ANSYSTheory Guide
User Manual:
Open the PDF directly: View PDF 
.
Page Count: 816
| Download | |
| Open PDF In Browser | View PDF |
ANSYS FLUENT 12.0
Theory Guide
April 2009
Copyright c 2009 by ANSYS, Inc.
All Rights Reserved. No part of this document may be reproduced or otherwise used in
any form without express written permission from ANSYS, Inc.
Airpak, Mechanical APDL, Workbench, AUTODYN, CFX, FIDAP, FloWizard, FLUENT,
GAMBIT, Iceboard, Icechip, Icemax, Icepak, Icepro, Icewave, MixSim, POLYFLOW, TGrid,
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. All other brand, product, service and
feature names or trademarks are the property of their respective owners.
CATIA V5 is a registered trademark of Dassault Systèmes. CHEMKIN is a registered
trademark of Reaction Design Inc.
Portions of this program include material copyrighted by PathScale Corporation
2003-2004.
ANSYS, Inc. is certified to ISO 9001:2008
See the on-line documentation for the complete Legal Notices for ANSYS proprietary
software and third-party software. If you are unable to access the Legal Notice, contact
ANSYS, Inc.
Contents
Preface
UTM-1
1 Basic Fluid Flow
1-1
1.1
Overview of Physical Models in ANSYS FLUENT . . . . . . . . . . . . .
1-2
1.2
Continuity and Momentum Equations . . . . . . . . . . . . . . . . . . .
1-3
1.3
User-Defined Scalar (UDS) Transport Equations . . . . . . . . . . . . . .
1-5
1.3.1
Single Phase Flow . . . . . . . . . . . . . . . . . . . . . . . . . .
1-5
1.3.2
Multiphase Flow . . . . . . . . . . . . . . . . . . . . . . . . . . .
1-6
Periodic Flows . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1-7
1.4.1
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1-8
1.4.2
Limitations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1-9
1.4.3
Physics of Periodic Flows . . . . . . . . . . . . . . . . . . . . . .
1-9
1.4
1.5
1.6
1.7
Swirling and Rotating Flows . . . . . . . . . . . . . . . . . . . . . . . . . 1-11
1.5.1
Overview of Swirling and Rotating Flows . . . . . . . . . . . . . 1-11
1.5.2
Physics of Swirling and Rotating Flows . . . . . . . . . . . . . . 1-14
Compressible Flows . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-16
1.6.1
When to Use the Compressible Flow Model . . . . . . . . . . . . 1-17
1.6.2
Physics of Compressible Flows . . . . . . . . . . . . . . . . . . . 1-18
Inviscid Flows . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-19
1.7.1
Euler Equations . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-20
Release 12.0 c ANSYS, Inc. January 29, 2009
TOC-1
CONTENTS
2 Flows with Rotating Reference Frames
2-1
2.1
Introduction
. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2-1
2.2
Flow in a Rotating Reference Frame . . . . . . . . . . . . . . . . . . . .
2-2
2.2.1
Equations for a Rotating Reference Frame . . . . . . . . . . . . .
2-3
2.2.2
Single Rotating Reference Frame (SRF) Modeling . . . . . . . .
2-6
Flow in Multiple Rotating Reference Frames . . . . . . . . . . . . . . . .
2-8
2.3.1
The Multiple Reference Frame Model . . . . . . . . . . . . . . .
2-8
2.3.2
The Mixing Plane Model . . . . . . . . . . . . . . . . . . . . . . 2-13
2.3
3 Flows Using Sliding and Deforming Meshes
3-1
3.1
Introduction
. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3-1
3.2
Sliding Mesh Theory . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3-4
3.2.1
3.3
The Sliding Mesh Concept . . . . . . . . . . . . . . . . . . . . . 3-10
Dynamic Mesh Theory . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-11
3.3.1
Dynamic Mesh Update Methods . . . . . . . . . . . . . . . . . . 3-11
3.3.2
Six DOF (6DOF) Solver Theory . . . . . . . . . . . . . . . . . . 3-31
4 Turbulence
4.1
Introduction
. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4-1
4.2
Choosing a Turbulence Model . . . . . . . . . . . . . . . . . . . . . . . .
4-3
4.2.1
Reynolds-Averaged Approach vs. LES . . . . . . . . . . . . . . .
4-3
4.2.2
Reynolds (Ensemble) Averaging . . . . . . . . . . . . . . . . . .
4-4
4.2.3
Boussinesq Approach vs. Reynolds Stress Transport Models . . .
4-5
Spalart-Allmaras Model . . . . . . . . . . . . . . . . . . . . . . . . . . .
4-6
4.3.1
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4-6
4.3.2
Transport Equation for the Spalart-Allmaras Model . . . . . . .
4-7
4.3.3
Modeling the Turbulent Viscosity . . . . . . . . . . . . . . . . .
4-8
4.3.4
Modeling the Turbulent Production . . . . . . . . . . . . . . . .
4-8
4.3.5
Modeling the Turbulent Destruction . . . . . . . . . . . . . . . . 4-10
4.3.6
Model Constants . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-10
4.3
TOC-2
4-1
Release 12.0 c ANSYS, Inc. January 29, 2009
CONTENTS
4.4
4.5
4.6
4.7
4.3.7
Wall Boundary Conditions . . . . . . . . . . . . . . . . . . . . . 4-10
4.3.8
Convective Heat and Mass Transfer Modeling . . . . . . . . . . . 4-11
Standard, RNG, and Realizable k- Models . . . . . . . . . . . . . . . . 4-11
4.4.1
Standard k- Model . . . . . . . . . . . . . . . . . . . . . . . . . 4-12
4.4.2
RNG k- Model . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-14
4.4.3
Realizable k- Model . . . . . . . . . . . . . . . . . . . . . . . . . 4-18
4.4.4
Modeling Turbulent Production in the k- Models . . . . . . . . 4-22
4.4.5
Effects of Buoyancy on Turbulence in the k- Models . . . . . . . 4-23
4.4.6
Effects of Compressibility on Turbulence in the k- Models . . . 4-24
4.4.7
Convective Heat and Mass Transfer Modeling in the
k- Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-24
Standard and SST k-ω Models . . . . . . . . . . . . . . . . . . . . . . . 4-26
4.5.1
Standard k-ω Model . . . . . . . . . . . . . . . . . . . . . . . . . 4-26
4.5.2
Shear-Stress Transport (SST) k-ω Model . . . . . . . . . . . . . 4-31
4.5.3
Wall Boundary Conditions . . . . . . . . . . . . . . . . . . . . . 4-35
k-kl-ω Transition Model . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-37
4.6.1
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-37
4.6.2
Transport Equations for the k-kl-ω Model . . . . . . . . . . . . . 4-37
Transition SST Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-41
4.7.1
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-42
4.7.2
Transport Equations for the Transition SST Model . . . . . . . . 4-42
4.7.3
Specifying Inlet Turbulence Levels . . . . . . . . . . . . . . . . . 4-46
4.8
The v 2 -f Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-47
4.9
Reynolds Stress Model (RSM) . . . . . . . . . . . . . . . . . . . . . . . . 4-48
4.9.1
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-48
4.9.2
Reynolds Stress Transport Equations . . . . . . . . . . . . . . . 4-49
4.9.3
Modeling Turbulent Diffusive Transport . . . . . . . . . . . . . . 4-50
4.9.4
Modeling the Pressure-Strain Term . . . . . . . . . . . . . . . . . 4-50
4.9.5
Effects of Buoyancy on Turbulence . . . . . . . . . . . . . . . . . 4-55
Release 12.0 c ANSYS, Inc. January 29, 2009
TOC-3
CONTENTS
4.9.6
Modeling the Turbulence Kinetic Energy . . . . . . . . . . . . . 4-55
4.9.7
Modeling the Dissipation Rate . . . . . . . . . . . . . . . . . . . 4-56
4.9.8
Modeling the Turbulent Viscosity . . . . . . . . . . . . . . . . . 4-57
4.9.9
Wall Boundary Conditions . . . . . . . . . . . . . . . . . . . . . 4-57
4.9.10
Convective Heat and Mass Transfer Modeling . . . . . . . . . . . 4-58
4.10 Detached Eddy Simulation (DES) . . . . . . . . . . . . . . . . . . . . . . 4-58
4.10.1
Spalart-Allmaras Based DES Model . . . . . . . . . . . . . . . . 4-59
4.10.2
Realizable k- Based DES Model . . . . . . . . . . . . . . . . . . 4-60
4.10.3
SST k-ω Based DES Model . . . . . . . . . . . . . . . . . . . . . 4-61
4.11 Large Eddy Simulation (LES) Model . . . . . . . . . . . . . . . . . . . . 4-61
4.11.1
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-62
4.11.2
Filtered Navier-Stokes Equations . . . . . . . . . . . . . . . . . . 4-63
4.11.3
Subgrid-Scale Models . . . . . . . . . . . . . . . . . . . . . . . . 4-64
4.11.4
Inlet Boundary Conditions for the LES Model
. . . . . . . . . . 4-68
4.12 Near-Wall Treatments for Wall-Bounded Turbulent Flows . . . . . . . . 4-71
4.12.1
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-71
4.12.2
Standard Wall Functions . . . . . . . . . . . . . . . . . . . . . . 4-74
4.12.3
Non-Equilibrium Wall Functions . . . . . . . . . . . . . . . . . . 4-79
4.12.4
Enhanced Wall Treatment . . . . . . . . . . . . . . . . . . . . . . 4-82
4.12.5
User-Defined Wall Functions . . . . . . . . . . . . . . . . . . . . 4-87
4.12.6
LES Near-Wall Treatment . . . . . . . . . . . . . . . . . . . . . . 4-88
5 Heat Transfer
TOC-4
5-1
5.1
Introduction
. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5-1
5.2
Modeling Conductive and Convective Heat Transfer . . . . . . . . . . . .
5-2
5.2.1
Heat Transfer Theory . . . . . . . . . . . . . . . . . . . . . . . .
5-2
5.2.2
Natural Convection and Buoyancy-Driven Flows Theory . . . . .
5-6
Release 12.0 c ANSYS, Inc. January 29, 2009
CONTENTS
5.3
Modeling Radiation . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5-7
5.3.1
Overview and Limitations . . . . . . . . . . . . . . . . . . . . . .
5-8
5.3.2
Radiative Transfer Equation . . . . . . . . . . . . . . . . . . . . 5-12
5.3.3
P-1 Radiation Model Theory . . . . . . . . . . . . . . . . . . . . 5-13
5.3.4
Rosseland Radiation Model Theory . . . . . . . . . . . . . . . . 5-17
5.3.5
Discrete Transfer Radiation Model (DTRM) Theory . . . . . . . 5-19
5.3.6
Discrete Ordinates (DO) Radiation Model Theory . . . . . . . . 5-22
5.3.7
Surface-to-Surface (S2S) Radiation Model Theory . . . . . . . . 5-43
5.3.8
Radiation in Combusting Flows
5.3.9
Choosing a Radiation Model . . . . . . . . . . . . . . . . . . . . 5-49
. . . . . . . . . . . . . . . . . . 5-46
6 Heat Exchangers
6.1
The Macro Heat Exchanger Models . . . . . . . . . . . . . . . . . . . . .
6.1.1
6.1.2
6.2
6-1
Overview and Restrictions of the Macro Heat Exchanger
Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
6-2
Macro Heat Exchanger Model Theory . . . . . . . . . . . . . . .
6-4
The Dual Cell Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6-12
6.2.1
Overview and Restrictions of the Dual Cell Model . . . . . . . . 6-12
6.2.2
Dual Cell Model Theory . . . . . . . . . . . . . . . . . . . . . . . 6-13
7 Species Transport and Finite-Rate Chemistry
7.1
7.2
6-1
7-1
Volumetric Reactions . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7-1
7.1.1
Species Transport Equations . . . . . . . . . . . . . . . . . . . .
7-2
7.1.2
The Generalized Finite-Rate Formulation for Reaction
Modeling . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7-4
Wall Surface Reactions and Chemical Vapor Deposition . . . . . . . . . 7-11
7.2.1
Surface Coverage Reaction Rate Modification . . . . . . . . . . . 7-13
7.2.2
Reaction-Diffusion Balance for Surface Chemistry
7.2.3
Slip Boundary Formulation for Low-Pressure Gas Systems . . . . 7-15
Release 12.0 c ANSYS, Inc. January 29, 2009
. . . . . . . . 7-14
TOC-5
CONTENTS
7.3
Particle Surface Reactions . . . . . . . . . . . . . . . . . . . . . . . . . . 7-17
7.3.1
General Description . . . . . . . . . . . . . . . . . . . . . . . . . 7-17
7.3.2
ANSYS FLUENT Model Formulation . . . . . . . . . . . . . . . . 7-18
7.3.3
Extension for Stoichiometries with Multiple Gas Phase
Reactants . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7-20
7.3.4
Solid-Solid Reactions . . . . . . . . . . . . . . . . . . . . . . . . 7-20
7.3.5
Solid Decomposition Reactions . . . . . . . . . . . . . . . . . . . 7-21
7.3.6
Solid Deposition Reactions . . . . . . . . . . . . . . . . . . . . . 7-21
7.3.7
Gaseous Solid Catalyzed Reactions on the Particle Surface . . . . 7-21
8 Non-Premixed Combustion
8.1
Introduction
. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8-2
8.2
Non-Premixed Combustion and Mixture Fraction Theory . . . . . . . . .
8-2
8.2.1
Mixture Fraction Theory . . . . . . . . . . . . . . . . . . . . . .
8-2
8.2.2
Modeling of Turbulence-Chemistry Interaction . . . . . . . . . .
8-8
8.2.3
Non-Adiabatic Extensions of the Non-Premixed Model . . . . . . 8-12
8.2.4
Chemistry Tabulation . . . . . . . . . . . . . . . . . . . . . . . . 8-15
8.3
8.4
TOC-6
8-1
Restrictions and Special Cases for Using the Non-Premixed Model . . . . 8-19
8.3.1
Restrictions on the Mixture Fraction Approach . . . . . . . . . . 8-19
8.3.2
Using the Non-Premixed Model for Liquid Fuel or Coal
Combustion . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8-20
8.3.3
Using the Non-Premixed Model with Flue Gas Recycle . . . . . . 8-23
8.3.4
Using the Non-Premixed Model with the Inert Model . . . . . . 8-24
The Laminar Flamelet Models Theory . . . . . . . . . . . . . . . . . . . 8-26
8.4.1
Restrictions and Assumptions . . . . . . . . . . . . . . . . . . . . 8-26
8.4.2
The Flamelet Concept . . . . . . . . . . . . . . . . . . . . . . . . 8-26
8.4.3
Flamelet Generation . . . . . . . . . . . . . . . . . . . . . . . . . 8-30
8.4.4
Flamelet Import . . . . . . . . . . . . . . . . . . . . . . . . . . . 8-31
Release 12.0 c ANSYS, Inc. January 29, 2009
CONTENTS
8.5
8.6
The Steady Laminar Flamelet Model Theory . . . . . . . . . . . . . . . 8-32
8.5.1
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8-33
8.5.2
Multiple Steady Flamelet Libraries . . . . . . . . . . . . . . . . . 8-34
8.5.3
Steady Laminar Flamelet Automated Grid Refinement . . . . . . 8-34
8.5.4
Non-Adiabatic Steady Laminar Flamelets . . . . . . . . . . . . . 8-35
The Unsteady Laminar Flamelet Model Theory . . . . . . . . . . . . . . 8-36
8.6.1
The Eulerian Unsteady Laminar Flamelet Model . . . . . . . . . 8-36
8.6.2
The Diesel Unsteady Laminar Flamelet Model . . . . . . . . . . 8-39
9 Premixed Combustion
9.1
9.2
9.3
9.4
9.5
9-1
Overview and Limitations . . . . . . . . . . . . . . . . . . . . . . . . . .
