature) is a ANSYS CFX System Variable recognized by ANSYS CFX-Pre,
denoting static temperature. All variables, expressions, locators, functions, and constants
can be viewed by double-clicking the appropriate entry (such as Additional Variables
or Expressions) in the tree view.
All expressions must have consistent units. You should be careful if using temperature in an
expression with units other than [K].
The Expressions tab lets you define, modify, evaluate, plot, copy, delete and browse
through expressions used within ANSYS CFX-Pre.

Procedure 1. From the main menu, select Insert > Expressions, Functions and Variables >
Expression.
2. In the New Expression dialog box, type Tupper.
3. Click OK.
The details view for the Tupper equation is displayed.
4. Under Definition, type 325 [K].
5. Click Apply to create the expression.
The expression is added to the list of existing expressions.
6. Right-click in the Expressions workspace and select New.
7. In the New Expression dialog box, type Tlower.
8. Click OK.
9. Under Definition, type 275 [K].
The expression is added to the list of existing expressions.
11. Create expressions for Visupper, Vislower and VisT using the following values.

Name Definition
Visupper 5.45E-04 [N s m^-2]
Vislower 1.8E-03 [N s m^-2]
VisT Vislower+(Visupper-Vislower)*(T-Tlower)/(Tupper-Tlower)



Plotting an Expression
Procedure 1. Right-click VisT in the Expressions tree view, and then select Edit.
The Expressions details view for VisT appears.
Tip: Alternatively, double-clicking the expression also opens the Expressions details
view.
2. Click the Plot tab and apply the following settings

Tab Setting Value
Plot Number of Points 10
T (Selected)
Start of Range 275 [K]
End of Range 325 [K]

3. Click Plot Expression.
A plot showing the variation of the expression VisT with the variable T is displayed.

Evaluating an Expression
Procedure 1. Click the Evaluate tab.
2. In T, type 300 [K].
This is between the start and end range defined in the last module.
3. Click Evaluate Expression.
The value of VisT for the given value of T appears in the Value field.

Modify Material Properties
Default material properties (such as those of Water) can be modified when required.

Procedure 1. Click the Outline tab.
2. Double click Water under Materials to display the Basic Settings tab.
3. Click the Material Properties tab.
4. Expand Transport Properties.
5. Select Dynamic Viscosity.
6. Under Dynamic Viscosity, click in Dynamic Viscosity.

7. Click Enter Expression .
8. Enter the expression VisT into the data box.
9. Click OK.

Creating the Domain
The domain will be set to use the thermal energy heat transfer model, and the k-ε
(k-epsilon) turbulence model.


Both General Options and Fluid Models are changed in this module. The Initialization tab
is for setting domain-specific initial conditions, which are not used in this tutorial. Instead,
global initialization is used to set the starting conditions.

Procedure 1. Select Insert > Domain from the main menu or click Domain .
2. In the Insert Domain dialog box, type InjectMixer.
3. Click OK.

Tab Setting Value
General Options Basic Settings > Location B1.P3
Basic Settings > Fluids List Water
Domain Models > Pressure > 0 [atm]
Reference Pressure

5. Click Fluid Models.

Setting Value
Heat Transfer > Option Thermal Energy

7. Click OK.

Creating the Side Inlet Boundary Conditions
The side inlet boundary condition needs to be defined.

Procedure 1. Select Insert > Boundary Condition from the main menu or click Boundary Condition
.
2. Set Name to side inlet.
3. Click OK.

Tab Setting Value
Basic Settings Boundary Type Inlet
Location side inlet
Boundary Details Mass and Momentum > Option Normal Speed
Heat Transfer > Option Static Temperature
Static Temperature 315 [K]

5. Click OK.



Creating the Main Inlet Boundary Conditions
The main inlet boundary condition needs to be defined. This inlet is defined using a velocity
profile found in the example directory. Profile data needs to be initialized before the
boundary condition can be created.
You will create a plot showing the velocity profile data, marked by higher velocities near the
center of the inlet, and lower velocities near the inlet walls.

Procedure 1. Select Tools > Initialize Profile Data.

2. Under Data File, click Browse .
3. From your working directory, select InjectMixer_velocity_profile.csv.
4. Click Open.
5. Click OK.
The profile data is read into memory.
6. Select Insert > Boundary Condition from the main menu or click Boundary Condition
.
7. Set name Name to main inlet.
8. Click OK.

Tab Setting Value
Location main inlet
Profile Boundary Conditions (Selected)
> Use Profile Data
Profile Boundary Setup > main inlet
Profile Name

10. Click Generate Values.
This causes the profile values of U, V, W to be applied at the nodes on the main inlet
boundary, and U, V, W entries to be made in Boundary Details. To later modify the
velocity values at the main inlet and reset values to those read from the BC Profile file,
revisit Basic Settings for this boundary condition and click Generate Values.

Tab Setting Value
Boundary Details Flow Regime > Option Subsonic
Turbulence > Option Medium (Intensity = 5%)
Static Temperature 285 [K]
Plot Options Boundary Contour (Selected)
Profile Variable W

12. Click OK.


13. Zoom into the main inlet to view the inlet velocity contour.

Creating the Main Outlet Boundary Condition
In this module you create the outlet boundary condition. All other surfaces which have not
been explicitly assigned a boundary condition will remain in the InjectMixer Default
object, which is shown in the tree view. This boundary condition uses a No-Slip
Adiabatic Wall by default.

Procedure 1. Select Insert > Boundary Condition from the main menu or click Boundary Condition
.
2. Set Name to outlet.
3. Click OK.

Tab Setting Value
Basic Settings Boundary Type Outlet
Location outlet
Mass and Momentum > Option Average Static Pressure

5. Click OK.

Setting Initial Values
Procedure 1. Click Global Initialization .
2. Select Turbulence Eddy Dissipation.
3. Click OK.




Tab Setting Value
Basic Settings Advection Scheme > Option Specified Blend Factor
Advection Scheme > Blend 0.75
Factor
Convergence Control > Max. 50
Iterations
Convergence Control > Physical Timescale
Fluid Timescale Control >
Timescale Control
Convergence Control > 2 [s]
Fluid Timescale Control >
Physical Timescale
Convergence Criteria > RMS
Residual Type
Convergence Criteria > 1.E-4*
Residual Target
*. An RMS value of at least 1.E-5 is usually required for adequate convergence, but the
default value is sufficient for demonstration purposes.

3. Click OK.

Once the problem has been defined you move from General Mode into ANSYS CFX-Solver.

The Write Solver File dialog box appears.

Setting Value
File name InjectMixer.def


This file is provided in the tutorial directory and may exist in your working folder if you
5. If prompted, click Yes or Save & Quit to save InjectMixer.cfx.
The definition file (InjectMixer.def), mesh file (InjectMixer.gtm) and the
simulation file (InjectMixer.cfx) are created. ANSYS CFX-Solver Manager
automatically starts and the definition file is set in the Definition File box of Define
Run.


Tutorial 3: Flow in a Process Injection Mixing Pipe: Obtaining a Solution Using ANSYS CFX-Solver Manager

If you have performed all the tasks in the previous steps, proceed directly to Obtaining a
Solution Using ANSYS CFX-Solver Manager (p. 87).

Standalone 2. Select Session > Play Tutorial.
3. Select InjectMixer.pre.
4. Click Open.
6. Launch ANSYS CFX-Solver Manager from CFX Launcher.
7. After ANSYS CFX-Solver starts, select File > Define Run.

9. Select InjectMixer.def, located in the working directory.

ANSYS 2. Click Empty Project.
Workbench

4. Under Filename, type InjectMixer.
5. Click Save.
8. Select InjectMixer.pre.
9. Click Open.

13. Select InjectMixer.def, located in the working directory.

At this point, ANSYS CFX-Solver Manager is running, and the Define Run dialog box is
displayed, with the definition file set.
1. Click Start Run.
2. Click No to close the message box that appears when the run ends.


Tutorial 3: Flow in a Process Injection Mixing Pipe: Viewing the Results in ANSYS CFX-Post

Moving from ANSYS CFX-Solver Manager to ANSYS CFX-Post

1. Select Tools > Post–Process Results or click Post–Process Results .
2. If using ANSYS CFX-Solver Manager in standalone mode, optionally select Shut down
Solver Manager.
3. Click OK.

When ANSYS CFX-Post starts, the viewer and Outline workspace display by default.

Workflow Overview
1. Modifying the Outline of the Geometry (p. 88)
2. Creating and Modifying Streamlines (p. 88)
3. Modifying Streamline Color Ranges (p. 89)
4. Coloring Streamlines with a Constant Color (p. 89)
5. Duplicating and Modifying a Streamline Object (p. 90)
6. Examining Turbulent Kinetic Energy (p. 90)

Modifying the Outline of the Geometry
Throughout this and the following examples, use your mouse and the Viewing Tools
toolbar to manipulate the geometry as required at any time.

Procedure 1. In the tree view, double click Wireframe.
2. Set the Edge Angle to 15 [degree].
3. Click Apply.

Creating and Modifying Streamlines
When you complete this module you will see streamlines (mainly blue and green) starting
at the main inlet of the geometry and proceeding to the outlet. Above where the side pipe
meets the main pipe, there is an area where the flow re-circulates rather than flowing
roughly tangent to the direction of the pipe walls.

Procedure 1. Select Insert > Streamline from the main menu or click Streamline .
2. Under Name, type MainStream.
3. Click OK.



Tab Setting Value
Geometry Type 3D Streamline
Definition > Start From main inlet

5. Click Apply.
6. Right-click a blank area in the viewer, select Predefined Camera from the shortcut
menu, then select Isometric View (Y up).
The pipe is displayed with the main inlet in the bottom right of the viewer.

Modifying Streamline Color Ranges
You can change the appearance of the streamlines using the Range setting on the Color
tab.

Procedure 1. Under User Locations and Plots, modify the streamline object MainStream by
applying the following settings

Tab Setting Value
Color Range Local

2. Click Apply.
The color map is fitted to the range of velocities found along the streamlines. The
streamlines therefore collectively contain every color in the color map.

Tab Setting Value
Color Range User Specified
Min 0.2 [m s^-1]
Max 2.2 [m s^-1]

Note: Portions of streamlines that have values outside the range shown in the legend are
colored according to the color at the nearest end of the legend. When using tubes or
symbols (which contain faces), more accurate colors are obtained with lighting turned off.
4. Click Apply.
The streamlines are colored using the specified range of velocity values.

Coloring Streamlines with a Constant Color

Tab Setting Value
Color Mode Constant
Color (Green)


Color can be set to green by selecting it from the color pallet, or by repeatedly clicking
on the color box until it cycles through to the default green color.
2. Click Apply.

Duplicating and Modifying a Streamline Object
Any object can be duplicated to create a copy for modification without altering the original.

Procedure 1. Right-click MainStream and select Duplicate from the shortcut menu.
2. In the Name window, type SideStream.
3. Click OK.
4. Double click on the newly created streamline, SideStream.

Tab Setting Value
Geometry Definition > Start From side inlet
Color Mode Constant
Color (Red)

6. Click Apply.
Red streamlines appear, starting from the side inlet.
7. For better view, select Isometric View (Y up).

Examining Turbulent Kinetic Energy
A common way of viewing various quantities within the domain is to use a slice plane, as
demonstrated in this module.

Note: This module has multiple changes compiled into single steps in preparation for other
tutorials that provide fewer specific instructions.

Procedure 1. Clear visibility for both the MainStream and the SideStream objects.
2. Create a plane named Plane 1 that is normal to X and passing through the X = 0 Point.
To do so, specific instructions follow.
a. From the main menu, select Insert > Location > Plane and click OK.
b. In the Details view set Definition > Method to YZ Plane and X to 0 [m].
c. Click Apply.
3. Color the plane using the variable Turbulence Kinetic Energy, to show regions of
high turbulence. To do so, apply the settings below.

Tab Setting Value
Color Mode Variable
Variable Turbulence Kinetic Energy

4. Click Apply.


5. Experiment with other variables to color this plane (for example, Temperature to show
the temperature mixing of the two streams).
Commonly used variables are in the drop-down menu. A full list of available variables
can be viewed by clicking next to the Variable data box.

When finished with ANSYS CFX-Post exit the current window.
either the Standalone procedure or the Workbench procedure.

Procedure in 1. When you are finished, select File > Quit to exit ANSYS CFX-Post.
Standalone 2. Click Quit if prompted to save.

Procedure in 1. When you are finished, select File > Close to close the current file.
Workbench 2. Click Close if prompted to save.


Tutorial 4:
Flow from a Circular Vent

Introduction
• Defining a Steady-State Simulation in ANSYS CFX-Pre (p. 95)
• Obtaining a Solution to the Steady-State Problem (p. 99)
• Defining a Transient Simulation in ANSYS CFX-Pre (p. 100)
• Obtaining a Solution to the Transient Problem (p. 104)

before beginning:
• CircVent.pre
• CircVentIni.pre
• CircVentIni_001.res
• CircVentMesh.gtm
• CircVentIni.cfx
• CircVentIni.gtm


Tutorial 4: Flow from a Circular Vent: Tutorial 4 Features

Tutorial 4 Features

Transient
Opening
Wall: No-Slip
Timestep Auto Time Scale
Transient Example
Transient Results File
Isosurface
Other Auto Annotation
MPEG Generation
Printing
Time Step Selection
Title/Text
Transient Animation

• Setting up a transient problem in ANSYS CFX-Pre.
• Using an opening type boundary condition in ANSYS CFX-Pre.
• Modeling smoke using additional variables in ANSYS CFX-Pre.
• Visualizing a smoke plume using an Isosurface in ANSYS CFX-Post.
• Creating an image for printing, and generating an MPEG file in ANSYS CFX-Post.


Tutorial 4: Flow from a Circular Vent: Overview of the Problem to Solve

In this example, a chimney stack releases smoke which is dispersed into the atmosphere
with an oncoming side wind. Unlike previous tutorials, which were steady-state, this
example is time-dependent. Initially, no smoke is being released. In the second part of the
tutorial, the chimney starts to release smoke and it shows how the plume of smoke above
the chimney develops with time.

smoke speed varying
from zero to 0.2 m/s
wind speed
1 m/s

r=10 m

Defining a Steady-State Simulation in ANSYS CFX-Pre
This section describes the step-by-step definition of the flow physics in ANSYS CFX-Pre for a
steady-state simulation with no smoke being produced by the chimney. The results from
this simulation will be used as the initial guess for the transient simulation.

then run the session file: CircVentIni.pre. After you have played the session file as
described in earlier tutorials under Playing the Session File and Starting ANSYS CFX-Solver
Manager (p. 87), proceed to Obtaining a Solution to the Steady-State Problem (p. 99).

1. Start ANSYS CFX-Pre.
3. Select General and click OK.
5. Under File name, type CircVentIni.
6. Click Save.


Tutorial 4: Flow from a Circular Vent: Defining a Steady-State Simulation in ANSYS CFX-Pre

Importing the Mesh
1. Select File > Import Mesh.
2. From your working directory, select CircVentMesh.gtm.
3. Click Open.

Creating an Additional Variable
In this tutorial, an additional variable (non-reacting scalar component) will be used to model
the dispersion of smoke from the vent.

Note: While smoke is not required for the steady-state simulation, including it here prevents
the user from having to set up timevalue interpolation in the transient simulation.
1. From the main menu, select Insert > Expressions, Functions and Variables >
Additional Variable or click Additional Variable .
2. Under Name, type smoke.
3. Click OK.
4. Under Variable Type, select Volumetric.
5. Set Units to [kg m^-3].
6. Click OK.

Creating the Domain
The fluid domain will be created that includes the additional variable.

To Create a New 1. Select Insert > Domain from the main menu, or click Domain , then set the name to
Domain CircVent and click OK.

Tab Setting Value
General Options Fluids List Air at 25 C
Reference Pressure 0 [atm]
Fluid Models Heat Transfer > Option None
Additional Variable Details > smoke (Selected)
Additional Variable Details > smoke > (Selected)
Kinematic Diffusivity
Additional Variable Details > smoke > 1.0E-5 [m^2 s^-1]
Kinematic Diffusivity > Kinematic
Diffusivity

3. Click OK.



Creating the Boundary Conditions
This is an example of external flow, since fluid is flowing over an object and not through an
enclosure such as a pipe network (which would be an example of internal flow). In such
problems, some inlets will be made sufficiently large that they do not affect the CFD
solution. However, the length scale values produced by the Default Intensity and
AutoCompute Length Scale option for turbulence are based on inlet size. They are
appropriate for internal flow problems and particularly, cylindrical pipes. In general, you
need to set the turbulence intensity and length scale explicitly for large inlets in external
flow problems. If you do not have a value for the length scale, you can use a length scale
based on a typical length of the object, over which the fluid is flowing. In this case, you will
choose a turbulence length scale which is one-tenth of the diameter of the vent.

Note: The boundary marker vectors used to display boundary conditions (Inlets, Outlets,
Openings) are normal to the boundary surface regardless of the actual direction
specification. To plot vectors in the direction of flow, select Boundary Vector under the
Plot Options tab for the inlet boundary condition and clear Show Inlet Markers on the
Boundary Marker Options tab of Labels and Markers (accessible by clicking
Label and Marker Visibility ).

For parts of the boundary where the flow direction changes, or is unknown, an opening
boundary condition can be used. An opening boundary condition allows flow to both enter
and leave the fluid domain during the course of the solution.

Inlet Boundary 1. Select Insert > Boundary Condition from the main menu or click Boundary Condition
.
2. Under Name, type Wind.
3. Click OK.

Tab Setting Value
Location Wind
Boundary Details Mass and Momentum > Option Cart. Vel. Components
Mass and Momentum > U 1 [m s^-1]
Mass and Momentum > V 0 [m s^-1]
Mass and Momentum > W 0 [m s^-1]
Turbulence > Option Intensity and Length Scale
Turbulence > Value 0.05
Turbulence > Eddy Len. Scale 0.25 [m]
Additional Variables > smoke > Option Value
Additional Variables > smoke > Value 0 [kg m^-3]

5. Click OK.


Opening 1. Select Insert > Boundary Condition from the main menu or click Boundary Condition
Boundary .
2. Under Name, type Atmosphere.
3. Click OK.

Tab Setting Value
Basic Settings Boundary Type Opening
Location Atmosphere
Boundary Details Mass and Momentum > Option Opening Pres. and Dirn
Mass and Momentum > Relative Pressure 0 [Pa]
Flow Direction > Option Normal to Boundary
Condition

5. Click OK.

Inlet for the 1. Select Insert > Boundary Condition from the main menu or click Boundary Condition
Vent .
2. Under Name, type Vent.
3. Click OK.

Tab Setting Value
Location Vent
Boundary Details Mass and Momentum > Normal Speed 0.01 [m s^-1]
Turbulence > Option Intensity and Eddy Viscosity
Ratio

5. Click OK.

1. Click Global Initialization .
2. Select Turbulence Eddy Dissipation.
3. Click OK.


Tutorial 4: Flow from a Circular Vent: Obtaining a Solution to the Steady-State Problem

ANSYS CFX-Solver has the ability to calculate physical timestep size for steady-state
problems. If you do not know the time step size to set for your problem, you can use the
Auto Timescale option.

1. Click Solver Control .

Tab Setting Value
Basic Settings Convergence Control > Max. Iterations 75

3. Click OK.

1. Click Write Solver File .

Setting Value
File name CircVentIni.def
Quit CFX–Pre * (Selected)


4. Quit ANSYS CFX-Pre, saving the simulation (.cfx) file.

Obtaining a Solution to the Steady-State Problem
When ANSYS CFX-Pre has shut down and ANSYS CFX-Solver Manager has started, you can
obtain a solution to the CFD problem by using the following procedure.
1. Click Start Run.
The residual plots for six equations will appear: U - Mom, V - Mom, W - Mom, P - Mass,
K-TurbKE and E-Diss.K (the three momentum conservation equations, the mass
conservation equation and equations for the turbulence kinetic energy and turbulence
eddy dissipation). The Momentum and Mass tab contains four of the plots and the
other two are under Turbulence Quantities. The variable smoke is also plotted but
registers no values since it is not initialized.
2. Click No to close the completion message, since you do not need to view the results in
ANSYS CFX-Post.
3. If using Standalone Mode, quit ANSYS CFX-Solver Manager.
You will now reload the simulation into ANSYS CFX-Pre to define the transient
simulation.


Tutorial 4: Flow from a Circular Vent: Defining a Transient Simulation in ANSYS CFX-Pre

Defining a Transient Simulation in ANSYS CFX-Pre
In this part of the tutorial, you alter the simulation settings used for the steady-state
calculation to set up the model for the transient calculation in ANSYS CFX-Pre.

then run the session file: CircVent.pre. After you have played the session file as described
in earlier tutorials under Playing the Session File and Starting ANSYS CFX-Solver Manager
(p. 87), proceed to Obtaining a Solution to the Transient Problem (p. 104).

Opening the Existing Simulation
2. Select File > Open Simulation.
3. If required, set the path location to the tutorial folder.
4. Select the simulation file CircVentIni.cfx.
5. Click Open.
7. Change the name to CircVent.cfx.
8. Click Save.

Modifying the Simulation Type
In this step you will make the problem transient. Later, you will set the concentration of
smoke to rise exponentially with time, so it is necessary to ensure that the interval between
the timesteps is smaller at the beginning of the simulation than at the end.

1. Click Simulation Type .

Tab Setting Value
Basic Settings Simulation Type > Option Transient
Simulation Type > Time Duration > 30 [s]
Total Time
Simulation Type > Time Steps > 4*0.25, 2*0.5, 2*1.0, 13*2.0 [s]
Timesteps*†
Simulation Type > Initial Time > Time 0 [s]

*. Do NOT click Enter Expression to enter lists of values. Enter the list without the
units, then set the units in the drop-down list.
†. This list specifies 4 timesteps of 0.25 [s], then 2 timesteps of 0.5 [s], etc.

3. Click OK.



Modifying the Boundary Conditions
The only boundary condition which needs altering is the Vent boundary condition. In the
steady-state calculation, this boundary had a small amount of air flowing through it. In the
transient calculation, more air passes through the vent and there is a time-dependent
concentration of smoke in the air. This is initially zero, but builds up to a larger value. The
smoke concentration will be specified using the CFX Expression Language.

To Modify the 1. In the Outline workspace, expand the tree to Simulation > CircVent > Vent.
Vent Inlet 2. Right-click Vent and select Edit.
Boundary
Condition 3. Apply the following settings

Tab Setting Value

Leave the Vent details view open for now.
You are going to create an expression for smoke concentration. The concentration is
zero for time t=0 and builds up to a maximum of 1 kg m^-3.
4. Create a new expression by selecting Insert > Expressions, Functions and Variables
> Expression from the main menu. Set the name to TimeConstant.

Name Definition
TimeConstant 3 [s]

7. Create the following expressions with specific settings, remembering to click Apply
after each is defined.

Name Definition
FinalConcentration 1 [kg m^-3]
ExpFunction * FinalConcentration*abs(1-exp(-t/TimeConstant))

*. When entering this function, you can select most of the required items by
right-clicking in the Definition window in the Expression details view instead of
typing them. The names of the existing expressions are under the Expressions
menu. The exp and abs functions are under Functions > CEL. The variable t is
under Variables.

Note: The abs function takes the modulus (or magnitude) of its argument. Even though the
expression (1- exp (-t/TimeConstant)) can never be less than zero, the abs function is
included to ensure that the numerical error in evaluating it near to zero will never make the
expression evaluate to a negative number.

Next you will visualize how the expressions have scheduled the concentration of smoke
issued from the vent.


Plotting Smoke 1. Double-click ExpFunction in the Expressions tree view.
Concentration 2. Apply the following settings

Tab Setting Value
Plot t (Selected)
Start of Range 0 [s]
End of Range 30 [s]

3. Click Plot Expression.
The button name then changes to Define Plot, as shown.

As can be seen, the smoke concentration rises exponentially, and reaches 90% of its final
value at around 7 seconds.
4. Click the Boundary: Vent tab.
In the next step, you will apply the expression ExpFunction to the additional variable
smoke as it applies to the boundary Vent.

Tab Setting Value
Boundary Details Additional Variables > smoke > Option Value
Additional Variables > smoke > Value* ExpFunction

*. Click Enter Expression to enter text.

6. Click OK.



Initialization Values
The steady state solution that you have finished calculating is used to supply the initial
values to the ANSYS CFX-Solver. You can leave all of the initialization data set to Automatic
and the initial values will be read automatically from the initial values file. Therefore, there
is no need to revisit the initialization tab.

Modifying the Solver Control

2. Set Convergence Control > Max. Coeff. Loops to 3.
3. Leave the other settings at their default values.
4. Click OK to set the solver control parameters.

Output Control
To allow results to be viewed at different timesteps, it is necessary to create transient results
files at specified times. The transient results files do not have to contain all solution data. In
this step, you will create minimal transient results files.

To Create 1. From the main menu, select Insert > Solver > Output Control.
Minimal 2. Click the Trn Results tab.
Transient
Results Files 3. Click Add new item and then click OK to accept the default name for the object.
This creates a new transient results object. Each object can result in the production of
many transient results files.
4. Apply the following settings to Transient Results 1

Setting Value
Option Selected Variables
Output Variables List* Pressure, Velocity, smoke
Output Frequency > Option Time List
Output Frequency > Time List† 1, 2 , 3 [s]

*. Click the ellipsis icon to select items if they do not appear in the drop-down list. Use
the <Ctrl> key to select multiple items.

†. Do NOT click Enter Expression to enter lists of values. Enter the list without the
units, then set the units in the drop-down list.

5. Click Apply.
6. Create a second item with the default name Transient Results 2 and apply the
following settings to that item

Setting Value
Output Variables List Pressure, Velocity, smoke


Tutorial 4: Flow from a Circular Vent: Obtaining a Solution to the Transient Problem

Setting Value
Output Frequency > Option Time Interval
Output Frequency > Time Interval* 4 [s]

*. A transient results file will be produced every 4 s (including 0 s) and at 1 s, 2 s and
3 s. The files will contain no mesh and data for only the three selected variables. This
reduces the size of the minimal results files. A full results file is always written at the
end of the run.
7. Click OK.


Setting Value
File name CircVent.def
Quit CFX–Pre * Select


4. Quit ANSYS CFX-Pre, saving the simulation (.cfx) file at your discretion.

Obtaining a Solution to the Transient Problem
In this tutorial the ANSYS CFX-Solver will read the initial values for the problem from a file.
For details, see Initialization Values (p. 103). You need to specify the file name.
Define Run will be displayed when the ANSYS CFX-Solver Manager launches. Definition
File will already be set to the name of the definition file just written.
Notice that the text output generated by the ANSYS CFX-Solver will be more than you have
seen for steady-state problems. This is because each timestep consists of several inner
(coefficient) iterations. At the end of each timestep, information about various quantities is
printed to the text output area.
The variable smoke is now plotted under the Additional Variables tab.

1. Under Initial Values File, click Browse .
2. Select CircVentIni_001.res, which is the results file of the steady-state problem with
no smoke issuing from the chimney. If you have not run the first part of this tutorial, copy
CircVentIni_001.res from the <CFXROOT>/examples/ directory to your working
directory.
3. Click Open.
4. Click Start Run.
5. You may see a notice that the mesh from the initial values file will be used. This mesh is
the same as in the definition file. Click OK to continue.

Tutorial 4: Flow from a Circular Vent: Viewing the Results in ANSYS CFX-Post
ANSYS CFX-Solver runs and attempts to obtain a solution. This can take a long time
depending on your system. Eventually a dialog box is displayed.
6. When ANSYS CFX-Solver has finished, click Yes to post-process the results.

In this tutorial, you will view the dispersion of smoke from the vent over time. When ANSYS
CFX-Post is loaded, the results that are immediately available are those at the final timestep;
in this case, at t = 30 s (this is nominally designated Final State).

Creating an Isosurface
An isosurface is a surface of constant value of a variable. For instance, it could be a surface
consisting of all points where the velocity is 1 [m s^-1]. In this case, you are going to create
an isosurface of smoke density (smoke is the additional variable that you specified earlier).
1. Right-click on a blank area in the viewer and select Predefined Camera > Isometric
View (Z up).
This ensures that the view is set to a position that is best suited to display the results.
2. From the main menu, select Insert > Location > Isosurface or under Location, click
Isosurface.
3. Click OK.

Tab Setting Value
Geometry Variable smoke
Value 0.005 [kg m^-3]

5. Click Apply.
• A bumpy surface will be displayed, showing the smoke starting to emerge from the
vent.
• The surface is rough because the mesh is coarse. For a smoother surface, you would
re-run the problem with a smaller mesh length scale.
• The surface will be a constant color as the default settings on the Color tab were
used.
• When Color Mode is set to either Constant or Use Plot Variable for an
isosurface, it appears as one color.
6. In Geometry, experiment by changing the Value so that you can see the shape of the
plume more clearly.
Zoom in and rotate the geometry, as required.
7. When you have finished, set the Value to 0.002 [kg m^-3].
8. Right-click on a blank spot in the viewer and select Predefined Camera > Isometric
View (Z up).



Viewing the Results at Different Timesteps
The Timestep Selector shows the Time Step (outer loop) number, the Time Value
(simulated time in seconds) and the Type of results file that was saved at that timestep. You
can see that Partial results files were saved (as requested in ANSYS CFX-Pre) for all timesteps
except for the last one.

1. Click Timestep Selector .
2. Load the results for a time value of 2 s by double-clicking the appropriate row in the
Timestep Selector.
After a short pause, the Current Timestep (located just below the title bar of the
Timestep Selector) will be updated with the new timestep number.
3. Load the time value of 4 s using the Timestep Selector.
The smoke has now spread out even more, and is being carried by the wind.
4. Double-click some more time values to see how the smoke plume grows with time.
5. Finish by loading a time value of 1 s.

Generating Output Files
You can produce image output from ANSYS CFX-Post.

Adding a title First, you will add text to the viewer so that the printed output has a title.

1. Select Insert > Text from the main menu or click Create text .
2. Click OK.
3. In the Text String box, enter the following text.
Isosurface showing smoke concentration of 0.002 kg/m^3 after

Note: Further text will be added at a later stage to complete this title.
4. Select Embed Auto Annotation.
5. Set Type to Time Value.
In the text line, note that <aa> has been added to the end. This is where the time value
will be placed.
6. Click Apply to create the title.
7. Click the Location tab to modify the position of the title.
The default settings for text objects center text at the top of the screen. To experiment
with the position of the text, change the settings on the Location tab.
8. Under Appearance, change Color Mode to User Specified and select a new color.
9. Click Apply.

JPEG output ANSYS CFX-Post can produce hard-copy output in several different forms. In the next
section you will print in JPEG format.
1. Ensure a time value of 1 s is loaded.

2. Select File > Print, or click Print .
3. Under Format select JPEG.



4. Click Browse next to the File data box.
5. Browse to the directory where you want the file saved.
6. Enter a name for the JPEG file.
7. Click Save to set the file name and directory.
This sets the path and name for the file.
8. To print to the file, click Print.
To view the file or make a hard copy, use an application that supports JPEG files.
9. Clear the visibility of the text object to hide it.

To Generate an You can generate an MPEG file to show the transient flow of the plume of smoke. To
MPEG File generate an MPEG file, you use the Animation dialog box in the same way as in Tutorial 1.
However, to animate the plume of smoke, you need to animate over several timesteps.

Note: On the Advanced tab of Animation Options, there is a check box option called Save
frames as image files. By selecting this option, the JPEG or PPM files used to encode each
frame of the MPEG will persist after MPEG creation; otherwise, they are deleted.

Setting Keyframes
1. Click Animation .
2. Ensure that Keyframe Animation is selected.
3. Position the geometry so that you will be able to see the plume of smoke.

4. In the Animation dialog box, click New to create KeyFrameNo1.
5. Load the time value of 30 s using the Timestep Selector.

6. Click New in the Animation dialog box to create KeyframeNo2.

Defining additional options
During the production of a transient animation, various timesteps will be loaded and all
objects will be updated to use the results from that timestep. Each frame of the animation
must use one of the available timesteps.
In Animation, Timestep can be set to Timestep Interpolation, TimeValue
Interpolation or Sequential Interpolation. This setting affects which timestep is
loaded for each frame.
1. Click More Animation Options to show more animation settings.
2. Click Options.

Tab Setting Value
Options Transient Case* TimeValue Interpolation

*. This causes each frame to use the transient file having the closest time value.

4. Click OK.
5. Single click KeyframeNo1, then set # of Frames to 27 and press <Enter>.


The animation now contains a total of 29 frames (27 intermediate frames plus the two
keyframes).
6. Select Save MPEG.

8. Under File name, type CircVent.mpg.
10. Click Save.
produced.
11. Click To Beginning .

• The MPEG will be created as the animation proceeds.
• This will be slow, since a timestep must be loaded and objects must be created for
each frame.
• To view the MPEG file, you need to use a viewer that supports the MPEG format.
13. When you have finished, quit ANSYS CFX-Post.


Tutorial 5:
Flow Around a Blunt Body

Introduction

before beginning:
• BluntBody.pre
• BluntBodyDist.cse
• BluntBodyMesh.gtm

Tutorial 5 Features


Tutorial 5: Flow Around a Blunt Body: Tutorial 5 Features

Fluid Type Ideal Gas
Turbulence Model Shear Stress Transport
Heat Transfer Isothermal
Outlet (Subsonic)
Symmetry Plane
Wall: No-Slip
Wall: Free-Slip
ANSYS CFX-Solver Manager Parallel processing
ANSYS CFX-Post Plots Default Locators
Sampling Plane
Streamline
Vector
Volume
Instancing Transformation
Lighting Adjustment
Symmetry
Viewing the Mesh

• Solving and post-processing a case where the geometry has been omitted on one side
of a symmetry plane.
• Using free slip wall boundaries on the sides of and above the domain as a compromise
between accurate flow modeling and computational grid size.
• Accurately modeling the near-wall flow using Shear Stress Transport (SST) turbulence
model.
• Running the ANSYS CFX-Solver in parallel (optional).
• Creating vector plots in ANSYS CFX-Post with uniform spacing between the vectors.
• Creating a macro using power syntax in ANSYS CFX-Post.