9-1
9.1.1
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9-1
9.1.2
Limitations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9-2
Zimont Turbulent Flame Closure Theory . . . . . . . . . . . . . . . . . .
9-3
9.2.1
Propagation of the Flame Front . . . . . . . . . . . . . . . . . .
9-3
9.2.2
Turbulent Flame Speed . . . . . . . . . . . . . . . . . . . . . . .
9-4
Extended Coherent Flamelet Model Theory . . . . . . . . . . . . . . . .
9-9
9.3.1
Closure for ECFM Source Terms . . . . . . . . . . . . . . . . . . 9-11
9.3.2
Turbulent Flame Speed in ECFM . . . . . . . . . . . . . . . . . 9-13
Calculation of Temperature . . . . . . . . . . . . . . . . . . . . . . . . . 9-13
9.4.1
Adiabatic Temperature Calculation . . . . . . . . . . . . . . . . 9-13
9.4.2
Non-Adiabatic Temperature Calculation . . . . . . . . . . . . . . 9-13
Calculation of Density . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9-14
10 Partially Premixed Combustion
10-1
10.1 Overview and Limitations . . . . . . . . . . . . . . . . . . . . . . . . . . 10-1
10.1.1
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10-1
10.1.2
Limitations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10-1
Release 12.0 c ANSYS, Inc. January 29, 2009
TOC-7
CONTENTS
10.2 Partially Premixed Combustion Theory . . . . . . . . . . . . . . . . . . 10-2
10.2.1
Calculation of Scalar Quantities . . . . . . . . . . . . . . . . . . 10-2
10.2.2
Laminar Flame Speed . . . . . . . . . . . . . . . . . . . . . . . . 10-3
11 Composition PDF Transport
11-1
11.1 Overview and Limitations . . . . . . . . . . . . . . . . . . . . . . . . . . 11-1
11.2 Composition PDF Transport Theory . . . . . . . . . . . . . . . . . . . . 11-2
11.3 The Lagrangian Solution Method . . . . . . . . . . . . . . . . . . . . . . 11-3
11.3.1
Particle Convection . . . . . . . . . . . . . . . . . . . . . . . . . 11-4
11.3.2
Particle Mixing . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11-5
11.3.3
Particle Reaction . . . . . . . . . . . . . . . . . . . . . . . . . . . 11-6
11.3.4
The ISAT Algorithm
. . . . . . . . . . . . . . . . . . . . . . . . 11-8
11.4 The Eulerian Solution Method . . . . . . . . . . . . . . . . . . . . . . . 11-9
12 Engine Ignition
12-1
12.1 Spark Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12-1
12.1.1
Overview and Limitations . . . . . . . . . . . . . . . . . . . . . . 12-1
12.1.2
Spark Model Theory . . . . . . . . . . . . . . . . . . . . . . . . . 12-2
12.2 Autoignition Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12-3
12.2.1
Overview and Limitations . . . . . . . . . . . . . . . . . . . . . . 12-4
12.2.2
Ignition Model Theory . . . . . . . . . . . . . . . . . . . . . . . . 12-5
12.3 Crevice Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12-9
12.3.1
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12-10
12.3.2
Limitations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12-12
12.3.3
Crevice Model Theory . . . . . . . . . . . . . . . . . . . . . . . . 12-13
13 Pollutant Formation
13-1
13.1 NOx Formation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13-1
TOC-8
13.1.1
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13-2
13.1.2
Governing Equations for NOx Transport . . . . . . . . . . . . . . 13-3
Release 12.0 c ANSYS, Inc. January 29, 2009
CONTENTS
13.1.3
Thermal NOx Formation . . . . . . . . . . . . . . . . . . . . . . 13-4
13.1.4
Prompt NOx Formation . . . . . . . . . . . . . . . . . . . . . . . 13-8
13.1.5
Fuel NOx Formation . . . . . . . . . . . . . . . . . . . . . . . . . 13-12
13.1.6
NOx Formation from Intermediate N2 O . . . . . . . . . . . . . . 13-24
13.1.7
NOx Reduction by Reburning . . . . . . . . . . . . . . . . . . . 13-26
13.1.8
NOx Reduction by SNCR . . . . . . . . . . . . . . . . . . . . . . 13-30
13.1.9
NOx Formation in Turbulent Flows . . . . . . . . . . . . . . . . 13-36
13.2 SOx Formation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13-39
13.2.1
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13-40
13.2.2
Governing Equations for SOx Transport . . . . . . . . . . . . . . 13-41
13.2.3
Reaction Mechanisms for Sulfur Oxidation . . . . . . . . . . . . 13-42
13.2.4
SO2 and H 2 S Production in a Gaseous Fuel . . . . . . . . . . . . 13-44
13.2.5
SO2 and H 2 S Production in a Liquid Fuel . . . . . . . . . . . . 13-44
13.2.6
SO2 and H 2 S Production from Coal . . . . . . . . . . . . . . . . 13-44
13.2.7
SOx Formation in Turbulent Flows . . . . . . . . . . . . . . . . . 13-45
13.3 Soot Formation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13-47
13.3.1
Overview and Limitations . . . . . . . . . . . . . . . . . . . . . . 13-47
13.3.2
Soot Model Theory . . . . . . . . . . . . . . . . . . . . . . . . . 13-48
14 Aerodynamically Generated Noise
14-1
14.1 Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14-1
14.1.1
Direct Method . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14-2
14.1.2
Integral Method Based on Acoustic Analogy . . . . . . . . . . . 14-2
14.1.3
Broadband Noise Source Models . . . . . . . . . . . . . . . . . . 14-3
14.2 Acoustics Model Theory . . . . . . . . . . . . . . . . . . . . . . . . . . . 14-4
14.2.1
The Ffowcs Williams and Hawkings Model . . . . . . . . . . . . 14-5
14.2.2
Broadband Noise Source Models . . . . . . . . . . . . . . . . . . 14-7
Release 12.0 c ANSYS, Inc. January 29, 2009
TOC-9
CONTENTS
15 Discrete Phase
15.1 Introduction
15-1
. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15-1
15.2 Particle Motion Theory . . . . . . . . . . . . . . . . . . . . . . . . . . . 15-2
15.2.1
Equations of Motion for Particles . . . . . . . . . . . . . . . . . . 15-2
15.2.2
Turbulent Dispersion of Particles . . . . . . . . . . . . . . . . . . 15-6
15.2.3
Integration of Particle Equation of Motion . . . . . . . . . . . . . 15-12
15.3 Laws for Drag Coefficients . . . . . . . . . . . . . . . . . . . . . . . . . . 15-15
15.3.1
Spherical Drag Law . . . . . . . . . . . . . . . . . . . . . . . . . 15-15
15.3.2
Non-spherical Drag Law . . . . . . . . . . . . . . . . . . . . . . . 15-15
15.3.3
Stokes-Cunningham Drag Law . . . . . . . . . . . . . . . . . . . 15-16
15.3.4
High-Mach-Number Drag Law . . . . . . . . . . . . . . . . . . . 15-16
15.3.5
Dynamic Drag Model Theory . . . . . . . . . . . . . . . . . . . . 15-16
15.3.6
Dense Discrete Phase Model Drag Laws . . . . . . . . . . . . . . 15-17
15.4 Laws for Heat and Mass Exchange . . . . . . . . . . . . . . . . . . . . . 15-18
15.4.1
Inert Heating or Cooling (Law 1/Law 6) . . . . . . . . . . . . . . 15-19
15.4.2
Droplet Vaporization (Law 2) . . . . . . . . . . . . . . . . . . . . 15-21
15.4.3
Droplet Boiling (Law 3) . . . . . . . . . . . . . . . . . . . . . . . 15-24
15.4.4
Devolatilization (Law 4) . . . . . . . . . . . . . . . . . . . . . . . 15-25
15.4.5
Surface Combustion (Law 5) . . . . . . . . . . . . . . . . . . . . 15-36
15.4.6
Multicomponent Particle Definition (Law 7) . . . . . . . . . . . . 15-42
15.5 Vapor Liquid Equilibrium Theory . . . . . . . . . . . . . . . . . . . . . . 15-43
15.6 Wall-Jet Model Theory
. . . . . . . . . . . . . . . . . . . . . . . . . . . 15-46
15.7 Wall-Film Model Theory . . . . . . . . . . . . . . . . . . . . . . . . . . . 15-47
15.7.1
Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15-47
15.7.2
Interaction During Impact with a Boundary . . . . . . . . . . . . 15-49
15.7.3
Splashing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15-50
15.7.4
Separation Criteria
15.7.5
Conservation Equations for Wall-Film Particles . . . . . . . . . . 15-54
. . . . . . . . . . . . . . . . . . . . . . . . . 15-53
15.8 Particle Erosion and Accretion Theory . . . . . . . . . . . . . . . . . . . 15-59
TOC-10
Release 12.0 c ANSYS, Inc. January 29, 2009
CONTENTS
15.9 Atomizer Model Theory . . . . . . . . . . . . . . . . . . . . . . . . . . . 15-60
15.9.1
The Plain-Orifice Atomizer Model . . . . . . . . . . . . . . . . . 15-61
15.9.2
The Pressure-Swirl Atomizer Model . . . . . . . . . . . . . . . . 15-69
15.9.3
The Air-Blast/Air-Assist Atomizer Model . . . . . . . . . . . . . 15-74
15.9.4
The Flat-Fan Atomizer Model . . . . . . . . . . . . . . . . . . . 15-75
15.9.5
The Effervescent Atomizer Model
. . . . . . . . . . . . . . . . . 15-76
15.10 Secondary Breakup Model Theory . . . . . . . . . . . . . . . . . . . . . 15-77
15.10.1 Taylor Analogy Breakup (TAB) Model . . . . . . . . . . . . . . . 15-78
15.10.2 Wave Breakup Model . . . . . . . . . . . . . . . . . . . . . . . . 15-83
15.11 Droplet Collision and Coalescence Model Theory . . . . . . . . . . . . . 15-86
15.11.1 Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15-86
15.11.2 Use and Limitations . . . . . . . . . . . . . . . . . . . . . . . . . 15-87
15.11.3 Theory . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15-88
15.12 One-Way and Two-Way Coupling . . . . . . . . . . . . . . . . . . . . . . 15-90
15.12.1 Coupling Between the Discrete and Continuous Phases . . . . . . 15-90
15.12.2 Momentum Exchange . . . . . . . . . . . . . . . . . . . . . . . . 15-91
15.12.3 Heat Exchange . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15-91
15.12.4 Mass Exchange . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15-92
15.12.5 Under-Relaxation of the Interphase Exchange Terms . . . . . . . 15-93
15.12.6 Interphase Exchange During Stochastic Tracking . . . . . . . . . 15-95
15.12.7 Interphase Exchange During Cloud Tracking . . . . . . . . . . . 15-95
16 Multiphase Flows
16.1 Introduction
16-1
. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-2
16.1.1
Multiphase Flow Regimes . . . . . . . . . . . . . . . . . . . . . . 16-2
16.1.2
Examples of Multiphase Systems . . . . . . . . . . . . . . . . . . 16-5
16.2 Choosing a General Multiphase Model . . . . . . . . . . . . . . . . . . . 16-5
16.2.1
Approaches to Multiphase Modeling . . . . . . . . . . . . . . . . 16-6
16.2.2
Model Comparisons . . . . . . . . . . . . . . . . . . . . . . . . . 16-7
Release 12.0 c ANSYS, Inc. January 29, 2009
TOC-11
CONTENTS
16.2.3
Time Schemes in Multiphase Flow . . . . . . . . . . . . . . . . . 16-11
16.2.4
Stability and Convergence . . . . . . . . . . . . . . . . . . . . . . 16-12
16.3 Volume of Fluid (VOF) Model Theory . . . . . . . . . . . . . . . . . . . 16-13
16.3.1
Overview and Limitations of the VOF Model . . . . . . . . . . . 16-14
16.3.2
Volume Fraction Equation . . . . . . . . . . . . . . . . . . . . . 16-15
16.3.3
Material Properties . . . . . . . . . . . . . . . . . . . . . . . . . 16-20
16.3.4
Momentum Equation . . . . . . . . . . . . . . . . . . . . . . . . 16-21
16.3.5
Energy Equation . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-21
16.3.6
Additional Scalar Equations . . . . . . . . . . . . . . . . . . . . 16-22
16.3.7
Time Dependence . . . . . . . . . . . . . . . . . . . . . . . . . . 16-22
16.3.8
Surface Tension and Wall Adhesion . . . . . . . . . . . . . . . . 16-22
16.3.9
Open Channel Flow . . . . . . . . . . . . . . . . . . . . . . . . . 16-25
16.3.10 Open Channel Wave Boundary Conditions . . . . . . . . . . . . 16-28
16.4 Mixture Model Theory . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-30
16.4.1
Overview and Limitations of the Mixture Model . . . . . . . . . 16-30
16.4.2
Continuity Equation . . . . . . . . . . . . . . . . . . . . . . . . . 16-32
16.4.3
Momentum Equation . . . . . . . . . . . . . . . . . . . . . . . . 16-32
16.4.4
Energy Equation . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-33
16.4.5
Relative (Slip) Velocity and the Drift Velocity . . . . . . . . . . . 16-33
16.4.6
Volume Fraction Equation for the Secondary Phases . . . . . . . 16-35
16.4.7
Granular Properties . . . . . . . . . . . . . . . . . . . . . . . . . 16-36
16.4.8
Granular Temperature . . . . . . . . . . . . . . . . . . . . . . . . 16-37
16.4.9
Interfacial Area Concentration . . . . . . . . . . . . . . . . . . . 16-38
16.4.10 Solids Pressure . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-41
16.5 Eulerian Model Theory
TOC-12
. . . . . . . . . . . . . . . . . . . . . . . . . . . 16-41
16.5.1
Overview and Limitations of the Eulerian Model . . . . . . . . . 16-42
16.5.2
Volume Fraction Equation . . . . . . . . . . . . . . . . . . . . . 16-43
16.5.3
Conservation Equations . . . . . . . . . . . . . . . . . . . . . . . 16-44
16.5.4
Interphase Exchange Coefficients . . . . . . . . . . . . . . . . . . 16-49
Release 12.0 c ANSYS, Inc. January 29, 2009
CONTENTS
16.5.5
Solids Pressure . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-57
16.5.6
Maximum Packing Limit in Binary Mixtures . . . . . . . . . . . 16-60
16.5.7
Solids Shear Stresses . . . . . . . . . . . . . . . . . . . . . . . . . 16-61
16.5.8
Granular Temperature . . . . . . . . . . . . . . . . . . . . . . . . 16-64
16.5.9
Interfacial Area Concentration . . . . . . . . . . . . . . . . . . . 16-66
16.5.10 Description of Heat Transfer . . . . . . . . . . . . . . . . . . . . 16-66
16.5.11 Turbulence Models . . . . . . . . . . . . . . . . . . . . . . . . . . 16-67
16.5.12 Solution Method in ANSYS FLUENT . . . . . . . . . . . . . . . . 16-77
16.5.13 Dense Discrete Phase Model . . . . . . . . . . . . . . . . . . . . 16-78
16.5.14 Immiscible Fluid Model . . . . . . . . . . . . . . . . . . . . . . . 16-81
16.6 Wet Steam Model Theory . . . . . . . . . . . . . . . . . . . . . . . . . . 16-82
16.6.1
Overview and Limitations of the Wet Steam Model . . . . . . . . 16-82
16.6.2
Wet Steam Flow Equations . . . . . . . . . . . . . . . . . . . . . 16-83
16.6.3
Phase Change Model . . . . . . . . . . . . . . . . . . . . . . . . 16-85
16.6.4
Built-in Thermodynamic Wet Steam Properties . . . . . . . . . . 16-87
16.7 Modeling Mass Transfer in Multiphase Flows . . . . . . . . . . . . . . . 16-89
16.7.1
Source Terms due to Mass Transfer . . . . . . . . . . . . . . . . 16-89
16.7.2
Unidirectional Constant Rate Mass Transfer . . . . . . . . . . . . 16-91
16.7.3
UDF-Prescribed Mass Transfer . . . . . . . . . . . . . . . . . . . 16-91
16.7.4
Cavitation Models . . . . . . . . . . . . . . . . . . . . . . . . . . 16-92
16.7.5
Evaporation-Condensation Model
. . . . . . . . . . . . . . . . . 16-104
16.8 Modeling Species Transport in Multiphase Flows . . . . . . . . . . . . . 16-107
16.8.1
Limitations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-108
16.8.2
Mass and Momentum Transfer with Multiphase Species
Transport . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-108
16.8.3
The Stiff Chemistry Solver . . . . . . . . . . . . . . . . . . . . . 16-111
Release 12.0 c ANSYS, Inc. January 29, 2009
TOC-13
CONTENTS
17 Solidification and Melting
17-1
17.1 Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17-1
17.2 Limitations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17-2
17.3 Introduction
. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17-3
17.4 Energy Equation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17-3
17.5 Momentum Equations . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17-4
17.6 Turbulence Equations . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17-5
17.7 Species Equations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17-5
17.8 Pull Velocity for Continuous Casting . . . . . . . . . . . . . . . . . . . . 17-7
17.9 Contact Resistance at Walls . . . . . . . . . . . . . . . . . . . . . . . . . 17-8
18 Solver Theory
18-1
18.1 Overview of Flow Solvers . . . . . . . . . . . . . . . . . . . . . . . . . . 18-1
18.1.1
Pressure-Based Solver . . . . . . . . . . . . . . . . . . . . . . . . 18-2
18.1.2
Density-Based Solver . . . . . . . . . . . . . . . . . . . . . . . . 18-5
18.2 General Scalar Transport Equation: Discretization and Solution . . . . . 18-8
18.2.1
Solving the Linear System . . . . . . . . . . . . . . . . . . . . . . 18-9
18.3 Discretization . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-10
18.3.1
Spatial Discretization . . . . . . . . . . . . . . . . . . . . . . . . 18-10
18.3.2
Temporal Discretization . . . . . . . . . . . . . . . . . . . . . . . 18-18
18.3.3
Evaluation of Gradients and Derivatives . . . . . . . . . . . . . . 18-20
18.3.4
Gradient Limiters . . . . . . . . . . . . . . . . . . . . . . . . . . 18-23
18.4 Pressure-Based Solver . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-25
TOC-14
18.4.1
Discretization of the Momentum Equation . . . . . . . . . . . . . 18-26
18.4.2
Discretization of the Continuity Equation . . . . . . . . . . . . . 18-28
18.4.3
Pressure-Velocity Coupling . . . . . . . . . . . . . . . . . . . . . 18-29
18.4.4
Steady-State Iterative Algorithm . . . . . . . . . . . . . . . . . . 18-35
18.4.5
Time-Advancement Algorithm . . . . . . . . . . . . . . . . . . . 18-36
Release 12.0 c ANSYS, Inc. January 29, 2009
CONTENTS
18.5 Density-Based Solver . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-40
18.5.1
Governing Equations in Vector Form . . . . . . . . . . . . . . . . 18-40
18.5.2
Preconditioning . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-41
18.5.3
Convective Fluxes . . . . . . . . . . . . . . . . . . . . . . . . . . 18-44
18.5.4
Steady-State Flow Solution Methods . . . . . . . . . . . . . . . . 18-46
18.5.5
Unsteady Flows Solution Methods . . . . . . . . . . . . . . . . . 18-48
18.6 Multigrid Method . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-51
18.6.1
Approach . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-51
18.6.2
Multigrid Cycles . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-54
18.6.3
Algebraic Multigrid (AMG) . . . . . . . . . . . . . . . . . . . . . 18-57
18.6.4
Full-Approximation Storage (FAS) Multigrid . . . . . . . . . . . 18-64
18.7 Full Multigrid (FMG) Initialization . . . . . . . . . . . . . . . . . . . . . 18-66
18.7.1
Overview of FMG Initialization . . . . . . . . . . . . . . . . . . . 18-66
18.7.2
Limitations of FMG Initialization . . . . . . . . . . . . . . . . . 18-67
19 Adapting the Mesh
19-1
19.1 Static Adaption Process . . . . . . . . . . . . . . . . . . . . . . . . . . . 19-2
19.1.1
Hanging Node Adaption . . . . . . . . . . . . . . . . . . . . . . . 19-2
19.2 Boundary Adaption . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19-5
19.3 Gradient Adaption . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19-5
19.3.1
Gradient Adaption Approach . . . . . . . . . . . . . . . . . . . . 19-5
19.3.2
Example of Steady Gradient Adaption . . . . . . . . . . . . . . . 19-9
19.4 Dynamic Gradient Adaption . . . . . . . . . . . . . . . . . . . . . . . . . 19-9
19.5 Isovalue Adaption . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19-9
19.6 Region Adaption . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19-11
19.6.1
Defining a Region . . . . . . . . . . . . . . . . . . . . . . . . . . 19-13
19.6.2
Region Adaption Example . . . . . . . . . . . . . . . . . . . . . 19-13
Release 12.0 c ANSYS, Inc. January 29, 2009
TOC-15
CONTENTS
19.7 Volume Adaption . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19-15
19.7.1
Volume Adaption Approach . . . . . . . . . . . . . . . . . . . . . 19-15
19.7.2
Volume Adaption Example . . . . . . . . . . . . . . . . . . . . . 19-16
19.8 Yplus/Ystar Adaption . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19-16
19.8.1
Yplus/Ystar Adaption Approach . . . . . . . . . . . . . . . . . . 19-16
19.9 Anisotropic Adaption . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19-19
19.10 Geometry-Based Adaption . . . . . . . . . . . . . . . . . . . . . . . . . . 19-19
19.10.1 Geometry-Based Adaption Approach . . . . . . . . . . . . . . . . 19-19
19.11 Registers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19-24
20 Reporting Alphanumeric Data
20-1
20.1 Fluxes Through Boundaries . . . . . . . . . . . . . . . . . . . . . . . . . 20-2
20.2 Forces on Boundaries . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 20-2
20.2.1
Computing Forces, Moments, and the Center of Pressure
. . . . 20-3
20.3 Surface Integration . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 20-6
20.3.1
Computing Surface Integrals . . . . . . . . . . . . . . . . . . . . 20-7
20.4 Volume Integration . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 20-11
20.4.1
TOC-16
Computing Volume Integrals . . . . . . . . . . . . . . . . . . . . 20-12
Release 12.0 c ANSYS, Inc. January 29, 2009
Using This Manual
The Contents of This Manual
The ANSYS FLUENT Theory Guide provides you with theoretical information about the
models used in ANSYS FLUENT.
i
Under U.S. and international copyright law, ANSYS, Inc. is unable to
distribute copies of the papers listed in the bibliography, other than those
published internally by ANSYS, Inc. Please use your library or a document
delivery service to obtain copies of copyrighted papers.
A brief description of what is in each chapter follows:
• Chapter 1: Basic Fluid Flow, describes the governing equations and physical models
used by ANSYS FLUENT to compute fluid flow (including periodic flow, swirling
and rotating flows, compressible flows, and inviscid flows).
• Chapter 2: Flows with Rotating Reference Frames, describes single rotating reference frames, multiple moving reference frames, and mixing planes in ANSYS
FLUENT.
• Chapter 3: Flows Using Sliding and Deforming Meshes, describes sliding and deforming meshes in ANSYS FLUENT.
• Chapter 4: Turbulence, describes ANSYS FLUENT’s models for turbulent flow.
• Chapter 5: Heat Transfer, describes the physical models used by ANSYS FLUENT to
compute heat transfer (including convective and conductive heat transfer, natural
convection, radiative heat transfer, and periodic heat transfer).
• Chapter 6: Heat Exchangers, describes the physical models used by ANSYS FLUENT
to simulate the performance of heat exchangers.
• Chapter 7: Species Transport and Finite-Rate Chemistry, describes the finite-rate
chemistry models in ANSYS FLUENT. This chapter also provides information about
modeling species transport in non-reacting flows.
• Chapter 8: Non-Premixed Combustion, describes the non-premixed combustion
model.
• Chapter 9: Premixed Combustion, describes the premixed combustion model.
Release 12.0 c ANSYS, Inc. January 29, 2009
UTM-1
Using This Manual
• Chapter 10: Partially Premixed Combustion, describes the partially premixed combustion model.
• Chapter 11: Composition PDF Transport, describes the composition PDF transport
model.
• Chapter 12: Engine Ignition, describes the engine ignition models available in ANSYS FLUENT.
• Chapter 13: Pollutant Formation, describes the models for the formation of NOx ,
SOx , and soot.
• Chapter 14: Aerodynamically Generated Noise, describes the acoustics model.
• Chapter 15: Discrete Phase, describes the discrete phase models available in ANSYS
FLUENT.
• Chapter 16: Multiphase Flows, describes the general multiphase models available
in ANSYS FLUENT (VOF, mixture, and Eulerian).
• Chapter 17: Solidification and Melting, describes ANSYS FLUENT’s model for solidification and melting.
• Chapter 18: Solver Theory, describes the ANSYS FLUENT solvers.
• Chapter 19: Adapting the Mesh, describes the solution-adaptive mesh refinement
feature in ANSYS FLUENT.
• Chapter 20: Reporting Alphanumeric Data, describes how to obtain reports of
fluxes, forces, surface integrals, and other solution data.
UTM-2
Release 12.0 c ANSYS, Inc. January 29, 2009
Using This Manual
The Contents of the Other Manuals
In addition to this Theory Guide, there are several other manuals available to help you
use ANSYS FLUENT and its associated programs:
• The Getting Started Guide describes the capabilities of ANSYS FLUENT, provides
an overview of the problem setup steps, and presents helpful tips in order for you to
create a successfull CFD simulation. The manual also includes information about
accessing the ANSYS FLUENT manuals.
• The User’s Guide contains detailed instructions for using ANSYS FLUENT.
• The Tutorial Guide contains a number of example problems with detailed instructions, commentary, and postprocessing of results.
• The UDF Manual contains information about writing and using user-defined functions (UDFs).
• The Text Command List provides a brief description of each of the commands in
ANSYS FLUENT’s text interface.
Typographical Conventions
Several typographical conventions are used in this manual’s text to facilitate your learning
process.
• An informational icon (
i
) marks an important note.
• Different type styles are used to indicate graphical user interface menu items and
text interface menu items (e.g., Iso-Surface dialog box, surface/iso-surface command).
• The text interface type style is also used when illustrating exactly what appears
on the screen or exactly what you need to type into a field in a dialog box. The
information displayed on the screen is enclosed in a large box to distinguish it from
the narrative text, and user inputs are often enclosed in smaller boxes.
• A mini flow chart is used to guide you through the navigation pane, which leads
you to a specific task page or dialog box. For example,
Models −→
Multiphase −→ Edit...
indicates that Models is selected in the navigation pane, which then opens the
corresponding task page. In the Models task page, Multiphase is selected from the
list. Clicking the Edit... button opens the Multiphase dialog box.
Release 12.0 c ANSYS, Inc. January 29, 2009
UTM-3
Using This Manual
Also, a mini flow chart is used to indicate the menu selections that lead you to a
specific command or dialog box. For example,
Define −→Injections...
indicates that the Injections... menu item can be selected from the Define pull-down
menu, and
display −→mesh
indicates that the mesh command is available in the display text menu.
In this manual, mini flow charts usually precede a description of a dialog box or
command, or a screen illustration showing how to use the dialog box or command.
They allow you to look up information about a command or dialog box and quickly
determine how to access it without having to search the preceding material.
• The menu selections that will lead you to a particular dialog box or task page
are also indicated (usually within a paragraph) using a “/”. For example, Define/Materials... tells you to choose the Materials... menu item from the Define
pull-down menu.
Mathematical Conventions
~
• Where possible, vector quantities are displayed with a raised arrow (e.g., ~a, A).
Boldfaced characters are reserved for vectors and matrices as they apply to linear
algebra (e.g., the identity matrix, I).
• The operator ∇, referred to as grad, nabla, or del, represents the partial derivative
of a quantity with respect to all directions in the chosen coordinate system. In
Cartesian coordinates, ∇ is defined to be
∂
∂
∂
~ı + ~ + ~k
∂x
∂y
∂z
∇ appears in several ways:
– The gradient of a scalar quantity is the vector whose components are the
partial derivatives; for example,
∇p =
∂p
∂p
∂p
~ı + ~ + ~k
∂x
∂y
∂z
– The gradient of a vector quantity is a second-order tensor; for example, in
Cartesian coordinates,
!
∇(~v ) =
UTM-4
∂
∂
∂
~ı + ~ + ~k vx~ı + vy~ + vz~k
∂x
∂y
∂z
Release 12.0 c ANSYS, Inc. January 29, 2009
Using This Manual
This tensor is usually written as
∂vx
∂x
∂vx
∂y
∂vx
∂z
∂vy
∂x
∂vy
∂y
∂vy
∂z
∂vz
∂x
∂vz
∂y
∂vz
∂z
– The divergence of a vector quantity, which is the inner product between ∇
and a vector; for example,
∇ · ~v =
∂vx ∂vy ∂vz
+
+
∂x
∂y
∂z
– The operator ∇ · ∇, which is usually written as ∇2 and is known as the
Laplacian; for example,
∇2 T =
∂2T
∂2T
∂2T
+
+
∂x2
∂y 2
∂z 2
∇2 T is different from the expression (∇T )2 , which is defined as
2
(∇T ) =
∂T
∂x
!2
∂T
+
∂y
!2
∂T
+
∂z
!2
• An exception to the use of ∇ is found in the discussion of Reynolds stresses in
Chapter 4: Turbulence, where convention dictates the use of Cartesian tensor notation. In this chapter, you will also find that some velocity vector components are
written as u, v, and w instead of the conventional v with directional subscripts.
Release 12.0 c ANSYS, Inc. January 29, 2009
UTM-5
Using This Manual
Technical Support
If you encounter difficulties while using ANSYS FLUENT, please first refer to the section(s)
of the manual containing information on the commands you are trying to use or the type
of problem you are trying to solve. The product documentation is available from the
online help, or from the User Services Center (www.fluentusers.com).
If you encounter an error, please write down the exact error message that appeared and
note as much information as you can about what you were doing in ANSYS FLUENT. Then
refer to the following resources available on the User Services Center (www.fluentusers.com):
• Installation and System FAQs - link available from the main page on the User
Services Center. The FAQs can be searched by word or phrase, and are available
for general installation questions as well as for products.
• Known defects for ANSYS FLUENT - link available from the product page. The
defects can be searched by word or phrase, and are listed by categories.
• Online Technical Support - link available from the main page on the User Services
Center. From the Online Technical Support Portal page, there is a link to the
Search Solutions & Request Support page, where the solutions can be searched by
word or phrase.
Contacting Technical Support
If none of the resources available on the User Services Center help in resolving the problem, or you have complex modeling projects, we invite you to log a technical support
request (www.fluentusers.com) to obtain further assistance. However, there are a few
things that we encourage you to do before logging a request:
• Note what you are trying to accomplish with ANSYS FLUENT.
• Note what you were doing when the problem or error occurred.
• Save a journal or transcript file of the ANSYS FLUENT session in which the problem
occurred. This is the best source that we can use to reproduce the problem and
thereby help to identify the cause.
UTM-6
Release 12.0 c ANSYS, Inc. January 29, 2009
Chapter 1.