Tutorial 5: Flow Around a Blunt Body: Overview of the Problem to Solve

This example demonstrates external air flow over a generic vehicle body. Since both the
geometry and the flow are symmetric about a vertical plane, only half of the geometry will
be used to find the CFD solution.
Figure 1 External Air Flow Over a Generic Vehicle Body

air speed
15.0 m/s 1.44 m

5.2 m

The following sections describe the simulation setup in ANSYS CFX-Pre.

then run the session file: BluntBody.pre. After you have played the session file as described
(p. 87), proceed to Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 116).

5. Under File name, type BluntBody.
6. Click Save.

Importing the Mesh
1. Right-click Mesh and select Import Mesh.


Tutorial 5: Flow Around a Blunt Body: Defining a Simulation in ANSYS CFX-Pre

Setting Value
File name BluntBodyMesh.gtm

3. Click Open.

Creating the Domain
The flow in the domain is expected to be turbulent and approximately isothermal. The
Shear Stress Transport (SST) turbulence model with automatic wall function treatment will
be used because of its highly accurate predictions of flow separation. To take advantage of
the SST model, the boundary layer should be resolved with at least 10 mesh nodes. In order
to reduce computational time, the mesh in this tutorial is much coarser than that.
This tutorial uses an ideal gas as the fluid whereas previous tutorials have used a specific
fluid. When modeling a compressible flow using the ideal gas approximation to calculate
density variations, it is important to set a realistic reference pressure. This is because some
fluid properties depend on the absolute fluid pressure (calculated as the static pressure plus
the reference pressure).

1. Click Domain , and set the name to BluntBody.
2. Apply the following settings to BluntBody:

Tab Setting Value
General Options Basic Settings > Fluids List Air Ideal Gas
Domain Models > Pressure > Reference Pressure 1 [atm]
Fluid Models Heat Transfer > Option Isothermal
Heat Transfer > Fluid Temperature 288 [K]
Turbulence > Option Shear Stress Transport

3. Click OK.

Creating Composite Regions
An imported mesh may contain many 2D regions. For the purpose of creating boundary
conditions, it can sometimes be useful to group several 2D regions together and apply a
single boundary condition to the composite 2D region. In this case, you are going to create
a Union between two regions that both require a free slip wall boundary condition.
1. From the main menu, select Insert > Composite Region.
2. Set the name to FreeWalls and click OK.

Tab Setting Value
Basic Settings Dimension (Filter) 2D

4. In the region list, hold down the <Ctrl> key and select Free1 and Free2.


5. Click OK.

The simulation requires inlet, outlet, wall (no slip and free slip) and symmetry plane
boundary conditions. The regions for these boundary conditions were defined when the
mesh was created (except for the composite region just created for the free slip wall
boundary condition).

Inlet Boundary 1. Click Boundary Condition .
2. Under Name, type Inlet.

Tab Setting Value
Location Inlet
Mass and Momentum > Option Normal Speed
Mass and Momentum > Normal Speed 15 [m s^-1]

4. Click OK.

Outlet 1. Create a new boundary condition named Outlet.
Boundary 2. Apply the following settings

Tab Setting Value
Location Outlet
Boundary Details Mass and Momentum > Option Static Pressure

3. Click OK.

Free Slip Wall The top and side surfaces of the rectangular region will use free slip wall boundary
Boundary conditions.
• On free slip walls the shear stress is set to zero so that the fluid is not retarded.
• The velocity normal to the wall is also set to zero.
• The velocity parallel to the wall is calculated during the solution.
This is not an ideal boundary condition for this situation since the flow around the body will
be affected by the close proximity to the walls. If this case was modeling a wind tunnel
experiment, the domain should model the size and shape of the wind tunnel and use no-slip
walls. If this case was modeling a blunt body open to the atmosphere, a much larger domain
should be used to minimize the effect of the walls.

You will apply a single boundary condition to both walls by using the composite region
defined earlier.
1. Create a new boundary condition named FreeWalls.

Tab Setting Value
Basic Settings Boundary Type Wall
Location FreeWalls
Boundary Details Wall Influence On Flow > Option Free Slip

3. Click OK.

Symmetry Plane 1. Create a new boundary condition named SymP.
Boundary 2. Apply the following settings:

Tab Setting Value
Basic Settings Boundary Type Symmetry
Location SymP

3. Click OK.

Wall Boundary 1. Create a new boundary condition named Body.
on the Blunt 2. Apply the following settings:
Body Surface

Tab Setting Value
Location Body
Boundary Details Wall Influence On Flow > Option No Slip

3. Click OK.
The remaining 2D regions (in this case, just the low Z face) will be assigned the default
boundary condition which is an adiabatic, no-slip wall condition. In this case, the name of
the default boundary condition is Default Boundary. Although the boundary conditions
Body and Default Boundary are identical (except for their locations), the Body boundary
condition was created so that, during post-processing, its location can by conveniently
distinguished from the other adiabatic, no-slip wall surfaces.




Tab Setting Value
Global Settings Initial Conditions > Cartesian Velocity Automatic with Value
Components > Option
Initial Conditions > Cartesian Velocity 15 [m s^-1]
Components > U
Components > V
Components > W
Initial Conditions > Turbulence Eddy (Selected)
Dissipation

3. Click OK.


Tab Setting Value
Timescale Control
Convergence Control > Fluid Timescale Control > 2 [s]
Physical Timescale
Convergence Criteria > Residual Target 1e-05

3. Click OK.


Setting Value
File name BluntBody.def


4. If using Standalone Mode, quit ANSYS CFX-Pre, saving the simulation (.cfx) file at your
discretion.


Tutorial 5: Flow Around a Blunt Body: Obtaining a Solution Using ANSYS CFX-Solver Manager

This tutorial introduces the parallel solver capabilities of ANSYS CFX.

Note: The results produced will be identical, whether produced by a parallel or serial run.
If you do not want to solve this tutorial in parallel (on more than one processor) or you do
not have a license to run the ANSYS CFX-Solver in parallel, proceed to Obtaining a Solution
in Serial (p. 116).
If you do not know if you have a license to run the ANSYS CFX-Solver in parallel, you should
either ask your system administrator, or query the license server (see the ANSYS, Inc.
Licensing Guide (which is installed with the ANSYS License Manager) for details).
Alternatively proceed to Obtaining a Solution in Serial (p. 116).
If you would like to solve this tutorial in parallel on the same machine, proceed to Obtaining
a Solution with Local Parallel (p. 117).
If you would like to solve this tutorial in parallel across different machines, proceed to
Obtaining a Solution with Distributed Parallel (p. 117).

Obtaining a Solution in Serial
1. Click Start Run.
2. Click Yes to process the results in ANSYS CFX-Post.
Continue this tutorial from Viewing the Results in ANSYS CFX-Post (p. 119).

Obtaining a Solution in Parallel
Background to Using the parallel capability of the ANSYS CFX-Solver allows you to divide a large CFD
Parallel Running problem so that it can run on more than one processor/machine at once. This saves time
in ANSYS CFX
and, when multiple machines are used, avoids problems which arise when a CFD calculation
requires more memory than a single machine has available. The partition (division) of the
CFD problem is automatic.
A number of events occur when you set up a parallel run and then ask the ANSYS CFX-Solver
to calculate the solution:
• Your mesh will be divided into the number of partitions that you have chosen.
• The ANSYS CFX-Solver runs separately on each of the partitions on the selected
machine(s).
• The results that one ANSYS CFX-Solver process calculates affects the other ANSYS
CFX-Solver processes at the interface between the different sections of the mesh.
• All of the ANSYS CFX-Solver processes are required to communicate with each other
and this is handled by the master process.


• The master process always runs on the machine that you are logged into when the
parallel run starts. The other ANSYS CFX-Solver processes are slave processes and may
be run on other machines.
• After the problem has been solved, a single results file is written. It will be identical to a
results file from the same problem run as a serial process, with one exception: an extra
variable Real partition number will be available for the parallel run. This variable will
be used later in this tutorial during post processing.

Obtaining a To run in local parallel mode, the machine you are on must have more than one processor.
Solution with
In ANSYS CFX-Solver Manager, the Define Run dialog box should already be open.
Local Parallel
1. Leave Type of Run set to Full.
If Type of Run was instead set to Partitioner Only, your mesh would be split into a
number of partitions but would not be run in the ANSYS CFX-Solver afterwards.
2. Set Run Mode to PVM Local Parallel .
This is the recommended method for most applications.

3. If required, click Add Partition to add more partitions.
By default, 2 partitions are assigned.
4. Select Show Advanced Controls.
5. Click the Partitioner tab at the top of the dialog box.
6. Use the default MeTiS partitioner.
Your model will be divided into two sections, with each section running in its own
ANSYS CFX-Solver process. The default is the MeTiS partitioner because it produces
more efficient partitions than either Recursive Coordinate Bisection or User
Specified Direction.
7. Click Start Run.

8. Click Post–Process Results .
9. If using ANSYS CFX-Solver in Standalone Mode, select Shut down Solver Manager, and
then click OK.
Continue this tutorial from Text Output when Running in Parallel (p. 118).

Obtaining a Before running in Distributed Parallel mode, please ensure that your system has been
Solution with configured as described in the installation documentation.
Distributed
Parallel In ANSYS CFX-Solver Manager, the Define Run dialog box should already be open.
1. Leave Type of Run set to Full.
If Type of Run was instead set to Partitioner Only, your mesh would be split into a
number of partitions but would not be run in the ANSYS CFX-Solver afterwards.
2. Set Run Mode to PVM Distributed Parallel.
The name of the machine that you are currently logged into should be in the Host
Name list. You are going to run with two partitions on two different machines, so
another machine must be added.

3. Click Insert Host to specify a new host machine.


• The Select Parallel Hosts dialog box is displayed. This is where you choose
additional machines to run your processes.
• Your system administrator should have set up a hosts file containing a list of the
machines that are available to run the parallel ANSYS CFX-Solver.
• The Host Name column displays names of available hosts.
• The second column shows the number of processors on that machine.
• The third shows the relative processor speed: a processor on a machine with a
relative speed of 1 would typically be twice as fast as a machine with a relative speed
of 0.5.
• The last column displays operating system information.
• This information is read from the hosts file; if any information is missing or incorrect
your system administrator should correct the hosts file.
Note: The # processors, relative speed and system information does not have to be specified
to be able to run on a host.

4. Select the name of another machine in the Host Name list.
Select a machine that you can log into.
5. Click Add.
The name of the machine is added to the Host Name column.
Note: Ensure that the machine that you are currently logged into is in the Hosts Name list
in the Define Run dialog box.
6. Close the Select Parallel Hosts dialog box.
7. Select Show Advanced Controls.
8. Click the Partitioner tab at the top of the dialog box.
9. Use the default MeTiS partitioner.
Your model will be divided into two sections, with each section running in its own
ANSYS CFX-Solver process. The default is the MeTiS partitioner because it produces
more efficient partitions than either Recursive Coordinate Bisection or User
Specified Direction.
10. Click Start Run to begin the parallel run.
11. Click OK on the pop-up message.
12. Click Yes to post-process the results when the completion message appears at the end
of the run.
13. Close ANSYS CFX-Solver Manager.

Text Output The text output area shows what is being written to the output file. You will see information
when Running similar to the following:
in Parallel +--------------------------------------------------------------------+
| Job Information |
+--------------------------------------------------------------------+
Run mode: partitioning run
Host computer: fastmachine1
Job started: Wed Nov 28 15:18:40 2005


Tutorial 5: Flow Around a Blunt Body: Viewing the Results in ANSYS CFX-Post
This tells you that the information following is concerned with the partitioning. After the
partitioning job has finished, you will find:
CPU-Time requirements:
- Preparations 1.460E+00 seconds
- Low-level mesh partitioning 1.000E-01 seconds
- Global partitioning information 3.100E-01 seconds
- Vertex, element and face partitioning information 1.600E-01 seconds
- Element and face set partitioning information 5.000E-02 seconds
- Summed CPU-time for mesh partitioning 2.080E+00 seconds
+--------------------------------------------------------------------+
| Job Information |
+--------------------------------------------------------------------+
Job finished: Wed Nov 28 15:19:16 2005
Total CPU time: 1.143E+01 seconds
or: ( 0: 0: 0: 11.428 )
( Days: Hours: Minutes: Seconds )
This marks the end of the partitioning job. The ANSYS CFX-Solver now begins to solve your
parallel run:
+--------------------------------------------------------------------+
| Job Information |
+--------------------------------------------------------------------+
Run mode: parallel run (PVM)
Par. Process: Master running on mesh partition: 1
Job started: Thu Nov 28 15:19:20 2005
Host computer: slowermachine
Par. Process: Slave running on mesh partition: 2
Job started: Thu Nov 28 15:24:55 2005
The machine that you are logged into runs the master process, and controls the overall
simulation. The second machine selected will run the slave process. If you had more than
two processes, each additional process is run as a slave process.
The master process in this example is running on the mesh partition number 1 and the slave
is running on partition number 2. You can find out which nodes and elements are in each
partition by using ANSYS CFX-Post later on in the tutorial.
When the ANSYS CFX-Solver finishes, the output file displays the job information and a
pop-up message to indicate completion of the run.

In this tutorial, a vector plot is created in ANSYS CFX-Post. This will let you see how the flow
behaves around the body. You will also use symmetry planes and learn more about
manipulating the geometry view in the viewer.

Using Symmetry Planes
Earlier in this tutorial you used a symmetry plane boundary condition because the entire
blunt body is symmetrical about a plane. Due to this symmetry, it was necessary to use only
half of the full geometry to calculate the CFD results. However, for visualization purposes, it
is helpful to use the full blunt body. ANSYS CFX-Post is able to recreate the full data set from
the half that was originally calculated. This is done by creating an Instance Transform
object.


Manipulating You need to manipulate the geometry so that you will be able to see what happens when
the Geometry you use the symmetry plane. The ANSYS CFX-Post features that you have used in earlier
tutorials will not be described in detail. New features will be described in detail.
+X.

Creating an Instance Transforms are used to visualize a full geometry representation in cases where the
Instance simulation took advantage of symmetry to solve for only part of the geometry. There are
Transform
three types of transforms that you can use: Rotation, Translation, Reflection. In this tutorial,
you will create a Reflection transform located on a plane.
1. Click Location > Plane and set the name to Reflection Plane .

Tab Setting Value
Geometry Definition > Method ZX Plane
Render Draw Faces (cleared)

3. Click Apply.
This creates a plane in the same location as the symmetry plane defined in ANSYS
CFX-Pre. Now the instance transform can be created using this Plane:
4. From the main menu, select Insert > Instance Transform and accept the default name.

Tab Setting Value
Definition Instancing Info From Domain (Cleared)
Apply Rotation (Cleared)
Apply Reflection (Selected)
Apply Reflection > Plane Reflection Plane

6. Click Apply.

Using the You can use the transform when creating or editing graphics objects. For example, you can
Reflection modify the Wireframe view to use it as follows:
Transform
1. Under the Outline tab, in User Locations and Plots, apply the following settings to
Wireframe:

Tab Setting Value
View Apply Instancing Transform > Transform Instance Transform 1

2. Click Apply.
3. Zoom so that the geometry fills the Viewer.
You will see the full blunt body.



Creating Vectors
You are now going to create a vector plot to show velocity vectors behind the blunt body.
You need to first create an object to act as a locator, which, in this case, will be a sampling
plane. Then, create the vector plot itself.

Creating the A sampling plane is a plane with evenly spaced sampling points on it.
Sampling Plane
+Y.
This ensures that the changes can be seen.
2. Create a new plane named Sample.

Tab Setting Value
Geometry Definition > Method Point and Normal
Definition > Point 6, -0.001, 1
Definition > Normal 0, 1, 0
Plane Bounds > Type Rectangular
Plane Bounds > X Size 2.5 [m]
Plane Bounds > Y Size 2.5 [m]
Plane Type Sample
Plane Type > X Samples 20
Plane Type > Y Samples 20

4. Click Apply.
You can zoom in on the sampling plane to see the location of the sampling points
(where lines intersect). There are a total of 400 (20 * 20) sampling points on the plane. A
vector can be created at each sampling point.
5. Hide the plane by clearing the visibility check box next to Sample.

Creating a 1. Click Vector and accept the default name.
Vector Plot 2. Apply the following settings:
Using Different
Sampling
Methods Tab Setting Value
Geometry Definition > Locations Sample
Definition > Sampling Vertex
Symbol Symbol Size 0.25

3. Click Apply.
4. Zoom until the vector plot is roughly the same size as the viewer.
You should be able to see a region of recirculation behind the blunt body.


5. Ignore the vertices on the sampling plane and increase the density of the vectors by
applying the following settings:

Tab Setting Value
Geometry Definition > Sampling Equally Spaced
Definition > # of Points 1000

6. Click Apply.
7. Change the location of the Vector plot by applying the following setting:

Tab Setting Value
Geometry Definition > Locations SymP

8. Click Apply.

Creating a Pressure Plot
1. Apply the following settings to the boundary condition named Body:

Tab Setting Value
Color Mode Variable
Variable Pressure

2. Click Apply.
3. Apply the following settings to SymP:

Tab Setting Value
Draw Line (Selected)

4. Click Apply.
You will be able to see the mesh around the blunt body, with the mesh length scale
decreasing near the body, but still coarse in the region of recirculation. By zooming in,
you will be able to see the layers of inflated elements near the body.

Creating Surface Streamlines
In order to show the path of air along the surface of the blunt body, surface streamlines can
be made as follows:
1. Clear the visibility of Body, SymP and Vector 1.
2. Create a new plane named Starter.



Tab Setting Value
Geometry Definition > Method YZ Plane
X -0.1 [m]

4. Click Apply.
The plane appears just upstream of the blunt body.
5. Clear the visibility check box for the plane.
This hides the plane from view, although the plane still exists.
6. Click Streamline . and click OK to accept the default name.

Tab Setting Value
Geometry Type Surface Streamline
Definition > Surfaces Body
Definition > Start From Locations
Definition > Locations Starter
Definition > Max Points 100
Definition > Direction Forward

8. Apply the following settings.
The surface streamlines appear on half of the surface of the blunt body. They start near
the upstream end because the starting points were formed by projecting nodes from
the plane to the blunt body.

Moving Objects
In ANSYS CFX-Post, you can reposition some locator objects directly in the viewer by using
the mouse.
1. Select the visibility check box for the plane named Starter.

2. Select the Single Select mouse pointer from the Selection Tools toolbar.
3. In the viewer, click the Starter plane to select it, then use the left mouse button to drag
it along the X axis.
Notice that the streamlines are redrawn as the plane moves.

Creating a Surface Plot of y+
The velocity next to a no-slip wall boundary changes rapidly from a value of zero at the wall
to the free stream value a short distance away from the wall. This layer of high velocity
gradient is known as the boundary layer. Many meshes are not fine enough near a wall to
accurately resolve the velocity profile in the boundary layer. Wall functions can be used in
these cases to apply an assumed functional shape of the velocity profile. Other grids are fine
enough that they do not require wall functions, and application of the latter has little effect.


The majority of cases fall somewhere in between these two extremes, where the boundary
layer is partially resolved by nodes near the wall and wall functions are used to supplement
accuracy where the nodes are not sufficiently clustered near the wall.
One indicator of the closeness of the first node to the wall is the dimensionless wall distance
+ +
y . It is good practice to examine the values of y at the end of your simulation. At the
+
lower limit, a value of y less than or equal to 11 indicates that the first node is within the
laminar sublayer of the boundary flow. Values larger than this indicate that an assumed
logarithmic shape of the velocity profile is being used to model the boundary layer portion
between the wall and the first node. Ideally you should confirm that there are several nodes
(3 or more) resolving the boundary layer profile. If this is not observed, it is highly
recommended that more nodes be added near the wall surfaces in order to improve
simulation accuracy. In this tutorial, a coarse mesh is used to reduce the run time. Thus, the
grid is far too coarse to resolve any of the boundary layer profile, and the solution is not
highly accurate.

Surface Plot of A surface plot is one which colors a surface according to the values of a variable: in this case,
y+ + +
y . A surface plot of y can be obtained as follows:
1. Clear the visibility of all previous plots.
2. Under the Outline tab, apply the following settings to BluntBodyDefault:

Tab Setting Value
Color Mode Variable
Variable Yplus*
*. Click the ellipsis icon to the right of the Variable dropdown menu to view a full list
of variables, including Yplus.

3. Click Apply.
4. Under the Outline tab, apply the following settings to Body:

Tab Setting Value
Color Mode Variable
Variable Yplus*
*. Click the ellipsis icon to the right of the Variable dropdown menu to view a full list
of variables, including Yplus.

5. Click Apply.



Demonstrating Power Syntax
This section demonstrates a power syntax macro used to evaluate the variation of any
variable in the direction of the x-axis. This is an example of power syntax programming in
ANSYS CFX-Post.

Synopsis A macro containing CCL and power syntax will be loaded by playing a session file. This
macro will be executed by entering a line of power syntax in the Command Editor dialog
box. The macro tells ANSYS CFX-Post to create slice planes, normal to the X axis, at 20
evenly-spaced locations from the beginning to the end of the domain. On each plane, it
measures and prints the minimum, maximum, and average values for a specified variable
(using conservative values). The planes are colored using the specified variable.

Note: The ANSYS CFX-Post engine can respond to CCL commands issued directly, or to
commands issued using the graphical user interface. The Command Editor dialog box can
be used to enter any valid CCL command directly.

Procedure 1. Play the session file named BluntBodyDist.cse.
-X.
3. Select Tools > Command Editor from the menu bar.
4. Type the following line into the Command Editor dialog box (the quotation marks and
the semi-colon are required):
!BluntBodyDist("Velocity u");
5. Click Process.
The minimum, maximum and average values of the variable at each X location are
written to the file BluntBody.txt. The results can be viewed by opening the file in a
text editor.
You can also run the macro with a different variable.
To view the content of the session file (which contains explanatory comments), open the
session file in a text editor. It contains all of the CCL and power syntax commands and will
provide a better understanding of how the macro works.

Viewing the Mesh Partitions (Parallel Only)
If you solved this tutorial in parallel, then an additional variable named Real partition
number will be available in ANSYS CFX-Post

1. Create an Isosurface of Real partition number equal to 1.
2. Create a second Isosurface of Real partition number equal to 1.999.
The two Isosurfaces show the edges of the two partitions. The gap between the two plots
shows the overlap nodes. These were contained in both partitions 1 and 2.
When you have finished looking at the results, quit ANSYS CFX-Post.


Tutorial 6:
Buoyant Flow in a Partitioned
Cavity

Introduction
• Obtaining a Solution using ANSYS CFX-Solver Manager (p. 134)

before beginning:
• Buoyancy2D.geo
• Buoyancy2D.pre


Tutorial 6: Buoyant Flow in a Partitioned Cavity: Tutorial 6 Features

Tutorial 6 Features

Simulation Type Transient
Turbulence Model Laminar
Buoyant Flow
Boundary Conditions Symmetry Plane
Outlet (Subsonic)
Wall: No-Slip
Wall: Adiabatic
Wall: Fixed Temperature
Output Control
Timestep Transient Example
Report
Other Time Step Selection
Transient Animation

• Using CFX-4 Mesh Import.
• Setting up a time dependent (transient) simulation.
• Modeling buoyant flow.

This tutorial demonstrates the capability of ANSYS CFX in modeling buoyancy-driven flows
which require the inclusion of gravitational effects.


Tutorial 6: Buoyant Flow in a Partitioned Cavity: Defining a Simulation in ANSYS CFX-Pre
The model is a 2D partitioned cavity containing air. The bottom of the cavity is kept at a
constant temperature of 75°C, while the top is held constant at 5°C. The cavity is also tilted
at an angle of 30 degrees to the horizontal. A transient simulation is set up to see how the
flow develops starting from stationary conditions. Since you are starting from stationary
conditions, there is no need to solve a steady-state simulation for use as the initial guess.

5 C

air

75 C

The mesh for the cavity was created in CFX-4 and has been provided.

You are going to import a hexahedral mesh originally generated in CFX-4. The mesh
contains labelled regions which will enable you to apply the relevant boundary conditions
for this problem.

then run the session file: Buoyancy2D.pre. After you have played the session file as
Manager (p. 87), proceed to Obtaining a Solution using ANSYS CFX-Solver Manager (p. 134).

2. Create a new simulation using General Mode.
3. Select File > Save Simulation As and set File name to Buoyancy2D.
4. Click Save.

Importing the Mesh
1. Right-click Mesh and select Import Mesh. The Import Mesh dialog box appears.



Setting Value
File type CFX-4
File name Buoyancy2D.geo*
*. This file is in your tutorial directory.

3. Click Open.

Simulation Type
The default units and coordinate frame settings are suitable for this tutorial, but the
simulation type needs to be set to transient.
You will notice physics validation messages as the case is set to Transient. These errors will
be fixed in the later part of the tutorial.


Tab Setting Value
Simulation Type > Time Duration > 2 [s]
Total Time*
Simulation Type > Time Steps > 0.025 [s]
Timesteps†
*. This is the total duration, in real time, for the simulation
†. This is the interval from one step, in real time, to the next. The simulation will
continue, moving forward in time by 0.025 s, until the total time has been reached

3. Click OK.



Creating the Domain

gsin30
30

gcos30
g

y
x
30

You will model the cavity as if it were tilted at an angle of 30°. You can do this by specifying
horizontal and vertical components of the gravity vector, which are aligned with the default
coordinate axes, as shown in the diagram above.

To Create a New 1. Click Domain , and set the name to Buoyancy2D.
Domain 2. Apply the following settings to Buoyancy2D

Tab Setting Value
General Basic Settings > Fluids List Air at 25 C
Options Domain Models > Pressure > Reference Pressure 1 [atm]
Domain Models > Buoyancy > Option Buoyant
Domain Models > Buoyancy > Gravity X Dirn. -4.9 [m s^-2]
Domain Models > Buoyancy > Gravity Y Dirn. -8.5 [m s^-2]
Domain Models > Buoyancy > Gravity Z Dirn. 0.0 [m s^-2]*
Domain Models > Buoyancy > Buoy. Ref. Temp. 40 [C]†
Fluid Models Heat Transfer > Option Thermal Energy
Turbulence > Option None (Laminar)
*. This produces a gravity vector which simulates the tilt of the cavity
†. Do not forget to change the units. This is just an approximate representative
domain temperature.

Initialization will be set up using Global Initialization , so there is no need to visit the
Initialization tab.
3. Click OK.



Hot and Cold You will create a wall boundary condition with a fixed temperature of 75 C on the bottom
Wall Boundary surface of the cavity, as follows:
1. Create a new boundary condition named hot.

Tab Setting Value
Location WALLHOT
Boundary Heat Transfer > Option Temperature
Details
Heat Transfer > Fixed Temperature 75 [C]

3. Click OK.
4. Create a new boundary condition named cold.

Tab Setting Value
Location WALLCOLD
Details Heat Transfer > Fixed Temperature 5 [C]

6. Click OK.

Symmetry Plane A single symmetry plane boundary condition can be used for the front and back of the
Boundary cavity.
1. Create a new boundary condition named SymP.

Tab Setting Value
Location SYMMET1, SYMMET2*
*. Use the <Ctrl> key to select more than one region.

3. Click OK.
The default adiabatic wall boundary condition will automatically be applied to the
remaining boundaries.

You should set initial settings using the Automatic with Value option when defining a
transient simulation. Using this option, the first run will use the specified initial conditions
while subsequent runs will use results file data for initial conditions.




Tab Setting Value
Global Settings Initial Conditions > Cartesian Velocity Automatic with
Components > Option Value
Components > U
Components > V
Components > W
Initial Conditions > Static Pressure > Relative 0 [Pa]
Pressure
Initial Conditions > Temperature > Temperature 5 [C]

3. Click OK.

Setting Output Control

1. Click Output Control .
2. Click the Trn Results tab.
3. Create a new Transient Results item with the default name.

Tab Setting Value
Trn Results Transient Results > Transient Results 1 > Selected Variables
Option
Transient Results > Transient Results 1 > Pressure, Temperature,
Output Variables List* Velocity
Transient Results > Transient Results 1 > Time Interval
Output Frequency > Option
Transient Results > Transient Results 1 > 0.1 [s]
Output Frequency > Time Interval
*. Click the ellipsis icon to select items if they do not appear in the drop-down list. Use
the <Ctrl> key to select multiple items.

5. Click OK.



Tutorial 6: Buoyant Flow in a Partitioned Cavity: Obtaining a Solution using ANSYS CFX-Solver Manager

Tab Setting Value
Basic Settings Advection Scheme > Option High Resolution
Convergence Control > Max. Coeff. Loops 5
Convergence Criteria > Residual Type RMS
Convergence Criteria > Residual Target 1.E-4*
*. An RMS value of at least 1.E-5 is usually required for adequate convergence, but the
default value of 1.E-4 is sufficient for demonstration purposes.

3. Click OK.


Setting Value
File name Buoyancy2D.def


discretion.

Obtaining a Solution using ANSYS CFX-Solver Manager

Note: Recall that the output displayed on the Out File tab of the ANSYS CFX-Solver Manager
is more complicated for transient problems than for steady-state problems. Each timestep
consists of several iterations, and after the timestep, information about various quantities is
printed.
1. Click Start Run.
of the run.


Tutorial 6: Buoyant Flow in a Partitioned Cavity: Viewing the Results in ANSYS CFX-Post

In this section, you will create a report in ANSYS CFX-Post. You will also make an animation
to see changes in temperature with time.

Simple Report
First, you will view a report that is created with little effort:
1. Click the Report Viewer tab. Note that the report loads with some
automatically-generated statistical information.
2. In the Outline tree view, under Report, experiment with the various settings for Mesh
Report, Physics Report and other report objects. These settings control the report
contents. On the Report Viewer tab, you can click Refresh to see the changes to your
report.

Plots
Here, you will create the following objects in preparation for generating a more customized
report:
• Contour plot of temperature
• Point locators (for observing temperature)
• Comment
• Figure showing the contour plot and point locator
• Time chart showing the temperature at the point locator
• Table

Contour Plot 1. Click the 3D Viewer tab and right-click a blank area of the viewer, then select
Predefined Camera > View Towards -Z.
2. Select Insert > Contour from the main menu.
3. Accept the default name by clicking OK.
4. Set Locations to SymP.
5. Set Variable to Temperature.
6. Click Apply.
The contour plot shows the temperature at the end of the simulation, since ANSYS CFX-Post
loads values for the last timestep by default. You can load different timesteps using the
Timestep Selector dialog box, accessible by selecting Tools > Timestep Selector from the
main menu.

Point Locators 1. From the main menu, select Insert > Location > Point.
3. Set Method to XYZ.
4. Set Point coordinates to 0.098, 0.05, 0.00125.
5. Click Apply.
Note the location of Point 1 in the viewer.


6. Right-click the Point 1 object in the tree view and select Duplicate from the shortcut
menu.
8. Right-click the Point 2 object in the tree view and select Edit from the shortcut menu.
9. Change the x-coordinate to 0.052.
10. Click Apply.
Note the location of Point 2 in the viewer.

Comment 1. Click Create comment .
A comment object appears in the tree view, under the Report object.
3. Set Heading to Buoyant Flow in a Partitioned Cavity.
4. In the large text box, type:
This is a sample paragraph.

Figure 1. Click the 3D Viewer tab.
2. Select Insert > Figure from the main menu.
The Make copies of objects check box determines whether or not the objects that are
visible in the viewer are copied. If objects are copied, then the copies are used in the
figure instead of the originals. Since you are not using multiple views or figures, the
check box setting does not matter.
A figure object will appear under the Report branch in the tree view.

Time Chart 1. Select Insert > Chart from the main menu.
3. Set Title to Temperature versus Time.
4. Set Type to Time.
5. Click the Chart Line 1 tab.
6. Set Line Name to Temperature at Point 1.
7. Set Method to Point.
8. Set Location to Point 1.
9. Set Time Variable > Variable to Temperature.
10. Click Apply.
A chart object will appear under the Report branch in the tree view. The chart itself will
appear in the Chart Viewer tab. It may take some time for the chart to appear because
every transient results file will be loaded in order to generate the time chart.
11. Click New Line (on the Chart Line 1 tab).
12. Set Line Name to Temperature at Point 2.
13. Set Location to Point 2 and Time Variable > Variable to Temperature.
14. Click Apply.
A second chart line will appear in the chart, representing the temperature at Point 2.

Table 1. Select Insert > Table from the main menu.


A table object will appear under the Report branch in the tree view.
3. Set the following:

Cell Value
A1 Location
A2 Point 1
A3 Point 2
B1 Temperature
B2 =probe(Temperature)@Point 1
B3 =probe(Temperature)@Point 2

The table shows temperatures at the end of the simulation, since ANSYS CFX-Post loads
values for the last timestep by default. You can load different timesteps using the Timestep
Selector dialog box, accessible by selecting Tools > Timestep Selector.

Customized Report
Right-click the Report object and select Refresh from the shortcut menu. Look at the report
in the Report Viewer tab. Note that, in addition to the automatically-generated objects that
you saw earlier when creating a simple report, this report also includes the customized
figure, time chart and table described above.

Animations
Use the animation feature to see the changing temperature field. The animation feature was
used in Tutorial 4: Flow from a Circular Vent (p. 93).

Completion
When you have finished, quit ANSYS CFX-Post.


Tutorial 7:
Free Surface Flow Over a Bump

Introduction
• Using a Supercritical Outlet Condition (p. 154)

before beginning.
• Bump2D.pre
• Bump2DExpressions.ccl
• Bump2Dpatran.out

Tutorial 7 Features
This tutorial addresses the following features of ANSYS CFX:


Tutorial 7: Free Surface Flow Over a Bump: Overview of the Problem to Solve

Heat Transfer None
Buoyant Flow
Multiphase
Outlet (Subsonic)
Symmetry Plane
Wall: No-Slip
Wall: Free-Slip
Mesh Adaption
Isosurface
Polyline
Sampling Plane
Vector
Volume
Other Chart Creation
Title/Text
Viewing the Mesh

• Mesh import in PATRAN Neutral format.
• Setting up a 2D problem.
• Setting up appropriate boundary conditions for a free surface simulation. (Free surface
simulations are more sensitive to incorrect boundary and initial guess settings than
other more basic models.)
• Mesh adaption to refine the mesh where the volume fraction gradient is greatest. (This
aids in the development of a sharp interface between the liquid and gas.)