Basic Fluid Flow
This chapter describes the theoretical background for some of the basic physical models
that ANSYS FLUENT provides for fluid flow. Models for flows in moving zones (including
sliding and dynamic meshes) are explained in Chapter 2: Flows with Rotating Reference
Frames and Chapter 3: Flows Using Sliding and Deforming Meshes, models for turbulence are described in Chapter 4: Turbulence, and models for heat transfer (including
radiation) are presented in Chapter 5: Heat Transfer. An overview of modeling species
transport and reacting flows is provided in Chapter 7: Species Transport and Finite-Rate
Chemistry, details about models for species transport and reacting flows are described in
Chapters 7–11, and models for pollutant formation are presented in Chapter 13: Pollutant
Formation. The discrete phase model is described in Chapter 15: Discrete Phase, general
multiphase models are described in Chapter 16: Multiphase Flows, and the melting and
solidification model is described in Chapter 17: Solidification and Melting. For information on modeling porous media, porous jumps, and lumped parameter fans and radiators,
see Chapter 7: Cell Zone and Boundary Conditions in the separate User’s Guide.
The information in this chapter is presented in the following sections:
• Section 1.1: Overview of Physical Models in ANSYS FLUENT
• Section 1.2: Continuity and Momentum Equations
• Section 1.3: User-Defined Scalar (UDS) Transport Equations
• Section 1.4: Periodic Flows
• Section 1.5: Swirling and Rotating Flows
• Section 1.6: Compressible Flows
• Section 1.7: Inviscid Flows
Release 12.0 c ANSYS, Inc. January 29, 2009
1-1
Basic Fluid Flow
1.1
Overview of Physical Models in ANSYS FLUENT
ANSYS FLUENT provides comprehensive modeling capabilities for a wide range of incompressible and compressible, laminar and turbulent fluid flow problems. Steady-state or
transient analyses can be performed. In ANSYS FLUENT, a broad range of mathematical
models for transport phenomena (like heat transfer and chemical reactions) is combined
with the ability to model complex geometries. Examples of ANSYS FLUENT applications include laminar non-Newtonian flows in process equipment; conjugate heat transfer
in turbomachinery and automotive engine components; pulverized coal combustion in
utility boilers; external aerodynamics; flow through compressors, pumps, and fans; and
multiphase flows in bubble columns and fluidized beds.
To permit modeling of fluid flow and related transport phenomena in industrial equipment and processes, various useful features are provided. These include porous media,
lumped parameter (fan and heat exchanger), streamwise-periodic flow and heat transfer,
swirl, and moving reference frame models. The moving reference frame family of models
includes the ability to model single or multiple reference frames. A time-accurate sliding
mesh method, useful for modeling multiple stages in turbomachinery applications, for example, is also provided, along with the mixing plane model for computing time-averaged
flow fields.
Another very useful group of models in ANSYS FLUENT is the set of free surface and multiphase flow models. These can be used for analysis of gas-liquid, gas-solid, liquid-solid,
and gas-liquid-solid flows. For these types of problems, ANSYS FLUENT provides the
volume-of-fluid (VOF), mixture, and Eulerian models, as well as the discrete phase model
(DPM). The DPM performs Lagrangian trajectory calculations for dispersed phases (particles, droplets, or bubbles), including coupling with the continuous phase. Examples of
multiphase flows include channel flows, sprays, sedimentation, separation, and cavitation.
Robust and accurate turbulence models are a vital component of the ANSYS FLUENT
suite of models. The turbulence models provided have a broad range of applicability, and
they include the effects of other physical phenomena, such as buoyancy and compressibility. Particular care has been devoted to addressing issues of near-wall accuracy via
the use of extended wall functions and zonal models.
Various modes of heat transfer can be modeled, including natural, forced, and mixed convection with or without conjugate heat transfer, porous media, etc. The set of radiation
models and related submodels for modeling participating media are general and can take
into account the complications of combustion. A particular strength of ANSYS FLUENT
is its ability to model combustion phenomena using a variety of models, including eddy
dissipation and probability density function models. A host of other models that are
very useful for reacting flow applications are also available, including coal and droplet
combustion, surface reaction, and pollutant formation models.
1-2
Release 12.0 c ANSYS, Inc. January 29, 2009
1.2 Continuity and Momentum Equations
1.2
Continuity and Momentum Equations
For all flows, ANSYS FLUENT solves conservation equations for mass and momentum.
For flows involving heat transfer or compressibility, an additional equation for energy
conservation is solved. For flows involving species mixing or reactions, a species conservation equation is solved or, if the non-premixed combustion model is used, conservation
equations for the mixture fraction and its variance are solved. Additional transport
equations are also solved when the flow is turbulent.
In this section, the conservation equations for laminar flow in an inertial (non-accelerating)
reference frame are presented. The equations that are applicable to rotating reference
frames are presented in Chapter 2: Flows with Rotating Reference Frames. The conservation equations relevant to heat transfer, turbulence modeling, and species transport
will be discussed in the chapters where those models are described.
The Euler equations solved for inviscid flow are presented in Section 1.7: Inviscid Flows.
The Mass Conservation Equation
The equation for conservation of mass, or continuity equation, can be written as follows:
∂ρ
+ ∇ · (ρ~v ) = Sm
∂t
(1.2-1)
Equation 1.2-1 is the general form of the mass conservation equation and is valid for
incompressible as well as compressible flows. The source Sm is the mass added to the
continuous phase from the dispersed second phase (e.g., due to vaporization of liquid
droplets) and any user-defined sources.
For 2D axisymmetric geometries, the continuity equation is given by
∂
∂
ρvr
∂ρ
+
(ρvx ) + (ρvr ) +
= Sm
∂t ∂x
∂r
r
(1.2-2)
where x is the axial coordinate, r is the radial coordinate, vx is the axial velocity, and vr
is the radial velocity.
Release 12.0 c ANSYS, Inc. January 29, 2009
1-3
Basic Fluid Flow
Momentum Conservation Equations
Conservation of momentum in an inertial (non-accelerating) reference frame is described
by [17]
∂
(ρ~v ) + ∇ · (ρ~v~v ) = −∇p + ∇ · (τ ) + ρ~g + F~
∂t
(1.2-3)
where p is the static pressure, τ is the stress tensor (described below), and ρ~g and F~ are
the gravitational body force and external body forces (e.g., that arise from interaction
with the dispersed phase), respectively. F~ also contains other model-dependent source
terms such as porous-media and user-defined sources.
The stress tensor τ is given by
2
τ = µ (∇~v + ∇~v ) − ∇ · ~v I
3
T
(1.2-4)
where µ is the molecular viscosity, I is the unit tensor, and the second term on the right
hand side is the effect of volume dilation.
For 2D axisymmetric geometries, the axial and radial momentum conservation equations
are given by
"
!#
∂
1 ∂
1 ∂
∂p 1 ∂
∂vx 2
(ρvx ) +
(rρvx vx ) +
(rρvr vx ) = −
+
rµ 2
− (∇ · ~v )
∂t
r ∂x
r ∂r
∂x r ∂x
∂x
3
"
!#
1 ∂
∂vx ∂vr
+
rµ
+
+ Fx
r ∂r
∂r
∂x
(1.2-5)
and
"
∂
1 ∂
1 ∂
∂p 1 ∂
∂vr ∂vx
(ρvr ) +
(rρvx vr ) +
(rρvr vr ) = − +
rµ
+
∂t
r ∂x
r ∂r
∂r r ∂x
∂x
∂r
"
!#
1 ∂
∂vr 2
+
rµ 2
− (∇ · ~v )
r ∂r
∂r
3
− 2µ
vr 2 µ
vz2
+
(∇
·
~
v
)
+
ρ
+ Fr
r2 3 r
r
!#
(1.2-6)
where
∇ · ~v =
∂vx ∂vr vr
+
+
∂x
∂r
r
(1.2-7)
and vz is the swirl velocity. (See Section 1.5: Swirling and Rotating Flows for information
about modeling axisymmetric swirl.)
1-4
Release 12.0 c ANSYS, Inc. January 29, 2009
1.3 User-Defined Scalar (UDS) Transport Equations
1.3
User-Defined Scalar (UDS) Transport Equations
ANSYS FLUENT can solve the transport equation for an arbitrary, user-defined scalar
(UDS) in the same way that it solves the transport equation for a scalar such as species
mass fraction. Extra scalar transport equations may be needed in certain types of combustion applications or for example in plasma-enhanced surface reaction modeling.
This section provides information on how you can specify user-defined scalar (UDS)
transport equations to enhance the standard features of ANSYS FLUENT. ANSYS FLUENT allows you to define additional scalar transport equations in your model in the
User-Defined Scalars dialog box. For more information about setting up user-defined
scalar transport equations in ANSYS FLUENT, see Section 9.1: User-Defined Scalar (UDS)
Transport Equations in the separate User’s Guide.
Information in this section is organized in the following subsections:
• Section 1.3.1: Single Phase Flow
• Section 1.3.2: Multiphase Flow
1.3.1
Single Phase Flow
For an arbitrary scalar φk , ANSYS FLUENT solves the equation
∂ρφk
∂
∂φk
+
(ρui φk − Γk
) = Sφk k = 1, ..., N
∂t
∂xi
∂xi
(1.3-1)
where Γk and Sφk are the diffusion coefficient and source term supplied by you for each
of the N scalar equations. Note that Γk is defined as a tensor in the case of anisotropic
diffusivity. The diffusion term is thus ∇ · (Γk · φk )
For isotropic diffusivity, Γk could be written as Γk I where I is the identity matrix.
For the steady-state case, ANSYS FLUENT will solve one of the three following equations,
depending on the method used to compute the convective flux:
• If convective flux is not to be computed, ANSYS FLUENT will solve the equation
−
∂
∂φk
(Γk
) = Sφk k = 1, ..., N
∂xi
∂xi
(1.3-2)
where Γk and Sφk are the diffusion coefficient and source term supplied by you for
each of the N scalar equations.
Release 12.0 c ANSYS, Inc. January 29, 2009
1-5
Basic Fluid Flow
• If convective flux is to be computed with mass flow rate, ANSYS FLUENT will solve
the equation
∂
∂φk
(ρui φk − Γk
) = Sφk k = 1, ..., N
∂xi
∂xi
(1.3-3)
• It is also possible to specify a user-defined function to be used in the computation
of convective flux. In this case, the user-defined mass flux is assumed to be of the
form
F =
Z
~
ρ~u · dS
(1.3-4)
S
~ is the face vector area.
where dS
1.3.2
Multiphase Flow
For multiphase flows, ANSYS FLUENT solves transport equations for two types of scalars:
per phase and mixture. For an arbitrary k scalar in phase-1, denoted by φkl , ANSYS
FLUENT solves the transport equation inside the volume occupied by phase-l
∂αl ρl φkl
+ ∇ · (αl ρl ~ul φkl − αl Γkl ∇φkl ) = Slk k = 1, ..., N
∂t
(1.3-5)
where αl , ρl , and ~ul are the volume fraction, physical density, and velocity of phase-l,
respectively. Γkl and Slk are the diffusion coefficient and source term, respectively, which
you will need to specify. In this case, scalar φkl is associated only with one phase (phase-l)
and is considered an individual field variable of phase-l.
The mass flux for phase-l is defined as
Fl =
Z
S
~
αl ρl ~ul · dS
(1.3-6)
If the transport variable described by scalar φkl represents the physical field that is shared
between phases, or is considered the same for each phase, then you should consider this
scalar as being associated with a mixture of phases, φk . In this case, the generic transport
equation for the scalar is
∂ρm φk
+ ∇ · (ρm~um φk − Γkm ∇φk ) = S km k = 1, ..., N
∂t
(1.3-7)
where mixture density ρm , mixture velocity ~um , and mixture diffusivity for the scalar k
Γkm are calculated according to
1-6
Release 12.0 c ANSYS, Inc. January 29, 2009
1.4 Periodic Flows
X
ρm =
αl ρl
(1.3-8)
l
ρm~um =
X
αl ρl ~ul
(1.3-9)
l
Fm =
Z
S
~
rhom~um · dS
Γkm =
X
(1.3-10)
αl Γkl
(1.3-11)
Slk
(1.3-12)
l
k
Sm
=
X
l
To calculate mixture diffusivity, you will need to specify individual diffusivities for each
material associated with individual phases.
Note that if the user-defined mass flux option is activated, then mass fluxes shown in
Equation 1.3-6 and Equation 1.3-10 will need to be replaced in the corresponding scalar
transport equations.
1.4
Periodic Flows
Periodic flow occurs when the physical geometry of interest and the expected pattern of
the flow/thermal solution have a periodically repeating nature. Two types of periodic
flow can be modeled in ANSYS FLUENT. In the first type, no pressure drop occurs across
the periodic planes. In the second type, a pressure drop occurs across translationally
periodic boundaries, resulting in “fully-developed” or “streamwise-periodic” flow.
This section discusses streamwise-periodic flow. A description of no-pressure-drop periodic flow is provided in Section 7.3.16: Periodic Boundary Conditions in the separate
User’s Guide, and a description of streamwise-periodic heat transfer is provided in Section 13.4: Modeling Periodic Heat Transfer in the separate User’s Guide. For more
information about setting up periodic flows in ANSYS FLUENT, see Section 9.2: Periodic
Flows in the separate User’s Guide.
Information about streamwise-periodic flow is presented in the following sections:
• Section 1.4.1: Overview
• Section 1.4.2: Limitations
• Section 1.4.3: Physics of Periodic Flows
Release 12.0 c ANSYS, Inc. January 29, 2009
1-7
Basic Fluid Flow
1.4.1
Overview
ANSYS FLUENT provides the ability to calculate streamwise-periodic—or “fully-developed”—
fluid flow. These flows are encountered in a variety of applications, including flows in
compact heat exchanger channels and flows across tube banks. In such flow configurations, the geometry varies in a repeating manner along the direction of the flow, leading
to a periodic fully-developed flow regime in which the flow pattern repeats in successive cycles. Other examples of streamwise-periodic flows include fully-developed flow in
pipes and ducts. These periodic conditions are achieved after a sufficient entrance length,
which depends on the flow Reynolds number and geometric configuration.
Streamwise-periodic flow conditions exist when the flow pattern repeats over some length
L, with a constant pressure drop across each repeating module along the streamwise
direction. Figure 1.4.1 depicts one example of a periodically repeating flow of this type
which has been modeled by including a single representative module.
3.57e-03
3.33e-03
3.09e-03
2.86e-03
2.62e-03
2.38e-03
2.14e-03
1.90e-03
1.67e-03
1.43e-03
1.19e-03
9.53e-04
7.15e-04
4.77e-04
2.39e-04
1.01e-06
Velocity Vectors Colored By Velocity Magnitude (m/s)
Figure 1.4.1: Example of Periodic Flow in a 2D Heat Exchanger Geometry
1-8
Release 12.0 c ANSYS, Inc. January 29, 2009
1.4 Periodic Flows
1.4.2
Limitations
The following limitations apply to modeling streamwise-periodic flow:
• The flow must be incompressible.
• The geometry must be translationally periodic. Note that transient simulations for
fully-developed fluid flow are not valid with translational periodic flow.
• If one of the density-based solvers is used, you can specify only the pressure jump;
for the pressure-based solver, you can specify either the pressure jump or the mass
flow rate.
• No net mass addition through inlets/exits or extra source terms is allowed.
• Species can be modeled only if inlets/exits (without net mass addition) are included
in the problem. Reacting flows are not permitted.
• Discrete phase and multiphase modeling are not allowed.
1.4.3
Physics of Periodic Flows
Definition of the Periodic Velocity
The assumption of periodicity implies that the velocity components repeat themselves in
space as follows:
~ = u(~r + 2L)
~ = ···
u(~r) = u(~r + L)
~ = v(~r + 2L)
~ = ···
v(~r) = v(~r + L)
(1.4-1)
~ = w(~r + 2L)
~ = ···
w(~r) = w(~r + L)
~ is the periodic length vector of the domain considered
where ~r is the position vector and L
(see Figure 1.4.2).
Definition of the Streamwise-Periodic Pressure
For viscous flows, the pressure is not periodic in the sense of Equation 1.4-1. Instead,
the pressure drop between modules is periodic:
~ = p(~r + L)
~ − p(~r + 2L)
~ = ···
∆p = p(~r) − p(~r + L)
(1.4-2)
If one of the density-based solvers is used, ∆p is specified as a constant value. For the
pressure-based solver, the local pressure gradient can be decomposed into two parts:
Release 12.0 c ANSYS, Inc. January 29, 2009
1-9
Basic Fluid Flow
A
→
L
B
→
L
uA = uB = uC
∼
pC
pA = ∼
pB = ∼
vA = vB = vC
pB - pA = pC - pB
C
Figure 1.4.2: Example of a Periodic Geometry
the gradient of a periodic component, ∇p̃(~r), and the gradient of a linearly-varying
~
component, β |LL|
~ :
∇p(~r) = β
~
L
+ ∇p̃(~r)
~
|L|
(1.4-3)
where p̃(~r) is the periodic pressure and β|~r| is the linearly-varying component of the
pressure. The periodic pressure is the pressure left over after subtracting out the linearlyvarying pressure. The linearly-varying component of the pressure results in a force acting
on the fluid in the momentum equations. Because the value of β is not known a priori,
it must be iterated on until the mass flow rate that you have defined is achieved in the
computational model. This correction of β occurs in the pressure correction step of the
SIMPLE, SIMPLEC, or PISO algorithm where the value of β is updated based on the
difference between the desired mass flow rate and the actual one. You have some control
over the number of sub-iterations used to update β. For more information about setting
up parameters for β in ANSYS FLUENT, see Section 9.2.2: Setting Parameters for the
Calculation of β in the separate User’s Guide.
1-10
Release 12.0 c ANSYS, Inc. January 29, 2009
1.5 Swirling and Rotating Flows
1.5
Swirling and Rotating Flows
Many important engineering flows involve swirl or rotation and ANSYS FLUENT is wellequipped to model such flows. Swirling flows are common in combustion, with swirl
introduced in burners and combustors in order to increase residence time and stabilize
the flow pattern. Rotating flows are also encountered in turbomachinery, mixing tanks,
and a variety of other applications.
When you begin the analysis of a rotating or swirling flow, it is essential that you classify
your problem into one of the following five categories of flow:
• axisymmetric flows with swirl or rotation
• fully three-dimensional swirling or rotating flows
• flows requiring a rotating reference frame
• flows requiring multiple rotating reference frames or mixing planes
• flows requiring sliding meshes
Modeling and solution procedures for the first two categories are presented in this section.
The remaining three, which all involve “moving zones”, are discussed in Chapter 2: Flows
with Rotating Reference Frames.
Information about rotating and swirling flows is provided in the following subsections:
• Section 1.5.1: Overview of Swirling and Rotating Flows
• Section 1.5.2: Physics of Swirling and Rotating Flows
For more information about setting up swirling and rotating flows in ANSYS FLUENT,
see Section 9.3: Swirling and Rotating Flows in the separate User’s Guide.
1.5.1
Overview of Swirling and Rotating Flows
Axisymmetric Flows with Swirl or Rotation
As discussed in Section 1.5.1: Overview of Swirling and Rotating Flows, you can solve
a 2D axisymmetric problem that includes the prediction of the circumferential or swirl
velocity. The assumption of axisymmetry implies that there are no circumferential gradients in the flow, but that there may be non-zero circumferential velocities. Examples
of axisymmetric flows involving swirl or rotation are depicted in Figures 1.5.1 and 1.5.2.
Your problem may be axisymmetric with respect to geometry and flow conditions but
still include swirl or rotation. In this case, you can model the flow in 2D (i.e., solve
Release 12.0 c ANSYS, Inc. January 29, 2009
1-11
Basic Fluid Flow
Rotating Cover
Ω
Region to
be modeled
x
y
Figure 1.5.1: Rotating Flow in a Cavity
Region to be modeled
Ω
Figure 1.5.2: Swirling Flow in a Gas Burner
1-12
Release 12.0 c ANSYS, Inc. January 29, 2009
1.5 Swirling and Rotating Flows
the axisymmetric problem) and include the prediction of the circumferential (or swirl)
velocity. It is important to note that while the assumption of axisymmetry implies
that there are no circumferential gradients in the flow, there may still be non-zero swirl
velocities.
Momentum Conservation Equation for Swirl Velocity
The tangential momentum equation for 2D swirling flows may be written as
"
#
"
1 ∂
1 ∂
1 ∂
∂w
1 ∂
∂
∂
(ρw)+
(rρuw)+
(rρvw) =
rµ
+ 2
r3 µ
∂t
r ∂x
r ∂r
r ∂x
∂x
r ∂r
∂r
w
r
#
−ρ
vw
(1.5-1)
r
where x is the axial coordinate, r is the radial coordinate, u is the axial velocity, v is the
radial velocity, and w is the swirl velocity.
Three-Dimensional Swirling Flows
When there are geometric changes and/or flow gradients in the circumferential direction,
your swirling flow prediction requires a three-dimensional model. If you are planning a 3D
ANSYS FLUENT model that includes swirl or rotation, you should be aware of the setup
constraints (Section 9.3.3: Coordinate System Restrictions in the separate User’s Guide).
In addition, you may wish to consider simplifications to the problem which might reduce
it to an equivalent axisymmetric problem, especially for your initial modeling effort.
Because of the complexity of swirling flows, an initial 2D study, in which you can quickly
determine the effects of various modeling and design choices, can be very beneficial.
i
For 3D problems involving swirl or rotation, there are no special inputs
required during the problem setup and no special solution procedures.
Note, however, that you may want to use the cylindrical coordinate system for defining velocity-inlet boundary condition inputs, as described in
Section 7.3.4: Defining the Velocity in the separate User’s Guide. Also,
you may find the gradual increase of the rotational speed (set as a wall or
inlet boundary condition) helpful during the solution process. For more
information, see Section 9.3.4: Improving Solution Stability by Gradually
Increasing the Rotational or Swirl Speed in the separate User’s Guide.
Release 12.0 c ANSYS, Inc. January 29, 2009
1-13
Basic Fluid Flow
Flows Requiring a Rotating Reference Frame
If your flow involves a rotating boundary which moves through the fluid (e.g., an impeller
blade or a grooved or notched surface), you will need to use a rotating reference frame
to model the problem. Such applications are described in detail in Section 2.2: Flow in
a Rotating Reference Frame. If you have more than one rotating boundary (e.g., several
impellers in a row), you can use multiple reference frames (described in Section 2.3.1: The
Multiple Reference Frame Model) or mixing planes (described in Section 2.3.2: The Mixing Plane Model).
1.5.2
Physics of Swirling and Rotating Flows
In swirling flows, conservation of angular momentum (rw or r2 Ω = constant) tends to
create a free vortex flow, in which the circumferential velocity, w, increases sharply as the
radius, r, decreases (with w finally decaying to zero near r = 0 as viscous forces begin
to dominate). A tornado is one example of a free vortex. Figure 1.5.3 depicts the radial
distribution of w in a typical free vortex.
r
axis
Figure 1.5.3: Typical Radial Distribution of w in a Free Vortex
It can be shown that for an ideal free vortex flow, the centrifugal forces created by the
circumferential motion are in equilibrium with the radial pressure gradient:
∂p
ρw2
=
∂r
r
(1.5-2)
As the distribution of angular momentum in a non-ideal vortex evolves, the form of
this radial pressure gradient also changes, driving radial and axial flows in response to
the highly non-uniform pressures that result. Thus, as you compute the distribution of
swirl in your ANSYS FLUENT model, you will also notice changes in the static pressure
distribution and corresponding changes in the axial and radial flow velocities. It is this
high degree of coupling between the swirl and the pressure field that makes the modeling
of swirling flows complex.
1-14
Release 12.0 c ANSYS, Inc. January 29, 2009
1.5 Swirling and Rotating Flows
In flows that are driven by wall rotation, the motion of the wall tends to impart a forced
vortex motion to the fluid, wherein w/r or Ω is constant. An important characteristic
of such flows is the tendency of fluid with high angular momentum (e.g., the flow near
the wall) to be flung radially outward (Figure 1.5.4). This is often referred to as “radial
pumping”, since the rotating wall is pumping the fluid radially outward.
7.69e-03
6.92e-03
6.15e-03
5.38e-03
4.62e-03
3.85e-03
3.08e-03
2.31e-03
1.54e-03
7.69e-04
0.00e+00
axis of rotation
Contours of Stream Function (kg/s)
Figure 1.5.4: Stream Function Contours for Rotating Flow in a Cavity (Geometry of Figure 1.5.1)
Release 12.0 c ANSYS, Inc. January 29, 2009
1-15
Basic Fluid Flow
1.6
Compressible Flows
Compressibility effects are encountered in gas flows at high velocity and/or in which there
are large pressure variations. When the flow velocity approaches or exceeds the speed of
sound of the gas or when the pressure change in the system (∆p/p) is large, the variation
of the gas density with pressure has a significant impact on the flow velocity, pressure,
and temperature. Compressible flows create a unique set of flow physics for which you
must be aware of the special input requirements and solution techniques described in
this section. Figures 1.6.1 and 1.6.2 show examples of compressible flows computed
using ANSYS FLUENT.
1.57e+00
1.43e+00
1.29e+00
1.16e+00
1.02e+00
8.82e-01
7.45e-01
6.07e-01
4.70e-01
3.32e-01
1.95e-01
Contours of Mach Number
Figure 1.6.1: Transonic Flow in a Converging-Diverging Nozzle
1-16
Release 12.0 c ANSYS, Inc. January 29, 2009
1.6 Compressible Flows
2.02e+04
1.24e+04
4.68e+03
-3.07e+03
-1.08e+04
-1.86e+04
-2.63e+04
-3.41e+04
-4.18e+04
-4.95e+04
-5.73e+04
Contours of Static Pressure (pascal)
Figure 1.6.2: Mach 0.675 Flow Over a Bump in a 2D Channel
For more information about setting up compressible flows in ANSYS FLUENT, see Section 9.4: Compressible Flows in the separate User’s Guide.
Information about compressible flows is provided in the following subsections:
• Section 1.6.1: When to Use the Compressible Flow Model
• Section 1.6.2: Physics of Compressible Flows
1.6.1
When to Use the Compressible Flow Model
Compressible flows can be characterized by the value of the Mach number:
M ≡ u/c
(1.6-1)
Here, c is the speed of sound in the gas:
c=
q
γRT
(1.6-2)
and γ is the ratio of specific heats (cp /cv ).
When the Mach number is less than 1.0, the flow is termed subsonic. At Mach numbers much less than 1.0 (M < 0.1 or so), compressibility effects are negligible and the
Release 12.0 c ANSYS, Inc. January 29, 2009
1-17
Basic Fluid Flow
variation of the gas density with pressure can safely be ignored in your flow modeling.
As the Mach number approaches 1.0 (which is referred to as the transonic flow regime),
compressibility effects become important. When the Mach number exceeds 1.0, the flow
is termed supersonic, and may contain shocks and expansion fans which can impact the
flow pattern significantly. ANSYS FLUENT provides a wide range of compressible flow
modeling capabilities for subsonic, transonic, and supersonic flows.
1.6.2
Physics of Compressible Flows
Compressible flows are typically characterized by the total pressure p0 and total temperature T0 of the flow. For an ideal gas, these quantities can be related to the static
pressure and temperature by the following:
p0
= exp(
p
R T0
T
Cp
dT
T
R
)
(1.6-3)
For constant Cp , Equation 1.6-3 reduces to
p0
=
p
γ−1 2
1+
M
2
T0
γ−1 2
= 1+
M
T
2
γ/(γ−1)
(1.6-4)
(1.6-5)
These relationships describe the variation of the static pressure and temperature in the
flow as the velocity (Mach number) changes under isentropic conditions. For example,
given a pressure ratio from inlet to exit (total to static), Equation 1.6-4 can be used to
estimate the exit Mach number which would exist in a one-dimensional isentropic flow.
For air, Equation 1.6-4 predicts a choked flow (Mach number of 1.0) at an isentropic
pressure ratio, p/p0 , of 0.5283. This choked flow condition will be established at the
point of minimum flow area (e.g., in the throat of a nozzle). In the subsequent area
expansion the flow may either accelerate to a supersonic flow in which the pressure will
continue to drop, or return to subsonic flow conditions, decelerating with a pressure rise.
If a supersonic flow is exposed to an imposed pressure increase, a shock will occur, with
a sudden pressure rise and deceleration accomplished across the shock.
Basic Equations for Compressible Flows
Compressible flows are described by the standard continuity and momentum equations
solved by ANSYS FLUENT, and you do not need to activate any special physical models (other than the compressible treatment of density as detailed below). The energy
equation solved by ANSYS FLUENT correctly incorporates the coupling between the flow
velocity and the static temperature, and should be activated whenever you are solving
1-18
Release 12.0 c ANSYS, Inc. January 29, 2009
1.7 Inviscid Flows
a compressible flow. In addition, if you are using the pressure-based solver, you should
activate the viscous dissipation terms in Equation 5.2-1, which become important in
high-Mach-number flows.
The Compressible Form of the Gas Law
For compressible flows, the ideal gas law is written in the following form:
ρ=
pop + p
R
T
Mw
(1.6-6)
where pop is the operating pressure defined in the Operating Conditions dialog box,
p is the local static pressure relative to the operating pressure, R is the universal gas
constant, and Mw is the molecular weight. The temperature, T , will be computed from
the energy equation.
1.7
Inviscid Flows
Inviscid flow analyses neglect the effect of viscosity on the flow and are appropriate for
high-Reynolds-number applications where inertial forces tend to dominate viscous forces.
One example for which an inviscid flow calculation is appropriate is an aerodynamic
analysis of some high-speed projectile. In a case like this, the pressure forces on the body
will dominate the viscous forces. Hence, an inviscid analysis will give you a quick estimate
of the primary forces acting on the body. After the body shape has been modified to
maximize the lift forces and minimize the drag forces, you can perform a viscous analysis
to include the effects of the fluid viscosity and turbulent viscosity on the lift and drag
forces.
Another area where inviscid flow analyses are routinely used is to provide a good initial solution for problems involving complicated flow physics and/or complicated flow
geometry. In a case like this, the viscous forces are important, but in the early stages of
the calculation the viscous terms in the momentum equations will be ignored. Once the
calculation has been started and the residuals are decreasing, you can turn on the viscous
terms (by enabling laminar or turbulent flow) and continue the solution to convergence.
For some very complicated flows, this is the only way to get the calculation started.
For more information about setting up inviscid flows in ANSYS FLUENT, see Section 9.5: Inviscid Flows in the separate User’s Guide.
Information about inviscid flows is provided in the following subsections:
• Section 1.7.1: Euler Equations
Release 12.0 c ANSYS, Inc. January 29, 2009
1-19
Basic Fluid Flow
1.7.1
Euler Equations
For inviscid flows, ANSYS FLUENT solves the Euler equations. The mass conservation
equation is the same as for a laminar flow, but the momentum and energy conservation
equations are reduced due to the absence of molecular diffusion.
In this section, the conservation equations for inviscid flow in an inertial (non-rotating)
reference frame are presented. The equations that are applicable to non-inertial reference
frames are described in Chapter 2: Flows with Rotating Reference Frames. The conservation equations relevant for species transport and other models will be discussed in the
chapters where those models are described.