This tutorial demonstrates the simulation of a free surface flow.
The geometry consists of a 2D channel in which the bottom of the channel is interrupted by
a semi-circular bump of radius 30 mm. The flow upstream of the bump is subcritical. The
downstream conditions are not known but can be estimated using an analytical 1D
calculation or data tables for flow over a bump.


Tutorial 7: Free Surface Flow Over a Bump: Defining a Simulation in ANSYS CFX-Pre


then run the session file: Bump2D.pre. After you have played the session file as described in
earlier tutorials under Playing the Session File and Starting ANSYS CFX-Solver Manager
(p. 87), proceed to Obtaining a Solution using ANSYS CFX-Solver Manager (p. 148).

5. Under File name, type Bump2D.
6. Click Save.

Importing the Mesh

Setting Value
File type PATRAN Neutral
File name Bump2Dpatran.out

3. Click Open.
-Z from the shortcut menu.

Viewing the 1. Click Label and Marker Visibility .
Region Labels 2. Apply the following settings

Tab Setting Value
Label Options Show Labels (Selected)
Show Labels > Show Primitive3D Labels (Selected)
Show Labels > Show Primitive2D Labels (Selected)

3. Click OK.



Creating Expressions for Initial and Boundary Conditions
Simulation of free surface flows usually requires defining boundary and initial conditions to
set up appropriate pressure and volume fraction fields. You will need to create expressions
using CEL (CFX Expression Language) to define these conditions.
In this simulation, the following conditions are set and require expressions:
• An inlet boundary where the volume fraction above the free surface is 1 for air and 0 for
water, and below the free surface is 0 for air and 1 for water.
• A pressure-specified outlet boundary, where the pressure above the free surface is
constant and the pressure below the free surface is a hydrostatic distribution. This
requires you to know the approximate height of the fluid at the outlet. In this case, an
analytical solution for 1D flow over a bump was used. The simulation is not sensitive to
the exact outlet fluid height, so an approximation is sufficient. You will examine the
effect of the outlet boundary condition in the post-processing section and confirm that
it does not affect the validity of the results. It is necessary to specify such a boundary
condition to force the flow downstream of the bump into the supercritical regime.
• An initial pressure field for the domain with a similar pressure distribution to that of the
outlet boundary.
Either create expressions using the Expressions workspace or import expressions from a
file.
• Creating Expressions (p. 142)
• Reading Expressions From a File (p. 143)

Creating 1. Right-click Expressions in the tree view and select Insert > Expression.
Expressions 2. Set the name to UpH and click OK.
3. Set Definition to 0.069 [m], and then click Apply.
4. Use the same method to create the expressions listed in the table below. These are
expressions for the downstream free surface height, the density of the fluid, the
upstream volume fractions of air and water, the upstream pressure distribution, the
downstream volume fractions of air and water, and the downstream pressure
distribution.

Name Definition
DownH 0.022 [m]
DenH 998 [kg m^-3]
UpVFAir step((y-UpH)/1[m])
UpVFWater 1-UpVFAir
UpPres DenH*g*UpVFWater*(UpH-y)
DownVFAir step((y-DownH)/1[m])
DownVFWater 1-DownVFAir
DownPres DenH*g*DownVFWater*(DownH-y)

5. Proceed to Creating the Domain (p. 143).


Reading 1. Copy the file Bump2DExpressions.ccl to your working directory from the ANSYS CFX
Expressions examples directory.
From a File 2. Select File > Import CCL.
3. When Import CCL appears, ensure that Append is selected.
4. Select Bump2DExpressions.ccl.
5. Click Open.
6. After the file has been imported, use the Expression tree view to view the expressions
that have been created.

Creating the Domain
1. Right click Simulation in the Outline tree view and ensure that Automatic Default
Domain is selected. A domain named Default Domain should now appear under the
Simulation branch.
2. Double click Default Domain and apply the following settings

Tab Setting Value
General Basic Settings > Fluids List Air at 25 C, Water
Domain Models > Buoyancy > Gravity X Dirn. 0 [m s^-2]
Domain Models > Buoyancy > Gravity Y Dirn.* -g
Domain Models > Buoyancy > Gravity Z Dirn. 0 [m s^-2]
Domain Models > Buoyancy > Buoy. Ref. Density† 1.185 [kg m^-3]
Domain Models > Buoyancy > Ref Location > Option Automatic
Fluid Models Multiphase Options > Homogeneous Model‡ (Selected)
Multiphase Options > Free Surface Model > Option Standard
Heat Transfer > Option Isothermal
Heat Transfer > Fluid Temperature 25 C
Turbulence > Option k-Epsilon

*. You need to click Enter Expression beside the field first.
†. Always set Buoyancy Reference Density to the density of the least dense fluid in free
surface calculations.
‡. The homogeneous model solves for a single solution field. This is only appropriate
in some simulations.

3. Click OK.

Inlet Boundary 1. Create a new boundary condition named inflow.



Tab Setting Value
Basic Boundary Type Inlet
Settings
Location INFLOW
Boundary Mass and Momentum > Option Normal Speed
Details
Mass and Momentum > Option > Normal Speed 0.26 [m s^-1]
Turbulence > Eddy Len. Scale* UpH
Fluid Values Boundary Conditions Air as 25 C
Air at 25 C > Volume Fraction > Volume Fraction UpVFAir
Boundary Conditions Water
Water > Volume Fraction > Volume Fraction UpVFWater
*. Click the Enter Expression icon.

3. Click OK.

Outlet 1. Create a new boundary condition named outflow.

Tab Setting Value
Basic Boundary Type Outlet
Settings Location OUTFLOW
Boundary Flow Regime> Option Subsonic
Details Mass and Momentum > Option Static Pressure
Mass and Momentum > Relative Pressure DownPres

3. Click OK.

Symmetry 1. Create a new boundary condition named front.

Tab Setting Value
Basic Boundary Type Symmetry
Settings
Location FRONT

3. Click OK.
4. Create a new boundary condition named back.

Tab Setting Value
Basic Boundary Type Symmetry
Settings
Location BACK


6. Click OK.

Wall and 1. Create a new boundary condition named top.
Opening 2. Apply the following settings
Boundaries

Tab Setting Value
Location TOP
Boundary Details Mass And Momentum > Option Static Pres. (Entrain)
Mass And Momentum > Relative Pressure 0 [Pa]
Turbulence > Option Zero Gradient
Fluid Values Boundary Conditions Air at 25 C
Boundary Conditions > Air at 25 C > 1.0
Volume Fraction > Volume Fraction
Boundary Conditions > Water > Volume 0.0
Fraction > Volume Fraction

3. Click OK.
4. Create a new boundary condition named bottom.

Tab Setting Value
Basic Boundary Type Wall
Settings Location BOTTOM1, BOTTOM2, BOTTOM3
Boundary Wall Influence on Flow > Option No Slip
Details Wall Roughness > Option Smooth Wall

6. Click OK.




Tab Setting Value
Components > Option
Initial Conditions > Cartesian Velocity 0.26 [m s^-1]
Components > U
Components > V
Components > W
Initial Conditions > Static Pressure > Option Automatic with Value
Initial Conditions > Static Pressure > Relative UpPres
Pressure
Initial Conditions > Turbulence Eddy Dissipation (Selected)
Fluid Settings Fluid Specific Initialization > Air at 25 C (Selected)
Air at 25 C > Initial Conditions > Volume Fraction > Automatic with Value
Option
Air at 25 C > Initial Conditions > Volume Fraction > UpVFAir
Volume Fraction
Fluid Settings Fluid Specific Initialization > Water (Selected)
Fluid Specific Initialization > Water > Initial Automatic with Value
Conditions > Volume Fraction > Option
Fluid Specific Initialization > Water > Initial UpVFWater
Conditions > Volume Fraction > Volume Fraction

3. Click OK.

Setting Mesh Adaption Parameters

1. Click Mesh Adaption .

Tab Setting Value
Basic Settings Activate Adaption (Selected)
Save Intermediate Files (Cleared)
Adaption Criteria > Variables List Air at 25 C.Volume Fraction
Adaption Criteria > Max. Num. Steps 2
Adaption Criteria > Option Multiple of Initial Mesh
Adaption Criteria > Node Factor 4
Adaption Convergence Criteria > Max. 100
Iter. per Step
Advanced Options Node Alloc. Param. 1.6
Number of Levels 2

3. Click OK.



Important: Setting Max Iterations to 200 and Number of Adaption Levels to 2 with a
maximum of 100 timesteps each, results in a total maximum number of timesteps of 400
(2*100+200=400).


Tab Setting Value
Convergence Control >Fluid Timescale Physical Timescale
Control > Timescale Control
Convergence Control >Fluid Timescale 0.25 [s]
Control > Physical Timescale
Advanced Options Multiphase Control (Selected)
Multiphase Control > Volume Fraction (Selected)
Coupling
Multiphase Control > Volume Fraction Coupled
Coupling > Option

Note: The options selected above activate the Coupled Volume Fraction solution algorithm.
This algorithm typically converges better than the Segregated Volume Faction algorithm for
buoyancy-driven problems such as this tutorial, which requires a 0.05 [s] timescale using the
Segregated Volume Faction algorithm compared with 0.25 [s] for the Coupled Volume
Fraction algorithm.
Note:
3. Click OK.


Setting Value
File name Bump2D.def


discretion.


Tutorial 7: Free Surface Flow Over a Bump: Obtaining a Solution using ANSYS CFX-Solver Manager

When ANSYS CFX-Pre has shut down and ANSYS CFX-Solver Manager has started, the
solution will be obtained.
Within 100 iterations, the first adaption step will be performed. Information will be written
to the OUT file, containing the number of elements refined and the size of the new mesh.
After mesh refinement, there will be a jump in the residual levels. This is because the
solution from the old mesh is interpolated on to the new mesh. A new residual plot will also
appear for the W-Mom-Bulk equation. Hexahedral mesh elements are refined orthogonally,
so the mesh is no longer 2D (it is more than 1 element thick in the z-direction).

Y
Before Refinement After Refinement

X
Z

Convergence to the target residual level has been achieved. It is common for convergence
in a residual sense to be difficult to obtain in a free surface simulation. This is due to the
presence of small waves at the surface preventing the residuals from dropping to the target
level. This is more frequently a problem in the subcritical flow regime, as the waves can
travel upstream. In the supercritical regime, the waves tend to get carried downstream and
out the domain.
To satisfy convergence in these cases, monitor the value of a global quantity, (for example,
drag for flow around a ship’s hull) to see when a steady state value is reached.
Where there is no obvious global quantity to monitor, you should view the results to see
where the solution is changing. You can do this by running transient for a few timesteps,
starting from a results file that you think is converged, or by writing some backup results
files at different timesteps.
In both cases look to see where the results are changing (this could be due to the presence
of small transient waves). Also confirm that the value of quantities that you are interested in
(for example, downstream fluid height for this case) has reached a steady state value.
1. Click Start Run.
of the run.


Tutorial 7: Free Surface Flow Over a Bump: Viewing the Results in ANSYS CFX-Post

1. Select View Towards -Z by right-clicking on a blank area in the viewer and selecting
Predefined Camera > View Towards -Z.
2. Zoom in so the geometry fills the Viewer.
3. In the tree view under Bump2D, edit front.

Tab Setting Value
Color Mode Variable
Variable Water.Volume Fraction

5. Click Apply.
6. Clear the check box next to front.

Creating Velocity Vector Plots
The next step involves creating a sampling plane to display velocity vectors for Water.
1. Create a new plane named Plane 1.

Tab Setting Value
Geometry Definition > Method XY Plane
Plane Bounds > X Angle 0 [degree]
Plane Type Sample
X Samples 160
Y Samples 40

3. Click Apply.
4. Clear the check box next to Plane 1.
5. Create a new vector named Vector 1.

Tab Setting Value
Geometry Definition > Locations Plane 1
Definition > Variable * Water.Velocity



*. Since fluids in a free-surface calculation share the same velocity field, only the
velocity of the first non-vapour fluid is available. The other allowed velocities are
superficial velocities. For details, see Further Post-processing (p. 154).
7. Click Apply.

Tab Setting Value
Geometry Definition > Variable Air at 25 C.Superficial
Velocity
Normalize Symbols (Selected)

9. Click Apply.

Viewing Mesh Refinement
In this section, you will view the surface mesh on one of the symmetry boundaries, create
volume objects to show where the mesh was modified, and create a vector plot to visualize
the added mesh nodes.
1. Clear the check box next to Vector 1..
3. In Outline under Default Domain, edit front.

Tab Setting Value
Color Mode Constant

5. Click Apply.
• The mesh has been refined near the free surface.
• In the transition region between different levels of refinement, tetrahedral and
pyramidal elements are used since it is not possible to recreate hexahedral elements
in ANSYS CFX. Near the inlet, the aspect ratio of these elements increases.


• Avoid performing mesh refinement on high-aspect-ratio hex meshes, as this will
produce high aspect ratio tetrahedral-elements, resulting in poor mesh quality.
Figure 1 Mesh around the bump

6. Create a new volume named first refinement elements.

Tab Setting Value
Definition > Variable Refinement Level
Definition > Mode At Value
Definition > Value 1
Draw Lines > Line Color (Green)

8. Click Apply.
You will see a band of green which indicates the elements that include nodes added
during the first mesh adaption.
9. Create a new volume named second refinement elements.

Tab Setting Value
Definition > Variable Refinement Level
Definition >Mode At Value
Definition > Value 2
Color Color White



Tab Setting Value
Draw Lines > Line Color (Black)
11. Click Apply.
You will see a band of white (with black lines) which indicates the elements that include
nodes added during the second mesh adaption.
12. Zoom in to a region where the mesh has been refined.
The Refinement Level variable holds an integer value at each node, which is either 0, 1
or 2 (since you used a maximum of two adaption levels).
The nodal values of refinement level will be visualized next.

Tab Setting Value
Geometry Definition > Location Bump2D
Definition > Variable * (Any Vector Variable)
Color Mode Variable
Variable Refinement Level
Symbol Symbol Cube
Symbol Size 0.02
*. The variable’s magnitude and direction do not matter since you will change the
vector symbol to a cube with a normalized size.

15. Click Apply.
Blue nodes (Refinement Level 0 according to the color legend) are part of the original mesh.
Green nodes (Refinement Level 1) were added during the first adaption step. Red nodes
(Refinement Level 2) were added during the second adaption step. Note that some
elements contain combinations of blue, green, and red nodes.

Creating a Chart
Next, you will create a chart to show how the height of the free surface varies along the
length of the channel. To do this, you will need a Polyline which follows the free surface. You
can create the Polyline from the intersecting line between one of the Symmetry planes and
an Isosurface which shows the free surface. First you must create the Isosurface.
1. Clear the visibility check boxes for all of the objects except Wireframe.
2. Create a new isosurface named Isosurface 1.



Tab Setting Value
Geometry Definition > Variable Water.Volume Fraction
Definition > Value 0.5

4. Click Apply.
Creating isosurfaces using this method is a good way to visualize a free surface in a 3D
simulation.
5. Right-click any blank area in the viewer, select Predefined Camera, then select
Isometric View (Y up).

Creating a These steps explain creating a Polyline which follows the free surface:
Polyline to
1. Clear the visibility check box for Isosurface 1.
Follow the Free
Surface 2. Create a new polyline named Polyline 1.

Tab Setting Value
Geometry Method Boundary Intersection
Boundary List front
Intersect With Isosurface 1

4. Click Apply.
A green line is displayed that follows the high-Z edge of the isosurface.

Creating a Chart 1. Create a new chart named Chart 1.
to Show the The Chart Viewer tab is selected.
Height of the
Surface

Tab Setting Value
Chart Line 1 Line Name free surface height
Location Polyline 1
X Axis > Variable X
Y Axis > Variable Y
Appearance > Symbols Rectangle
Chart Title Free Surface Height for Flow
over a Bump

3. Click Apply.
As discussed in Creating Expressions for Initial and Boundary Conditions (p. 142), an
approximate outlet elevation is imposed as part of the boundary condition, even though
the flow is supercritical. The chart illustrates the effect of this, in that the water level rises just
before the exit plane. It is evident from this plot that imposing the elevation does not affect
the upstream flow.


Tutorial 7: Free Surface Flow Over a Bump: Using a Supercritical Outlet Condition
The chart shows a wiggle in the elevation of the free surface interface at the inlet. This is
related to an overspecification of conditions at the inlet, since both the inlet velocity and
elevation were specified. For a subcritical inlet, only the velocity or the total energy should
be specified. The wiggle is due to a small inconsistency between the specified elevation and
the elevation computed by the solver to obtain critical conditions at the bump. The wiggle
is analogous to one found if pressure and velocity were both specified at a subsonic inlet, in
a converging-diverging nozzle with choked flow at the throat.

Further Post-processing
You may wish to create some plots using the <Fluid>.Superficial Velocity variables.
This is the fluid volume fraction multiplied by the fluid velocity and is sometimes called the
volume flux. It is useful to use this variable for vector plots in separated multiphase flow, as
you will only see a vector where a significant amount of that phase exists.

Using a Supercritical Outlet Condition
For supercritical free surface flows, the supercritical outlet boundary condition is usually the
most appropriate boundary condition for the outlet, since it does not rely on the
specification of the outlet pressure distribution (which depends on an estimate of the free
surface height at the outlet). The supercritical outlet boundary condition requires a relative
pressure specification for the gas only; no pressure information is required for the liquid at
the outlet. For this tutorial, the relative gas pressure at the outlet should be set to 0 [Pa].
The supercritical outlet condition may admit multiple solutions. To find the supercritical
solution, it is often necessary to start with a static pressure outlet condition (as previously
done in this tutorial) or an average static pressure condition where the pressure is set
consistent with an elevation to drive the solution into the supercritical regime. The outlet
condition can then be changed to the supercritical option.


Tutorial 8:
Supersonic Flow Over a Wing

Introduction

before beginning:
• WingSPS.pre
• WingSPSMesh.out

Tutorial 8 Features


Tutorial 8: Supersonic Flow Over a Wing: Tutorial 8 Features

Turbulence Model Shear Stress Transport
Heat Transfer Total Energy
Boundary Conditions Inlet (Supersonic)
Outlet (Supersonic)
Symmetry Plane
Wall: No-Slip
Wall: Adiabatic
Wall: Free-Slip
Domain Interfaces Fluid-Fluid (No Frame Change)
ANSYS CFX-Post Plots Contour
Default Locators
Vector
Other Variable Details View

• Setting up a supersonic flow simulation.
• Using the Shear Stress Transport turbulence model to accurately resolve flow around
the wing surface.
• Defining custom vector variables for use in visualizing pressure distribution.


Tutorial 8: Supersonic Flow Over a Wing: Overview of the Problem to Solve

This example demonstrates the use of ANSYS CFX in simulating supersonic flow over a
symmetric NACA0012 airfoil at 0° angle of attack. A 2D section of the wing is modeled. A 2D
hexahedral mesh is provided that is imported into ANSYS CFX-Pre.

air speed 1.25 [m]
u = 600 m/s

outlet
30 [m]

wing surface

70 [m]


then run the session file: WingSPS.pre. After you have played the session file as described

5. Under File name, type WingSPS.
6. Click Save.


Tutorial 8: Supersonic Flow Over a Wing: Defining a Simulation in ANSYS CFX-Pre

Importing the Mesh

Setting Value
File type PATRAN Neutral
File name WingSPSMesh.out

3. Click Open.
(Y up) from the shortcut menu.

Creating the Domain
Creating a New 1. Right click Simulation in the Outline tree view and ensure that Automatic Default
Domain Domain is selected. A domain named Default Domain should now appear under the
Simulation branch.
2. Double click it and apply the following settings

Tab Setting Value
General Options Basic Settings > Location WING
Fluids List Air Ideal Gas
Domain Models > Pressure > 1 [atm]
Reference Pressure*
Fluid Models Heat Transfer > Option Total Energy†
Turbulence > Option Shear Stress Transport
*. When using an ideal gas, it is important to set an appropriate reference pressure
since some properties depend on the absolute pressure level.
†. The Total Energy model is appropriate for high speed flows since it includes kinetic
energy effects.

3. Click OK.

Inlet Boundary 1. Create a new boundary condition named Inlet.

Tab Setting Value
Location INLET



Tab Setting Value
Boundary Details Flow Regime > Option Supersonic
Mass and Momentum > Option Cart. Vel. & Pressure
Mass and Momentum > U 600 [m s^-1]
Mass and Momentum > V 0 [m s^-1]
Mass and Momentum > W 0 [m s^-1]
Mass and Momentum > Rel. Static Pres. 0 [Pa]
Heat Transfer > Static Temperature 300 [K]
3. Click OK.


Tab Setting Value
Location OUTLET
Boundary Details Flow Regime > Option Supersonic

3. Click OK.

Symmetry Plane 1. Create a new boundary condition named SymP1.

Tab Setting Value
Location SIDE1

3. Click OK.
4. Create a new boundary condition named SymP2.

Tab Setting Value
Location SIDE2

6. Click OK.
7. Create a new boundary condition named Bottom.



Tab Setting Value
Location BOTTOM

9. Click OK.

Free Slip 1. Create a new boundary condition named Top.

Tab Setting Value
Location TOP
Boundary Details Wall Influence on Flow > Option Free Slip

3. Click OK.

Wall Boundary 1. Create a new boundary condition named WingSurface.

Tab Setting Value
Location WING_Nodes*

*. Click the ellipsis icon to select items if they do not appear in the drop-down
list.

3. Click OK.

Creating Domain Interfaces
The imported mesh contains three regions which will be connected with domain interfaces.
1. Create a new domain interface named Domain Interface 1.

Tab Setting Value
Basic Settings Interface Type Fluid Fluid
Interface Side 1 > Region List Primitive 2D A*
Interface Side 2 > Region List Primitive 2D, Primitive 2D B

*. Click the ellipsis icon to select items if they do not appear in the drop-down
list.

3. Click OK.



For high speed compressible flow, the ANSYS CFX-Solver usually requires sensible initial
conditions to be set for the velocity field.


Tab Setting Value
Global Initial Conditions > Cartesian Velocity Components > Option Automatic
Settings with Value
Initial Conditions > Cartesian Velocity Components > U 600 [m s^-1]
Initial Conditions > Cartesian Velocity Components > V 0 [m s^-1]
Initial Conditions > Cartesian Velocity Components > W 0 [m s^-1]
Initial Conditions > Temperature > Option Automatic
with Value
Initial Conditions > Temperature > Temperature 300 [K]

3. Click OK.

The residence time for the fluid is approximately:
70 [m] / 600 [m s^-1] = 0.117 [s]
In the next step, you will start with a conservative time scale that gradually increases
towards the fluid residence time as the residuals decrease. A user specified maximum time
scale can be combined with an auto timescale in ANSYS CFX-Pre.


Tab Setting Value
Basic Settings Convergence Control > Fluid Timescale (Selected)
Control > Maximum Timescale
Convergence Control > Fluid Timescale 0.1 [s]
Control > Maximum Timescale > Maximum
Timescale
Convergence Criteria > Residual Target 1.0e-05

3. Click OK.

Since this tutorial uses domain interfaces and the Summarize Interface Data toggle was
selected, an information window is displayed that informs you of the connection type used
for each domain interface.


Tutorial 8: Supersonic Flow Over a Wing: Obtaining a Solution using ANSYS CFX-Solver Manager


Setting Value
File name WingSPS.def
Summarize Interface Data (Selected)


4. The Interface Summary dialog box is displayed. This displays information related to the
summary of interface connections. Click OK.
discretion.

When ANSYS CFX-Pre has shut down, and the ANSYS CFX-Solver Manager has started,
obtain a solution to the CFD problem by following the instructions below.
1. In the ANSYS CFX-Solver Manager, click Start Run.
of the run.

The following topics will be discussed:
• Displaying Mach Information (p. 162)
• Displaying Pressure Information (p. 163)
• Displaying Temperature Information (p. 163)
• Displaying Pressure With User Vectors (p. 163)

Displaying Mach Information
The first view configured shows that the bulk of the flow over the wing has a Mach Number
of over 1.5.
1. Select View Towards -Z by typing <Shift>+<Z>.
3. Create a new contour named SymP2Mach.


Tutorial 8: Supersonic Flow Over a Wing: Viewing the Results in ANSYS CFX-Post

Tab Setting Value
Geometry Locations SymP2
Variable Mach Number
Min 1
Max 2
# of Contours 21

5. Click Apply.
6. Clear the check box next to SymP2Mach.

Displaying Pressure Information
You will now create a contour plot that shows the pressure field.
1. Create a new contour named SymP2Pressure.

Tab Setting Value
Variable Pressure
Range Global

3. Click Apply.
4. Clear the check box next to SymP2Pressure.

Displaying Temperature Information
You can confirm that a significant energy loss occurs around the wing leading edge by
plotting temperature on SymP2. The temperature at the wing tip is approximately 180 K
higher than the inlet temperature.
1. Create a new contour named SymP2Temperature.

Tab Setting Value
Range Global

3. Click Apply.
4. Clear the check box next to SymP2Temperature.

Displaying Pressure With User Vectors
You can also try creating a user vector to show the pressure acting on the wing:


Tutorial 8: Supersonic Flow Over a Wing: Viewing the Results in ANSYS CFX-Post
1. Create a new variable named Variable 1.

Name Setting Value
Variable 1 Vector (Selected)
X Expression (Pressure+101325[Pa])*Normal X
Y Expression (Pressure+101325[Pa])*Normal Y
Z Expression (Pressure+101325[Pa])*Normal Z

3. Click Apply.

Tab Setting Value
Geometry Locations WingSurface
Variable Variable 1

6. Click Apply.
7. Zoom in on the wing in order to see the created vector plot.


Tutorial 9:
Flow Through a Butterfly Valve

Introduction

before beginning:
• PipeValve.pre
• PipeValve_inlet.F
• PipeValveMesh.gtm
• PipeValveUserF.pre

Tutorial 9 Features


Tutorial 9: Flow Through a Butterfly Valve: Overview of the Problem to Solve

Heat Transfer None
Particle Tracking
Boundary Conditions Inlet (Profile)
Inlet (Subsonic)
Outlet (Subsonic)
Symmetry Plane
Wall: No-Slip
Wall: Rough
User Fortran
ANSYS CFX-Solver Manager Power-Syntax
Default Locators
Particle Track
Point
Slice Plane
MPEG Generation
Particle Track Animation
Quantitative Calculation
Symmetry

• using a rough wall boundary condition in ANSYS CFX-Pre to simulate the pipe wall
• creating a fully developed inlet velocity profile using either the CFX Expression
Language or a User CEL Function
• setting up a Particle Tracking simulation in ANSYS CFX-Pre to trace sand particles
• animating particle tracks in ANSYS CFX-Post to trace sand particles through the domain
• quantitative calculation of average static pressure in ANSYS CFX-Post on the outlet
boundary

In industry, pumps and compressors are commonplace. An estimate of the pumping
requirement can be calculated based on the height difference between source and
destination and head loss estimates for the pipe and any obstructions/joints along the way.


Tutorial 9: Flow Through a Butterfly Valve: Defining a Simulation in ANSYS CFX-Pre
Investigating the detailed flow pattern around a valve or joint however, can lead to a better
understanding of why these losses occur. Improvements in valve/joint design can be
simulated using CFD, and implemented to reduce pumping requirement and cost.

Max. Vel. 5 m/s r = 20 mm
288 K

Valve Plate

Flows can also contain particulates that affect the flow and cause erosion to pipe and valve
components. The particle tracking capability of ANSYS CFX can be used to simulate these
effects.
In this example, water flows through a 20 mm radius pipe with a rough internal surface. The
equivalent sand grain roughness is 0.2 mm. The flow is controlled by a butterfly valve, which
is set at an angle of 55° to the vertical axis. The velocity profile is assumed to be fully
developed at the pipe inlet. The flow contains sand particles ranging in size from 50 to 500
microns.


then run one of the following session files available for this tutorial:
• PipeValve.pre sets the inlet velocity profile using a CEL (ANSYS CFX Expression
Language) expression.
• PipeValveUserF.pre sets the inlet velocity profile using a User CEL Function that is
defined by a Fortran subroutine. This session file requires that you have the required
Fortran compiler installed and set in your system path. For details on which Fortran
compiler is required for your platform, see the applicable ANSYS, Inc. installation guide.
If you are not sure which Fortran compiler is installed on your system, try running the
cfx5mkext command (found in <CFXROOT>/bin) from the command line and read the
output messages.


If you choose to run a session file do so using the procedure described in earlier tutorials
under Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 87), and then
proceed to Obtaining a Solution using ANSYS CFX-Solver Manager (p. 180) once the
simulation setup is complete.

5. Under File name, type PipeValve.
6. Click Save.

Importing the Mesh

Setting Value
File name PipeValveMesh.gtm

3. Click Open.

Defining the Properties of Sand
The material properties of the sand particles used in the simulation need to be defined. Heat
transfer and radiation modeling are not used in this simulation, so the only property that
needs to be defined is the density of the sand.
To calculate the effect of the particles on the continuous fluid, between 100 and 1000
particles are usually required. However, if accurate information about the particle volume
fraction or local forces on wall boundaries is required, then a much larger number of
particles needs to be modeled.
When you create the domain, choose either full coupling or one-way coupling between the
particle and continuous phase. Full coupling is needed to predict the effect of the particles
on the continuous phase flow field but has a higher CPU cost than one-way coupling.
One-way coupling simply predicts the particle paths during post-processing based on the
flow field, but without affecting the flow field.
To optimise CPU usage, you can create two sets of identical particles. The first set will be fully
coupled and between 100 and 1000 particles will be used. This allows the particles to
influence the flow field. The second set will use one-way coupling but a much higher
number of particles will be used. This provides a more accurate calculation of the particle
volume fraction and local forces on walls.

1. Click Material then create a new material named Sand Fully Coupled.



Tab Setting Value
Basic Settings Material Group Particle Solids
Thermodynamic State (Selected)
Material Properties Thermodynamic Properties > Equation of 2300 [kg m^-3]
State > Density
Thermodynamic Properties >Specific Heat (Selected)
Capacity
Thermodynamic Properties >Specific Heat 0 [J kg^-1 K^-1]*
Capacity > Specific Heat Capacity
Thermodynamic Properties > Reference (Selected)
State
Thermodynamic Properties > Reference Specified Point
State > Option
Thermodynamic Properties > Reference 300 [K]
State > Ref. Temperature
*. This value is not used because heat transfer is not modeled in this tutorial.

3. Click OK.
4. Under Materials, right-click Sand Fully Coupled and select Duplicate from the
shortcut menu.
5. Name the duplicate Sand One Way Coupled.
6. Click OK.
Sand One Way Coupled is created with properties identical to Sand Fully Coupled.

Creating the Domain
Simulation branch.

Tab Setting Value
General Options Basic Settings > Fluids List Water
Basic Settings > Particle Tracking (Selected)
Basic Settings > Particle Tracking > Particles List Sand Fully Coupled,
Sand One Way Coupled
Fluid Models Heat Transfer > Option None
Turbulence > Option k-Epsilon*



Tab Setting Value
Fluid Details Sand Fully Coupled (Selected)
Sand Fully Coupled > Morphology > Option Solid Particles
Sand Fully Coupled > Morphology > Particle (Selected)
Diameter Distribution
Sand Fully Coupled > Morphology > Particle Normal in Diameter by
Diameter Distribution > Option Mass
Sand Fully Coupled > Morphology > Particle 50e-6 [m]
Diameter Distribution > Minimum Diameter
Diameter Distribution > Maximum Diameter
Diameter Distribution > Mean Diameter
Diameter Distribution > Std. Deviation
Sand Fully Coupled > Erosion Model (Selected)
Sand Fully Coupled > Erosion Model > Option Finnie
Sand Fully Coupled > Erosion Model > Vel. 2.0
Power Factor
Sand Fully Coupled > Erosion Model > Reference 1 [m s^-1]
Velocity
*. The turbulence model only applies to the continuous phase and not the particle
phases.



Tab Setting Value
Fluid Details Sand One Way Coupled (Selected)
Sand One Way Coupled > Morphology > Solid Particles
Option
Sand One Way Coupled > Morphology > (Selected)
Particle Diameter Distribution
Sand One Way Coupled > Morphology > Normal in Diameter by Mass
Particle Diameter Distribution > Option
Sand One Way Coupled > Morphology > 50e-6 [m]
Particle Diameter Distribution > Minimum
Diameter
Particle Diameter Distribution > Maximum
Diameter
Particle Diameter Distribution > Mean
Diameter
Particle Diameter Distribution > Std.
Deviation
Sand One Way Coupled > Erosion Model (Selected)
Sand One Way Coupled > Erosion Model > Finnie
Option
Sand One Way Coupled > Erosion Model > 2.0
Vel. Power Factor
Sand One Way Coupled > Erosion Model > 1 [m s^-1]
Reference Velocity


Tab Setting Value
Fluid Details Water (Selected)
Water > Morphology > Option Continuous Fluid
Fluid Pairs Fluid Pairs Water | Sand Fully
Coupled
Fluid Pairs > Water | Sand Fully Coupled > Fully Coupled
Particle Coupling
Fluid Pairs > Water | Sand Fully Coupled > Schiller Naumann
Momentum Transfer > Drag Force > Option
Fluid Pairs Water | Sand One Way
Coupled
Fluid Pairs > Water | Sand One Way Coupled > One-way Coupling
Particle Coupling
Fluid Pairs > Water | Sand One Way Coupled > Schiller Naumann
Momentum Transfer > Drag Force > Option

5. Click OK.



Creating the Inlet Velocity Profile
In previous tutorials you have often defined a uniform velocity profile at an inlet boundary.
This means that the inlet velocity near to the walls is the same as that at the center of the
inlet. If you look at the results from these simulations, you will see that downstream of the
inlet, a boundary layer will develop, so that the downstream near wall velocity is much lower
than the inlet near wall velocity.
You can simulate an inlet more accurately by defining an inlet velocity profile, so that the
boundary layer is already fully developed at the inlet. The one seventh power law will be
used in this tutorial to describe the profile at the pipe inlet. The equation for this is:

1
--
r 7
U = W max ⎛ 1 – ---------- ⎞
- (Eqn. 1)
⎝ R max⎠

where W max is the pipe centerline velocity, R max is the pipe radius, and r is the distance
from the pipe centerline.
A non uniform (profile) boundary condition can be created by:
• Creating an expression using CEL that describes the inlet profile.
OR
• Creating a User CEL Function which uses a user subroutine (linked to the ANSYS
CFX-Solver during execution) to describe the inlet profile.
OR
• Loading a BC profile file (a file which contains profile data).
Profiles created from data files are not used in this tutorial, but are used in the tutorial
Tutorial 3: Flow in a Process Injection Mixing Pipe (p. 77).
In this tutorial, you use one of the first two methods listed above to define the velocity
profile for the inlet boundary condition. The results from each method will be identical.
Using a CEL expression is the easiest way to create the profile. The User CEL Function
method is more complex but is provided as an example of how to use this feature. For more
complex profiles, it may be necessary to use a User CEL Function or a BC profile file.
To use the User CEL Function method, continue with this tutorial from User CEL Function
Method for the Inlet Velocity Profile (p. 173). Note that you will need access to a Fortran
compiler to be able to complete the tutorial by the User CEL Function method.
To use the expression method, continue with the tutorial from this point.

Expression 1. Create the following expressions.
Method for the
Inlet Velocity
Profile Name Definition
Rmax 20 [mm]
Wmax 5 [m s^-1]
Wprof Wmax*(abs(1-r/Rmax)^0.143)


In the definition of Wprof, the variable r (radius) is a ANSYS CFX System Variable defined
as:

2 2
r = x +y (Eqn. 2)

In this equation, x and y are defined as directions 1 and 2 (X and Y for Cartesian
coordinate frames) respectively, in the selected reference coordinate frame.
You should now continue with the tutorial from Creating the Boundary Conditions (p. 175).

User CEL The Fortran subroutine has already been written for this tutorial.
Function
Method for the Important: You must have the required Fortran compiler installed and set in your system
Inlet Velocity path in order to run this part of the tutorial. If you do not have a Fortran compiler, you should
Profile use the expression method for defining the inlet velocity, as described in Expression
Method for the Inlet Velocity Profile (p. 172). For details on which Fortran compiler is
required for your platform, see the applicable ANSYS, Inc. installation guide. If you are not
sure which Fortran compiler is installed on your system, try running the cfx5mkext
command (found in <CFXROOT>/bin) from the command line and read the output
messages.

Compiling the Subroutine
1. Copy the subroutine PipeValve_inlet.F to your working directory. It is located in the
<CFXROOT>/examples/ directory.
2. Examine the contents of this file in any text editor to gain a better understanding of this
subroutine.
This file was created by modifying the ucf_template.F file, which is available in the
You can compile the subroutine and create the required library files used by the ANSYS
CFX-Solver at any time before running the ANSYS CFX-Solver. The operation is
performed at this point in the tutorial so that you have a better understanding of the
values you need to specify in ANSYS CFX-Pre when creating a User CEL Function. The
cfx5mkext command is used to create the required objects and libraries as described
below.
3. From the main menu, select Tools > Command Editor.
4. Type the following in the Command Editor dialog box (make sure you do not miss the
semi-colon at the end of the line):
! system ("cfx5mkext PipeValve_inlet.F") < 1 or die;
• This is equivalent to executing the following at an OS command prompt:
cfx5mkext PipeValve_inlet.F
• The ! indicates that the following line is to be interpreted as power syntax and not
CCL. Everything after the ! symbol is processed as Perl commands.
• system is a Perl function to execute a system command.
• The < 1 or die will cause an error message to be returned if, for some reason, there
is an error in processing the command.
5. Click Process to compile the subroutine.


The output produced when this command is executed will be printed to your terminal
window.
Note: You can use the -double option (that is, cfx5mkext -double PipeValve_inlet.F)
to compile the subroutine for use with double precision.
A subdirectory will have been created in your working directory whose name is system
dependent (for example, on IRIX it is named irix). This subdirectory contains the
shared object library.
Note: If you are running problems in parallel over multiple platforms then you will need to
create these subdirectories using the cfx5mkext command for each different platform.

• You can view more details about the cfx5mkext command by running
cfx5mkext -help
• You can set a Library Name and Library Path using the -name and -dest options
respectively.
• If these are not specified, the default Library Name is that of your Fortran file and the
default Library Path is your current working directory.
6. Close the Command Editor dialog box.

Creating the Input Arguments
Next, you will create some values that will be used as input arguments when the subroutine
is called.

1. Click Expression .
2. Set Name to Wmax, and then click OK.
3. Type 5 [m s^-1] into the Definition box, and then click Apply.
The expression will be listed in the Expressions tree view.
4. Use the same method to create an expression named Rmax defined to be 20 [mm].

Creating the User CEL Function
Two steps are required to define a User CEL Function that uses the compiled Fortran
subroutine. First, a User Routine that points to the Fortran subroutine will be created. Then
a User CEL Function that points to the User Routine will be created.

1. From the main toolbar, click User Routine .
2. Set Name to WprofRoutine, and then click OK.
The User Routine details view appears.
3. Set Option to User CEL Function.
4. Set Calling Name to inlet_velocity.
• This is the name of the subroutine within the Fortran file.
• Always use lower case letters for the calling name, even if the subroutine name in
the Fortran file is in upper case.
5. Set Library Name to PipeValve_inlet.
• This is the name passed to the cfx5mkext command by the -name option.
• If the -name option is not specified, a default is used.


• The default is the Fortran file name without the .F extension.
6. Set Library Path to the directory where the cfx5mkext command was executed
(usually the current working directory). For example:
• UNIX: /home/user/cfx/tutorials/PipeValve.
• Windows: c:usercfxtutorialsPipeValve.

This can be accomplished quickly by clicking Browse (next to Library Path),
browsing to the appropriate folder in Select Directory (not necessary if selecting
the working directory), and clicking OK (in Select Directory).
7. Click OK to complete the definition of the user routine.

8. Click User Function .
9. Set Name to WprofFunction, and then click OK.
The Function details view appears.
Important: You must not use the same name for the function and the routine.
10. Set Option to User Function.
11. Set User Routine Name to WprofRoutine.
12. Set Argument Units to [m s^-1], [m], [m]. These are the units for the three input
arguments: Wmax, r, and Rmax.
Set Result Units to [m s^-1], since the result will be a velocity for the inlet.
1. Click OK to complete the User Function specification.
You can now use the user function (WprofFunction) in place of a velocity value by
entering the expression WprofFunction(Wmax, r, Rmax) (although it only makes
sense for the W component of the inlet velocity in this tutorial).
In the definition of WprofFunction, the variable r (radius) is a system variable defined
as:

2 2
r = x +y (Eqn. 3)

In this equation, x and y are defined as directions 1 and 2 (X and Y for Cartesian
coordinate frames) respectively, in the selected reference coordinate frame.

Inlet Boundary 1. Create a new boundary condition named inlet.

Tab Setting Value
Location inlet



Tab Setting Value
Boundary Mass And Momentum > Option Cart. Vel. Components
Details Mass And Momentum > U 0 [m s^-1]
Mass And Momentum > V 0 [m s^-1]
Mass And Momentum > W Wprof -OR-
WprofFunction(Wmax,
r, Rmax)*
Fluid Values† Boundary Conditions Sand Fully Coupled
Sand Fully Coupled > Particle Behavior > Define (Selected)
Particle Behavior
Sand Fully Coupled > Mass and Momentum > Cart. Vel. Components‡
Option
Sand Fully Coupled > Mass And Momentum > U 0 [m s^-1]
Sand Fully Coupled > Mass And Momentum > V 0 [m s^-1]
Sand Fully Coupled > Mass And Momentum > W Wprof -OR-
WprofFunction(Wmax,
r, Rmax)**
Sand Fully Coupled > Particle Position > Option Uniform Injection
Sand Fully Coupled > Particle Position > Number Direct Specification
of Positions > Option
Sand Fully Coupled > Particle Position > Number 200
of Positions > Number
Sand Fully Coupled > Particle Mass Flow > Mass 0.01 [kg s^-1]
Flow Rate
Fluid Values Boundary Conditions Sand One Way Coupled
Sand One Way Coupled > Particle Behavior > (Selected)
Define Particle Behavior
Sand One Way Coupled > Mass and Momentum > Cart. Vel. Components††
Option
Sand One Way Coupled > Mass And Momentum > 0 [m s^-1]
U
Sand One Way Coupled > Mass And Momentum > 0 [m s^-1]
V
Sand One Way Coupled > Mass And Momentum > Wprof -OR-
W WprofFunction(Wmax,
r, Rmax)‡‡
Sand One Way Coupled > Particle Position > Uniform Injection
Option
Sand One Way Coupled > Particle Position > Direct Specification
Number of Positions > Option
Sand One Way Coupled > Particle Position > 5000
Number of Positions > Number
Sand One Way Coupled > Particle Position > 0.01 [kg s^-1]
Particle Mass Flow Rate > Mass Flow Rate



*. Use the Expressions details view to enter either Wprof if using the expression
method, or WprofFunction(Wmax, r, Rmax) if using the User CEL Function
method.
†. Do NOT select Particle Diameter Distribution. The diameter distribution was
defined when creating the domain; this option would override those settings for
this boundary only.
‡. Instead of manually specifying the same velocity profile as the fluid, you can also
select the Zero Slip Velocity option.
**. as you did on the Boundary Details tab
††. Instead of manually specifying the same velocity profile as the fluid, you can also
select the Zero Slip Velocity option.
‡‡. as you did on the Boundary Details tab
3. Click OK.
One-way coupled particles are tracked as a function of the fluid flow field. The latter is not
influenced by the one-way coupled particles. The fluid flow will therefore be influenced by
the 0.01 [kg s^-1] flow of two-way coupled particles, but not by the 0.01 [kg s^-1] flow of
one-way coupled particles.

Outlet 1. Create a new boundary condition named outlet.

Tab Setting Value
Location outlet
Boundary Flow Regime > Option Subsonic
Details Mass and Momentum > Option Average Static Pressure

3. Click OK.

Symmetry Plane 1. Create a new boundary condition named symP.

Tab Setting Value
Location symP

3. Click OK.

Pipe Wall 1. Create a new boundary condition named pipe wall.

Tab Setting Value
Settings
Location pipe wall



Tab Setting Value
Boundary Wall Roughness > Option Rough Wall
Details Roughness Height 0.2 [mm]*
Fluid Boundary Conditions Sand Fully Coupled
Values Boundary Conditions > Sand Fully Coupled > Velocity Restitution Coefficient
> Option
Boundary Conditions > Sand Fully Coupled > Velocity 0.8
> Perpendicular Coeff.
Boundary Conditions > Sand Fully Coupled > Velocity 1
> Parallel Coeff.
Boundary Conditions Sand One Way Coupled
Boundary Conditions > Sand One Way Coupled > Restitution Coefficient
Velocity > Option
Boundary Conditions > Sand One Way Coupled > 0.8
Velocity > Perpendicular Coeff.
Boundary Conditions > Sand One Way Coupled > 1
Velocity > Parallel Coeff.
*. Make sure that you change the units to millimetres. The thickness of the first
element should be of the same order as the roughness height.
3. Click OK.

Editing the 1. In the Outline tree view, edit the boundary condition named Default Domain
Default Default.
Condition

Tab Setting Value
Fluid Values Boundary Conditions Sand Fully Coupled
Boundary Conditions > Sand Fully 0.9
Coupled > Velocity > Perpendicular Coeff.
Boundary Conditions Sand One Way Coupled
Boundary Conditions > Sand One Way 0.9
Coupled > Velocity > Perpendicular Coeff.

3. Click OK.




Tab Setting Value
Components > Option
Components > Option > U
Components > Option > V
Initial Conditions > Cartesian Velocity Wprof -OR-
Components > Option > W WprofFunction(Wmax, r,
Rmax)*
Dissipation

*. Use Enter Expression to enter Wprof if using the Expression method; enter
WprofFunction(Wmax, r, Rmax) if using the User CEL Function method.

3. Click OK.


Tab Setting Value
Basic Settings Advection Scheme > Option Specified Blend Factor
Advection Scheme > Blend Factor 0.75
Particle Control Particle Integration > Maximum Tracking Time (Selected)
Particle Integration > Maximum Tracking Time 10 [s]
> Value
Particle Integration > Maximum Tracking (Selected)
Distance
Particle Integration > Maximum Tracking 10 [m]
Distance > Value
Particle Integration > Max. Num. Integration (Selected)
Steps
Particle Integration > Max. Num. Integration 10000
Steps > Value
Particle Integration > Max. Particle Intg. Time (Selected)
Step
Particle Integration > Max. Particle Intg. Time 1e+10 [s]
Step > Value

3. Click OK.


Tutorial 9: Flow Through a Butterfly Valve: Obtaining a Solution using ANSYS CFX-Solver Manager


Setting Value
File name PipeValve.def


discretion.


Note: If you followed the User CEL Function method, and you wish to run this tutorial in
distributed parallel on machines with different architectures, you must first compile the
PipeValve_inlet.F subroutine on all architectures.

1. Ensure the Define Run dialog box is displayed and click Start Run.
of the run.

In this section, you will first plot erosion on the valve surface and side walls due to the sand
particles. You will then create an animation of particle tracks through the domain.

Erosion Due to Sand Particles
An important consideration in this simulation is erosion to the pipe wall and valve due to the
sand particles. A good indication of erosion is given by the Erosion Rate Density
parameter, which corresponds to pressure and shear stress due to the flow.
1. Edit the object named Default Domain Default.

2. Apply the following settings using the Ellipsis as required for selections


Tutorial 9: Flow Through a Butterfly Valve: Viewing the Results in ANSYS CFX-Post

Tab Setting Value
Color Mode Variable
Variable Sand One Way Coupled.Erosion Rate Density*
Min 0 [kg m^-2 s^-1]
Max 25 [kg m^-2 s^-1]†
*. This is statistically better than Sand Fully Coupled.Erosion Rate Density since
many more particles were calculated for Sand One Way Coupled.
†. This range is used to gain a better resolution of the wall shear stress values around
the edge of the valve surfaces.

3. Click Apply.
As can be seen, the highest values occur on the edges of the valve where most particles
strike. Erosion of the low Z side of the valve would occur more quickly than for the high
Z side.

Particle Tracks
Default particle track objects are created at the start of the session. One particle track is
created for each set of particles in the simulation. You are going to make use of the default
object for Sand Fully Coupled.
The default object draws 10 tracks as lines from the inlet to outlet. Info shows information
about the total number of tracks, index range and the track numbers which are drawn.
1. Edit the object named Res PT for Sand Fully Coupled.

Tab Setting Value
Geometry Max Tracks 20

3. Click Apply.

Erosion on the Pipe Wall
The User Specified range for coloring will be set to resolve areas of stress on the pipe wall
near of the valve.
1. Clear the check box next to Res PT for Sand Fully Coupled.
2. Clear the check box next to Default Domain Default.
3. Edit the object named pipe wall.



Tab Setting Value
Color Mode Variable
Variable Sand One Way Coupled.Erosion Rate Density
Min 0 [kg m^-2 s^-1]
Max 25 [kg m^-2 s^-1]

5. Click Apply.

Particle Track Symbols
1. Clear visibility for all objects except Wireframe.
2. Edit the object named Res PT for Sand Fully Coupled.

Tab Setting Value
Color Mode Variable
Variable Sand Fully Coupled.Velocity w
Symbol Draw Symbols (Selected)
Draw Symbols > Max Time 0 [s]
Draw Symbols > Min Time 0 [s]
Draw Symbols > Interval 0.07 [s]
Draw Symbols > Symbol Fish3D
Draw Symbols > Symbol Size 0.5

4. Clear Draw Tracks.
5. Click Apply.
Symbols are placed at the start of each track.

Creating a Particle Track Animation
The following steps describe how to create a particle tracking animation using Quick
Animation. Similar effects can be achieved in more detail using the Keyframe Animation
option, which allows full control over all aspects on an animation.

1. Select Tools > Animation or click Animation .
2. Select Quick Animation.
3. Select Res PT for Sand Fully Coupled:
4. Click Options to display the Animation Options dialog box, then clear Override
Symbol Settings to ensure the symbol type and size are kept at their specified settings
for the animation playback. Click OK.
Note: The arrow pointing downward in the bottom right corner of the Animation Window
will reveal the Options button if it is not immediately visible.


5. Select Loop.

6. Deselect Repeat forever and ensure Repeat is set to 1.
7. Select Save MPEG.

8. Click Browse and enter tracks.mpg as the file name.

10. If prompted to overwrite an existing movie, click Overwrite.
The animation plays and builds an .mpg file.

Performing Quantitative Calculations
On the outlet boundary condition you created in ANSYS CFX-Pre, you set the Average
Static Pressure to 0.0 [Pa]. To see the effect of this:
1. From the main menu select Tools > Function Calculator.
The Function Calculator is displayed. It allows you to perform a wide range of
quantitative calculations on your results.
Note: You should use Conservative variable values when performing calculations and
Hybrid values for visualization purposes. Conservative values are set by default in ANSYS
CFX-Post but you can manually change the setting for each variable in the Variables
Workspace, or the settings for all variables by using the Function Calculator.
2. Set Function to maxVal.
3. Set Location to outlet.
4. Set Variable to Pressure.
5. Click Calculate.
The result is the maximum value of pressure at the outlet.
6. Perform the calculation again using minVal to obtain the minimum pressure at the
outlet.
7. Select areaAve, and then click Calculate.
• This calculates the area weighted average of pressure.
• The average pressure is approximately zero, as specified by the boundary condition.

Other Features The geometry was created using a symmetry plane. You can display the other half of the
geometry by creating a YZ Plane at X = 0 and then editing the Default Transform object
to use this plane as a reflection plane.
1. When you have finished viewing the results, quit ANSYS CFX-Post.


Tutorial 10:
Flow in a Catalytic Converter

Introduction

before beginning:
• CatConv.pre
• CatConvHousing.hex
• CatConvMesh.gtm

Tutorial 10 Features


Tutorial 10: Flow in a Catalytic Converter: Overview of the Problem to Solve

Subdomains Resistance Source
Outlet (Subsonic)
Wall: No-Slip
Domain Interfaces Fluid-Fluid (No Frame Change)
Default Locators
Polyline
Slice Plane
Vector
Data Export
Title/Text
Viewing the Mesh

• Using multiple meshes in ANSYS CFX-Pre.
• Joining meshes together using static fluid-fluid domain interfaces between the
inlet/outlet flanges and the central catalyst body.
• Applying a source of resistance using a directional loss model.
• Creating a chart to show pressure drop through the domain in ANSYS CFX-Post.
• Exporting data from a line locator to a file.

Catalytic converters are used on most vehicles on the road today. They reduce harmful
emissions from internal combustion engines (such as oxides of nitrogen, hydrocarbons, and
carbon monoxide) that are the result of incomplete combustion. Most new catalytic


Tutorial 10: Flow in a Catalytic Converter: Defining a Simulation in ANSYS CFX-Pre
converters are the honeycomb ceramic type and are usually coated with platinum, rhodium,
or palladium. The exhaust gases flow through the honeycomb structure and a pressure
gradient is established between the inlet and outlet.
exhaust gas
25.0 m/s
288.0 K

catalyst material

flange

20 cm

In this tutorial, a catalytic converter is modeled without chemical reactions in order to
determine the pressure drop. The inlet flange (joining the pipe to the catalyst) is designed
to distribute exhaust gas evenly across the catalyst material.
A hexahedral mesh for the housing, which was created in ICEM-Hexa, is provided.
The different meshes are connected together in ANSYS CFX-Pre. You will import each mesh
then create a domain, which spans all of them. Within the converter, a subdomain is added
to model a honeycomb structure using a directional loss model. The physics is then
specified in the same way as for other tutorials.


then run the session file: CatConv.pre. After you have played the session file as described



5. Under File name, type CatConv.
6. Click Save.

Importing the Meshes
The catalytic converter is comprised of three distinct parts:
• The inlet section (pipe and flange).
• The outlet section (pipe and flange).
• The catalyst (or monolith).
Next you will import a generic inlet/outlet section and the catalyst housing from provided
files.

Housing Section The first mesh that you will import is the hexahedral mesh for the catalyst housing, created
in ICEM-Hexa, named CatConvHousing.hex. This mesh was created using units of
centimetres; however, the units are not stored with the mesh file for this type of mesh. You
must set the mesh import units to cm when importing the mesh into ANSYS CFX-Pre so that
the mesh remains the intended size. The imported mesh has a width in the x-direction of 21
cm and a length in the z-direction of 20 cm.

Setting Value
File type All Types
Definition > Mesh Format ICEM CFD
File name CatConvHousing.hex
Definition > Mesh Units cm

3. Click Open.

Pipe and Flange This mesh was created in units of centimetres. When importing GTM files, ANSYS CFX-Pre
Section uses the units used in the mesh file.
1. Right-click Mesh and select Import Mesh to import the second section.

Setting Value
File type CFX Mesh (gtm)
File name CatConvMesh.gtm

3. Click Open.
You only need to import this mesh once, as you will be copying and rotating the flange
through 180 degrees in the next step to create the inlet side pipe and flange.



Applying a Transform
The pipe and flange are located at the outlet end of the housing. The flange will be rotated
about an axis that points in the y-direction and is located at the center of the housing.
1. Right-click CatConvMesh.gtm and select Transform Mesh. The Mesh Transformation
Editor dialog box appears.

Tab Setting Value
Definition Apply Rotation > Rotation Option Rotation Axis
Apply Rotation > From 0, 0, 0.16
Apply Rotation > To 0, 1, 0.16*
Apply Rotation > Rotation Angle 180 [degree]
Multiple Copies (Selected)
Multiple Copies > # of Copies 1
*. This specifies an axis located at the center of the housing parallel to the y-axis.

3. Click OK.

Creating a Union Region
Three separate regions now exist, but since there is no relative motion between each region,
you only need to create a single domain. This can be done by simply using all three regions
in the domain Location list or, as in this case, by using the Region details view to create a
union of the three regions.
1. Create a new composite region named CatConverter.

Tab Setting Value
Basic Settings Dimension (Filter) 3D
Region List B1.P3, B1.P3 2, LIVE

3. Click OK.

Creating the Domain
For this simulation you will use an isothermal heat transfer model and assume turbulent
flow.

1. Click Domain and set the name to CatConv.



Tab Setting Value
General Basic Settings > Location CatConverter
Options
Basic Settings > Fluid List Air Ideal Gas

3. Click OK.

Creating a Subdomain to Model the Catalyst Structure
The catalyst-coated honeycomb structure will be modeled using a subdomain with a
directional source of resistance.
For quadratic resistances, the pressure drop is modeled using:

∂p
------ = – K Q U U i
- (Eqn. 1)
∂x i

where K Q is the quadratic resistance coefficient, U i is the local velocity in the i direction,

∂p
and ------ is the pressure drop gradient in the i direction.
-
∂x i

1. Select Insert > Subdomain from the main menu or click Subdomain
2. In the Insert Subdomain dialog box, type catalyst.

Tab Setting Value
Basic Settings Location LIVE*
Sources† Sources (Selected)
Sources > Momentum Source/Porous Loss (Selected)
Sources > Momentum Source/Porous Loss > (Selected)
Directional Loss
*. This is the entire housing section.
†. Used to set sources of momentum, resistance and mass for the subdomain (Other
sources are available for different problem physics).

4. Apply the following settings in the Directional Loss section

Setting Value
Streamwise Direction > X Component 0
Streamwise Direction > Y Component 0
Streamwise Direction > Z Component 1



Setting Value
Streamwise Loss > Option Linear and Quadratic
Coefs
Streamwise Loss > Quadratic Resistance Coefficient (Selected)
Streamwise Loss > Quadratic Resistance Coefficient > Quadratic 650 [kg m^-4]
Coefficient
5. Click OK.

Creating Boundary Conditions

Tab Setting Value
Location PipeEnd 2
Boundary Details Mass and Momentum > Normal Speed 25 [m s^-1]

3. Click OK.


Tab Setting Value
Location PipeEnd

3. Click OK.
The remaining surfaces are automatically grouped into the default no slip wall
boundary condition.

Creating the Domain Interfaces
Domain interfaces are used to define the connecting boundaries between meshes where
the faces do not match or when a frame change occurs. Meshes are ‘glued’ together using
the General Grid Interface (GGI) functionality of ANSYS CFX. Different types of GGI
connections can be made. In this case, you require a simple Fluid-Fluid Static connection (no
Frame Change). Other options allow you to change reference frame across the interface or
create a periodic boundary with dissimilar meshes on each periodic face.
Two Interfaces are required, one to connect the inlet flange to the catalyst housing and one
to connect the outlet flange to the catalyst housing.


Inlet Pipe / 1. Create a new domain interface named InletSide.
Housing 2. Apply the following settings
Interface

Tab Setting Value
Basic Settings Interface Side 1 > Region List FlangeEnd 2
Interface Side 2 > Region List INLET

3. Click OK.

Outlet Pipe / 1. Create a new domain interface named OutletSide.
Housing 2. Apply the following settings
Interface

Tab Setting Value
Basic Settings Interface Side 1 > Region List FlangeEnd
Interface Side 2 > Region List OUTLET

3. Click OK.

A sensible guess for the initial velocity is to set it to the expected velocity through the
catalyst housing. As the inlet velocity is 25 [m s^-1] and the cross sectional area of the inlet
and housing are known, you can apply conservation of mass to obtain an approximate
velocity of 2 [m s^-1] through the housing.


Tab Setting Value
Global Initial Conditions > Cartesian Velocity Automatic with Value
Settings Components > Option
Components > U
Components > V
Initial Conditions > Cartesian Velocity -2 [m s^-1]
Components > W
Dissipation

3. Click OK.

Assuming velocities of 25 [m s^-1] in the inlet and outlet pipes, and 2 [m s^-1] in the catalyst
housing, an approximate fluid residence time of 0.1 [s] can be calculated. A sensible
timestep of 0.04 [s] (1/4 to 1/2 of the fluid residence time) will be applied.


Tutorial 10: Flow in a Catalytic Converter: Obtaining a Solution using ANSYS CFX-Solver Manager
For the convergence criteria, an RMS value of at least 1e-05 is usually required for adequate
convergence, but the default value is sufficient for demonstration purposes.


Tab Setting Value
Basic Settings Convergence Control > Fluid Timescale Physical Timescale
Convergence Control >Fluid Timescale 0.04 [s]

3. Click OK.

While writing the solver file, you will use the Summarize Interface Data option to display
information about the connection type used for each domain interface.


Setting Value
File name CatConv.def


4. Once ANSYS CFX-Solver Manager launches, return to ANSYS CFX-Pre.
The Interface Summary dialog box is displayed. This displays information related to the
summary of interface connections.
5. Click OK.
discretion.

When ANSYS CFX-Pre has shut down and the ANSYS CFX-Solver Manager has started, you
can obtain a solution to the CFD problem by following the instructions below:
1. Ensure Define Run is displayed.
2. Click Start Run.


Tutorial 10: Flow in a Catalytic Converter: Viewing the Results in ANSYS CFX-Post
3. Click Yes to post-process the results.

When ANSYS CFX-Post opens, you will need to experiment with the Edge Angle setting for
the Wireframe object in order to view an appropriate amount of the mesh.
Under the Outline tab, several interface boundaries are available. The two connections
between the catalyst housing mesh and the mesh for the inlet and outlet pipes have two
interface boundaries each, one for each side of the connection.
1. Zoom in so the geometry fills the viewer.
2. In the Outline tree view, edit InletSide Side 1.

Tab Setting Value
Draw Lines > Line Color (Red)

4. Click Apply.
5. In the Outline tree view, edit InletSide Side 2.

Tab Setting Value
Draw Lines > Line Color (Green)

7. Click Apply.
8. In the Outline tree view, clear Wireframe to hide it.
-Z.
You should now have a clear view of the tetrahedral / prism and hexahedral mesh on each
side of the interface. The General Grid Interface (GGI) capability of ANSYS CFX was used to
produce a connection between these two dissimilar meshes before the solution was
calculated. Notice that there are more tetrahedral / prism elements than hexahedral
elements and that the extent of the two meshes is not quite the same (this is most
noticeable on the curved edges). The extent of each side of the interface does not have to
match to allow a GGI connection to be made.



Creating User Locations and Plots
1. In the Outline tree view, select Wireframe to show it.
2. In the Outline tree view, clear both InletSide Side 1 and InletSide Side 2.


Tab Setting Value
Color Mode Variable
Variable Pressure

3. Click Apply.
-Y.

Creating a Contour Plot
The pressure falls steadily throughout the main body of the catalytic converter. You can
confirm this with a contour plot.
1. Clear Plane 1 in the Outline tab.
2. Create a new contour plot named Contour 1.

Tab Setting Value
Geometry Locations Plane 1
Variable Pressure
# of Contours 30

4. Click Apply.

Creating a Vector Plot Using the Slice Plane
1. Create a new vector plot named Vector 1.

Tab Setting Value
Geometry Locations Plane 1

3. Click Apply.


Notice the flow separates from the walls, where the inlet pipe expands into the flange,
setting up a recirculation zone. The flow is uniform through the catalyst housing.
Suppose for now that you want to see if the pressure drop is linear by plotting a line graph
of pressure against the z-coordinate. In this case you will use ANSYS CFX-Post to produce the
graph, but you could also export the data, then read it into any standard plotting package.
Graphs are produced using the chart object, but before you can create the chart you must
define the points at which you require the data. To define a set of points in a line, you can
use the polyline object.

Creating a Polyline
The Method used to create the polyline can be From File, Boundary Intersection or
From Contour. If you select From File, you must specify a file containing point definitions
in the required format.
In this tutorial, you will use the Boundary Intersection method. This creates a polyline
from the intersecting line between a boundary object and a location (e.g., between a wall
and a plane). The points on the polyline are where the intersecting line cuts through a
surface mesh edge.
You will be able to see the polyline following the intersecting line between the wall, inlet
and outlet boundaries and the slice plane.
1. In the Outline tree view, clear Contour 1 and Vector 1.
2. Create a new polyline named Polyline 1.

Tab Setting Value
Boundary List CatConv Default, Inlet, Outlet*
Intersect With Plane 1
Color Color (Yellow)
Render Line Width 3
*. Click the ellipsis icon to select multiple items using the <Ctrl> key.

4. Click Apply.
(Y up).

Creating a Chart
Now that a polyline has been defined, a chart can be created. Charts are defined by creating
chart line objects. A chart line is listed in the tree view beneath the chart object to which it
belongs.
1. Create a new chart named Chart 1.



Tab Setting Value
Chart Title Pressure Drop through a Catalytic
Converter
Chart Line 1 Line Name Pressure Drop
Location Polyline 1
X Axis > Variable Z
Y Axis > Variable Pressure
Appearance > Symbols Rectangle
Appearance Sizes > Line 3

3. Click Apply.
Through the main body of the catalytic converter you can see that the pressure drop is
linear. This is in the region from approximately Z=0.05 to Z=0.25. The two lines show the
pressure on each side of the wall. You can see a noticeable difference in pressure
between the two walls on the inlet side of the housing (at around Z=0.25).
4. If required, in the Outline tree view, select Contour 1, Polyline 1, and Vector 1.
5. Click the 3D Viewer tab, then right-click a blank area and select Predefined Camera >
View Towards +Y.
You should now see that the flow enters the housing from the inlet pipe at a slight angle,
producing a higher pressure on the high X wall of the housing.
6. Under Report, expand Chart 1, and edit Chart Line 1.

Tab Setting Value
Chart Line 1 X Axis > Variable Chart Count*
*. This is the data point number (e.g. 1,2,3,4...), it does NOT represent the distance
between each point along the polyline.

8. Click Apply.

Exporting Data
1. From the main menu, select File > Export.

Tab Setting Value
Options Locations Polyline 1
Export Geometry Information (Selected)*
Select Variables Pressure
Formatting Precision 3
*. This ensures X, Y, and Z to be sent to the output file.

3. Click Save.


The file export.csv will be written to the current working directory. This file can be
opened in any text editor. You can use the exported data file to plot charts in other
software.
4. When finished, quit ANSYS CFX-Post.


Tutorial 11:
Non-Newtonian Fluid Flow in
an Annulus

Introduction

before beginning:
• NonNewton.pre
• NonNewtonMesh.gtm


Tutorial 11: Non-Newtonian Fluid Flow in an Annulus: Tutorial 11 Features


Turbulence Model Laminar
Heat Transfer None
Boundary Conditions Symmetry Plane
Wall: No-Slip
Wall: Moving
ANSYS CFX-Post Plots Sampling Plane
Slice Plane
Vector

• Using CFX Expression Language (CEL) to define the properties of a shear-thickening
fluid.
• Using the Moving Wall feature to apply a rotation to the fluid at a wall boundary.


Tutorial 11: Non-Newtonian Fluid Flow in an Annulus: Overview of the Problem to Solve

In this example a non-Newtonian, shear-thickening liquid rotates in a 2D eccentric annular
pipe gap. The motion, shown by the arrow, is brought about solely by viscous fluid
interactions caused by the rotation of the inner pipe.


then run the session file: NonNewton.pre. After you have played the session file as described

5. Under File name, type NonNewton.
6. Click Save.


Tutorial 11: Non-Newtonian Fluid Flow in an Annulus: Defining a Simulation in ANSYS CFX-Pre

Importing the Mesh

Setting Value
File name NonNewtonMesh.gtm

3. Click Open.

Creating an Expression for Shear Rate Dependent Viscosity
You can use an expression to define the dependency of fluid properties on other variables.
In this case, the fluid does not obey the simple linear Newtonian relationship between shear
stress and shear strain rate. The general relationship for the fluid you will model is given by:

n–1
µ = Kγ (Eqn. 1)

where γ is the shear strain rate and K and n are constants. For your fluid, n =1.5 and this
results in shear-thickening behavior of the fluid, i.e., the viscosity increases with increasing
shear strain rate. The shear strain rate is available as a ANSYS CFX-Pre System Variable
(sstrnr).
In order to describe this relationship using CEL, the dimensions must be consistent on both
sides of the equation. Clearly this means that K must have dimensions and requires units to
satisfy the equation. If the units of viscosity are kg m^-1 s^-1, and those of γ are s^-1, then
the expression is consistent if the units of K are kg m^-1 s^(-0.5).
1. Create the following expressions, remembering to click Apply after each is defined.