The Mass Conservation Equation
The equation for conservation of mass, or continuity equation, can be written as follows:
∂ρ
+ ∇ · (ρ~v ) = Sm
∂t
(1.7-1)
Equation 1.7-1 is the general form of the mass conservation equation and is valid for
incompressible as well as compressible flows. The source Sm is the mass added to the
continuous phase from the dispersed second phase (e.g., due to vaporization of liquid
droplets) and any user-defined sources.
For 2D axisymmetric geometries, the continuity equation is given by
∂ρ
∂
∂
ρvr
+
(ρvx ) + (ρvr ) +
= Sm
∂t ∂x
∂r
r
(1.7-2)
where x is the axial coordinate, r is the radial coordinate, vx is the axial velocity, and vr
is the radial velocity.
Momentum Conservation Equations
Conservation of momentum is described by
∂
(ρ~v ) + ∇ · (ρ~v~v ) = −∇p + ρ~g + F~
∂t
(1.7-3)
where p is the static pressure and ρ~g and F~ are the gravitational body force and external
body forces (e.g., forces that arise from interaction with the dispersed phase), respectively.
F~ also contains other model-dependent source terms such as porous-media and userdefined sources.
1-20
Release 12.0 c ANSYS, Inc. January 29, 2009
1.7 Inviscid Flows
For 2D axisymmetric geometries, the axial and radial momentum conservation equations
are given by
∂
1 ∂
1 ∂
∂p
(ρvx ) +
(rρvx vx ) +
(rρvr vx ) = −
+ Fx
∂t
r ∂x
r ∂r
∂x
(1.7-4)
∂
1 ∂
1 ∂
∂p
(ρvr ) +
(rρvx vr ) +
(rρvr vr ) = − + Fr
∂t
r ∂x
r ∂r
∂r
(1.7-5)
and
where
∇ · ~v =
∂vx ∂vr vr
+
+
∂x
∂r
r
(1.7-6)
Energy Conservation Equation
Conservation of energy is described by
X
∂
(ρE) + ∇ · (~v (ρE + p)) = −∇ · hj Jj + Sh
∂t
j
Release 12.0 c ANSYS, Inc. January 29, 2009
(1.7-7)
1-21
Basic Fluid Flow
1-22
Release 12.0 c ANSYS, Inc. January 29, 2009
Chapter 2.
Flows with Rotating Reference Frames
This chapter describes the theoretical background modeling flows in rotating reference
frames. The information in this chapter is presented in the following sections:
• Section 2.1: Introduction
• Section 2.2: Flow in a Rotating Reference Frame
• Section 2.3: Flow in Multiple Rotating Reference Frames
2.1
Introduction
ANSYS FLUENT solves the equations of fluid flow and heat transfer, by default, in a
stationary (or inertial) reference frame. However, there are many problems where it is
advantageous to solve the equations in a moving (or non-inertial) reference frame. Such
problems typically involve moving parts (such as rotating blades, impellers, and similar
types of moving surfaces), and it is the flow around these moving parts that is of interest.
In most cases, the moving parts render the problem unsteady when viewed from the
stationary frame. With a moving reference frame, however, the flow around the moving
part can (with certain restrictions) be modeled as a steady-state problem with respect
to the moving frame.
ANSYS FLUENT’s moving reference frame modeling capability allows you to model problems involving moving parts by allowing you to activate moving reference frames in
selected cell zones. When a moving reference frame is activated, the equations of motion are modified to incorporate the additional acceleration terms which occur due to
the transformation from the stationary to the moving reference frame. By solving these
equations in a steady-state manner, the flow around the moving parts can be modeled.
For many problems, it may be possible to refer the entire computational domain to a
single moving reference frame. This is known as the single reference frame (or SRF)
approach. The use of the SRF approach is possible; provided the geometry meets certain
requirements (as discussed in Section 2.2: Flow in a Rotating Reference Frame). For
more complex geometries, it may not be possible to use a single reference frame. In
such cases, you must break up the problem into multiple cell zones, with well-defined
interfaces between the zones. The manner in which the interfaces are treated leads to
two approximate, steady-state modeling methods for this class of problem: the multiple
reference frame (or MRF) approach, and the mixing plane approach. These approaches
Release 12.0 c ANSYS, Inc. January 29, 2009
2-1
Flows with Rotating Reference Frames
will be discussed in Sections 2.3.1 and 2.3.2. If unsteady interaction between the stationary and moving parts is important, you can employ the Sliding Mesh approach to
capture the transient behavior of the flow. The sliding meshing model will be discussed
in Chapter 3: Flows Using Sliding and Deforming Meshes.
outlet
periodic
boundaries
inlet
Figure 2.1.1: Single Component (Blower Wheel Blade Passage)
2.2
Flow in a Rotating Reference Frame
The principal reason for employing a moving reference frame is to render a problem
which is unsteady in the stationary (inertial) frame steady with respect to the moving
frame. For a steadily rotating frame (i.e., the rotational speed is constant), it is possible
to transform the equations of fluid motion to the rotating frame such that steady-state
solutions are possible. By default, ANSYS FLUENT permits the activation of a moving
reference frame with a steady rotational speed. If the rotational speed is not constant,
the transformed equations will contain additional terms which are not included in ANSYS
FLUENT’s formulation (although they can be added as source terms using user-defined
functions). It should also be noted that you can run an unsteady simulation in a moving
reference frame with constant rotational speed. This would be necessary if you wanted
to simulate, for example, vortex shedding from a rotating fan blade. The unsteadiness
in this case is due to a natural fluid instability (vortex generation) rather than induced
from interaction with a stationary component.
The information in this section is presented in the following:
• Section 2.2.1: Equations for a Rotating Reference Frame
• Section 2.2.2: Single Rotating Reference Frame (SRF) Modeling
2-2
Release 12.0 c ANSYS, Inc. January 29, 2009
2.2 Flow in a Rotating Reference Frame
stationary
zone
interface
rotating
zone
Figure 2.1.2: Multiple Component (Blower Wheel and Casing)
2.2.1 Equations for a Rotating Reference Frame
Consider a coordinate system which is rotating steadily with angular velocity ω
~ relative
to a stationary (inertial) reference frame, as illustrated in Figure 2.2.1. The origin of the
rotating system is located by a position vector r~0 .
The axis of rotation is defined by a unit direction vector â such that
ω
~ = ωâ
(2.2-1)
The computational domain for the CFD problem is defined with respect to the rotating
frame such that an arbitrary point in the CFD domain is located by a position vector ~r
from the origin of the rotating frame.
The fluid velocities can be transformed from the stationary frame to the rotating frame
using the following relation:
~vr = ~v − ~ur
(2.2-2)
~ur = ω
~ × ~r
(2.2-3)
where
Release 12.0 c ANSYS, Inc. January 29, 2009
2-3
Flows with Rotating Reference Frames
Figure 2.2.1: Stationary and Rotating Reference Frames
In the above, ~vr is the relative velocity (the velocity viewed from the rotating frame), ~v
is the absolute velocity (the velocity viewed from the stationary frame), and ~ur is the
“whirl” velocity (the velocity due to the moving frame).
When the equations of motion are solved in the rotating reference frame, the acceleration of the fluid is augmented by additional terms that appear in the momentum
equations [17]. Moreover, the equations can be formulated in two different ways:
• Expressing the momentum equations using the relative velocities as dependent variables (known as the relative velocity formulation).
• Expressing the momentum equations using the absolute velocities as dependent
variables in the momentum equations (known as the absolute velocity formulation).
The exact forms of the governing equations for these two formulations will be provided
in the sections below. It can be noted here that ANSYS FLUENT’s pressure-based solvers
provide the option to use either of these two formulations, whereas the density-based
solvers always use the absolute velocity formulation. For more information about the
advantages of each velocity formulation, see Section 10.7.1: Choosing the Relative or
Absolute Velocity Formulation (in the separate User’s Guide).
2-4
Release 12.0 c ANSYS, Inc. January 29, 2009
2.2 Flow in a Rotating Reference Frame
Relative Velocity Formulation
For the relative velocity formulation, the governing equations of fluid flow for a steadily
rotating frame can be written as follows:
Conservation of mass:
∂ρ
+ ∇ · ρ~vr = 0
∂t
(2.2-4)
Conservation of momentum:
∂
(ρ~vr ) + ∇ · (ρ~vr~vr ) + ρ(2~ω × ~vr + ω
~ ×ω
~ × ~r) = −∇p + ∇ · τ r + F~
∂t
(2.2-5)
Conservation of energy:
∂
(ρEr ) + ∇ · (ρ~vr Hr ) = ∇ · (k∇T + τ r · ~vr ) + Sh
∂t
(2.2-6)
The momentum equation contains two additional acceleration terms: the Coriolis acceleration (2~ω ×~vr ), and the centripetal acceleration (~ω ×~ω ×~r). In addition, the viscous stress
(τ r ) is identical to Equation 1.2-4 except that relative velocity derivatives are used. The
energy equation is written in terms of the relative internal energy (Er ) and the relative
total enthalpy (Hr ), also known as the rothalpy. These variables are defined as:
Er = h −
p 1 2
+ (vr − ur 2 )
ρ 2
(2.2-7)
p
ρ
(2.2-8)
Hr = Er +
Absolute Velocity Formulation
For the absolute velocity formulation, the governing equations of fluid flow for a steadily
rotating frame can be written as follows:
Conservation of mass:
∂ρ
+ ∇ · ρ~vr = 0
∂t
(2.2-9)
∂
ρ~v + ∇ · (ρ~vr~v ) + ρ(~ω × ~v ) = −∇p + ∇ · τ + F~
∂t
(2.2-10)
Conservation of momentum:
Release 12.0 c ANSYS, Inc. January 29, 2009
2-5
Flows with Rotating Reference Frames
Conservation of energy:
∂
ρE + ∇ · (ρ~vr H + p~ur ) = ∇ · (k∇T + τ · ~v ) + Sh
∂t
(2.2-11)
In this formulation, the Coriolis and centripetal accelerations can be collapsed into a
single term (~ω × ~v ).
2.2.2 Single Rotating Reference Frame (SRF) Modeling
Many problems permit the entire computational domain to be referred to a single rotating
reference frame (hence the name SRF modeling). In such cases, the equations given in
Section 2.2.1: Equations for a Rotating Reference Frame are solved in all fluid cell zones.
Steady-state solutions are possible in SRF models provided suitable boundary conditions
are prescribed. In particular, wall boundaries must adhere to the following requirements:
• Any walls which are moving with the reference frame can assume any shape. An
example would be the blade surfaces associated with a pump impeller. The no slip
condition is defined in the relative frame such that the relative velocity is zero on
the moving walls.
• Walls can be defined which are non-moving with respect to the stationary coordinate system, but these walls must be surfaces of revolution about the axis of
rotation. Here the so slip condition is defined such that the absolute velocity is
zero on the walls. An example of this type of boundary would be a cylindrical wind
tunnel wall which surrounds a rotating propeller.
Rotationally periodic boundaries may also be used, but the surface must be periodic
about the axis of rotation. As an example, it is very common to model flow through a
blade row on a turbomachine by assuming the flow to be rotationally periodic and using
a periodic domain about a single blade. This permits good resolution of the flow around
the blade without the expense of modeling all blades in the blade row (see Figure 2.2.2).
Flow boundary conditions in ANSYS FLUENT (inlets and outlets) can, in most cases, be
prescribed in either the stationary or rotating frames. For example, for a velocity inlet,
one can specify either the relative velocity or absolute velocity, depending on which is
more convenient. For additional information on these and other boundary conditions, see
Section 10.7: Setting Up a Single Rotating Reference Frame Problem and Chapter 7: Cell
Zone and Boundary Conditions in the separate User’s Guide.
2-6
Release 12.0 c ANSYS, Inc. January 29, 2009
2.2 Flow in a Rotating Reference Frame
Figure 2.2.2: Single Blade Model with Rotationally Periodic Boundaries
Release 12.0 c ANSYS, Inc. January 29, 2009
2-7
Flows with Rotating Reference Frames
2.3
Flow in Multiple Rotating Reference Frames
Many problems involve multiple moving parts or contain stationary surfaces which are
not surfaces of revolution (and therefore cannot be used with the Single Reference Frame
modeling approach). For these problems, you must break up the model into multiple
fluid/solid cell zones, with interface boundaries separating the zones. Zones which contain
the moving components can then be solved using the moving reference frame equations
(Section 2.2.1: Equations for a Rotating Reference Frame), whereas stationary zones can
be solved with the stationary frame equations. The manner in which the equations are
treated at the interface lead to two approaches which are supported in ANSYS FLUENT:
• Multiple Rotating Reference Frames
– Multiple Reference Frame model (MRF) (see Section 2.3.1: The Multiple Reference Frame Model)
– Mixing Plane Model (MPM) (see Section 2.3.2: The Mixing Plane Model)
• Sliding Mesh Model (SMM)
Both the MRF and mixing plane approaches are steady-state approximations, and differ
primarily in the manner in which conditions at the interfaces are treated. These approaches will be discussed in the sections below. The sliding mesh model approach is,
on the other hand, inherently unsteady due to the motion of the mesh with time. This
approach is discussed in Chapter 3: Flows Using Sliding and Deforming Meshes.
2.3.1
The Multiple Reference Frame Model
Overview
The MRF model [209] is, perhaps, the simplest of the two approaches for multiple zones.
It is a steady-state approximation in which individual cell zones can be assigned different
rotational and/or translational speeds. The flow in each moving cell zone is solved using
the moving reference frame equations (see Section 2.2: Flow in a Rotating Reference
Frame). If the zone is stationary (ω = 0), the equations reduce to their stationary forms.
At the interfaces between cell zones, a local reference frame transformation is performed
to enable flow variables in one zone to be used to calculate fluxes at the boundary of
the adjacent zone. The MRF interface formulation will be discussed in more detail in
Section 2.3.1: The MRF Interface Formulation.
It should be noted that the MRF approach does not account for the relative motion of
a moving zone with respect to adjacent zones (which may be moving or stationary); the
mesh remains fixed for the computation. This is analogous to freezing the motion of the
moving part in a specific position and observing the instantaneous flowfield with the rotor
in that position. Hence, the MRF is often referred to as the “frozen rotor approach.”
2-8
Release 12.0 c ANSYS, Inc. January 29, 2009
2.3 Flow in Multiple Rotating Reference Frames
While the MRF approach is clearly an approximation, it can provide a reasonable model
of the flow for many applications. For example, the MRF model can be used for turbomachinery applications in which rotor-stator interaction is relatively weak, and the flow
is relatively uncomplicated at the interface between the moving and stationary zones.
In mixing tanks, for example, since the impeller-baffle interactions are relatively weak,
large-scale transient effects are not present and the MRF model can be used.
Another potential use of the MRF model is to compute a flow field that can be used as
an initial condition for a transient sliding mesh calculation. This eliminates the need for
a startup calculation. The multiple reference frame model should not be used, however,
if it is necessary to actually simulate the transients that may occur in strong rotor-stator
interactions, the sliding mesh model alone should be used (see Section 3.2: Sliding Mesh
Theory).
Examples
For a mixing tank with a single impeller, you can define a rotating reference frame that
encompasses the impeller and the flow surrounding it, and use a stationary frame for
the flow outside the impeller region. An example of this configuration is illustrated in
Figure 2.3.1. (The dashes denote the interface between the two reference frames.) Steadystate flow conditions are assumed at the interface between the two reference frames. That
is, the velocity at the interface must be the same (in absolute terms) for each reference
frame. The mesh does not move.
You can also model a problem that includes more than one rotating reference frame.
Figure 2.3.2 shows a geometry that contains two rotating impellers side by side. This
problem would be modeled using three reference frames: the stationary frame outside
both impeller regions and two separate rotating reference frames for the two impellers.
(As noted above, the dashes denote the interfaces between reference frames.)
The MRF Interface Formulation
The MRF formulation that is applied to the interfaces will depend on the velocity formulation being used. The specific approaches will be discussed below for each case. It
should be noted that the interface treatment applies to the velocity and velocity gradients, since these vector quantities change with a change in reference frame. Scalar
quantities, such as temperature, pressure, density, turbulent kinetic energy, etc., do not
require any special treatment, and thus are passed locally without any change.
Release 12.0 c ANSYS, Inc. January 29, 2009
2-9
Flows with Rotating Reference Frames
Figure 2.3.1: Geometry with One Rotating Impeller
Figure 2.3.2: Geometry with Two Rotating Impellers
2-10
Release 12.0 c ANSYS, Inc. January 29, 2009
2.3 Flow in Multiple Rotating Reference Frames
Interface Treatment: Relative Velocity Formulation
In ANSYS FLUENT’s implementation of the MRF model, the calculation domain is divided into subdomains, each of which may be rotating and/or translating with respect
to the laboratory (inertial) frame. The governing equations in each subdomain are written with respect to that subdomain’s reference frame. Thus, the flow in stationary and
translating subdomains is governed by the equations in Section 1.2: Continuity and Momentum Equations, while the flow in rotating subdomains is governed by the equations
presented in Section 2.2.1: Equations for a Rotating Reference Frame.
At the boundary between two subdomains, the diffusion and other terms in the governing
equations in one subdomain require values for the velocities in the adjacent subdomain
(see Figure 2.3.3). ANSYS FLUENT enforces the continuity of the absolute velocity, ~v , to
provide the correct neighbor values of velocity for the subdomain under consideration.
(This approach differs from the mixing plane approach described in Section 2.3.2: The
Mixing Plane Model, where a circumferential averaging technique is used.)
When the relative velocity formulation is used, velocities in each subdomain are computed
relative to the motion of the subdomain. Velocities and velocity gradients are converted
from a moving reference frame to the absolute inertial frame using Equation 2.3-1.
For a translational velocity v~t , we have
~v = ~vr + (~ω × ~r) + ~vt
(2.3-1)
From Equation 2.3-1, the gradient of the absolute velocity vector can be shown to be
∇~v = ∇~vr + ∇ (~ω × ~r)
(2.3-2)
Note that scalar quantities such as density, static pressure, static temperature, species
mass fractions, etc., are simply obtained locally from adjacent cells.
Release 12.0 c ANSYS, Inc. January 29, 2009
2-11
Flows with Rotating Reference Frames
stationary zone
v, v
interface
vr , vr
All velocities converted to
absolute frame and applied
to interface along with local
scalars.
rotating zone
Figure 2.3.3: Interface Treatment for the MRF Model
2-12
Release 12.0 c ANSYS, Inc. January 29, 2009
2.3 Flow in Multiple Rotating Reference Frames
Interface Treatment: Absolute Velocity Formulation
When the absolute velocity formulation is used, the governing equations in each subdomain are written with respect to that subdomain’s reference frame, but the velocities
are stored in the absolute frame. Therefore, no special transformation is required at the
interface between two subdomains. Again, scalar quantities are determined locally from
adjacent cells.
2.3.2
The Mixing Plane Model
The mixing plane model in ANSYS FLUENT provides an alternative to the multiple
reference frame and sliding mesh models for simulating flow through domains with one
or more regions in relative motion. This section provides a brief overview of the model
and a list of its limitations.
Overview
As discussed in Section 2.3.1: The Multiple Reference Frame Model, the MRF model
is applicable when the flow at the interface between adjacent moving/stationary zones
is nearly uniform (“mixed out”). If the flow at this interface is not uniform, the MRF
model may not provide a physically meaningful solution. The sliding mesh model (see Section 3.2: Sliding Mesh Theory) may be appropriate for such cases, but in many situations
it is not practical to employ a sliding mesh. For example, in a multistage turbomachine,
if the number of blades is different for each blade row, a large number of blade passages
is required in order to maintain circumferential periodicity. Moreover, sliding mesh calculations are necessarily unsteady, and thus require significantly more computation to
achieve a final, time-periodic solution. For situations where using the sliding mesh model
is not feasible, the mixing plane model can be a cost-effective alternative.
In the mixing plane approach, each fluid zone is treated as a steady-state problem.
Flow-field data from adjacent zones are passed as boundary conditions that are spatially
averaged or “mixed” at the mixing plane interface. This mixing removes any unsteadiness
that would arise due to circumferential variations in the passage-to-passage flow field
(e.g., wakes, shock waves, separated flow), thus yielding a steady-state result. Despite
the simplifications inherent in the mixing plane model, the resulting solutions can provide
reasonable approximations of the time-averaged flow field.
Release 12.0 c ANSYS, Inc. January 29, 2009
2-13
Flows with Rotating Reference Frames
Rotor and Stator Domains
Consider the turbomachine stages shown schematically in Figures 2.3.4 and 2.3.5, each
blade passage contains periodic boundaries. Figure 2.3.4 shows a constant radial plane
within a single stage of an axial machine, while Figure 2.3.5 shows a constant θ plane
within a mixed-flow device. In each case, the stage consists of two flow domains: the
rotor domain, which is rotating at a prescribed angular velocity, followed by the stator
domain, which is stationary. The order of the rotor and stator is arbitrary (that is, a
situation where the rotor is downstream of the stator is equally valid).
rotor
stator
rotor outlet: ps α r α t α z
stator inlet: p0 α r αt α z k ε
Rθ
x
mixing plane interface
Figure 2.3.4: Axial Rotor-Stator Interaction (Schematic Illustrating the Mixing Plane Concept)
In a numerical simulation, each domain will be represented by a separate mesh. The
flow information between these domains will be coupled at the mixing plane interface
(as shown in Figures 2.3.4 and 2.3.5) using the mixing plane model. Note that you may
couple any number of fluid zones in this manner; for example, four blade passages can
be coupled using three mixing planes.
i
2-14
Note that the stator and rotor passages are separate cell zones, each with
their own inlet and outlet boundaries. You can think of this system as a
set of SRF models for each blade passage coupled by boundary conditions
supplied by the mixing plane model.
Release 12.0 c ANSYS, Inc. January 29, 2009
2.3 Flow in Multiple Rotating Reference Frames
stator
stator inlet:
p α α α k ε
0 r t z
mixing plane
r
interface
x
rotor outlet:
p α α α
s r t z
rotor
Ω
Figure 2.3.5: Radial Rotor-Stator Interaction (Schematic Illustrating the
Mixing Plane Concept)
Release 12.0 c ANSYS, Inc. January 29, 2009
2-15
Flows with Rotating Reference Frames
The Mixing Plane Concept
The essential idea behind the mixing plane concept is that each fluid zone is solved
as a steady-state problem. At some prescribed iteration interval, the flow data at the
mixing plane interface are averaged in the circumferential direction on both the stator
outlet and the rotor inlet boundaries. The ANSYS FLUENT implementation gives you the
choice of three types of averaging methods: area-weighted averaging, mass averaging, and
mixed-out averaging. By performing circumferential averages at specified radial or axial
stations, “profiles” of boundary condition flow variables can be defined. These profiles—
which will be functions of either the axial or the radial coordinate, depending on the
orientation of the mixing plane—are then used to update boundary conditions along the
two zones of the mixing plane interface. In the examples shown in Figures 2.3.4 and 2.3.5,
profiles of averaged total pressure (p0 ), direction cosines of the local flow angles in the
radial, tangential, and axial directions (αr , αt , αz ), total temperature (T0 ), turbulence
kinetic energy (k), and turbulence dissipation rate () are computed at the rotor exit
and used to update boundary conditions at the stator inlet. Likewise, a profile of static
pressure (ps ), direction cosines of the local flow angles in the radial, tangential, and axial
directions (αr , αt , αz ), are computed at the stator inlet and used as a boundary condition
on the rotor exit.
Passing profiles in the manner described above assumes specific boundary condition types
have been defined at the mixing plane interface. The coupling of an upstream outlet
boundary zone with a downstream inlet boundary zone is called a “mixing plane pair”.
In order to create mixing plane pairs in ANSYS FLUENT, the boundary zones must be
of the following types:
Upstream
pressure outlet
pressure outlet
pressure outlet
Downstream
pressure inlet
velocity inlet
mass flow inlet
For specific instructions about setting up mixing planes, see Section 10.10.2: Setting Up
the Mixing Plane Model in the separate User’s Guide.
2-16
Release 12.0 c ANSYS, Inc. January 29, 2009
2.3 Flow in Multiple Rotating Reference Frames
Choosing an Averaging Method
Three profile averaging methods are available in the mixing plane model:
• area averaging
• mass averaging
• mixed-out averaging
Area Averaging
Area averaging is the default averaging method and is given by
f=
i
1Z
f dA
A A
(2.3-3)
The pressure and temperature obtained by the area average may not be
representative of the momentum and energy of the flow.
Mass Averaging
Mass averaging is given by
1 Z
f=
f ρV~ · n̂dA
ṁ A
(2.3-4)
where
ṁ =
Z
ρV~ · n̂dA
A
This method provides a better representation of the total quantities than the areaaveraging method. Convergence problems could arise if severe reverse flow is present
at the mixing plane. Therefore, for solution stability purposes, it is best if you initiate
the solution with area averaging, then switch to mass averaging after reverse flow dies
out.
i
Mass averaging averaging is not available with multiphase flows.
Release 12.0 c ANSYS, Inc. January 29, 2009
2-17
Flows with Rotating Reference Frames
Mixed-Out Averaging
The mixed-out averaging method is derived from the conservation of mass, momentum
and energy:
F =
M1 =
M2 =
M3 =
E =
Z
ZA
ZA
ZA
A
ρ(V~ · n̂)dA
ρ(V~ · n̂)udA +
ρ(V~ · n̂)vdA +
ρ(V~ · n̂)wdA +
(2.3-5)
Z
ZA
ZA
P (eˆx · n̂)dA
P (eˆy · n̂)dA
A
P (eˆz · n̂)dA
γR Z
1Z
ρ(V~ · n̂)T dA +
ρ(V~ · n̂)(u2 + v 2 + w2 )dA
(γ − 1) A
2 A
Because it is based on the principals of conservation, the mixed-out average is considered
a better representation of the flow since it reflects losses associated with non-uniformities
in the flow profiles. However, like the mass-averaging method, convergence difficulties
can arise when severe reverse flow is present across the mixing plane. Therefore, it is
best if you initiate the solution with area averaging, then switch to mixed-out averaging
after reverse flow dies out.
Mixed-out averaging assumes that the fluid is a compressible ideal-gas with constant specific heat, Cp .
i
2-18
Mixed-out averaging is not available with multiphase flows.
Release 12.0 c ANSYS, Inc. January 29, 2009
2.3 Flow in Multiple Rotating Reference Frames
ANSYS FLUENT’s Mixing Plane Algorithm
ANSYS FLUENT’s basic mixing plane algorithm can be described as follows:
1. Update the flow field solutions in the stator and rotor domains.
2. Average the flow properties at the stator exit and rotor inlet boundaries, obtaining
profiles for use in updating boundary conditions.
3. Pass the profiles to the boundary condition inputs required for the stator exit and
rotor inlet.
4. Repeat steps 1–3 until convergence.
i
Note that it may be desirable to under-relax the changes in boundary
condition values in order to prevent divergence of the solution (especially
early in the computation). ANSYS FLUENT allows you to control the
under-relaxation of the mixing plane variables.
Mass Conservation
Note that the algorithm described above will not rigorously conserve mass flow across the
mixing plane if it is represented by a pressure outlet and pressure inlet mixing plane pair.
If you use a pressure outlet and mass flow outlet pair instead, ANSYS FLUENT will force
mass conservation across the mixing plane. The basic technique consists of computing
the mass flow rate across the upstream zone (pressure outlet) and adjusting the mass flux
profile applied at the mass flow inlet such that the downstream mass flow matches the
upstream mass flow. This adjustment occurs at every iteration, thus ensuring rigorous
conservation of mass flow throughout the course of the calculation.
i
Note that, since mass flow is being fixed in this case, there will be a jump
in total pressure across the mixing plane. The magnitude of this jump is
usually small compared with total pressure variations elsewhere in the flow
field.
Release 12.0 c ANSYS, Inc. January 29, 2009
2-19
Flows with Rotating Reference Frames
Swirl Conservation
By default, ANSYS FLUENT does not conserve swirl across the mixing plane. For applications such as torque converters, where the sum of the torques acting on the components
should be zero, enforcing swirl conservation across the mixing plane is essential, and is
available in ANSYS FLUENT as a modeling option. Ensuring conservation of swirl is
important because, otherwise, sources or sinks of tangential momentum will be present
at the mixing plane interface.
Consider a control volume containing a stationary or rotating component (e.g., a pump
impeller or turbine vane). Using the moment of momentum equation from fluid mechanics, it can be shown that for steady flow,
T =
ZZ
S
rvθ ρ~v · n̂dS
(2.3-6)
where T is the torque of the fluid acting on the component, r is the radial distance from
the axis of rotation, vθ is the absolute tangential velocity, ~v is the total absolute velocity,
and S is the boundary surface. (The product rvθ is referred to as swirl.)
For a circumferentially periodic domain, with well-defined inlet and outlet boundaries,
Equation 2.3-6 becomes
T =
ZZ
outlet
rvθ ρ~v · n̂dS +
ZZ
inlet
rvθ ρ~v · n̂dS
(2.3-7)
where inlet and outlet denote the inlet and outlet boundary surfaces.
Now consider the mixing plane interface to have a finite streamwise thickness. Applying
Equation 2.3-7 to this zone and noting that, in the limit as the thickness shrinks to zero,
the torque should vanish, the equation becomes
ZZ
downstream
rvθ ρ~v · n̂dS =
ZZ
upstream
rvθ ρ~v · n̂dS
(2.3-8)
where upstream and downstream denote the upstream and downstream sides of the
mixing plane interface. Note that Equation 2.3-8 applies to the full area (360 degrees)
at the mixing plane interface.
Equation 2.3-8 provides a rational means of determining the tangential velocity component. That is, ANSYS FLUENT computes a profile of tangential velocity and then
uniformly adjusts the profile such that the swirl integral is satisfied. Note that interpolating the tangential (and radial) velocity component profiles at the mixing plane does
not affect mass conservation because these velocity components are orthogonal to the
face-normal velocity used in computing the mass flux.
2-20
Release 12.0 c ANSYS, Inc. January 29, 2009
2.3 Flow in Multiple Rotating Reference Frames
Total Enthalpy Conservation
By default, ANSYS FLUENT does not conserve total enthalpy across the mixing plane. For
some applications, total enthalpy conservation across the mixing plane is very desirable,
because global parameters such as efficiency are directly related to the change in total
enthalpy across a blade row or stage. This is available in ANSYS FLUENT as a modeling
option.
The procedure for ensuring conservation of total enthalpy simply involves adjusting the
downstream total temperature profile such that the integrated total enthalpy matches
the upstream integrated total enthalpy. For multiphase flows, conservation of mass, swirl,
and enthalpy are calculated for each phase. However, for the Eulerian multiphase model,
since mass flow inlets are not permissible, conservation of the above quantities does not
occur.
Release 12.0 c ANSYS, Inc. January 29, 2009
2-21
Flows with Rotating Reference Frames
2-22
Release 12.0 c ANSYS, Inc. January 29, 2009
Chapter 3.
Flows Using Sliding and Deforming Meshes
This chapter describes the theoretical background of the sliding and dynamic mesh models in ANSYS FLUENT. To learn more about using sliding meshes in ANSYS FLUENT, see
Section 11.2: Using Sliding Meshes in the separate User’s Guide. Also, for more information about using dynamic meshes in ANSYS FLUENT, see Section 11.3: Using Dynamic
Meshes in the separate User’s Guide.