Name Definition
K 10.0 [kg m^-1 s^-0.5]
n 1.5

You should bound the viscosity to ensure that it remains physically meaningful. To do
so, you will create two additional parameters that will be used to guarantee the value of
the shear strain rate.
2. Create the following expressions for upper and lower bounds.

Name Definition
UpperS 100 [s^-1]
LowerS 1.0E-3 [s^-1]
ViscEqn K*(min(UpperS,max(sstrnr,LowerS))^(n-1))

3. Close the Expressions tab.



Creating a New Fluid
1. Create a new material named myfluid.

Tab Setting Value
Basic Settings Thermodynamic State (Selected)
Material Properties Equation of State > Molar Mass 1 [kg kmol^-1]*
Equation of State > Density 1.0E+4 [kg m^-3]
Specific Heat Capacity (Selected)
Specific Heat Capacity > Specific Heat Capacity 0 [J kg^-1 K^-1]†
Reference State (Selected)
Reference State > Option Specified Point
Reference State > Ref. Temperature 25 [C]
Reference State > Reference Pressure 1 [atm]
Transport Properties > Dynamic Viscosity (Selected)
Transport Properties > Dynamic Viscosity > ViscEqn
Dynamic Viscosity
*. This is not the correct Molar Mass value, but this material property will not be used
by the ANSYS CFX-Solver for this case. In other cases it will be used.
†. This is not the correct value for specific heat, but this property will not be used in
the ANSYS CFX-Solver.

3. Click OK.

Creating the Domain

1. Click Domain and set the name to NonNewton.
2. Apply the following settings to NonNewton

Tab Setting Value
General Basic Settings > Fluids List myfluid
Turbulence > Option None (Laminar)

3. Click OK.

Wall Boundary 1. Create a new boundary condition named rotwall.



Tab Setting Value
Location rotwall
Boundary Details Wall Influence on Flow > Wall Velocity (Selected)
Wall Influence on Flow > Wall Velocity > Rotating Wall
Option
Wall Influence on Flow > Wall Velocity > 31.33 [rev min^-1]
Angular Velocity

3. Click OK.

Symmetry Plane 1. Create a new boundary condition named SymP1.

Tab Setting Value
Location SymP1

3. Click OK.

Tab Setting Value
Location SymP2

6. Click OK.
The outer annulus surfaces will default to the no-slip stationary wall boundary
condition.

A reasonable initial guess for the velocity field is a value of zero throughout the domain.


Tab Setting Value
Global Initial Conditions > Cartesian Velocity Components > Option Automatic with
Settings Value

3. Click OK.


Tutorial 11: Non-Newtonian Fluid Flow in an Annulus: Obtaining a Solution using ANSYS CFX-Solver Manager



Tab Setting Value
Basic Settings Advection Scheme > Option Specific Blend Factor
Advection Scheme > Blend Factor 1*
Convergence Control > Max. Iterations 50
Convergence Criteria > Residual Target 1e-05
*. This is the most accurate but least robust advection scheme.

3. Click OK.


Setting Value
File name NonNewton.def


discretion.

When ANSYS CFX-Pre has shut down and the ANSYS CFX-Solver Manager has started, you
can obtain a solution to the CFD problem by following the instructions below:
2. Click Start Run.


Tutorial 11: Non-Newtonian Fluid Flow in an Annulus: Viewing the Results in ANSYS CFX-Post

In this tutorial you have used CEL to create an expression for the dynamic viscosity. If you
now perform calculations or color graphics objects using the Dynamic Viscosity variable, its
values will have been calculated from the expression you defined in ANSYS CFX-Pre.
These steps instruct the user on how to create a vector plot to show the velocity values in
the domain.
-Z from the shortcut menu.

Tab Setting Value
Geometry Definition > Method Point and Normal
Definition > Point 0, 0, 0.02
Definition > Normal 0, 0, 1
Plane Bounds > Type Circular
Plane Bounds > Radius 0.3 [m]
Plane Type Sample
Plane Type > R Samples 32
Plane Type > Theta Samples 24

4. Click Apply.

Tab Setting Value
Definition > Variable Velocity

7. Click Apply.
8. Try creating some plots of your own, including one that shows the variation of dynamic
viscosity.


Tutorial 12:
Flow in an Axial Rotor/Stator

Introduction
• Defining a Frozen Rotor Simulation in ANSYS CFX-Pre (p. 210)
• Obtaining a Solution to the Frozen Rotor Model (p. 214)
• Viewing the Frozen Rotor Results in ANSYS CFX-Post (p. 215)
• Setting up a Transient Rotor-Stator Calculation (p. 216)
• Obtaining a Solution to the Transient Rotor-Stator Model (p. 219)
• Viewing the Transient Rotor-Stator Results in ANSYS CFX-Post (p. 220)

If this is the first tutorial you are working with it is important to review the following topics
before beginning:
• Axial.pre
• AxialIni.pre
• AxialIni_001.res
• rotor.grd
• stator.gtm


Tutorial 12: Flow in an Axial Rotor/Stator: Tutorial 12 Features


ANSYS CFX-Pre User Mode Turbo Wizard
Transient
Domain Type Multiple Domain
Rotating Frame of Reference
Heat Transfer Total Energy
Outlet (Subsonic)
Wall: No-Slip
Wall: Adiabatic
Domain Interfaces Frozen Rotor
Periodic
Transient Rotor Stator
Transient Example
ANSYS CFX-Solver Manager Restart
Parallel Processing
Isosurface
Surface Group
Turbo Post
Chart Creation
Instancing Transformation
MPEG Generation
Time Step Selection
Transient Animation

• Using the Turbo Wizard in ANSYS CFX-Pre to quickly specify a turbomachinery
application.
• Multiple Frames of Reference and Generalized Grid Interface.
• Using a Frozen Rotor interface between the rotor and stator domains.
• Modifying an existing simulation.
• Setting up a transient calculation.
• Using a Transient Rotor-Stator interface condition to replace a Frozen Rotor interface.


Tutorial 12: Flow in an Axial Rotor/Stator: Overview of the Problem to Solve
• Creating a transient animation showing domain movement in ANSYS CFX-Post.

The following tutorial demonstrates the versatility of GGI and MFR in ANSYS CFX-Pre by
combining two dissimilar meshes. The first mesh to be imported (the rotor) was created in
CFX-TASCflow. This is combined with a second mesh (the stator) which was created using
ANSYS CFX-Mesh.
The geometry to be modeled consists of a single stator blade passage and two rotor blade
passages. The rotor rotates about the Z-axis while the stator is stationary. Periodic
boundaries are used to allow only a small section of the full geometry to be modeled.
Figure 1 Geometry subsection

Outflow

Shroud

Stator Blade

Rotor Blade

Hub

Inflow

At the change in reference frame between the rotor and stator, two different interface
models are considered. First a solution is obtained using a Frozen Rotor model. After
viewing the results from this simulation, the latter is modified to use a transient rotor-stator
interface model. The Frozen Rotor solution is used as an initial guess for the transient
rotor-stator simulation.


Tutorial 12: Flow in an Axial Rotor/Stator: Defining a Frozen Rotor Simulation in ANSYS CFX-Pre
The full geometry contains 60 stator blades and 113 rotor blades. To help you visualize how
the modeled geometry fits into the full geometry, the following figure shows approximately
half of the full geometry. The Inflow and Outflow labels show the location of the modeled
section in .

Outflow

Inflow

Axis of Rotation

As previously indicated, the modeled geometry contains two rotor blades and one stator
blade. This is an approximation to the full geometry since the ratio of rotor blades to stator
blades is close to, but not exactly, 2:1. In the stator blade passage a 6° section is being
modeled (360°/60 blades), while in the rotor blade passage a 6.372° section is being
modeled (2*360°/113 blades). This produces a pitch ratio at the interface between the stator
and rotor of 0.942. As the flow crosses the interface it is scaled to allow this type of geometry
to be modeled. This results in an approximation of the inflow to the rotor passage.
Furthermore, the flow across the interface will not appear continuous due to the scaling
applied.
The periodic boundary conditions will introduce an additional approximation since they
cannot be periodic when a pitch change occurs.
You should always try to obtain a pitch ratio as close to 1 as possible in your model to
minimize approximations, but this must be weighed against computational resources. A full
machine analysis can be performed (modeling all rotor and stator blades) which will always
eliminate any pitch change, but will require significant computational time. For this
rotor/stator geometry, a 1/4 machine section (28 rotor blades, 15 stator blades) would
produce a pitch change of 1.009, but this would require a model about 15 times larger than
in this tutorial example.

Defining a Frozen Rotor Simulation in ANSYS CFX-Pre


then run the session file: AxialIni.pre. After you have played the session file as described
(p. 87), proceed to Obtaining a Solution to the Frozen Rotor Model (p. 214).

This tutorial will use the Turbomachinery wizard in ANSYS CFX-Pre. This pre-processing
mode is designed to simplify the setup of turbomachinery simulations.
3. Select Turbomachinery and click OK.
5. Under File name, type AxialIni.
6. Click Save.

Basic Settings
1. Set Machine Type to Axial Turbine.
2. Click Next.

Component Definition
Two new components are required. As they are created, meshes are imported.
1. Right-click in the blank area and select New Component from the shortcut menu.
2. Create a new component of type Stationary, named S1.
3. Apply the following setting

Setting Value
Mesh > File stator.gtm*
*. You may have to select the CFX Mesh option under File Type.

4. Create a new component of type Rotating, named R1.



Setting Value
Component Type > Value 523.6 [radian s^-1]
Mesh File > File rotor.grd*
*. You may have to select the CFX-TASCflow option under File Type.

Note: The components must be ordered as above (stator then rotor) in order for the
interface to be created correctly. The order of the two components can be changed by right
clicking on S1 and selecting Move Component Up.

When a component is defined, Turbo Mode will automatically select a list of regions that
correspond to certain boundary condition types. This information should be reviewed
in the Region Information section to ensure that all is correct. This information will be
used to help set up boundary conditions and interfaces. The upper case turbo regions
that are selected (e.g., HUB) correspond to the region names in the CFX-TASCflow grd
file. CFX-TASCflow turbomachinery meshes use these names consistently.
6. Click Next.

Physics Definition
In this section, you will set properties of the fluid domain and some solver parameters.

Tab Setting Value
Physics Fluid Air Ideal Gas
Definition Simulation Type > Type Steady State
Model Data > Reference Pressure 0.25 [atm]
Model Data > Heat Transfer Total Energy
Model Data > Turbulence k-Epsilon
Boundary Templates > P-Total Inlet Mass Flow Outlet (Selected)
Boundary Templates > P-Total 0 [atm]
Boundary Templates > T-Total 340 [K]
Boundary Templates > Mass Flow Rate 0.06 [kg s^-1]
Interface > Default Type Frozen Rotor
Solver Parameters > Convergence Control Physical Timescale
Solver Parameters > Physical Timescale 0.002 [s]*

*. This time scale is approximately equal to 1 / ω , which is often appropriate for
rotating machinery applications.

2. Click Next.



Interface Definition
ANSYS CFX-Pre will try to create appropriate interfaces using the region names presented
previously in the Region Information section. In this case, you should see that a periodic
interface has been generated for both the rotor and the stator. These are required when
modeling a small section of the true geometry. An interface is also required to connect the
two components together across the frame change.
1. Review the various interfaces but do not change them.
2. Click Next.

Boundary Definition
ANSYS CFX-Pre will try to create appropriate boundary conditions using the region names
presented previously in the Region Information section. In this case, you should see a list
of boundary conditions that have been generated. They can be edited or deleted in the
same way as the interface connections that were set up earlier.
1. Review the various boundary definitions but do not change them.
2. Click Next.

Final Operations
1. Set Operation to Enter General Mode.
2. Click Finish.


Setting Value
File name AxialIni.def


discretion.
You should see ANSYS CFX-Solver Manager appear.


Tutorial 12: Flow in an Axial Rotor/Stator: Obtaining a Solution to the Frozen Rotor Model

Obtaining a Solution to the Frozen Rotor Model
Compared to previous tutorials, the mesh for this tutorial contains many more nodes
(although it is still too coarse to perform a high quality CFD simulation). This results in a
corresponding increase in solution time for the problem. Solving this problem in parallel is
recommended, if possible. Your machine should have a minimum of 256MB of memory to
run this tutorial.
More detailed information about setting up ANSYS CFX to run in parallel is available. For
details, see Tutorial 5: Flow Around a Blunt Body (p. 109).
You can solve this example using Serial, Local Parallel or Distributed Parallel.
• Obtaining a Solution in Serial (p. 214)
• Obtaining a Solution With Local Parallel (p. 214)
• Obtaining a Solution with Distributed Parallel (p. 215)

Obtaining a Solution in Serial
If you do not have a license to run ANSYS CFX in parallel you can run in serial by clicking the
Start Run button when ANSYS CFX-Solver Manager has opened up. Solution time in serial
is approximately 45 minutes on a 1GHz processor.
1. Click Start Run on the Define Run dialog box.
2. Click Yes to start ANSYS CFX-Post.
When you are finished, proceed to Viewing the Frozen Rotor Results in ANSYS CFX-Post
(p. 215).

Obtaining a Solution With Local Parallel
To run in local parallel, the machine you are on must have more than one processor.
1. Set Run Mode to PVM Local Parallel in the Define Run dialog box.
This is the recommended method for most applications.

2. If required, click Add Partition to add more partitions.
By default, 2 partitions are assigned.
3. Click Start Run.
of the run.
When you are finished, proceed to Viewing the Frozen Rotor Results in ANSYS CFX-Post
(p. 215).


Tutorial 12: Flow in an Axial Rotor/Stator: Viewing the Frozen Rotor Results in ANSYS CFX-Post

Obtaining a Solution with Distributed Parallel
1. Set Run Mode to PVM Distributed Parallel in the Define Run dialog box.
One partition should already be assigned to the host that you are logged into.

2. Click Insert Host to specify a new parallel host.
3. In Select Parallel Hosts, select another host name (this should be a machine that you
can log into using the same user name).
4. Click Add, and then Close.
The names of the two selected machines should be listed in the Host Name column of
5. Click Start Run.
of the run.

Viewing the Frozen Rotor Results in ANSYS CFX-Post
The Turbo-Post feature will be demonstrated in the following sections. This feature is
designed to greatly reduce the effort taken to post-process turbomachinery simulations.

Initializing Turbo-Post
To initialize Turbo-Post, the properties of each component must be entered. This includes
entering information about the inlet, outlet, hub, shroud, blade and periodic regions.
1. Click the Turbo tab.
The Turbo Initialization dialog box is displayed, and asks you whether you want to
auto-initialize all components.

Note: If you do not see the Turbo Initialization dialog box, or as an alternative to using that
dialog box, you can initialize all components by clicking the Initialize All Components
button which is visible initially by default, or after double-clicking the Initialization object
in the Turbo tree view.
2. Click Yes.
The Turbo tree view shows the two components in domains R1 and S1. In this case, the
initialization works without problems. If there was a problem initializing a component,
this would be indicated in the tree view.

Viewing Three Domain Passages
Next, you will create an instancing transformation to plot three blade passages for the stator
and six blade passages for the rotor.
The instancing properties of each domain have already been entered during Initialization.
In the next steps, you will create a surface group plot to color the blade and hub surfaces
with the same variable.


Tutorial 12: Flow in an Axial Rotor/Stator: Setting up a Transient Rotor-Stator Calculation
1. From the main menu, select Insert > Location > Surface Group.
2. Click OK.
The default name is accepted.

Tab Setting Value
Geometry Locations R1 Blade, R1 Hub, S1 Blade, S1 Hub
Color Mode Variable
Variable Pressure

4. Click Apply.
6. Open Plots > 3D View for editing.

Tab Setting Value
3D View Instancing > Domain R1
Instancing > # of Copies 3

8. Click Apply.

Tab Setting Value
3D View Instancing > Domain S1
Instancing > # of Copies 3

10. Click Apply.

Blade Loading Turbo Chart
In this section, you will create a plot of pressure around the stator blade at a given spanwise
location.
1. In the Turbo tree view, double-click Blade Loading.
This profile of the pressure curve is typical for turbomachinery applications.
When you are finished viewing the chart, quit ANSYS CFX-Post.

Setting up a Transient Rotor-Stator Calculation
This section describes the step-by-step definition of the flow physics in ANSYS CFX-Pre. The
existing frozen-rotor simulation is modified to define the transient rotor-stator simulation.
If you have not already completed the frozen-rotor simulation, please refer to Defining a
Frozen Rotor Simulation in ANSYS CFX-Pre (p. 210) before proceeding with the transient
rotor-stator simulation.



then run the session file: Axial.pre. After you have played the session file as described in
earlier tutorials under Playing the Session File and Starting ANSYS CFX-Solver Manager
(p. 87), proceed to Obtaining a Solution to the Transient Rotor-Stator Model (p. 219).

Note: The session file creates a new simulation named Axial.cfx and will not modify the
existing database. It also copies the required initial values files from the examples directory
to the current working directory.

Opening the Existing Simulation
This step involves opening the original simulation and saving it to a different location.
2. Open the results file named AxialIni_001.res.
3. Save the simulation as Axial.cfx in your working directory.
4. Select Tools > Turbo Mode.
Basic Settings is displayed

Modifying the Physics Definition
You need to modify the domain to define a transient simulation. You are going to run for a
time interval such that the rotor blades pass through 1 pitch (6.372°) using 10 timesteps.
This is generally too few timesteps to obtain high quality results, but is sufficient for tutorial
purposes. The timestep size is calculated as follows:
Rotational Speed = 523.6 rad/s
Rotor Pitch Modelled = 2*(2π/113) = 0.1112 rad
Time to pass through 1 pitch = 0.1112/523.6 = 2.124e-4 s
Since 10 time steps are used over this interval each timestep should be 2.124e-5 s.
1. Click Next.
Component Definition is displayed.
2. Click Next.
Physics Definition is displayed.



Tab Setting Value
Physics Fluid Air Ideal Gas
Definition
Simulation Type > Type Transient
Simulation Type > Total Time 2.124e-4 [s]*
Simulation Type > Time Steps 2.124e-5 [s]†
Interface > Default Type Transient Rotor Stator
*. This gives 10 timesteps of 2.124e-5 s
†. This timestep will be used until the total time is reached

Note: A transient rotor-stator calculation often runs through more than one pitch. In these
cases, it may be useful to look at variable data averaged over the time interval required to
complete 1 pitch. You can then compare data for each pitch rotation to see if a “steady state”
has been achieved, or if the flow is still developing.
4. Click Next.
Interface Definition is displayed.
5. Click Next.
Boundary Definition is displayed.
6. Click Next.
Final Operations is displayed.
7. Ensure that Operation is set to Enter General Mode.
8. Click Finish.
Initial values are required, but will be supplied later using a results file.


2. Click the Trn Results tab.
3. Create a new transient result with the name Transient Results 1.

Setting Value
Output Variables List * Pressure, Velocity, Velocity in Stn Frame
Output Frequency > Time Interval 2.124e-5 [s]
*. Use the <Ctrl> key to select more than one variable.

5. Click OK.



Tutorial 12: Flow in an Axial Rotor/Stator: Obtaining a Solution to the Transient Rotor-Stator Model
A warning will appear, due to a lack of initial values.
2. Click Yes.
Initial values are required, but will be supplied later using a results file.

Setting Value
File name Axial.def


discretion.

Obtaining a Solution to the Transient Rotor-Stator Model
When the ANSYS CFX-Solver Manager has started you will need to specify an initial values
file before starting the ANSYS CFX-Solver.

Serial Solution
If you do not have a license, or do not want to run ANSYS CFX in parallel, you can run it in
serial. Solution time in serial is similar to the first part of this tutorial.

1. Under Initial Values File, click Browse .
2. Select AxialIni_001.res.
3. Click Open.
4. Click Start Run.
5. You may see a notice that the mesh from the initial values file will be used. This mesh is
the same as in the definition file. Click OK to continue.
of the run.
When you are finished, continue with Monitoring the Run (p. 220).

Parallel Solution
You can solve this example using either local parallel or distributed parallel, in the same way
as in the first part of this tutorial. For details, see Obtaining a Solution to the Frozen Rotor
Model (p. 214).


Tutorial 12: Flow in an Axial Rotor/Stator: Viewing the Transient Rotor-Stator Results in ANSYS CFX-Post

Monitoring the Run
During the solution, look for the additional information that is provided for transient
rotor-stator runs. Each time the rotor is rotated to its next position, the number of degrees
of rotation and the fraction of a pitch moved is given. You should see that after 10 timesteps
the rotor has been moved through 1 pitch.

Viewing the Transient Rotor-Stator Results in ANSYS CFX-Post
To examine the transient interaction between the rotor and stator, you are going to create
a blade-to-blade animation of pressure. A turbo surface will be used as the basis for this plot.

Initializing Turbo-Post
The Turbo Initialization dialog box is displayed, and asks you whether you want to
auto-initialize all components.
Note: If you do not see the Turbo Initialization dialog box, or as an alternative to using that
dialog box, you can initialize all components by clicking the Initialize All Components
button which is visible initially by default, or after double-clicking the Initialization object
in the Turbo tree view.

2. Click Yes.
Both components (domains) are now being initialized based on the automatically
selected turbo regions. When the process is complete, a green turbine icon appears next
to each component entry in the list. Also, the viewer displays a green background mesh
for each initialized component.
3. Double-click Component 1 (S1) and review the automatically-selected turbo regions.

Displaying a Surface of Constant Span
1. In the Turbo tree view, double-click Blade-to-Blade.
A surface of constant span appears, colored by pressure. This object can be edited and
then redisplayed using the details view.

Using Multiple Turbo Viewports
1. In the Turbo tree view, double-click Initialization.
2. Click Three Views.
Left view is 3D View, top right is Blade-to-Blade and bottom right is Meridional view.
3. Click Single View.

Creating a Turbo Surface Midway Between the Hub and Shroud
1. Create a Turbo Surface from the Insert drop down menu with a Constant Span and
value of 0.5.


2. Under the Color panel select Variable and set it to Pressure with a user specified range
of -10000 [Pa] to -7000 [Pa].

Setting up Instancing Transformations
Next, you will use instancing transformations to view a larger section of the model. The
properties for each domain have already been entered during the initialization phase, so
only the number of instances needs to be set.
1. In the Turbo tree view, double-click the 3D View object.
2. In the Instancing section of the form, set # of Copies to 6 for R1.
3. Click Apply.
4. In the Instancing section of the form, set # of Copies to 6 for S1.
5. Click Apply.
6. Return to the Outline tab and ensure that the turbo surface is visible again.

Creating a Transient Animation
Start by loading the first timestep:

2. Select time value 0.
3. Click Apply to load the timestep.
The rotor blades move to their starting position. This is exactly 1 pitch from the previous
position so the blades will not appear to move.
4. Clear Visibility for Wireframe.
5. Position the geometry as shown below, ready for the animation. During the animation
the rotor blades will move to the right. Make sure you have at least two rotor blades out
of view to the left side of the viewer. They will come into view during the animation.

6. In the toolbar at the top of the window click Animation .

7. In the Animation dialog box, click New to create KeyFrameNo1.
8. Highlight KeyframeNo1, then set # of Frames to 9.
9. Use the Timestep Selector to load the final timestep.



10. In the Animation dialog box, click New to create KeyframeNo2.
11. Click More Animation Options to expand the Animation dialog box.
12. Click Options and set Transient Case to TimeValue Interpolation. Click OK.
The animation now contains a total of 11 frames (9 intermediate frames plus the two
Keyframes), one for each of the available time values.
13. In the expanded Animation dialog box, select Save MPEG.

14. Click Browse , next to the Save MPEG box and then set the file name to an
appropriate file name.
15. If frame 1 is not loaded (shown in the F: text box at the bottom of the Animation dialog
box), click To Beginning to load it.
Wait for ANSYS CFX-Post to finish loading the objects for this frame before proceeding.

• It takes a while for the animation to complete.
• To view the MPEG file, you will need to use a media player that supports the MPEG
format.
You will be able to see from the animation, and from the plots created previously, that
the flow is not continuous across the interface. This is because a pitch change occurs.
The relatively coarse mesh and the small number of timesteps used in the transient
simulation also contribute to this. The movie was created with a narrow pressure range
compared to the global range which exaggerates the differences across the interface.

Further Postprocessing
You can use the Turbo Calculator to produce a report on the performance of the turbine.
1. Edit the Gas Turbine Performance macro in the Turbo tree view.
2. Set Ref Radius to 0.4575 and leave other settings at their default values.
3. Click Calculate.
4. Click View Report.


Tutorial 13:
Reacting Flow in a Mixing Tube

Introduction
• Outline of the Process (p. 224)

before beginning:
• Reactor.pre
• ReactorExpressions.ccl
• ReactorMesh.gtm



Tutorial 13: Reacting Flow in a Mixing Tube: Overview of the Problem to Solve

Fluid Type Variable Composition Mixture
Particle Tracking Component Source
Outlet (Subsonic)
Symmetry Plane
Wall: Adiabatic
Additional Variables
ANSYS CFX-Post Plots Isosurface
Slice Plane

• Creating and using a multicomponent fluid in ANSYS CFX-Pre.
• Using CEL to model a reaction in ANSYS CFX-Pre.
• Using an algebraic additional variable to model a scalar distribution.
• Using a subdomain as the basis for component sources.

Reaction engineering is one of the main core components in the chemical industry.
Optimizing reactor design leads to higher yields, lower costs and, as a result, higher profit.
This example demonstrates the capability of ANSYS CFX in modeling basic reacting flows
using a multicomponent fluid model.

Outline of the Process
The model is a mixing tube into which acid and alkali are injected through side holes. The
reaction to be modeled is:

H 2 SO 4 + 2NaOH → Na 2 SO 4 + 2H 2 O (Eqn. 1)

The tube is modeled as an axisymmetric section.


Tutorial 13: Reacting Flow in a Mixing Tube: Defining a Simulation in ANSYS CFX-Pre
The reaction between acid and alkali is represented as a single step irreversible liquid-phase
reaction

A+B→C (Eqn. 2)

Reagent A (dilute sulphuric acid) is injected through a ring of holes near the start of the
tube. As it flows along the tube it reacts with Reagent B (dilute sodium hydroxide) which is
injected through a further two rings of holes downstream. The product, C , remains in
solution.
The composition and pH of the mixture within the tube are principal quantities of interest
to be predicted by the model.
The flow is assumed to be fully turbulent and turbulence is assumed to have a significant
effect on the process. The process is also exothermic.


then run the session file: Reactor.pre. After you have played the session file as described

5. Under File name, type Reactor.
6. Click Save.

Importing the Mesh



Setting Value
File name ReactorMesh.gtm

3. Click Open.

Creating a Multicomponent Fluid
In addition to providing template fluids, ANSYS CFX allows you to create custom fluids for
use in all your ANSYS CFX models. These fluids may be defined as a pure substance, but may
also be defined as a mixture, consisting of a number of transported fluid components. This
type of fluid model is useful for applications involving mixtures, reactions, and combustion.
In order to define custom fluids, ANSYS CFX-Pre provides the Material details view. This tool
allows you to define your own fluids as pure substances, fixed composition mixtures or
variable composition mixtures using a range of template property sets defined for common
materials.
The mixing tube application requires a fluid made up from four separate materials (or
components). The components are the reactants and products of a simple chemical
reaction together with a neutral carrier liquid. You are first going to define the materials that
take part in the reaction (acid, alkali and product) as pure substances. The neutral carrier
liquid is water; this material is already defined since it is commonly used. Finally, you will
create a variable composition mixture consisting of these four materials. This is the fluid that
you will use in your simulation. A variable composition mixture (as opposed to a fixed
composition mixture) is required because the proportion of each component will change
throughout the simulation due to the reaction.

Acid properties 1. Create a new material named acid.

Tab Setting Value
Basic Settings Option Pure Substance
Thermodynamic State > Thermodynamic State Liquid



Tab Setting Value
Material Properties Thermodynamic Properties > Equation of State 19.52 [kg kmol^-1]*
> Molar Mass
Thermodynamic Properties > Equation of State 1080 [kg m^-3]
> Density
Thermodynamic Properties > Specific Heat (Selected)
Capacity
Thermodynamic Properties > Specific Heat 4190 [J kg^-1 K^-1]
Transport Properties > Dynamic Viscosity > Value
Option
Transport Properties > Dynamic Viscosity > 0.001 [kg m^-1 s^-1]
Dynamic Viscosity
Transport Properties > Thermal Conductivity (Selected)
Transport Properties > Thermal Conductivity > 0.6 [W m^-1 K^-1]
Thermal Conductivity
*. The Molar Masses for the three materials created are only set for completeness
since they are not used when solving this problem.
3. Click OK.

Alkali 1. Create a new material named alkali.
properties 2. Apply the following settings

Tab Setting Value
Material Properties Thermodynamic Properties > Equation of State 20.42 [kg kmol^-1]
> Molar Mass
> Density
Capacity
Dynamic Viscosity

3. Click OK.


Product of the 1. Create a new material named product.
reaction 2. Apply the following settings
properties

Tab Setting Value
Material Properties Thermodynamic Properties > Equation of State 21.51 [kg kmol^-1]
> Molar Mass
> Density
Capacity
Dynamic Viscosity

3. Click OK.

Fluid properties 1. Create a new material named mixture.

Tab Setting Value
Basic Settings Option Variable Composition Mixture
Material Group User, Water Data
Materials List Water, acid, alkali, product
Thermodynamic State > Liquid
Thermodynamic State

3. Click OK.

Creating an Additional Variable to Model pH
You are going to use an additional variable to model the distribution of pH in the mixing
tube. You can create additional variables and use them in selected fluids in your domain.
1. Create a new additional variable named MixturePH.



Tab Setting Value
Basic Settings Units [kg kg^-1]

3. Click OK.
This additional variable is now available for use when you create or modify a domain.

Defining the Reaction
Reactions and reaction kinetics can be modeled using CFX Expression Language (CEL),
together with appropriate settings for Component sources. This section shows you how to
develop an Eddy Break Up (EBU) type term using CEL to simulate the reaction between acid
and alkali.

Reaction Source The reaction and reaction rate are modeled using a basic Eddy Break Up formulation for the
Terms component and energy sources, so that, for example, the transport equation for mass
fraction of acid is

∂
d ---- ( ρm f acid ) + ∇•( ρU mf acid ) – ∇ • ( ρD A ∇m f acid )
-
∂t
(Eqn. 3)
ε mf alkali
= – 4ρ --min ⎛ mf acid, ---------------- ⎞
-
k ⎝ i ⎠

where mf is mass fraction, D A is the kinematic diffusivity (set above) and i is the
stoichiometric ratio. The right hand side represents the source term applied to the transport
equation for the mass fraction of acid. The left hand side consists of the transient, advection
and diffusion terms.
For acid-alkali reactions, the stoichiometric ratio is usually based on volume fractions. To
correctly model the reaction using an Eddy Break Up formulation based on mass fractions,
you must calculate the stoichiometric ratio based on mass fractions.
In this tutorial the reaction is modeled by introducing source terms for the acid, alkali and
product components. You can now also model this type of flow more easily using a reacting
mixture as your fluid. There is also a tutorial example using a reacting mixture. For details,
see Tutorial 18: Combustion and Radiation in a Can Combustor (p. 299).

Technical Note (Reference Only)
In ANSYS CFX, Release 11.0, a source is fully specified by an expression for its value S.
A source coefficient C is optional, but can be specified to provide convergence
enhancement or stability for strongly-varying sources. The value of C may affect the rate of
convergence but should not affect the converged results.



If no suitable value is available for C , the solution time scale or timestep can still be reduced
to help improve convergence of difficult source terms.

Important: C must never be positive.

An optimal value for C when solving an individual equation for a positive variable φ with a
source S whose strength decreases with increasing φ is

∂S
C = (Eqn. 4)
∂φ

Where this derivative cannot be computed easily,

S
C = --
- (Eqn. 5)
φ

may be sufficient to ensure convergence.
Another useful recipe for C is

ρ
C = – --
- (Eqn. 6)
τ

where τ is a local estimate for the source time scale. Provided that the source time scale is
not excessively short compared to flow or mixing time scales, this may be a useful approach
for controlling sources with positive feedback ( ∂S ⁄ ∂φ > 0 ) or sources that do not depend
directly on the solved variable φ .

Calculating pH The pH (or acidity) of the mixture is a function of the mass fraction of acid, alkali and product.
For the purposes of this calculation, acid is assumed to be dilute and fully dissociated into
+ -
its respective ions ( H and X ); alkali is assumed to be dilute and fully dissociated into its
+ -
respective ions ( Y and OH ); product is assumed to be a salt solution including further
+ -
H and OH ions in a stoichiometric ratio.
The concentrations of hydrogen and hydroxyl ions can be calculated from the mass
fractions of the components using the following expressions:

mf prod
[ H ] acid = αρ ⎛ mf acid + --------------- ⎞ = [ X ]
+ i–i
- (Eqn. 7)
⎝ 1+i ⎠

imf prod
[ OH ] alkali = βρ ⎛ mf alkali + ----------------- ⎞ = [ Y ]
- i+i
- (Eqn. 8)
⎝ 1+i ⎠


- +
where α and β are the X ion and Y ion concentrations in the acid and alkali
-
respectively. For this problem, α is set to 1.0E-05 kmole X per kg of acid, and β = α ⁄ i .
Applying charge conservation and equilibrium conditions,

+ + - -
[ H ] + [ Y ] = [ X ] + [ OH ] (Eqn. 9)

+ -
[ H ] [ OH ] = K W (Eqn. 10)

gives the following quadratic equation for free hydrogen ion concentration:

+ + + -
[ H ] ( [ H ] + [ Y ] –[ X ] ) = K W (Eqn. 11)

+ 2 + - +
[H ] + ([Y ] – [X ])[H ] – K W = 0 (Eqn. 12)

i+i
pH = – log 10 [ H ] (Eqn. 13)

where K W is the equilibrium constant (1.0 x 10E-14 kmoles2 m-6).

+
The quadratic equation can be solved for [ H ] using the equation
2
+ – b + b – 4ac + -
[ H ] = ------------------------------------- where a = 1 , b = [ Y ] – [ X ] and c = – K W .
-
2a

Creating You can create the expressions required to model the reaction sources and pH by either
expressions to reading them in from a file or by defining them in the Expressions workspace. Note that the
model the
expressions used here do not refer to a particular fluid since there is only a single fluid. In a
reaction
multiphase simulation you must prefix variables with a fluid name, for example
Mixture.acid.mf instead of acid.mf.

In this tutorial the expressions can be imported from a file to avoid typing them.

Reading 1. Select File > Import CCL.
expressions 2. Ensure that Import Method is set to Append.
from a file
3. Select ReactorExpressions.ccl, which should be in your working directory.
4. Click Open.
Note that the expressions have been loaded.

Creating the Domain
Simulation branch.



Tab Setting Value
General Basic Settings > Domain Type Fluid Domain
Options
Basic Settings > Fluids List mixture
Component Details acid
Component Details > acid > Option Transport Equation
Component Details > acid > Kinematic Diffusivity (Selected)
Component Details > acid > Kinematic Diffusivity > 0.001 [m^2 s^-1]
Kinematic Diffusivity

3. Use the same Option and Kinematic Diffusivity settings for alkali and product as
you have just set for acid.
4. For Water, set Option to Constraint as follows

Tab Setting Value
Fluid Models Component Details Water
Component Details > Water > Option Constraint

One component must always use Constraint. This is the component used to balance
the mass fraction equation; the sum of the mass fractions of all components of a fluid
must equal unity.

Tab Setting Value
Fluid Models Additional Variable Details > MixturePH (Selected)
Additional Variable Details > MixturePH > Algebraic Equation
Option
Additional Variable Details > MixturePH > pH
Value

6. Click OK.

Creating a Subdomain to Model the Chemical Reactions
To provide the correct modeling for the chemical reaction you need to define sources for
the fluid components acid, alkali ,and product. To do this, you need to create a
subdomain where the relevant sources can be specified. In this case, sources need to be
provided within the entire domain of the mixing tube since the reaction occurs throughout
the domain.
1. Create a new subdomain named sources.



Tab Setting Value
Sources Sources (Selected)
Sources > Equation Sources acid.mf
Sources > Equation Sources > acid.mf (Selected)
Sources > Equation Sources > acid.mf > Source AcidSource
Sources > Equation Sources > acid.mf > Source Coefficient (Selected)
Sources > Equation Sources > acid.mf > Source Coefficient > AcidSourceCoeff
Source Coefficient
Sources > Equation Sources alkali.mf
Sources > Equation Sources > alkali.mf (Selected)
Sources > Equation Sources > alkali.mf > Source AlkaliSource
Sources > Equation Sources > alkali.mf > Source Coefficient (Selected)
Sources > Equation Sources > alkali.mf > Source Coefficient > AlkaliSourceCoeff
Source Coefficient
Sources > Equation Sources Energy
Sources > Equation Sources > Energy (Selected)
Sources > Equation Sources > Energy > Source HeatSource
Sources > Equation Sources product.mf
Sources > Equation Sources > product.mf (Selected)
Sources > Equation Sources > product.mf > Source ProductSource
Sources > Equation Sources > product.mf > Source Coefficient (Selected)
Sources > Equation Sources > product.mf > Source Coefficient 0 [kg m^-3 s^-1]
> Source Coefficient

3. Click OK.

Water Inlet 1. Create a new boundary condition named InWater.

Tab Setting Value
Location InWater

3. Leave mass fractions for all components set to zero. Since Water is the constraint fluid,
it will be automatically given a mass fraction of 1 on this inlet.
4. Click OK.

Acid Inlet 1. Create a new boundary condition named InAcid.
Boundary


Tab Setting Value
Location InAcid
Component Details acid
Component Details > acid > Mass Fraction 1.0
Component Details alkali
Component Details > alkali > Mass Fraction 0
Component Details product
Component Details > product > Mass Fraction 0

3. Click OK.

Alkali Inlet The inlet area for the alkali is twice that of the acid and it also enters at a higher velocity. The
Boundary result is an acid-to-alkali volume inflow ratio of 1:2.667. Recall that a stoichiometric ratio of
2.7905 was specified based on mass fractions. When the density of the acid (1080 [kg m^3])
and alkali (1130 [kg m^3]) are considered, the acid-to-alkali mass flow ratio can be
calculated as 1:2.7905. You are therefore providing enough acid and alkali to produce a
neutral solution if they react together completely.
1. Create a new boundary condition named InAlkali.

Tab Setting Value
Location InAlkali
Component Details > acid (Selected)
Component Details > acid > Mass Fraction 0
Component Details > alkali (Selected)
Component Details > alkali > Mass Fraction 1
Component Details > product (Selected)
Component Details > product > Mass Fraction 0

3. Click OK.

Outlet 1. Create a new boundary condition named out.



Tab Setting Value
Location out

3. Click OK.

Symmetry 1. Create a new boundary condition named sym1.

Tab Setting Value
Location sym1

3. Click OK.
4. Create a new boundary condition named sym2.

Tab Setting Value
Location sym2

6. Click OK.
remaining unspecified boundary.

The values for acid, alkali and product will be initialized to 0. Since Water is the
constrained component, it will make up the remaining mass fraction which, in this case, is 1.




Tab Setting Value
Global Initial Conditions > Cartesian Velocity Components > Automatic with Value
Settings Option
Initial Conditions > Turbulence Eddy Dissipation > Automatic
Option
Initial Conditions > Component Details acid
Initial Conditions > Component Details > acid > Option Automatic with Value
Initial Conditions > Component Details > acid > Mass 0
Fraction
Initial Conditions > Component Details alkali
Initial Conditions > Component Details > alkali > Option Automatic with Value
Initial Conditions > Component Details > alkali > Mass 0
Fraction
Initial Conditions > Component Details product
Initial Conditions > Component Details > product > Automatic with Value
Option
Initial Conditions > Component Details > product > Mass 0
Fraction

3. Click OK.


Tab Setting Value
Basic Settings Advection Scheme > Option Specific Blend Factor
Advection Scheme > Blend Factor 0.75
Convergence Control > Max. Iterations 50
Convergence Control > Fluid Timescale Physical Timescale
Convergence Control > Fluid Timescale 0.01 [s]*
*. The length of mixing tube is 0.06 [m] and inlet velocity is 2 [m s^-1]. An estimate of
the dynamic time scale is 0.03 [s]. An appropriate timestep would be 1/4 to 1/2 of
this value.


Tutorial 13: Reacting Flow in a Mixing Tube: Obtaining a Solution using ANSYS CFX-Solver Manager
3. Click OK.

Note: At this point, you might see a physics validation message regarding a change in the
advection scheme. This change will not affect the outcome of the simulation; you will still be
able to run this simulation in the ANSYS CFX-Solver.


Setting Value
File name Reactor.def


discretion.

When the ANSYS CFX-Solver Manager has started, obtain a solution to the CFD problem by
following the instructions below.
Using the double precision ANSYS CFX-Solver executable is recommended for this case:
2. Select Show Advanced Controls. On the Solver tab, select Double Precision under
Executable Settings.
3. Click Start Run.

Try the following:
• Create an XY plane through Z = 0 colored by MixturePH. The lower and upper bounds
depend on the precision setting used in the ANSYS CFX-Solver should approximately
range from 2 to 15 (single) or 2 to 11 (double).


Tutorial 13: Reacting Flow in a Mixing Tube: Viewing the Results in ANSYS CFX-Post
Figure 1 shows two planes colored by MixturePH, with the plane on the right having a
more accurate solution throughout the domain.
Figure 1 Comparison of Single and Double Precision Results for pH Variance

• View the acid, alkali and product mass fractions on the same plane.
• Create isosurfaces of Turbulence Kinetic Energy and Turbulence Eddy
Dissipation.


Tutorial 14:
Conjugate Heat Transfer in a
Heating Coil

Introduction

before beginning:
• HeatingCoil.pre
• HeatingCoil_001.res
• HeatingCoilMesh.gtm


Tutorial 14: Conjugate Heat Transfer in a Heating Coil: Tutorial 14 Features


Conjugate Heat Transfer
Subdomains Energy Source
Opening
Wall: No-Slip
Wall: Adiabatic
ANSYS CFX-Post Plots Cylinder
Default Locators
Isosurface
Expression Details View
Lighting Adjustment
Variable Details View

• Creating and using a solid domain as a heater coil in ANSYS CFX-Pre.
• Modeling conjugate heat transfer in ANSYS CFX-Pre.
• Specifying a subdomain to specify a heat source.
• Creating a cylinder locator using CEL in ANSYS CFX-Post.
• Examining the temperature distribution which is affected by heat transfer from the coil
to the fluid.


Tutorial 14: Conjugate Heat Transfer in a Heating Coil: Overview of the Problem to Solve

This example demonstrates the capability of ANSYS CFX in modeling conjugate heat
transfer. In this example, part of the model of a simple heat exchanger is used to model the
transfer of heat from a solid to a fluid. The model consists of a fluid domain and a solid
domain. The fluid domain is an annular region through which water flows at a constant rate.
The heater is a solid copper coil modeled as a constant heat source.

Outflow

Solid Heater

Inflow

This tutorial also includes an optional step that demonstrates the use of the CFX to ANSYS
Data Transfer Tool to export thermal and mechanical stress data for analysis in ANSYS. A
results file is provided in case you wish to skip the model creation and solution steps within
ANSYS CFX.


then run the session file: HeatingCoil.pre. After you have played the session file as

5. Under File name, type HeatingCoil.


Tutorial 14: Conjugate Heat Transfer in a Heating Coil: Defining a Simulation in ANSYS CFX-Pre
6. Click Save.

Importing the Mesh

Setting Value
File name HeatingCoilMesh.gtm

3. Click Open.

Creating the Domains
This simulation requires both a fluid and a solid domain. First, you will create a fluid domain
for the annular region of the heat exchanger.

Creating a Fluid The fluid domain will include the region of fluid flow but exclude the solid copper heater.
Domain
1. Click Domain and set the name to FluidZone.
2. Apply the following settings to FluidZone

Tab Setting Value
General Basic Settings > Location B1.P3*
Options
Basic Settings > Fluids List Water
Initialization Domain Initialization (Selected)
Domain Initialization > Initial Conditions (Selected)
Domain Initialization > Initial Conditions > Turbulence (Selected)
Eddy Dissipation
*. This region name may be different depending on how the mesh was created. You
should pick the region that forms the exterior surface of the volume surrounding
the coil.

3. Click OK.

Creating a Solid Since you know that the copper heating element will be much hotter than the fluid, you can
Domain initialize the temperature to a reasonable value. The initialization option that is set when
creating a domain applies only to that domain.
1. Create a new domain named SolidZone.



Tab Setting Value
General Basic Settings > Location B2.P3
Options
Basic Settings > Domain Type Solid Domain
Basic Settings > Solids List Copper
Solid Models Heat Transfer > Option Thermal Energy
Initialization Domain Initialization (Selected)
Domain Initialization > Initial Conditions (Selected)
Domain Initialization > Initial Conditions > Automatic with
Temperature > Option Value
Domain Initialization > Initial Conditions > 550 [K]
Temperature > Temperature

3. Click OK.

Creating a Subdomain to Specify a Thermal Energy Source
To allow a thermal energy source to be specified for the copper heating element, you need
to create a subdomain.
1. Create a new subdomain named Heater in the domain SolidZone.

Tab Setting Value
Basic Settings Basic Settings > Location B2.P3*
Sources Sources (Selected)
Sources > Equation Sources > Energy (Selected)
Sources > Equation Sources > Energy > Source 1.0E+07 [W m^-3]
*. This is the same location as for the domain SolidZone, because you want the source
term to apply to the entire solid domain.

3. Click OK.

Inlet Boundary You will now create an inlet boundary condition for the cooling fluid (Water).
1. Create a new boundary condition named inflow in the domain FluidZone.

Tab Setting Value
Location inflow

3. Click OK.

Opening The opening boundary condition type is used in this case because at some stage during the
boundary solution, the coiled heating element will cause some recirculation at the exit. At an opening
boundary you need to set the temperature of fluid that enters through the boundary. In this
case it is useful to base this temperature on the fluid temperature at the outlet, since you
expect the fluid to be flowing mostly out through this opening.
1. Create a new expression named OutletTemperature.
2. Set Definition to areaAve(T)@REGION:outflow
3. Click Apply.
4. Create a new boundary condition named outflow in the domain FluidZone.

Tab Setting Value
Location outflow
Boundary Details Mass and Momentum > Option Opening Pres. and Dirn
Heat Transfer > Static Temperature OutletTemperature

6. Click OK.
remaining unspecified external boundaries of the fluid domain. The default Fluid-Solid
Interface boundary condition (flux conserved) will be applied to the surfaces between
the solid domain and the fluid domain.

Creating the Domain Interface
If you have the Generate Default Domain Interfaces option turned on (from Edit >
Options > CFX-Pre), then you will see that an interface called
Default Fluid Solid Interface already exists, and is listed in the Outline tree view. If
this is the case, you can optionally skip the following instructions for creating a domain
interface (since the domain interface set here will have the same settings as, and will
automatically replace, the default domain interface).
If you have the Generate Default Domain Interfaces option turned off, then there is no
domain interface defined at this point. In this case, create a domain interface using either
one of the following methods (the result is the same):

Creating a 1. Right click Simulation in the Outline tree view and ensure that Automatic Default
Default Domain Interfaces is selected. An interface named Default Fluid Solid Interface should
Interface
now appear under the Simulation branch.

Creating a 1. Double click Default Fluid Solid Interface and apply the following settings:
Domain
Interface
Manually



Tab Setting Value
Basic Settings Interface Type Fluid Solid
Interface Side 1 > Domain (Filter) FluidZone
Interface Side 1 > Region List F10.B1.P3, F5.B1.P3,
F6.B1.P3, F7.B1.P3, F8.B1.P3,
F9.B1.P3
Interface Side 2 > Domain (Filter) SolidZone
Interface Side 2 > Region List F10.B2.P3, F5.B2.P3,
F6.B2.P3, F7.B2.P3, F8.B2.P3,
F9.B2.P3
Interface Models > Option General Connection
Interface Models > Frame Change/Mixing None
Model > Option
Interface Models > Pitch Change > Option None
Mesh Connection Method > Option Automatic

2. Click OK.


Tab Setting Value
Convergence Control >Fluid Timescale 2 [s]

For the Convergence Criteria, an RMS value of at least 1e-05 is usually required for
adequate convergence, but the default value is sufficient for demonstration purposes.
3. Click OK.


Setting Value
File name HeatingCoil.def




Tutorial 14: Conjugate Heat Transfer in a Heating Coil: Obtaining a Solution using ANSYS CFX-Solver Manager
discretion.

While the calculations proceed, you can see residual output for various equations in both
the text area and the plot area. Use the tabs to switch between different plots (e.g., Heat
Transfer, Turbulence Quantities, etc.) in the plot area. You can view residual plots for the
fluid and solid domains separately by editing the Workspace Properties.
2. Click Start Run.

• Creating a Cylindrical Locator (p. 246)
• Specular Lighting (p. 247)
• Moving the Light Source (p. 247)

Creating a Cylindrical Locator
Next, you will create a cylindrical locator close to the outside wall of the annular domain.
This can be done by using an expression to specify radius and locating a particular radius
with an isosurface.

Expression 1. Create a new expression named expradius.

Setting Value
Definition (x^2 + y^2)^0.5

3. Click Apply.

Variable 1. Create a new variable named radius.

Setting Value
Expression expradius


Tutorial 14: Conjugate Heat Transfer in a Heating Coil: Exporting the Results to ANSYS
3. Click Apply.

Isosurface of the 1. Create a new isosurface named Isosurface 1.
variable 2. Apply the following settings

Tab Setting Value
Geometry Definition > Variable radius
Definition > Value 0.8 [m]*
Color Mode Variable
Min 300 [K]
Max 302 [K]
*. The maximum radius is 1 m, so a cylinder locator at a radius of 0.8 m is suitable.

3. Click Apply.

Specular Lighting
Specular lighting is on by default. Specular lighting allows glaring bright spots on the
surface of an object, depending on the orientation of the surface and the position of the
light.
1. Apply the following settings to Isosurface 1

Tab Setting Value
Render Draw Faces > Specular (Cleared)

2. Click Apply.

Moving the Light Source
To move the light source, click within the 3-D Viewer, then press and hold <Shift> while
pressing the arrow keys left, right, up or down.
Tip: If using the Standalone version, you can move the light source by positioning the
mouse pointer in the viewer, holding down the <Ctrl> key, and dragging using the right
mouse button.

Exporting the Results to ANSYS
This optional step involves generating an ANSYS .cdb data file from the results generated
in ANSYS CFX-Solver. The .cdb file could then be used with the ANSYS Multi-field solver to
measure the combined effects of thermal and mechanical stresses on the solid heating coil.
There are two possible ways to export data to ANSYS:


• Use ANSYS CFX-Solver Manager to export data. For details, see Exporting Data from
ANSYS CFX-Solver Manager (p. 248).
• Use ANSYS CFX-Post to export data. This involves:
a. Importing a surface mesh from ANSYS into ANSYS CFX-Post, and associating the
surface with the corresponding 2D region in the ANSYS CFX-Solver results file.
b. Exporting the data to a file containing SFE commands that represent surface
element thermal or mechanical stress values.
c. Loading the commands created in the previous step into ANSYS and visualizing the
loads.

Exporting Data from ANSYS CFX-Solver Manager
Since the heat transfer in the solid domain was calculated in ANSYS CFX, the 3D thermal data
will be exported to ANSYS Element Type as 3D Thermal (70) data. The mechanical
stresses are calculated on the liquid side of the liquid-solid interface. These values will be
exported to ANSYS Element Type as 2D Stress (154) data.

Thermal Data 1. Start ANSYS CFX-Solver Manager.
2. Select Tools > Export to ANSYS MultiField.
Export to ANSYS MultiField Solver dialog box appears.

Setting Value
Results File HeatingCoil_001.res
Export File HeatingCoil_001_ansysfsi_70.csv
Domain Name > Domain SolidZone
Domain Name > Boundary * *
Export Options > ANSYS Element Type 3D Thermal (70)
*. Leave Boundary empty.

4. Click Export.
When the export is complete, click OK to acknowledge the message and continue with
the next steps to export data for Mechanical Stresses.

Mechanical 1. Apply the following settings in the Export to ANSYS MultiField Solver dialog box (see
Stresses Step 2 above):

Setting Value
Results File HeatingCoil_001.res
Export File HeatingCoil_001_ansysfsi_154.csv
Domain Name > Domain FluidZone
Domain Name > Boundary FluidZone Default
Export Options > ANSYS Element Type 2D Stress (154)

2. Click Export.

You now have two exported files that can be loaded into ANSYS Multiphysics. When you are
finished, close ANSYS CFX-Solver Manager and ANSYS CFX-Post.


Tutorial 15:
Multiphase Flow in Mixing
Vessel

Introduction

before beginning:
• MixerImpellerMesh.gtm
• MixerTank.geo
• MultiphaseMixer.pre


Tutorial 15: Multiphase Flow in Mixing Vessel: Tutorial 15 Features


Rotating Frame of Reference
Turbulence Model Dispersed Phase Zero Equation
Fluid-Dependant Turbulence
Model
k-Epsilon
Heat Transfer None
Buoyant Flow
Multiphase
Outlet (Degassing)
Wall: Thin Surface
Wall: (Slip Depends on Volume
Fraction)
Domain Interfaces Frozen Rotor
Periodic
Output Control
Isosurface
Slice Plane
Other Quantitative Calculation

• Importing meshes that have CFX-4 and ANSYS CFX .def/.res file formats.
• Setting up a simulation using multiple frames of reference.
• Connecting two domains (one for the impeller and one for the tank) via Frozen Rotor
interfaces.
• Modeling rotational periodicity using periodic boundary conditions.
• Using periodic GGI interfaces where the mesh does not map exactly.
• Using thin surfaces for the blade and baffle surfaces.
• Setting up a multiphase flow problem.


Tutorial 15: Multiphase Flow in Mixing Vessel: Overview of the Problem to Solve

This example simulates the mixing of two fluids in a mixing vessel. The geometry consists of
a mixing tank vessel containing four baffles. A rotating impeller blade is connected to a shaft
which runs vertically through the vessel. Air is injected into the vessel through an inlet pipe
located below the impeller blade at a speed of 5 m/s.
Figure 1 Cut-away diagram of Mixing Vessel

Shaft Baffles

Mixing Tank
Air Inlet Impeller

The figure above shows the full geometry, with part of the tank walls and one baffle cut
away. The symmetry of the vessel allows a 1/4 section of the full geometry to be modeled.


then run the session file: MultiphaseMixer.pre. After you have played the session file as


Tutorial 15: Multiphase Flow in Mixing Vessel: Defining a Simulation in ANSYS CFX-Pre
5. Under File name, type MultiphaseMixer.
6. Click Save.

Importing the Meshes
In this tutorial, a CFX-4 mesh is imported using advanced options. These options control
how the CFX-4 mesh is imported into ANSYS CFX.
By creating 3D regions on fluid regions, you prevent import of USER3D and POROUS regions.
Turn off this option if you do not need these regions for sub-domains. This will simplify the
regions available in ANSYS CFX-Pre. In this case, the mesh file contains USER3D regions that
were created as a location for a thin surface and you do not need them for defining any
subdomains.

Importing the 1. Right-click Mesh and select Import Mesh.
Mixer Tank 2. Apply the following settings
Mesh

Setting Value
File type CFX-4 (*geo)
File name MixerTank.geo
Advanced Options > Create 3D Regions on > Fluid Regions (Cleared)
(USER3D, POROUS)

3. Click Open.

Importing the 1. Right-click Mesh and select Import Mesh to import the second mesh.
Impeller Mesh 2. Apply the following settings

Setting Value
File type CFX Mesh (*gtm)
File name MixerImpellerMesh.gtm

3. Click Open.
(X up) to view the mesh assemblies.

Transforming In the next step you will move the impeller mesh to its correct position.
the Impeller
1. Right-click MixerImpellerMesh.gtm and select Transform Mesh.
Mesh
The Mesh Transformation Editor dialog box appears.



Tab Setting Value
Definition Transformation Translation
Apply Translation > Method Deltas
Apply Translation > Dx, Dy, Dz 0.275, 0, 0

3. Click OK.

Viewing the 1. Click Label and Marker Visibility .
Mesh at the 2. Apply the following setting
Tank Periodic
Boundary
Tab Setting Value
Label Options Show Labels (Cleared)

3. Click OK.
4. In the Outline workspace, expand MixerImpellerMesh.gtm and MixerTank.geo to
view associated 2D primitives.
5. Under MixerTank.geo > Principal 3D regions > Primitive 3D, click the primitive
region BLKBDY_TANK_PER2.
You can now see the mesh on one of the periodic regions of the tank. To reduce the solution
time for this tutorial, the mesh used is very coarse. This is not a suitable mesh to obtain
accurate results, but it is sufficient for demonstration purposes.

Note: If you do not see the surface mesh, highlighting may be turned off. If highlighting is
disabled, toggle Highlight . The default highlight type will show the surface mesh for any
selected regions. If you see a different highlighting type, you can alter it by selecting Edit >
Options and browsing to CFX-Pre > Viewer.

Creating the Domains
Rotating 1. Click Domain and set the name to impeller.
Domain for the 2. Apply the following settings
Impeller



Tab Setting Value
General Basic Settings > Location Main
Options
Basic Settings > Fluids List Air at 25 C, Water
Domain Models > Buoyancy > Gravity X Dirn. -9.81 [m s^-2]
Domain Models > Buoyancy > Gravity Y Dirn. 0 [m s^-2]
Domain Models > Buoyancy > Buoy. Ref. Density* 997 [kg m^-3]
Domain Models > Domain Motion > Option Rotating
Domain Models > Domain Motion > Angular Velocity 84 [rev min-1]†
Domain Models > Domain Motion > Axis Definition > Global X
Rotation Axis
Fluid Multiphase Options > Homogeneous Model (Cleared)
Models Multiphase Options > Allow Musig Fluids (Cleared)
Multiphase Options > Free Surface Model > Option None
Heat Transfer > Homogeneous Model (Cleared)
Heat Transfer > Fluid Temperature 25 [C]
Turbulence > Homogeneous Model (Cleared)
Turbulence > Option Fluid Dependent
Fluid Fluid Details Air at 25 C
Details
Fluid Details > Air at 25 C > Morphology > Option Dispersed Fluid
Fluid Details > Air at 25 C > Morphology > Mean Diameter 3 [mm]
Fluid Fluid Pairs Air at 25 C | Water
Pairs Fluid Pairs > Air at 25 C | Water > Surface Tension Coefficient (Selected)
Fluid Pairs > Air at 25 C | Water > Surface Tension Coefficient 0.073 [N m^-1]‡
> Surf. Tension Coeff.
Fluid Pairs > Air at 25 C | Water > Momentum Transfer > Drag Grace
Force > Option
Fluid Pairs > Air at 25 C | Water > Momentum Transfer > Drag (Selected)
Force > Volume Fraction Correction Exponent
Fluid Pairs > Air at 25 C | Water > Momentum Transfer > Drag 4
Force > Volume Fraction Correction Exponent > Value
Fluid Pairs > Air at 25 C | Water > Momentum Transfer > Lopez de
Non-drag forces > Turbulent Dispersion Force > Option Bertodano
Fluid Pairs > Air at 25 C | Water > Momentum Transfer > 0.1
Non-drag forces > Turbulent Dispersion Force > Dispersion
Coeff.
Fluid Pairs > Air at 25 C | Water > Turbulence Transfer > Sato Enhanced
Option Eddy Viscosity



*. For dilute dispersed multiphase flow, always set the buoyancy reference density to
that for continuous fluid.
†. Note the unit.
‡. This must be set to allow the Grace drag model to be used.
3. Click OK.

Stationary Next, you will create a stationary domain for the main tank by copying the properties of the
Domain for the existing fluid domain.
Main Tank
1. Right-click impeller and select Duplicate from the shortcut menu.
2. Set the name of this domain to tank and open it for editing.

Tab Setting Value
General Options Basic Settings > Location Primitive 3D
Domain Models > Domain Motion > Stationary
Option

4. Click OK.

The following boundary conditions that define the problem will be set:
• An inlet through which air enters the mixer.
• A degassing outlet, so that only the gas phase can leave the domain.
• Thin surfaces for the baffle and impeller blade.
• A wall for the hub and shaft in the rotating domain. This will be stationary relative to the
rotating domain.
• A wall for the shaft in the stationary domain. This will be rotating relative to the
stationary domain.
• Periodic domain interfaces for the periodic faces of the tank and impeller.
Periodic domain interfaces can either be one-to-one or GGI interfaces. One-to-one
transformations occur for topologically similar meshes whose nodes match within a given
tolerance. One-to-one periodic interfaces are more accurate and reduce CPU and memory
requirements.
When the default wall boundary condition is generated, the internal 2D regions of an
imported mesh are ignored, while the regions that form domain boundaries are included.

Air Inlet 1. Create a new boundary condition in the domain tank named Airin.

Tab Setting Value
Location INLET_DIPTUBE
Boundary Details Mass and Momentum > Option Fluid Dependent



Tab Setting Value
Boundary Conditions > Air at 25 C > Velocity 5 [m s^-1]
> Normal Speed
Boundary Conditions > Air at 25 C > Volume 1
Boundary Conditions > Water > Velocity > 5 [m s^-1]
Normal Speed
Boundary Conditions > Water > Volume 0
3. Click OK.

Degassing 1. Create a new boundary condition in the domain tank named LiquidSurface.
Outlet 2. Apply the following settings
Boundary

Tab Setting Value
Location WALL_LIQUID_SURFACE
Boundary Details Mass and Momentum > Option Degassing Condition

3. Click OK.

Thin Surface for In ANSYS CFX-Pre, thin surfaces can be created by specifying wall boundary conditions on
the Baffle both sides of internal 2D regions. Both sides of the baffle regions will be specified as walls in
this case.
1. Create a new boundary condition in the domain tank named Baffle.

Tab Setting Value
Location WALL_BAFFLES*
Boundary Details Wall Influence On Flow > Option Fluid Dependent
Boundary Conditions > Air at 25 C > Wall Free Slip
Influence on Flow > Option
Boundary Conditions > Water > Wall No Slip†
*. The WALL_BAFFLES region includes the surfaces on both sides of the baffle (you can
confirm this by examining WALL_BAFFLES in the region selector). Therefore, you do
not need to use the Create Thin Surface Partner option.
†. The Free Slip condition can be used for the gas phase since the contact area with
the walls is near zero for low gas phase volume fractions.

3. Click OK.

Wall Boundary The next stage involves setting up a boundary condition for the shaft, which exists in the
Condition for tank (stationary domain). These regions are connected to the shaft in the impeller domain.
the Shaft
Since the tank domain is not rotating, you need to specify a moving wall to account for the
rotation of the shaft.
Part of the shaft is located directly above the air inlet, so the volume fraction of air in this
location will be high and the assumption of zero contact area for the gas phase is not
physically correct. In this case, a no slip boundary condition is more appropriate than a free
slip condition for the air phase. When the volume fraction of air in contact with a wall is low,
a free slip condition is more appropriate for the air phase.
In cases where it is important to correctly model the dispersed phase slip properties at walls
for all volume fractions, you can declare both fluids as no slip, but set up an expression for
the dispersed phase wall area fraction. The expression should result in an area fraction of
zero for dispersed phase volume fractions from 0 to 0.3, for example, and then linearly
increase to an area fraction of 1 as the volume fraction increases to 1.
1. Create a new boundary condition in the domain tank named TankShaft.

Tab Setting Value
Location WALL_SHAFT,
WALL_SHAFT_CENTER
Boundary Conditions > Air at 25 C > Wall No Slip
Boundary Conditions > Air at 25 C > Wall (Selected)
Influence on Flow > Wall Velocity
Boundary Conditions > Air at 25 C > Wall Rotating Wall
Influence on Flow > Wall Velocity > Option
Boundary Conditions > Air at 25 C > Wall 84 [rev min-1]*
Influence on Flow > Wall Velocity > Angular
Velocity
Boundary Conditions > Air at 25 C > Wall Global X
Influence on Flow > Wall Velocity > Axis
Definition > Rotation Axis
*. Note the unit.

3. Select Water and set the same values as for Air at 25 C.
4. Click OK.

Required 1. Create a new boundary condition in the domain impeller named Blade.
Conditions in
the Impeller
Domain



Tab Setting Value
Location Blade
Thin Surfaces > Create Thin Surface Partner (Selected)*
Boundary Conditions > Water > Wall No Slip
*. The Blade region only includes the surface from one side of the blade (you can
confirm this by examining Blade in the region selector). Therefore, you can select
Create Thin Surface Partner to include the surfaces from the other side of the
blade.

3. Click OK.
You will see in the tree view that a boundary named Blade Other Side has
automatically been created.
4. Create a new boundary condition in the domain impeller named HubShaft.

Tab Setting Value
Location Hub, Shaft

6. Click OK.

Modifying the 1. On the tree view, open tank Default for editing.
Default Wall 2. Apply the following settings
Boundary
Condition
Tab Setting Value



Tab Setting Value
3. Click OK.
It is not necessary to set the default boundary in the impeller domain since the
remaining surfaces will be assigned interface conditions in the next section.

Creating the Domain Interfaces
Impeller 1. Create a new domain interface named ImpellerPeriodic.
Domain 2. Apply the following settings

Tab Setting Value
Interface Side 1 > Domain (Filter) impeller
Interface Side 1 > Region List Periodic1
Interface Side 2 > Region List Periodic2
Interface Models > Option Rotational Periodicity
Interface Models > Axis Definition > Global X
Rotation Axis

3. Click OK.

Tank Domain 1. Create a new domain interface named TankPeriodic.

Tab Setting Value
Interface Side 1 > Domain (Filter) tank
Interface Side 1 > Region List BLKBDY_TANK_PER1
Interface Side 2 > Region List BLKBDY_TANK_PER2
Interface Models > Option Rotational Periodicity
Interface Models > Axis Definition > Global X
Rotation Axis

3. Click OK.


Frozen Rotor Next, you will create three Frozen Rotor interfaces for the regions connecting the two
Interface domains. In this case three separate interfaces are created. You should not try to create a
single domain interface for multiple surfaces that lie in different planes.
1. Create a new domain interface named Top.

Tab Setting Value
Interface Side 1 > Region List Top
Interface Side 2 > Region List BLKBDY_TANK_TOP
Interface Models > Frame Change/Mixing Frozen Rotor
Model > Option

3. Click OK.
4. Create a new domain interface named Bottom.

Tab Setting Value
Interface Side 1 > Region List Bottom
Interface Side 2 > Region List BLKBDY_TANK_BOT
Model > Option

6. Click OK.
7. Create a new domain interface named Outer.

Tab Setting Value
Interface Side 1 > Region List Outer
Interface Side 2 > Region List BLKBDY_TANK_OUTER
Model > Option

9. Click OK.



The initialization for volume fraction is 0 for air and automatic for water. Therefore, the initial
volume fraction for water will be set to 1 so that the sum of the two fluid volume fractions is
1.
It is important to understand how the velocity is initialized in this tutorial. Here, both fluids
use Automatic for the Cartesian Velocity Components. When the Automatic option is
used, the initial velocity field will be based on the velocity values set at inlets, openings, and
outlets. In this tutorial, the only boundary that has a set velocity value is the inlet, which
specifies a velocity of 5 [m s^-1] for both phases. Without setting the Velocity Scale
parameter, the resulting initial guess would be a uniform velocity of 5 [m s^-1] in the
X-direction throughout the domains for both phases. This is clearly not suitable since the
water phase is enclosed by the tank. When the boundary velocity conditions are not
representative of the expected domain velocities, the Velocity Scale parameter should be
used to set a representative domain velocity. In this case the velocity scale for water is set to
zero, causing the initial velocity for the water to be zero. The velocity scale is not set for air,
resulting in an initial velocity of 5 [m s^-1] in the X-direction for the air. This should not be a
problem since the initial volume fraction of the air is zero everywhere.


Tab Setting Value
Fluid Settings Fluid Specific Initialization Air at 25 C
Fluid Specific Initialization > Air at 25 C > Initial Automatic with Value
Fluid Specific Initialization > Air at 25 C > Initial 0
Fluid Specific Initialization Water
Fluid Specific Initialization > Water > Initial (Selected)
Conditions > Cartesian Velocity Components >
Velocity Scale
Fluid Specific Initialization > Water > Initial 0 [m s^-1]
Velocity Scale > Value
Conditions > Turbulence Eddy Dissipation

3. Click OK.

Generally, two different time scales exist for multiphase mixers. The first is a small time scale
based on the rotational speed of the impeller, typically taken as 1 / ω , resulting in a time
scale of 0.11 s for this case. The second time scale is usually larger and based on the
recirculation time of the continuous phase in the mixer.


Using a timestep based on the rotational speed of the impeller will be more robust, but
convergence will be slow since it takes time for the flow field in the mixer to develop. Using
a larger timestep reduces the number of iterations required for the mixer flow field to
develop, but reduces robustness. You will need to experiment to find an optimum timestep.

Note: You may find it useful to monitor the value of an expression during the solver run so
that you can view the volume fraction of air in the tank (the gas hold up). The gas hold up is
often used to judge convergence in these types of simulations by converging until a
steady-state value is achieved. You could create the following expressions:
TankAirHoldUp = volumeAve(Air at 25 C.vf)@tank
ImpellerAirHoldUp = volumeAve(Air at 25 C.vf)@impeller
TotalAirHoldUp = (volume()@tank * TankAirHoldUp + volume()@impeller *
ImpellerAirHoldUp) / (volume()@tank + volume()@impeller)
and then monitor the value of TotalAirHoldUp.


Tab Setting Value
Convergence Control > Fluid Timescale 2 [s]*
*. This is an aggressive timestep for this case.

3. Click OK.

In the next step, you will choose to write additional data to the results file which allows force
and torque calculations to be performed in post-processing.


Tab Setting Value
Results Output Boundary Flows (Selected)
Output Boundary Flows > Boundary Flows All

3. Click OK.

Since this tutorial uses domain interfaces and you choose to summarize the interface data,
an information window is displayed that informs you of the connection type used for each
domain interface.


Tutorial 15: Multiphase Flow in Mixing Vessel: Obtaining a Solution using ANSYS CFX-Solver Manager

Setting Value
File name MultiphaseMixer.def
Quit CFX–Pre* (Cleared)


If you are notified the file already exists, click Overwrite.
A message about interface connections appears.
4. Click OK.
discretion.

The ANSYS CFX-Solver Manager will be launched after ANSYS CFX-Pre has closed down. You
will be able to obtain a solution to the CFD problem by following the instructions below.
2. Click Start Run.
depending on your system.
After a run has finished, examine some of the information printed at the end of the OUT
file.
A common quantity of interest is the mass balance; this compares the amount of fluid
leaving the domain to the amount entering.
• You usually want the Global Imbalance, in %: to be less than 0.1 % in a converged
solution.
• For a single phase calculation, the mass balance is the P-Mass equation.
• For a multiphase calculation, examine the information given for the P-Vol equation.
• This is not the volumetric flow balance information, but is the summation of the
phasic continuity mass balance information.
of the run.

When ANSYS CFX-Post has started you will be able to see the mixer geometry in the Viewer.
You will create some plots showing how effective mixing has occurred. You will also
calculate the torque and power required by the impeller.


Tutorial 15: Multiphase Flow in Mixing Vessel: Viewing the Results in ANSYS CFX-Post

Visualizing the Mixing Process
Creating a plane 1. Create a new plane named Plane 1.

Tab Setting Value
Geometry Definition > Method Three Points
Definition > Point 1 1, 0, 0
Definition > Point 2 0, 1, -0.9
Definition > Point 3 0, 0, 0
Color Mode Variable
Variable Air at 25 C.Volume Fraction
Min 0
Max 0.04

3. Click Apply.
4. Observe the plane, then apply the following settings:

Tab Setting Value
Color Variable Air at 25 C.Shear Strain Rate
Min 0 [s^-1]
Max 15 [s^-1]

5. Click Apply.
Areas of high shear strain rate or shear stress are typically also areas where the highest
mixing occurs.
6. Observe the plane, then apply the following settings:

Tab Setting Value
Color Variable Pressure
Range Local

7. Click Apply.
Note that the hydrostatic contribution to pressure is excluded due to the use of an
appropriate buoyancy reference density. If you plot the variable called Absolute
Pressure, you will see the true pressure including the hydrostatic contribution.

Creating a 1. Create a new vector named Vector 1.
vector 2. Apply the following settings



Tab Setting Value
Variable Water.Velocity in Stn Frame*
*. Using this variable, instead of Water.Velocity, results in the velocity vectors
appearing to be continuous at the interface between the rotating and stationary
domains. Velocity variables that do not include a frame specification always use the
local reference frame.

3. Observe the vector plot, then change the variable to Air at 25 C.Velocity in Stn
Frame. Observe this as well, then clear the visibility of Vector 1.
4. Modify the tank Default object.

Tab Setting Value
Color Mode Variable
Variable Water.Wall Shear
Range Local

The legend for this plot shows the range of wall shear values.
The global maximum wall shear is much higher than the maximum value on the default
walls. The global maximum values occur on the TankShaft boundary directly above the
inlet. Although these values are very high, the shear force exerted on this boundary will
be small since the contact area fraction of water here is very small.

Calculating 1. Select Tools > Function Calculator from the main menu or click Show Function
Power and
Calculator from the main toolbar.
Torque
Required by the 2. Apply the following settings:
Impeller
Tab Setting Value
Function Function torque
Calculator Location Blade
Axis Global X
Fluid All Fluids

3. Click Calculate to find the torque required to rotate Blade about the X-axis.
4. Repeat the calculation setting Location to Blade Other Side.
The sum of these two results is the torque required by the single impeller blade,
approximately 70 [N m]. This must be multiplied by the number of blades in the full
geometry to obtain the total torque required by the impeller; the result is a value of
approximately 282 [N m]. You could also include the results from the locations HubShaft
and TankShaft; however in this case their contributions are negligible.


The power requirement is simply the required torque multiplied by the rotational speed
(8.8 rad/s): Power = 282*8.8 = 2482 [W].
Remember that this value is the power requirement for the work done on the fluid only, it
does not account for any mechanical losses, efficiencies etc. Also note that the accuracy of
these results is significantly affected by the coarseness of the mesh. You should not use a
mesh of this length scale to obtain accurate quantitative results.


Tutorial 16:
Gas-Liquid Flow in an Airlift
Reactor

Introduction
• Additional Fine Mesh Simulation Results (p. 280)

before beginning:
• BubbleColumn.pre
• BubbleColumnMesh.gtm


Tutorial 16: Gas-Liquid Flow in an Airlift Reactor: Tutorial 16 Features


ANSYS CFX-Pre User Mode General
Turbulence Model Dispersed Phase Zero Equation
Fluid-Dependent Turbulence
Model
k-Epsilon
Heat Transfer None
Buoyant Flow
Multiphase
Outlet (Degassing)
Symmetry Plane
Wall: Thin Surface
Wall: (Slip Depends on Volume
Fraction)
Vector
Symmetry

• Setting up a multiphase flow involving air and water
• Using a fluid dependent turbulence model to set different turbulence options for each
fluid.
• Specifying buoyant flow.
• Specifying a degassing outlet boundary condition to allow air, but not water, to escape
from the boundary.

This tutorial demonstrates the Eulerian–Eulerian multiphase model in ANSYS CFX. The
tutorial simulates a bubble column with an internal tube (draft tube) used to direct
recirculation of the flow. This configuration is known as an airlift reactor. Bubble columns are
tall gas-liquid contacting vessels and are often used in processes where gas absorption is
important (e.g., bioreactors to dissolve oxygen in broths) and to limit the exposure of
micro-organisms to excessive shear, imparted by mechanically driven mixers.


Tutorial 16: Gas-Liquid Flow in an Airlift Reactor: Defining a Simulation in ANSYS CFX-Pre
This example models the dispersion of air bubbles in water. The gas is supplied through a
sparger at the bottom of the vessel and the rising action of the bubbles provides gentle
agitation of the liquid.
Simple bubble columns that are without the draft tube tend to develop irregular flow
patterns and poor overall mixing. The draft tube in the airlift reactor helps establish a regular
flow pattern in the column and achieve better uniformity of temperature, concentration
and pH in the liquid phase, but sometimes at the expense of decreased mass transfer from
the gas to the liquid.
This tutorial also demonstrates the use of thin surfaces. Thin surfaces are internal two
dimensional wall boundaries used to model thin three dimensional features (e.g., baffles,
guide vanes within ducts, etc.).
The airlift reactor that is modeled here is very similar to the laboratory bench scale prototype
used by García-Calvo and Letón.
If you are interested, a formal analysis of this simulation involving a finer mesh is available
at the end of this tutorial. For details, see Additional Fine Mesh Simulation Results (p. 280).


then run the session file: BubbleColumn.pre. After you have played the session file as

5. Under File name, type BubbleColumn.
6. Click Save.

Importing the Mesh



Setting Value
File name BubbleColumnMesh.gtm

3. Click Open.

Creating the Domain
Simulation branch.
2. Double click Default Domain and apply the following settings:

Tab Setting Value
General Basic Settings > Location B1.P3, B2.P3
Options
Basic Settings > Fluids List Air at 25 C, Water
Domain Models > Buoyancy > Gravity Y Dirn. -9.81 [m s^-2]
Domain Models > Buoyancy > Buoy. Ref. Density* 997 [kg m^-3]
Fluid Multiphase Options > Homogeneous Model (Cleared)
Models
Multiphase Options > Allow Musig Fluids (Cleared)
Free Surface Model > Option None
Turbulence > Option Fluid Dependent
Fluid Fluid Details Air at 25 C
Details Fluid Details > Air at 25 C > Morphology > Option Dispersed Fluid
Fluid Details > Air at 25 C > Morphology > Mean Diameter 6 [mm]



Tab Setting Value
Fluid Fluid Pairs > Air at 25 C | Water > Surface Tension Coefficient (Selected)
Pairs Fluid Pairs > Air at 25 C | Water > Surface Tension Coefficient 0.072 [N m^-1]†
> Surf. Tension Coeff.
Fluid Pairs > Air at 25 C | Water > Momentum Transfer > Drag Grace
Force > Option
Fluid Pairs > Air at 25 C | Water > Momentum Transfer > Drag (Selected)
Force > Volume Fraction Correction Exponent
Fluid Pairs > Air at 25 C | Water > Momentum Transfer > Drag 2
Force > Volume Fraction Correction Exponent > Value
Fluid Pairs > Air at 25 C | Water > Momentum Transfer > Lopez de
Non-drag Forces > Turbulent Dispersion Force > Option Bertodano
Fluid Pairs > Air at 25 C | Water > Momentum Transfer > 0.3
Non-drag Forces > Turbulent Dispersion Force > Dispersion
Coeff.
Fluid Pairs > Air at 25 C | Water > Turbulence Transfer > Sato Enhanced
Option Eddy Viscosity
*. For dilute dispersed multiphase flow, always set the buoyancy reference density to
that for continuous fluid.
†. This must be set to allow the Grace drag model to be used.
3. Click OK.

For this simulation of the airlift reactor, the boundary conditions required are:
• An inlet for air on the sparger.
• A degassing outlet for air at the liquid surface.
• A thin surface wall for the draft tube.
• An exterior wall for the outer wall, base and sparger tube.
• Symmetry planes for the cross sections.

Inlet Boundary There are an infinite number of inlet velocity/volume fraction combinations that will
produce the same mass inflow of air. The combination chosen gives an air inlet velocity
close to the terminal rise velocity. Since the water inlet velocity is zero, you can adjust its
volume fraction until the required mass flow rate of air is obtained for a given air inlet
velocity.
1. Create a new boundary condition named Sparger.

Tab Setting Value
Location Sparger
Boundary Details Mass And Momentum > Option Fluid Dependent



Tab Setting Value
Boundary Conditions > Air at 25 C > Velocity 0.3 [m s^-1]
> Normal Speed
Boundary Conditions > Air at 25 C > Volume 0.25
Boundary Conditions > Water > Velocity > 0 [m s^-1]
Normal Speed
Boundary Conditions > Water > Volume 0.75
3. Click OK.

Outlet The top of the reactor will be a degassing boundary, which is classified as an outlet
Boundary boundary.
1. Create a new boundary condition named Top.

Tab Setting Value
Location Top
Boundary Details Mass and Momentum > Option Degassing Condition

3. Click OK.

Thin Surface Thin surfaces are created by specifying a wall boundary condition on both sides of an
Draft Tube internal region. If only one side has a boundary condition then the ANSYS CFX-Solver will
Boundary
fail. To assist with this, you can select only one side of a thin surface and then enable the
Create Thin Surface Partner toggle. ANSYS CFX-Pre will then try to automatically create
another boundary condition for the other side.
1. Create a new boundary condition named DraftTube.

Tab Setting Value
Location Draft Tube
Thin Surfaces > Create Thin Surface Partner (Selected)
Influence On Flow > Option
Influence On Flow > Option


3. Click OK.
A boundary condition named DraftTube Other Side will now be created automatically.

Symmetry Plane In this step you will create symmetry plane boundary conditions on the Symmetry1 and
Boundary Symmetry2 locators, one for each of the two vertical cross sections of the reactor sector.


Tab Setting Value
Location Symmetry1

3. Click OK.

Tab Setting Value
Location Symmetry2

6. Click OK.

Modifying the The remaining external regions are assigned to the default wall boundary condition. This
Default needs to be modified to set the Air phase to Free Slip.
Boundary
1. In the Outline workspace, open Default Domain Default for editing.

Tab Setting Value
Boundary Details Wall Influence on Flow > Option Fluid Dependent

3. Click OK.
The boundary condition specifications are now complete.

It often helps to set an initial velocity for a dispersed phase that is different to that of the
continuous phase. This results in a non-zero drag between the phases which can help
stability at the start of a simulation.
For some bubble column problems, improved convergence can be obtained by using CEL
(CFX Expression Language) to specify a non zero volume fraction, for air in the riser and a
zero value in the downcomer. This should be done if two solutions are possible (for example,
if the flow could go up the downcomer and down the riser).


Since a single pressure field exists for a multiphase calculation you do not set pressure
values on a per fluid basis.

Tab Setting Value
Fluid Settings Fluid Specific Initialization Air at 25 C
Fluid Specific Initialization > Air at 25 C (Selected)
Fluid Specific Initialization > Air at 25 C > Initial Automatic with Value
Option
Fluid Specific Initialization > Air at 25 C > Initial 0 [m s^-1]
Conditions > Cartesian Velocity Components > U
Fluid Specific Initialization > Air at 25 C > Initial 0.3 [m s^-1]
Conditions > Cartesian Velocity Components > V
Fluid Specific Initialization > Air at 25 C > Initial 0 [m s^-1]
Conditions > Cartesian Velocity Components > W
Fluid Specific Initialization Water*
Fluid Specific Initialization > Water (Selected)
Option
Conditions > Cartesian Velocity Components > U
Conditions > Cartesian Velocity Components > V
Conditions > Cartesian Velocity Components > W
Fluid Specific Initialization > Water > Initial Automatic
Conditions > Turbulence Kinetic Energy > Option
Conditions > Turbulence Eddy Dissipation
Fluid Specific Initialization > Water > Initial Automatic
Conditions > Turbulence Eddy Dissipation >
Option
Fluid Specific Initialization > Water > Initial 1†
*. Since there is no water entering or leaving the domain, a stationary initial guess is
recommended.
†. The volume fractions must sum to unity over all fluids. Since a value has been set for
water, the volume fraction of air will be calculated as the remaining difference, in
this case, 0.

3. Click OK.


Tutorial 16: Gas-Liquid Flow in an Airlift Reactor: Obtaining a Solution using ANSYS CFX-Solver Manager

If you are using a maximum edge length of 0.005 m or less to produce a finer mesh, use a
Target Residual of 1.0E-05 to obtain a more accurate solution.


Tab Setting Value
Convergence Control > Fluid Timescale 1 [s]

3. Click OK.


Setting Value
File name BubbleColumn.def


discretion.

The ANSYS CFX-Solver Manager will be launched after ANSYS CFX-Pre has closed down. You
will be able to obtain a solution to the CFD problem by following the instructions below.

Note: If a fine mesh is used for a formal quantitative analysis of the flow in the reactor, the
solution time will be significantly longer than for the coarse mesh. You can run the
simulation in parallel to reduce the solution time. For details, see Obtaining a Solution in
Parallel (p. 116).

2. Click Start Run.
depending on your system. Eventually a dialog box is displayed stating that the
simulation has completed.


Tutorial 16: Gas-Liquid Flow in an Airlift Reactor: Viewing the Results in ANSYS CFX-Post
of the run.

• Creating Velocity Vector Plots (p. 278)
• Viewing Volume Fractions (p. 279)
• Displaying the Entire Airlift Reactor Geometry (p. 280)

Creating Velocity Vector Plots
Because the simulation in this tutorial is conducted on a coarse grid, the results are only
suitable for a qualitative demonstration of the multiphase capability of ANSYS CFX, Release
11.0. You will first examine the distribution of velocities and fluid volume fraction by
creating the following plots. The results will then be verified to check if the values are
reasonable.
-Z.
2. Zoom in as required.
3. Turn on the visibility of SymP1.
4. Apply the following settings to SymP1.

Tab Setting Value
Color Mode Variable
Min 0
Max 0.025

5. Click Apply. Observe the volume fraction values throughout the domain.
6. Turn off the visibility of SymP1.

Tab Setting Value
Geometry Definition > Locations SymP1
Definition > Variable Water.Velocity

9. Click Apply.

Tutorial 16: Gas-Liquid Flow in an Airlift Reactor: Viewing the Results in ANSYS CFX-Post

Tab Setting Value
Geometry Definition > Locations SymP1
Definition > Variable Air at 25 C.Velocity

12. Click Apply.
13. Compare the vector fields by toggling the visibility of each and zooming in as needed.

Viewing Volume Fractions
In creating the geometry for the airlift reactor, a thin surface was used to model the draft
tube. You will next plot the volume fraction of air on the thin surface.
1. Right-click on a blank area in the viewer, and select Predefined Camera > Isometric
View (Y up).
2. Zoom in as required.
3. Turn off the visibility of any vector plots and turn on the visibility of DraftTube.
4. Modify DraftTube by applying the following settings

Tab Setting Value
Color Mode Variable
Min 0
Max 0.02

5. Click Apply.
• This boundary represents one side of the thin surface. When viewing plots on thin
surfaces, you must ensure that you are viewing the correct side of the thin surface.
• The plot just created is displaying the volume fraction for air in the downcomer
region of the airlift reactor. If you rotate the geometry you will see that the same plot
is visible from both sides of the thin surface.
• You will make use of the face culling feature whichs turns off the visibility of the plot
on one side of the thin surface. In this case, you need to turn off the “front” faces.
6. Modify DraftTube by applying the following settings

Tab Setting Value
Render Draw Faces > Face Culling Front Faces

7. Click Apply.
8. Rotate the image in the viewer to see the effect of face culling on DraftTube. You
should see that the color appears only on one side: the downcomer side.
9. Turn on the visibility of DraftTube Other Side.


Tutorial 16: Gas-Liquid Flow in an Airlift Reactor: Additional Fine Mesh Simulation Results
10. Color the DraftTube Other Side object using the same color settings as for
DraftTube.

Tab Setting Value
Color Mode Variable
Min 0
Max 0.02

11. Modify DraftTube Other Side by applying the following settings

Tab Setting Value
Render Draw Faces > Face Culling Front Faces

This will create a plot of air volume fraction on the riser side of the bubble column.
12. Click Apply.
Rotating the geometry will now show correct plots of the air volume fraction on each side
of the draft tube.
To see why face culling was needed to prevent interference between the plots on each side
of the draft tube, try turning off face culling for DraftTube and watch the effect on the riser
side (Results may vary, which is why face culling was used to prevent interference.).

Displaying the Entire Airlift Reactor Geometry
Display the entire airlift reactor geometry by expanding User Locations and Plots and
double-clicking the Default Transform object:
1. Apply the following settings to Default Transform

Tab Setting Value
Definition Instancing Info From Domain (Cleared)
# of Copies 12
Apply Rotation > Axis Y
Apply Rotation > # of Passages 12

2. Click Apply.

Additional Fine Mesh Simulation Results
A formal analysis of this airlift reactor was carried out on a finer grid (having 21000+ nodes
and a maximum edge length of 0.005 m).


The analysis showed a region of air bubble recirculation at the top of the reactor on the
downcomer side. This was confirmed by zooming in on a vector plot of
Air at 25 C.Velocity on SymP1 near the top of the downcomer. A similar plot of
Water.Velocity revealed no recirculation of the water.

Other results of the simulation:
• Due to their large 0.006 m diameter, the air bubbles quickly attained a significant
terminal slip velocity (i.e., the terminal velocity relative to water). The resulting terminal
slip velocity, obtained using the Grace drag model, is consistent with the prediction by
Maneri and Mendelson and the prediction by Baker and Chao. These correlations
predict a terminal slip velocity of about 0.23 m s-1 to 0.25 m s-1 for air bubbles of the
diameter specified.
• The values of gas hold up (the average volume fraction of air in the riser), the superficial
gas velocity (the rising velocity, relative to the reactor vessel, of gas bubbles in the riser,
multiplied by the gas holdup), and the liquid velocity in the downcomer agree with the
results reported by García-Calvo and Letón, for gas holdup values of 0.03 or less. At
higher values of gas holdup, the multifluid model does not account for pressure-volume
work transferred from gas to liquid due to isothermal expansion of the bubbles. The
simulation therefore tends to under-predict both the superficial gas velocity in the riser,
and the liquid velocity in the downcomer for gas holdup values greater than 0.03.
Note: Multiphase results files contain the vector variable Fluid.Superficial Velocity
defined as Fluid.Volume Fraction multiplied by Fluid.Velocity. This is sometimes also
referred to as the fluid volume flux. The components of this vector variable are available as
scalar variables (e.g., Fluid.Superficial Velocity X).

Many reference texts on bubble columns cite the Hughmark correlation as a standard for
gas hold up and superficial gas velocity in bubble columns. However, the Hughmark
correlation should not be used when liquid flow is concurrent with gas at velocities
exceeding 0.1 m s-1. In the airlift reactor described in this tutorial, the liquid velocity in the
riser clearly exceeds 0.2 m s-1 and the Hughmark correlation is therefore not applicable.


Tutorial 17:
Air Conditioning Simulation

Introduction

before beginning:
• HVAC.pre
• HVAC_expressions.ccl
• HVACMesh.gtm
• TStat_Control.F
Note: You must have a Fortran compiler installed on your system to perform this tutorial.


Tutorial 17: Air Conditioning Simulation: Tutorial 17 Features


Simulation Type Transient
Radiation
Buoyant Flow
Boundary Conditions Boundary Profile Visualization
Inlet (Profile)
Outlet (Subsonic)
Wall: No-Slip
Wall: Adiabatic
Wall: Fixed Temperature
Output Control
User Fortran
Timestep Transient Example
Isosurface
Point
Slice Plane
Other Auto Annotation
Changing the Color Range
Legend
MPEG Generation
Time Step Selection
Title/Text
Transient Animation

• Using the Monte Carlo radiation model with a directional source of radiation.
• Setting a monitor point to observe the temperature at a prescribed location.


Tutorial 17: Air Conditioning Simulation: Overview of the Problem to Solve

This tutorial demonstrates a simple air conditioning case in a room. The room contains
windows and an inlet vent for cooled air. The windows are set up to include heat and
radiation sources that act to raise the temperature of the room. The inlet vent introduces
cool air into the room to lower the temperature to a set level. The room also contains an
outlet vent, which removes ambient air from the room.
Roof Inlet
Windows

Outlet

This section describes the step-by-step definition of the flow physics in ANSYS CFX-Pre.

Important: You must have the required Fortran compiler installed and set in your system
path in order to run this tutorial. For details on which Fortran compiler is required for your
platform, see the applicable ANSYS, Inc. installation guide. If you are not sure which Fortran
compiler is installed on your system, try running the cfx5mkext command (found in
<CFXROOT>/bin) from the command line and read the output messages.

then run the session file: HVAC.pre.
After performing this step, you can continue from Obtaining a Solution using ANSYS
CFX-Solver Manager (p. 295).


Tutorial 17: Air Conditioning Simulation: Defining a Simulation in ANSYS CFX-Pre

5. Under File name, type HVAC.
6. Click Save.

Importing the Mesh

Setting Value
File name HVACMesh.gtm

3. Click Open.

Creating Expressions
This tutorial requires some CEL expressions. In this tutorial, a transient simulation will be
performed over 3 minutes 45 seconds with 3 second timesteps for a total of 75 timesteps.
Expressions will be used to enter these values. The expressions are also used to calculate the
inlet temperature of air under different conditions.
As the air conditioner will remove a specified amount of heat, the inlet vent temperature is
a function of the outlet vent temperature. A CEL function is used to find the outlet
temperature. A User CEL Function is used to simulate behavior of a thermostat that turns on
cold air when the temperature (measured at a particular location) is above 22 °C (295.15 K)
and turns off the cold air when the temperature falls below 20 °C (293.15 K).

Note: The expression for TSensor requires a monitor point named Thermometer to provide
room temperature feedback to the thermostat. This will be set up later.

Importing the 1. Select File > Import CCL.
Expressions 2. Select the file HVAC_expressions.ccl.
3. Click Open.
The expression for ACOn requires a User CEL Function that indicates the thermostat
output: whether the air conditioner should be on or off. This will be set up next.


Inlet Velocity Expressions are used to simulate guiding vanes at the inlet, as the following diagram shows:
Profile Figure 1 Intended airflow direction from the roof inlet vent

Roof Inlet Vent

z x=0.15 x=0.05

Wall

x

The two x locations indicated on the diagram correspond to the x values across the width of
the inlet vent. When x is 0.05, the z component of velocity will be -1 and the x component
will be zero. When x is 0.15, the x component of velocity will be 0.5 and the z component will
be -0.5. The x component of velocity varies linearly with x. The following expression can be
used to calculate the x component of velocity:

x – 0.05
XCompInlet = 0.5 × ------------------ = 5 ( x – 0.05 )
0.1 (Eqn. 1)
ZCompInlet = – 1 + XCompInlet

Setting up the Thermostat
A Fortran subroutine that simulates the thermostat has already been written for this tutorial.

Compiling the You can compile the subroutine and create the required library file used by ANSYS
Subroutine CFX-Solver at any time before running the ANSYS CFX-Solver. The operation is performed at
this point in the tutorial so that you have a better understanding of the values you need to
specify in ANSYS CFX-Pre when creating a User CEL Function. The cfx5mkext command is
used to compile the subroutine as described below.

Important: You must have the required Fortran compiler installed and set in your system
path in order to run the cfx5mkext command successfully. For details on which Fortran
compiler is required for your platform, see the applicable ANSYS, Inc. installation guide. If
you are not sure which Fortran compiler is installed on your system, try running the
cfx5mkext command (found in <CFXROOT>/bin) from the command line and read the
output messages.
1. Copy the subroutine TStat_Control.F to your working directory (if you have not
already done so).
2. Examine the contents of this file in any text editor to gain a better understanding of this
subroutine.
This file was created by modifying the ucf_template.F file, which is available in the


3. Select Tools > Command Editor.
4. Type the following command in the Command Editor dialog box (make sure you do
not miss the semi-colon at the end of the line):
! system (“cfx5mkext TStat_Control.F”) < 1 or die “cfx5mkext failed”;
• This is equivalent to executing the following at an OS command prompt:
cfx5mkext TStat_Control.F
• The ! indicates that the following line is to be interpreted as power syntax and not
CCL. Everything after the ! symbol is processed as Perl commands.
• system is a Perl function to execute a system command.
• The < 1 or die will cause an error message to be returned if, for some reason, there
is an error in processing the command.
5. Click Process to compile the subroutine.
Note: You can use the -double option (i.e., cfx5mkext -double TStat_Control.F) to
compile the subroutine for use with double precision ANSYS CFX-Solver executables.

A subdirectory will have been created in your working directory whose name is system
dependent (e.g., on IRIX it is named irix). This sub directory contains the shared object
library.

Note: If you are running problems in parallel over multiple platforms then you will need to
create these subdirectories using the cfx5mkext command for each different platform.

• You can view more details about the cfx5mkext command by running
cfx5mkext -help.
• You can set a Library Name and Library Path using the -name and -dest options
respectively.
• If these are not specified, the default Library Name is that of your Fortran file and the
default Library Path is your current working directory.
1. Close the Command Editor dialog box.

Creating the A User CEL Function is required to link the subroutine into ANSYS CFX. The complete
User CEL definition for the function is defined in two steps. First, a user routine that contains the
Function
calling name, library name, and library path is created. Then, a user function that points to
the user routine, and also contains the argument and result units, is defined.
1. From the main menu, select Insert > Expressions, Functions and Variables > User
Routine or click User Routine .
2. Set the name to Thermostat Routine.

Tab Setting Value
Basic Settings Option User CEL Function
Calling Name ac_on*
Library Name‘ TStat_Control†
Library Path (Working Directory)‡



*. This is the name of the subroutine within the Fortran file. Always use lower case
letters for the calling name, even if the subroutine name in the Fortran file is in
upper case.
†. This is the name passed to the cfx5mkext command by the -name option. If the
-name option is not specified, a default is used. The default is the Fortran file name
without the .F extension.
‡. Set this to your working directory.
4. Click OK.
5. Create a new user function named Thermostat Function by selecting Insert >
Expressions, Functions and Variables > User Function from the main menu.

Tab Setting Value
Basic Settings Option User Function
Argument Units [K], [K], [K], []*
Result Units []†
*. These are the units for the four input arguments: TSensor, TSet, TTol, and aitern.
†. The result will be a dimensionless integer flag of values 1 or 0.

7. Click OK.
The function you have just prepared is called during the evaluation of the expression for
ACOn (that you imported earlier). The expression is:
Thermostat Function(TSensor,TSet,TTol,aitern)
It evaluates to 1 or 0, depending on whether the air conditioner should be on (1) or off
(0).

Setting the Simulation Type


Tab Setting Value
Simulation Type > Time Duration > Total Time tTotal
Simulation Type > Time Steps > Timesteps tStep

3. Click OK.

Creating the Domain
Simulation branch.
2. Double click Default Domain and apply the following settings:



Tab Setting Value
General Basic Settings > Location B1.P3
Options
Fluids List Air Ideal Gas
Domain Models > Buoyancy > Gravity Y Dirn. 0 [m s^-2]
Domain Models > Buoyancy > Gravity Z Dirn. -g
Domain Models > Buoyancy > Buoy. Ref. Density 1.2 [kg m^-3]
Thermal Radiation Model > Option Monte Carlo

3. Click OK.

Setting Boundary Conditions
In this section you will define the locations and values of the boundary conditions.


Tab Setting Value
Location Inlet
Boundary Details Mass and Momentum > Option Mass Flow Rate
Mass and Momentum > Mass Flow Rate MassFlow
Flow Direction > Option Cartesian Components
Flow Direction > X Component XCompInlet
Flow Direction > Y Component 0
Flow Direction > Z Component ZCompInlet
Heat Transfer > Static Temperature TIn
Plot Options Boundary Vector (Selected)

3. Click OK.
Note: Ignore the physics errors that appear. They will be fixed by setting up the rest of the
simulation. The error you see is due to a reference to Thermometer which has not been set
up yet. This will be done as part of the output control.

Outlet 1. Create a new boundary condition named VentOut.



Tab Setting Value
Location VentOut
Boundary Details Mass and Momentum > Relative Pressure 0 [Pa]

3. Click OK.

Window To model incoming radiation at the window boundaries, a directional radiation source will
Boundary be created. The windows will also contribute heat to the room via a fixed temperature of
26 [C].
1. Create a new boundary condition named Windows.

Tab Setting Value
Settings Location Window1, Window2


Tab Setting Value
Sources Boundary Source (Selected)
Boundary Source > Sources (Selected)

4. Create a new radiation source item by clicking Add New Item and accepting the
default name.
5. Apply the following settings to Radiation Source 1

Setting Value
Option Directional Radiation Flux
Radiation Flux 600 [W m^-2]
Direction > Option Cartesian Components
Direction > X Component 0.33
Direction > Y Component 0.33
Direction > Z Component -0.33


Tab Setting Value
Plot Boundary Vector (Selected)
Options


7. Click OK.
The directional source of radiation is displayed.

Default Wall The default boundary condition for any undefined surface in ANSYS CFX-Pre is a no-slip,
Boundary smooth, adiabatic wall. For radiation purposes, the default wall is assumed to be a perfectly
absorbing and emitting surface (emissivity = 1), and this will be preserved when setting up
the boundary condition.
In this tutorial, a fixed temperature of 26 °C will be assumed to exist at the wall during the
simulation. A more detailed analysis would model heat transfer through the walls, but as
this tutorial is designed only for demonstration purposes, a fixed temperature wall is
sufficient.
1. Modify the boundary condition named Default Domain Default.

Tab Setting Value

3. Click OK.
This setting will include the Door region, which will be modeled as a wall (closed door) for
simplicity. Since the region is part of the entire default boundary, it will not appear in the
wireframe when the results file is opened in ANSYS CFX-Post (but can still be viewed in the
Regions list).




Tab Setting Value
Global Settings Initial Conditions > Velocity Type Cartesian
Initial Conditions > Cartesian Velocity Automatic with Value
Components > Option
Components > U
Components > V
Components > W
Initial Conditions > Static Pressure > Relative 0 [Pa]
Pressure
Initial Conditions > Temperature > Temperature 22 [C]
Initial Conditions > Turbulence Kinetic Energy > (Selected)
Fractional Intensity
> Eddy Length Scale
Initial Conditions > Turbulence Eddy Dissipation 0.25 [m]
> Eddy Length Scale > Eddy Len. Scale
Initial Conditions > Radiation Intensity > (Selected)
Blackbody Temperature
Initial Conditions > Radiation Intensity > 22 [C]
Blackbody Temperature > Blackbody Temp.

3. Click OK.


Tab Setting Value
Basic Settings Transient Scheme > Option Second Order Backward
Euler
Convergence Control > Max. Coeff. Loops 3

3. Click OK.

Transient results files will be set up to record transient values of a chosen set of variables.
Monitor points will be created to show the on/off status of the air conditioner, the
temperature at the inlet, the temperature at the outlet, and the temperature at a prescribed
thermometer location.



2. Click Trn Results.

3. Create a new Transient Results item by clicking Add New Item and accept the the
default name.

Setting Value
Output Variables List Pressure, Radiation Intensity, Temperature,
Velocity
Output Variables Operators (Selected)
Output Variables Operators > Output Var. All*
Operators
Output Frequency > Time Interval tStep
*. This causes the gradients of the selected variables to be written to the transient
files, along with other information.


Tab Setting Value
Monitor Monitor Options (Selected)

6. Create a new Monitor Points and Expressions item named Temp at Inlet.
7. Apply the following settings to Temp at Inlet

Setting Value
Option Expression
Expression Value TIn

8. Create a new Monitor Points and Expressions item named Thermometer.
9. Apply the following settings to Thermometer

Setting Value
Output Variable List Temperature
Cartesian Coordinates 2.95, 1.5, 1.25

10. Create a new Monitor Points and Expressions item named Temp at VentOut.
11. Apply the following settings to Temp at VentOut

Setting Value
Option Expression
Expression Value TVentOut


Tutorial 17: Air Conditioning Simulation: Obtaining a Solution using ANSYS CFX-Solver Manager
12. Create a new Monitor Points and Expressions item named ACOnStatus.
13. Apply the following settings to ACOnStatus

Setting Value
Option Expression
Expression Value ACOn

14. Click OK.


Setting Value
File name HVAC.def


discretion.

When ANSYS CFX-Pre has shut down and the ANSYS CFX-Solver Manager has started, obtain
a solution to the CFD problem by following the instructions below.
1. Click Start Run.
2. When the User Points tab appears, click it to view the value of the temperature at
VentOut as the solution progresses.
of the run.

The temperature of air in the house is distributed in both space and time. While the transient
behavior of the temperature field can easily be shown with an animation, it is not easy to
visualize a complicated 3D distribution. In order to show the key features of the temperature
field, graphic objects will be produced on strategically-placed locators; Plane locators will
be used to show contour plots of temperature, while Isosurfaces will be used sparingly to
show the general shape of thermal plumes.


Tutorial 17: Air Conditioning Simulation: Viewing the Results in ANSYS CFX-Post

Creating Graphics Objects
Plane locators will be placed vertically through the vents and horizontally above the floor.

Plane Locators 1. Load the res file (HVAC_001.res) if you did not elect to load the results directly from the
ANSYS CFX-Solver Manager.
2. Right-click a blank area in the viewer, select Predefined Camera > Isometric View (Z
up).
3. Create a ZX-Plane named Plane 1 with Y=1.5 [m]. Color it by Temperature using a
user specified range from 19 [C] to 23 [C], and clear Lighting.
4. Create an XY Plane named Plane 2 with Z=0.35 [m]. Color it using the same settings
as for the first plane, and clear Lighting.

Isosurface 1. Click Timestep Selector .
Locator The Timestep Selector appears.
2. Double-click the value (12s) in the Timestep Selector.
The Timestep is set to 12s so that the cold plume is visible.
3. Create an isosurface named Cold Plume which is a surface of Temperature=19 [C].
Use conservative values for Temperature.
4. Color the isosurface by Temperature and use the same range as for the planes.
Although the color of the isosurface will not show variation (by definition), it will be
consistent with the other graphic objects.
5. On the Render tab for the isosurface, set Transparency to 0.5, and clear Lighting.
6. Click Apply.
Note: The isosurface will not be visible in some timesteps, but you will be able to see it when
playing the animation (a step carried out later).

Adjusting the The legend title should not name the locator of any particular object since all objects are
Legend colored by the same variable and use the same range.
1. In the tree view, double-click Default Legend View 1.
2. In the Definition tab, change Title Mode to Variable.
This will remove the locator name from the legend.
3. Click the Appearance tab, then:
a. Change Precision to 2, Fixed.
b. Change Text Height to 0.03.
4. Click Apply.
A label will be used to show the simulation time and the temperature of the thermometer
which controls the thermostat. This will be especially useful for the animation which is
created later in this tutorial.


Before creating the label, you will need to support the expression for TSensor by creating a
point called Thermometer at the location of the sensor thermometer. This point will replace
the monitor point called Thermometer which was used during the solver run, but no longer
exists.

Note: The actual thermometer data generated during the run was stored in the results file,
but is not easily accessible, and cannot currently be used in an auto-annotation label.

Creating a Point 1. From the main menu, select Insert > Location > Point.
for the 2. Set Name to Thermometer.
Thermometer
3. Set Point to (2.95,1.5,1.25).
4. Click Apply.
Now the expression TSensor will once again measure temperature at the prescribed
location.

Creating the 1. Click Text .
Text Label 2. Accept the default name and click OK.
3. Set Text String to Time Elapsed
The full text string should now be Time Elapsed: <aa>. The <aa> represents the
location where the auto annotation will be substituted.
5. Set Type to Time Value.
This will show the amount of simulated time that has passed in the simulation.
6. Click More.
This adds a second line of text to the text object.
7. Set Text String to Sensor Temperature:
9. Set Type to Expression.
10. Set Expression to TSensor.
11. Click the Appearance tab, change Height to 0.03, then click Apply.
Ensure the visibility check box next to Text 1 is selected. A label appears at the top of
the figure. The large font is used so that the text will be clearly visible in the animation
which will be produced in the next section.

Creating an Animation
1. Ensure that the view is set to Isometric View (Z up).

The Timestep Selector appears.
3. Double-click the first time value (0 s) in the Timestep Selector.

4. Click Animation found in the toolbar.
The Animation dialog box appears.
5. In the Animation dialog box:



a. Click New to create KeyframeNo1.
b. Highlight KeyframeNo1, change # of Frames to 200, then press <Enter> while in
the # of Frames box.
Tip: Be sure to press <Enter> and confirm that the new number appears in the list before
continuing.
This will place 200 intermediate frames between the first and (yet to be created)
second key frames, for a total of 202 frames. This will produce an animation lasting
about 8.8 s since the frame rate will be 24 frames per second. Since there are 76
unique frames, each frame will be shown at least once.
6. Load the last time value (225 s) using the Timestep Selector dialog box.
7. In the Animation dialog box:

a. Click New to create KeyframeNo2.
The # of Frames parameter has no effect for the last keyframe, so leave it at the
default value.
b. Click More Animation Options to expand the Animation dialog box.
c. Select Save MPEG.
d. Specify a file name for the MPEG file.
e. Click the Options button.
f. Change MPEG Size to 720 x 480 (or a similar resolution).
g. Click the Advanced tab, and note the Quality setting.
If your MPEG player does not play the MPEG, you can try using the Low or Custom
quality settings.
h. Click OK.
i. Click To Beginning to rewind the active key frame to KeyframeNo1.

j. Click Save animation state and save the animation to a file. This will enable you
to quickly restore the animation in case you want to make changes. Animations are
not restored by loading ordinary state files (those with the .cst extension).

9. If prompted to overwrite an existing movie, click Overwrite.
The animation plays and builds an .mpg file.

Further Steps 1. This tutorial uses an aggressive value for the flow rate of air, a coarse mesh, and the
timesteps are too large for a satisfactory analysis. Running this tutorial with a finer mesh,
a flow rate of air that is closer to 5 changes of air per hour (0.03 m3 s-1), and smaller
timesteps will produce more accurate results.
2. Running the simulation for a longer total time period will allow you to see more on/off
cycles of the thermostat.


Tutorial 18:
Combustion and Radiation in a
Can Combustor

Introduction
• Using Eddy Dissipation and P1 Models (p. 301)
• Laminar Flamelet and Discrete Transfer Models (p. 311)
• Further Postprocessing (p. 316)

before beginning:
• CombustorMesh.gtm
• CombustorEDM.pre
• CombustorFlamelet.pre
• CombustorEDM.cfx


Tutorial 18: Combustion and Radiation in a Can Combustor: Tutorial 18 Features


Fluid Type Reacting Mixture
Combustion
Radiation
Outlet (Subsonic)
Wall: No-Slip
Wall: Adiabatic
Wall: Thin Surface
ANSYS CFX-Post Plots Outline Plot (Wireframe)
Sampling Plane
Slice Plane
Vector
Color map
Legend

• Creating thin surfaces for the inlet vanes.
• Using a Reacting Mixture.
• Using the Eddy Dissipation Combustion Model.
• Using the Flamelet Model.
• Changing the Combustion model in a simulation.
• Using the P1 Radiation Model in ANSYS CFX-Pre.
• Using the Discrete Transfer Radiation Model in ANSYS CFX-Pre.
• Using the NOx model in ANSYS CFX-Pre.
• Changing object color maps in ANSYS CFX-Post to prepare a greyscale image.


Tutorial 18: Combustion and Radiation in a Can Combustor: Overview of the Problem to Solve

The can combustor is a feature of the gas turbine engine. Arranged around a central
annulus, can combustors are designed to minimize emissions, burn very efficiently and keep
wall temperatures as low as possible. This tutorial is designed to give a qualitative
impression of the flow and temperature distributions. The basic geometry is shown below
with a section of the outer wall cut away.

The Outlet has a surface
area of 150 cm2.

There are six side air
inlets, each with a
surface area of
2 cm2.

There are six small fuel
inlets, each with a
surface area of 0.14 cm2.

Main air inlet. The inlet
is guided by vanes to
give the air a swirling
velocity component.
Total surface area is
57 cm2.

Using Eddy Dissipation and P1 Models
This tutorial demonstrates two different combustion and radiation model combinations.
The first uses the Eddy Dissipation Combustion model with the P1 Radiation model; the NOx
model is also included. The second uses the Laminar Flamelet model with the Discrete
Transfer Radiation model. If you wish to use the Flamelet Combustion model and Discrete
Transfer Radiation model, see Laminar Flamelet and Discrete Transfer Models (p. 311),
otherwise continue from this point.


Tutorial 18: Combustion and Radiation in a Can Combustor: Defining a Simulation in ANSYS CFX-Pre

You will define a domain that includes a variable composition mixture. These mixtures are
used to model combusting and reacting flows in ANSYS CFX.

then run the session file: CombustorEDM.pre. After you have played the session file as

5. Under File name, type CombustorEDM.
6. Click Save.

Importing the Mesh

Setting Value
File name CombustorMesh.gtm

3. Click Open.

Creating a Reacting Mixture
To allow combustion modeling, you must create a variable composition mixture.

To create the 1. Create a new material named Methane Air Mixture.
variable 2. Apply the following settings
composition
mixture
Tab Setting Value
Basic Settings Option Reacting Mixture
Material Group Gas Phase Combustion
Reactions List Methane Air WD1 NO PDF*



Tab Setting Value
Mixture Mixture Properties (Selected)
Properties Mixture Properties > Radiation Properties > (Selected)†
Refractive Index
Mixture Properties > Radiation Properties > (Selected)
Absorption Coefficient
Mixture Properties > Radiation Properties > (Selected)
Scattering Coefficient
*. The Methane Air WD1 NO PDF reaction specifies complete combustion of the fuel
into its products in a single-step reaction. The formation of NO is also modeled and
occurs in an additional reaction step.

Click to display the Reactions List dialog box, then click Import Library Data

and select the appropriate reaction to import.
†. Setting the radiation properties explicitly will significantly shorten the solution time
since the ANSYS CFX-Solver will not have to calculate radiation mixture properties.
3. Click OK.

Creating the Domain
Simulation branch.

Tab Setting Value
General Basic Settings > Locations B152, B153, B154,
Options B155, B156
Basic Settings > Fluids List Methane Air Mixture
Domain Models > Pressure > Reference Pressure 1 [atm]*
Reaction or Combustion > Option Eddy Dissipation
Reaction or Combustion > Eddy Dissipation Model (Selected)
Coefficient B
Reaction or Combustion > Eddy Dissipation Model 0.5†
Coefficient B > EDM Coeff. B
Thermal Radiation Model > Option P1
Component Details > N2 (Selected)
Component Details > N2 > Option Constraint
*. It is important to set a realistic reference pressure in this tutorial because the
components of Methane Air Mixture are ideal gases.
†. This includes a simple model for partial premixing effects by turning on the Product
Limiter. When it is selected, non-zero initial values are required for the products. The
products limiter is not recommended for multi-step eddy dissipation reactions, and
so is set for this single step reaction only.

3. Click OK.



Fuel Inlet 1. Create a new boundary condition named fuelin.

Tab Setting Value
Location fuelin
Component Details CH4
Component Details > CH4 > Mass Fraction 1

3. Click OK.

Bottom Air Inlet Two separate boundary conditions will be applied for the incoming air. The first is at the
Boundary base of the can combustor. The can combustor employs vanes downstream of the fuel inlet
to give the incoming air a swirling velocity.
1. Create a new boundary condition named airin.

Tab Setting Value
Location airin
Component Details O2
Component Details > O2 > Mass Fraction 0.232*
*. The remaining mass fraction at the inlet will be made up from the constraint
component, N2.

3. Click OK.

Side Air Inlet The secondary air inlets are located on the side of the vessel and introduce extra air to aid
Boundary combustion.
1. Create a new boundary condition named secairin.

Tab Setting Value
Location secairin



Tab Setting Value
Boundary Details Mass and Momentum > Option Normal Speed
Mass and Momentum > Normal Speed 6 [m s^-1]
Component Details O2
Component Details > O2 > Mass Fraction 0.232*
*. The remaining mass fraction at the inlet will be made up from the constraint
component, N2.
3. Click OK.

Outlet 1. Create a new boundary condition named out.

Tab Setting Value
Location out
Boundary Details Mass and Momentum > Option Average Static Pressure

3. Click OK.

Vanes Boundary The vanes above the main air inlet are to be modeled as thin surfaces. To create a vane as a
thin surface in ANSYS CFX-Pre, you must specify a wall boundary condition on each side of
the vanes. The Create Thin Surface Partner feature in ANSYS CFX-Pre will automatically
match the other side of a thin surface if you pick just a single side.
You will first create a new region which contains one side of each of the eight vanes, then
use the Create Thin Surface Partner feature to match the other side.
1. Create a new composite region named Vane Surfaces.

Tab Setting Value
Basic Settings Dimension (Filter) 2D*
Region List F129.152, F132.152, F136.152,
F138.152, F141.152, F145.152,
F147.152, F150.152
*. This will filter out the 3D regions, leaving only 2D regions

3. Click OK.
4. Create a new boundary condition named vanes.



Tab Setting Value
Location Vane Surfaces
Create Thin Surface Partner (Selected)*
*. This feature will attempt to match all primitives specified in the location list to
create a thin surface boundary condition.

6. Click OK.

Default Wall The default boundary condition for any undefined surface in ANSYS CFX-Pre is a no-slip,
Boundary smooth, adiabatic wall.
• For radiation purposes, the wall is assumed to be a perfectly absorbing and emitting
surface (emissivity = 1).
• The wall is non-catalytic, i.e., it does not take part in the reaction.
Since this tutorial serves as a basic model, heat transfer through the wall is neglected. As a
result, no further boundary conditions need to be defined.


Tab Setting Value
Settings Option
Initial Conditions > Turbulence Eddy Dissipation > Automatic
Option
Initial Conditions > Component Details O2
Initial Conditions > Component Details > O2> Option Automatic with Value
Initial Conditions > Component Details > O2 > Mass 0.232*
Fraction
Initial Conditions > Component Details CO2
Initial Conditions > Component Details > CO2 > Option Automatic with Value
Initial Conditions > Component Details > CO2 > Mass 0.01
Fraction
Initial Conditions > Component Details H2O
Initial Conditions > Component Details> H2O > Option Automatic with Value
Initial Conditions > Component Details > H2O > Mass 0.01
Fraction


Tutorial 18: Combustion and Radiation in a Can Combustor: Obtaining a Solution using ANSYS CFX-Solver Manager

*. The initial conditions assume the domain consists mainly of air and the fraction of
oxygen in air is 0.232. A small mass fraction of reaction products (CO2 and H2O) is
needed for the EDM model to initiate combustion.
3. Click OK.


Tab Setting Value
Timescale Control
Convergence Control > Fluid Timescale Control > 0.025 [s]
Physical Timescale

3. Click OK.


Setting Value
File name CombustorEDM.def


4. If using Standalone Mode, quit ANSYS CFX-Pre, saving the simulation (.cfx) file.

The ANSYS CFX-Solver Manager will be launched after ANSYS CFX-Pre saves the definition
file. You will be able to obtain a solution to the CFD problem by following the instructions
below.

Note: If a fine mesh is used for a formal quantitative analysis of the flow in the combustor,
the solution time will be significantly longer than for the coarse mesh. You can run the
simulation in parallel to reduce the solution time. For details, see Obtaining a Solution in
Parallel (p. 116).

Definition File should be set to CombustorEDM.def.


Tutorial 18: Combustion and Radiation in a Can Combustor: Viewing the Results in ANSYS CFX-Post
2. Click Start Run.
depending on your system. Eventually a dialog box is displayed stating that the run has
finished.

When ANSYS CFX-Post opens, experiment with the Edge Angle setting for the Wireframe
object and the various rotation and zoom features in order to place the geometry in a
sensible position. A setting of about 8.25 should result in a detailed enough geometry for
this exercise.

Temperature Within the Domain

Tab Setting Value
Color Mode Variable
Mode > Variable Temperature

3. Click Apply.
The large area of high temperature through most of the vessel is due to forced convection.

Note: Later in this tutorial (see Laminar Flamelet and Discrete Transfer Models (p. 311)), the
Laminar Flamelet combustion model will be used to simulate the combustion again,
resulting in an even higher concentration of high temperatures throughout the combustor.

The NO Concentration in the Combustor
In the next step you will color Plane 1 by the mass fraction of NO to view the distribution
of NO within the domain. The NO concentration is highest in the high temperature region
close to the outlet of the domain.
1. Modify the plane named Plane 1.

Tab Setting Value
Color Mode > Variable NO.Mass Fraction

3. Click Apply.



Printing a Greyscale Graphic
Here you will change the color map (for Plane 1) to a greyscale map. The result will be a
plot with different levels of grey representing different mass fractions of NO. This technique
is especially useful for printing, to a black and white printer, any image that contains a color
map. Conversion to greyscale by conventional means (i.e., using graphics software, or
letting the printer do the conversion) will generally cause color legends to change to a
non-linear distribution of levels of grey.

Tab Setting Value
Color Color Map Inverse Greyscale

3. Click Apply.

Calculating NO Mass Fraction at the Outlet
The emission of pollutants into the atmosphere is always a design consideration for
combustion applications. In the next step, you will calculate the mass fraction of NO in the
outlet stream.
1. Select Tools > Function Calculator or click the Tools tab and select Function
Calculator.

Tab Setting Value
Function Function massFlowAve
Calculator Location out
Variable NO.Mass Fraction

3. Click Calculate.
A small amount of NO is released from the outlet of the combustor. This amount is lower
than can normally be expected, and is mainly due to the coarse mesh and the short
residence times in the combustor.

Viewing Flow Field
To investigate the reasons behind the efficiency of the combustion process, you will next
look at the velocity vectors to show the flow field. You may notice a small recirculation in the
center of the combustor. Running the problem with a finer mesh would show this region to
be a larger recirculation zone. The coarseness of the mesh in this tutorial means that this
region of flow is not accurately resolved.
1. Select the Outline tab.
2. Under User Locations and Plots, clear Plane 1.
Plane 1 is no longer visible.



Tab Setting Value

5. Click Apply.

Tab Setting Value
Definition > Z 0.03
Plane Type > Sample (Selected)
Plane Type > X Samples 30
Plane Type > Y Samples 30

8. Click Apply.
9. Modify Vector 1.

Tab Setting Value

11. Click Apply.
To view the swirling velocity field, right-click in the viewer and select Predefined Camera >
View Towards -Z.
You may also want to turn off the wireframe visibility. In the region near the fuel and air
inlets, the swirl component of momentum (theta direction) results in increased mixing with
the surrounding fluid and a higher residence time in this region. As a result, more fuel is
burned.

Viewing Radiation
Try examining the distribution of Incident Radiation and Radiation Intensity
throughout the domain.
When you are finished, quit ANSYS CFX-Post.


Tutorial 18: Combustion and Radiation in a Can Combustor: Laminar Flamelet and Discrete Transfer Models

Laminar Flamelet and Discrete Transfer Models
In this second part of the tutorial, you will start with the simulation from the first part of the
tutorial and modify it to use the Laminar Flamelet combustion and Discrete Transfer
radiation models. Running the simulation a second time will demonstrate the differences in
the combustion models, including the variance in carbon dioxide distribution, which is
shown below.

then run the session file: CombustorFlamelet.pre. After you have played the session file as
Manager (p. 87), proceed to Obtaining a Solution (p. 314).

1. If you have not completed the first part of this tutorial, or otherwise do not have the
simulation file from the first part, start ANSYS CFX-Pre and then play the session file
CombustorEDM.pre. The simulation file CombustorEDM.cfx will be created.
2. Start ANSYS CFX-Pre (unless it is already running).
3. Select File > Open Simulation.
4. Load the simulation named CombustorEDM.cfx.
The simulation from the first part of this tutorial is loaded.


6. Save the simulation as CombustorFlamelet.cfx.
This creates a separate simulation file which will be modified to use the Laminar
Flamelet and Discrete Transfer models.

Modifying the Reacting Mixture
A flamelet library will be used to create the variable composition mixture.
1. Expand Materials and open Methane Air Mixture for editing.

Tab Setting Value
Basic Settings Reactions List Methane Air FLL STP and NO PDF*

*. Click to display the Reactions List dialog box, then click Import Library Data

and select the appropriate reaction to import.

3. Click OK.
Note: Some physics validation messages appear after this reaction is selected. In this
situation, the messages can be safely ignored as the physics will be corrected once the
domains and boundary conditions are modified.

Modifying the Domain
1. Double-click the Default Domain.

Tab Setting Value
Fluid Models Reaction or Combustion > Option PDF Flamelet
Thermal Radiation Model > Option Discrete Transfer
Component Details N2
Component Details > N2 > Option Constraint
Component Details NO
Component Details > NO > Option Transport Equation
Component Details (All other components)*
Component Details > (All other components) Automatic
> Option
*. Select these one at a time and check each of them.

3. Click OK.

Modifying the Boundary Conditions
Fuel Inlet 1. Modify the boundary condition named fuelin.



Tab Setting Value
Boundary Details Mixture > Option Fuel
Component Details > NO > Option Mass Fraction
Component Details > NO > Mass Fraction 0

3. Click OK.

Bottom Air Inlet 1. Modify the boundary condition named airin.

Tab Setting Value
Boundary Details Mixture > Option Oxidiser

3. Click OK.

Side Air Inlet 1. Modify the boundary condition named secairin.

Tab Setting Value
Boundary Details Mixture > Option Oxidiser

3. Click OK.


Tab Setting Value
Global Initial Conditions > Component Details NO
Settings
Initial Conditions > Component Details > NO > Option Automatic with Value
Initial Conditions > Component Details > NO > Mass 0
Fraction

3. Click OK.



To reduce the amount of CPU time required for solving the radiation equations, you can
select to solve them only every 10 iterations.


Tab Setting Value
Advanced Dynamic Model Control > Global Dynamic Model Control (Selected)
Options
Thermal Radiation Control (Selected)
Thermal Radiation Control > Iteration Interval (Selected)
Thermal Radiation Control > Iteration Interval > Iteration 10
Interval

3. Click OK.


Setting Value
File name CombustorFlamelet.def


discretion.

Obtaining a Solution
When ANSYS CFX-Pre has shut down and the ANSYS CFX-Solver Manager has started, obtain
a solution to the CFD problem by following the instructions below.
Definition File should be set to CombustorFlamelet.def.
2. Click Start Run.



Viewing the Results
Viewing 1. Create a new plane named Plane 1.
Temperature
within the Note: If ANSYS CFX-Post was not closed since CombustorEDM.def was processed, all
Domain meshes and locators from that session will be retained and updated when the
CombustorFlamelet.def is opened. In this way Plane 1 does not need to be remade.


Tab Setting Value
Definition > Y 0
Color Mode Variable
Mode > Variable Temperature

3. Click Apply.

Viewing the NO 1. Modify the plane named Plane 1.
concentration in 2. Apply the following settings
the Combustor

Tab Setting Value
Color Mode > Variable NO.Mass Fraction

3. Click Apply.

Calculating NO The next calculation shows the amount of NO at the outlet.
Concentration
Calculator.

Tab Setting Value
Calculator Location out
Variable NO.Mass Fraction

3. Click Calculate.

Viewing CO The next plot will show the concentration of CO (carbon monoxide), which is a by-product
Concentration of incomplete combustion and is poisonous in significant concentrations. As you will see,
the highest values are very close to the fuel inlet and in the regions of highest temperature.


Tutorial 18: Combustion and Radiation in a Can Combustor: Further Postprocessing

Tab Setting Value
Color Mode > Variable CO.Mass Fraction
Range Local

3. Click Apply.

Calculating CO In the next step, you will calculate the mass fraction of CO in the outlet stream.
Mass Fraction at
the Outlet
Calculator.

Tab Setting Value
Calculator
Location out
Variable CO.Mass Fraction

3. Click Calculate.
There is approximately 0.4% CO by mass in the outlet stream.

Further Postprocessing
1. Try putting some plots of your choice into the Viewer. You can plot the concentration of
other species and compare values to those found for the Eddy Dissipation model.
2. Examine the distribution of Incident Radiation and Radiation Intensity
throughout the domain.
3. Load one combustion model, then load the other using the Add to current results
option in the Load Results File dialog box. You can compare both models in the viewer
at once, in terms of mass fractions of various materials, as well as total temperature and
other relevant measurements.


Tutorial 19:
Cavitation Around a Hydrofoil

Introduction
• Creating an Initial Simulation (p. 319)
• Obtaining an Initial Solution using ANSYS CFX-Solver Manager (p. 323)
• Viewing the Results of the Initial Simulation (p. 324)
• Preparing a Simulation with Cavitation (p. 326)
• Obtaining a Cavitation Solution using ANSYS CFX-Solver Manager (p. 328)
• Viewing the Results of the Cavitation Simulation (p. 328)

before beginning:
• HydrofoilExperimentalCp.csv
• HydrofoilGrid.def
• HydrofoilIni.pre
• Hydrofoil.pre
• HydrofoilIni_001.res


Tutorial 19: Cavitation Around a Hydrofoil: Tutorial 19 Features


Multiphase
Outlet (Subsonic)
Symmetry Plane
Wall: No-Slip
Wall: Free-Slip
ANSYS CFX-Solver Manager Restart
Line Locator
Polyline
Slice Plane
Streamline
Vector
Data Export
Printing
Title/Text
Variable Details View

• Modeling flow with cavitation.
• Using vector reduction in ANSYS CFX-Post to clarify a vector plot with many arrows.
• Importing and exporting data along a polyline.
• Plotting computed and experimental results.


Tutorial 19: Cavitation Around a Hydrofoil: Overview of the Problem to Solve

This example demonstrates cavitation in the flow of water around a hydrofoil. A
two-dimensional solution is obtained by modeling a thin slice of the hydrofoil and using
two symmetry boundary conditions.
cavitation zone

16.91 m s^-1

In this tutorial, an initial solution with no cavitation is generated to provide an accurate
initial guess for a full cavitation solution, which is generated afterwards.

Creating an Initial Simulation
This section describes the step-by-step definition of the flow physics in ANSYS CFX-Pre.

then run the session file: HydrofoilIni.pre. After you have played the session file as
Manager (p. 87), proceed to Obtaining an Initial Solution using ANSYS CFX-Solver Manager
(p. 323).

Defining the Simulation
5. Under File name, type HydrofoilIni.
6. Click Save.

Importing the Mesh


Tutorial 19: Cavitation Around a Hydrofoil: Creating an Initial Simulation

Setting Value
File type CFX-Solver (*.def, *.ref, *.trn, *.bak)
File name HydrofoilGrid.def

3. Click Open.
-Z.

Loading Materials
Since this tutorial uses Water Vapour at 25 C and Water at 25 C you need to load these
materials.
1. In the Outline tree view, right-click Materials and select Import Library Data.
The Select Library Data to Import dialog box is displayed.
2. Expand Water Data.
3. Select both Water Vapour at 25 C and Water at 25 C by holding <Crtl> when
selecting.
4. Click OK.

Creating the Domain
The fluid domain used for this simulation contains liquid water and water vapour. The
volume fractions are initially set so that the domain is filled entirely with liquid.
Simulation branch.

Tab Setting Value
General Basic Settings > Fluids List * Water at 25 C, Water
Options Vapour at 25 C
Fluid Models Multiphase Options > Homogeneous Model (Selected)
Turbulence > Option k-Epsilon
*. These two fluids have consistent reference enthalpies.

3. Click OK.

The simulation requires inlet, outlet, wall and symmetry plane boundary conditions. The
regions for these boundary conditions were imported with the grid file.



Tab Setting Value
Location IN
Fluid Values Boundary Conditions Water at 25 C
Boundary Conditions > Water at 25 C> 1
Boundary Conditions Water Vapour at 25 C
Boundary Conditions > Water Vapour at 25 C > 0

3. Click OK.


Tab Setting Value
Location OUT

3. Click OK.

Free Slip Wall 1. Create a new boundary condition named SlipWalls.

Tab Setting Value
Location BOT, TOP
Boundary Details Wall Influence on Flow > Option Free Slip

3. Click OK.

Symmetry Plane 1. Create a new boundary condition named Sym1.
Boundaries 2. Apply the following settings



Tab Setting Value
Location SYM1

3. Click OK.
1. Create a new boundary condition named Sym2.

Tab Setting Value
Location SYM2

3. Click OK.


Tab Setting Value
Settings Option
Initial Conditions > Cartesian Velocity Components > U 16.91 [m s^-1]
Fluid Fluid Specific Initialization Water
Settings at 25 C
Fluid Specific Initialization > Water at 25 C (Selected)
Fluid Specific Initialization > Water at 25 C > Initial Automatic with Value
Fluid Specific Initialization > Water at 25 C > Initial 1
Fluid Specific Initialization Water Vapour at 25 C
Fluid Specific Initialization > Water Vapour at 25 C (Selected)
Fluid Specific Initialization > Water Vapour at 25 C > Initial Automatic with Value
Fluid Specific Initialization > Water Vapour at 25 C > Initial 0

3. Click OK.


Tutorial 19: Cavitation Around a Hydrofoil: Obtaining an Initial Solution using ANSYS CFX-Solver Manager


Tab Setting Value
Convergence Control > Fluid Timescale Physical Timescale
Convergence Control > Fluid Timescale 0.01 [s]

Note: For the Convergence Criteria, an RMS value of at least 1e-05 is usually required for
adequate convergence, but the default value is sufficient for demonstration purposes.
3. Click OK.


Setting Value
File name HydrofoilIni.def


4. Quit ANSYS CFX-Pre, saving the simulation (.cfx) file at your discretion.

Obtaining an Initial Solution using ANSYS CFX-Solver Manager
While the calculations proceed, you can see residual output for various equations in both
the text area and the plot area. Use the tabs to switch between different plots (e.g.,
Momentum and Mass, Turbulence Quantities, etc.) in the plot area. You can view residual
plots for the fluid and solid domains separately by editing the workspace properties.
1. Ensure that the Define Run dialog box is displayed.
2. Click Start Run.


Tutorial 19: Cavitation Around a Hydrofoil: Viewing the Results of the Initial Simulation

Viewing the Results of the Initial Simulation
• Plotting Pressure Distribution Data (p. 324)
• Exporting Pressure Distribution Data (p. 325)
• Saving the Post-Processing State (p. 326)

Plotting Pressure Distribution Data
In this section, you will create a plot of the pressure coefficient distribution around the
hydrofoil. The data will then be exported to a file for later comparison with data from the
cavitating flow case, which will be run later in this tutorial.
-Z.
2. Insert a new plane named Slice.

Tab Setting Value
Definition > Z 5e-5 [m]

4. Click Apply.
5. Create a new polyline named Foil by selecting Insert > Location > Polyline from the
main menu.

Tab Setting Value
Boundary List Default Domain Default
Intersect With Slice

7. Click Apply.
Zoom in on the center of the hydrofoil (near the cavity) to confirm the polyline wraps
around the hydrofoil.
8. Create a new variable named Pressure Coefficient.

Setting Value
Expression (Pressure-51957[Pa])/(0.5*996.2[kg m^-3]*16.91[m s^-1]^2)

10. Click Apply.
11. Create a new variable named Chord.


Tutorial 19: Cavitation Around a Hydrofoil: Viewing the Results of the Initial Simulation

Setting Value
Expression (X-minVal(X)@Foil)/(maxVal(X)@Foil-minVal(X)@Foil)

This creates a normalized chord, measured in the X direction, ranging from 0 at the
leading edge to 1 at the trailing edge of the hydrofoil.
13. Click Apply.
Note: Although the variables that were just created are only needed at points along the
polyline, they exist throughout the domain.

Now that the variables Chord and Pressure Coefficient exist, they can be associated
with the previously defined polyline (the locator) to form a chart line. This chart line will be
added to the chart object, which is created next.
1. Select Insert > Chart from the main menu.
2. Set the name to Pressure Coefficient Distribution.

Tab Setting Value
Chart Title Pressure Coefficient Distribution
Labels > Use Data For Axis Label (Cleared)
Labels > X Axis Normalized Chord Position
Labels > Y Axis Pressure Coefficient
Chart Line 1 Line Name Solver Cp
Location Foil
X Axis > Variable Chord
Y Axis > Variable Pressure Coefficient
Axes X Axis > Determine Ranges Automatically (Cleared)
X Axis > Min 0
X Axis > Max 1
Y Axis > Determine Ranges Automatically (Cleared)
Y Axis > Min -0.5
Y Axis > Max 0.4
Y Axis > Invert Axis (Selected)

4. Click Apply.
5. The chart appears on the Chart Viewer tab.

Exporting Pressure Distribution Data
You will now export the chord and pressure coefficient data along the polyline. This data will
be imported and used in a chart later in this tutorial for comparison with the results for when
cavitation is present.
1. Select File > Export. The Export dialog box appears

ANSYS CFX Tutorials. ANSY

Ansys 11 tutorial

More Related Content

What's hot

Viewers also liked

Similar to Ansys 11 tutorial

Recently uploaded

Ansys 11 tutorial