Theoretical information about sliding and deforming mesh models is presented in the
following sections:
• Section 3.1: Introduction
• Section 3.2: Sliding Mesh Theory
• Section 3.3: Dynamic Mesh Theory
3.1
Introduction
In sliding meshes, the relative motion of stationary and rotating components in a rotating
machine will give rise to unsteady interactions. These interactions are illustrated in
Figure 3.1.1, and generally classified as follows:
• Potential interactions: flow unsteadiness due to pressure waves which propagate
both upstream and downstream.
• Wake interactions: flow unsteadiness due to wakes from upstream blade rows, convecting downstream.
• Shock interactions: for transonic/supersonic flow unsteadiness due to shock waves
striking the downstream blade row.
Where the multiple reference frame (MRF) and mixing plane (MP) models, discussed
in Chapter 2: Flows with Rotating Reference Frames, are models that are applied to
steady-state cases, thus neglecting unsteady interactions, the sliding mesh model cannot
neglect unsteady interactions. The sliding mesh model accounts for the relative motion
of stationary and rotating components.
Release 12.0 c ANSYS, Inc. January 29, 2009
3-1
Flows Using Sliding and Deforming Meshes
Figure 3.1.1: Illustration of Unsteady Interactions
The dynamic mesh model uses the ANSYS FLUENT solver to move boundaries and/or
objects, and to adjust the mesh accordingly. The dynamic mesh model is used when
boundaries move rigidly (linear or rotating) with respect to each other. For example
• A piston moving with respect to an engine cylinder.
• A flap moving with respect to an airplane wing.
The dynamic mesh model can also be used when boundaries deform or deflect. For
example
• A balloon that is being inflated.
• An artificial wall responding to the pressure pulse from the heart.
3-2
Release 12.0 c ANSYS, Inc. January 29, 2009
3.1 Introduction
Conservation Equations
With respect to dynamic meshes, the integral form of the conservation equation for a
general scalar, φ, on an arbitrary control volume, V , whose boundary is moving can be
written as
Z
Z
Z
d Z
~
~
ρφdV +
ρφ (~u − ~ug ) · dA =
Γ∇φ · dA + Sφ dV
dt V
∂V
∂V
V
where
(3.1-1)
ρ is the fluid density
~u is the flow velocity vector
~ug is the mesh velocity of the moving mesh
Γ is the diffusion coefficient
Sφ is the source term of φ
Here ∂V is used to represent the boundary of the control volume V .
The time derivative term in Equation 3.1-1 can be written, using a first-order backward
difference formula, as
(ρφV )n+1 − (ρφV )n
d Z
ρφdV =
dt V
∆t
(3.1-2)
where n and n + 1 denote the respective quantity at the current and next time level. The
(n + 1)th time level volume V n+1 is computed from
V n+1 = V n +
dV
∆t
dt
(3.1-3)
where dV /dt is the volume time derivative of the control volume. In order to satisfy the
mesh conservation law, the volume time derivative of the control volume is computed
from
n
Z
f
X
dV
~=
~j
=
~ug · dA
~ug,j · A
dt
∂V
j
(3.1-4)
~ j is the j face area vector.
where nf is the number of faces on the control volume and A
~ j on each control volume face is calculated from
The dot product ~ug,j · A
~ j = δVj
~ug,j · A
∆t
(3.1-5)
where δVj is the volume swept out by the control volume face j over the time step ∆t.
Release 12.0 c ANSYS, Inc. January 29, 2009
3-3
Flows Using Sliding and Deforming Meshes
In the case of the sliding mesh, the motion of moving zones is tracked relative to the
stationary frame. Therefore, no moving reference frames are attached to the computational domain, simplifying the flux transfers across the interfaces. In the sliding mesh
formulation, the control volume remains constant, therefore from Equation 3.1-3, dV
=0
dt
n+1
n
and V
= V . Equation 3.1-2 can now be expressed as follows:
d Z
[(ρφ)n+1 − (ρφ)n ]V
ρφdV =
dt V
∆t
3.2
(3.1-6)
Sliding Mesh Theory
When a time-accurate solution for rotor-stator interaction (rather than a time-averaged
solution) is desired, you must use the sliding mesh model to compute the unsteady flow
field. As mentioned in Section 2.1: Introduction, the sliding mesh model is the most
accurate method for simulating flows in multiple moving reference frames, but also the
most computationally demanding.
Most often, the unsteady solution that is sought in a sliding mesh simulation is timeperiodic. That is, the unsteady solution repeats with a period related to the speeds of the
moving domains. However, you can model other types of transients, including translating
sliding mesh zones (e.g., two cars or trains passing in a tunnel, as shown in Figure 3.2.1).
Interface
Figure 3.2.1: Two Passing Trains in a Tunnel
3-4
Release 12.0 c ANSYS, Inc. January 29, 2009
3.2 Sliding Mesh Theory
Note that for flow situations where there is no interaction between stationary and moving
parts (i.e., when there is only a rotor), it is more efficient to use a rotating reference frame.
(See Section 2.2: Flow in a Rotating Reference Frame for details.) When transient rotorstator interaction is desired (as in the examples in Figures 3.2.2 and 3.2.3), you must use
sliding meshes. If you are interested in a steady approximation of the interaction, you
may use the multiple reference frame model or the mixing plane model, as described in
Sections 2.3.1 and 2.3.2.
stationary
vanes
rotating
blades
flow
direction of
motion
Figure 3.2.2: Rotor-Stator Interaction (Stationary Guide Vanes with Rotating Blades)
Release 12.0 c ANSYS, Inc. January 29, 2009
3-5
Flows Using Sliding and Deforming Meshes
Interface
Figure 3.2.3: Blower
The Sliding Mesh Technique
In the sliding mesh technique two or more cell zones are used. (If you generate the mesh
in each zone independently, you will need to merge the mesh files prior to starting the
calculation, as described in Section 6.3.15: Reading Multiple Mesh/Case/Data Files in
the separate User’s Guide.) Each cell zone is bounded by at least one “interface zone”
where it meets the opposing cell zone. The interface zones of adjacent cell zones are
associated with one another to form a “mesh interface.” The two cell zones will move
relative to each other along the mesh interface.
During the calculation, the cell zones slide (i.e., rotate or translate) relative to one another
along the mesh interface in discrete steps. Figures 3.2.4 and 3.2.5 show the initial position
of two meshes and their positions after some translation has occurred.
As the rotation or translation takes place, node alignment along the mesh interface is
not required. Since the flow is inherently unsteady, a time-dependent solution procedure
is required.
3-6
Release 12.0 c ANSYS, Inc. January 29, 2009
3.2 Sliding Mesh Theory
Figure 3.2.4: Initial Position of the Meshes
Figure 3.2.5: Rotor Mesh Slides with Respect to the Stator
Release 12.0 c ANSYS, Inc. January 29, 2009
3-7
Flows Using Sliding and Deforming Meshes
Mesh Interface Shapes
The mesh interface and the associated interface zones can be any shape, provided that the
two interface boundaries are based on the same geometry. Figure 3.2.6 shows an example
with a linear mesh interface and Figure 3.2.7 shows a circular-arc mesh interface. (In
both figures, the mesh interface is designated by a dashed line.)
Figure 3.2.6: 2D Linear Mesh Interface
If Figure 3.2.6 was extruded to 3D, the resulting sliding interface would be a planar
rectangle; if Figure 3.2.7 was extruded to 3D, the resulting interface would be a cylinder.
Figure 3.2.8 shows an example that would use a conical mesh interface. (The slanted,
dashed lines represent the intersection of the conical interface with a 2D plane.)
For an axial rotor/stator configuration, in which the rotating and stationary parts are
3-8
Release 12.0 c ANSYS, Inc. January 29, 2009
3.2 Sliding Mesh Theory
Figure 3.2.7: 2D Circular-Arc Mesh Interface
Figure 3.2.8: 3D Conical Mesh Interface
Release 12.0 c ANSYS, Inc. January 29, 2009
3-9
Flows Using Sliding and Deforming Meshes
aligned axially instead of being concentric (see Figure 3.2.9), the interface will be a planar
sector. This planar sector is a cross-section of the domain perpendicular to the axis of
rotation at a position along the axis between the rotor and the stator.
portion of domain being modeled
planar sector
grid interface
Figure 3.2.9: 3D Planar-Sector Mesh Interface
3.2.1 The Sliding Mesh Concept
As discussed in Section 3.2: Sliding Mesh Theory, the sliding mesh model allows adjacent meshes to slide relative to one another. In doing so, the mesh faces do not need
to be aligned on the mesh interface. This situation requires a means of computing the
flux across the two non-conformal interface zones of each mesh interface. For information about how ANSYS FLUENT handles non-conformal interfaces, see Section 6.4: NonConformal Meshes in the separate User’s Guide.
3-10
Release 12.0 c ANSYS, Inc. January 29, 2009
3.3 Dynamic Mesh Theory
3.3
Dynamic Mesh Theory
The dynamic mesh model in ANSYS FLUENT can be used to model flows where the
shape of the domain is changing with time due to motion on the domain boundaries.
The dynamic mesh model can also be used for steady-state applications, where it is
beneficial to move the mesh in the steady-state solver. The motion can be a prescribed
motion (e.g., you can specify the linear and angular velocities about the center of gravity
of a solid body with time) or an unprescribed motion where the subsequent motion
is determined based on the solution at the current time (e.g., the linear and angular
velocities are calculated from the force balance on a solid body, which is what the six
degree of freedom (6DOF) solver does (see Section 11.3.7: Using the Six DOF Solver in
the separate User’s Guide). The update of the volume mesh is handled automatically
by ANSYS FLUENT at each time step based on the new positions of the boundaries.
To use the dynamic mesh model, you need to provide a starting volume mesh and the
description of the motion of any moving zones in the model. ANSYS FLUENT allows you
to describe the motion using either boundary profiles, user-defined functions (UDFs), or
the Six Degree of Freedom solver (6DOF).
ANSYS FLUENT expects the description of the motion to be specified on either face or
cell zones. If the model contains moving and non-moving regions, you need to identify
these regions by grouping them into their respective face or cell zones in the starting
volume mesh that you generate. Furthermore, regions that are deforming due to motion
on their adjacent regions must also be grouped into separate zones in the starting volume
mesh. The boundary between the various regions need not be conformal. You can use the
non-conformal or sliding interface capability in ANSYS FLUENT to connect the various
zones in the final model.
The information in this section is presented in the following:
• Section 3.3.1: Dynamic Mesh Update Methods
• Section 3.3.2: Six DOF (6DOF) Solver Theory
3.3.1
Dynamic Mesh Update Methods
Three groups of mesh motion methods are available in ANSYS FLUENT to update the
volume mesh in the deforming regions subject to the motion defined at the boundaries:
• smoothing methods
• dynamic layering
• local remeshing methods
Note that you can use ANSYS FLUENT’s dynamic mesh models in conjunction with
hanging node adaption, with the exception of dynamic layering and face remeshing. For
more information on hanging node adaption, see Section 19.1.1: Hanging Node Adaption.
Release 12.0 c ANSYS, Inc. January 29, 2009
3-11
Flows Using Sliding and Deforming Meshes
Spring-Based Smoothing Method
In the spring-based smoothing method, the edges between any two mesh nodes are idealized as a network of interconnected springs. The initial spacings of the edges before
any boundary motion constitute the equilibrium state of the mesh. A displacement at
a given boundary node will generate a force proportional to the displacement along all
the springs connected to the node. Using Hook’s Law, the force on a mesh node can be
written as
F~i =
ni
X
kij (∆~xj − ∆~xi )
(3.3-1)
j
where ∆~xi and ∆~xj are the displacements of node i and its neighbor j, ni is the number
of neighboring nodes connected to node i, and kij is the spring constant (or stiffness)
between node i and its neighbor j. The spring constant for the edge connecting nodes i
and j is defined as
1
kij = q
| ~xi − ~xj |
(3.3-2)
At equilibrium, the net force on a node due to all the springs connected to the node must
be zero. This condition results in an iterative equation such that
Pni
∆~xm+1
i
=
j
kij ∆~xm
j
k
ij
j
Pni
(3.3-3)
Since displacements are known at the boundaries (after boundary node positions have
been updated), Equation 3.3-3 is solved using a Jacobi sweep on all interior nodes. At
convergence, the positions are updated such that
~xn+1
= ~xni + ∆~xm,converged
i
i
(3.3-4)
where n + 1 and n are used to denote the positions at the next time step and the current
time step, respectively. The spring-based smoothing is shown in Figures 3.3.1 and 3.3.2
for a cylindrical cell zone where one end of the cylinder is moving.
3-12
Release 12.0 c ANSYS, Inc. January 29, 2009
3.3 Dynamic Mesh Theory
Figure 3.3.1: Spring-Based Smoothing on Interior Nodes: Start
Figure 3.3.2: Spring-Based Smoothing on Interior Nodes: End
Release 12.0 c ANSYS, Inc. January 29, 2009
3-13
Flows Using Sliding and Deforming Meshes
Laplacian Smoothing Method
Laplacian smoothing is the most commonly used and the simplest mesh smoothing
method. This method adjusts the location of each mesh vertex to the geometric center of its neighboring vertices. This method is computationally inexpensive but it does
not guarantee an improvement on mesh quality, since repositioning a vertex by Laplacian smoothing can result in poor quality elements. To overcome this problem, ANSYS
FLUENT only relocates the vertex to the geometric center of its neighboring vertices if
and only if there is an improvement in the mesh quality (i.e., the skewness has been
improved).
This improved Laplacian smoothing can be enabled on deforming boundaries only (i.e.,
the zone with triangular elements in 3D and zones with linear elements in 2D). The
computation of the node positions works as follows:
→
−
xm
i
Pni −
→m
=
xj
j
ni
(3.3-5)
→
→m
−
where −
xm
i is the averaged node position of node i at iteration m, x j is the node position
→
of neighbor node of −
xm
i at iteration m, and ni is the number nodes neighboring node i.
→
The new node position −
x m+1
is then computed as follows:
i
−
→
→
→m
−
x m+1
=−
xm
i
i (1 − β) + x i β
(3.3-6)
where β is the boundary node relaxation factor.
→
This update only happens if the maximum skewness of all faces adjacent to −
x m+1
is
i
m
→
−
improved in comparison to x i .
Boundary Layer Smoothing Method
The boundary layer smoothing method is used to deform the boundary layer during
a moving-deforming mesh simulation. For cases that have a Mesh Motion UDF (see
Section 11.3.9: User-Defined Motion in the separate User’s Guide) applied to a face zone
with adjacent boundary layers, the boundary layer will deform according to the UDF
that is applied to the face zone. This smoothing method preserves the height of each
boundary layer and can be applied to boundary layer zones of all mesh types (wedges
and hexahedra in 3D, quadrilaterals in 2D).
Consider the example below, where a UDF of the form DEFINE_GRID_MOTION provides the
moving-deforming mesh model with the locations of the nodes located on the compliant
strip on an idealized airfoil. The node motion varies sinusoidally (Figures 3.3.5 and
3.3.6), both in time and space as seen by the deformation of the face zone and the
respective boundary layer. A deforming flag is set on the adjacent cell zone, such that
the cells adjacent to the deforming wall will also be deformed, in order to avoid skewness.
3-14
Release 12.0 c ANSYS, Inc. January 29, 2009
3.3 Dynamic Mesh Theory
Compare the original mesh (Figure 3.3.3) prior to applying the Mesh Motion UDF to that
mesh whose boundary layer has been deformed (Figure 3.3.5).
Figure 3.3.3: The Mesh Prior to Applying Boundary Layer Smoothing
To find out how to set up a deforming boundary layer for smoothing, see Section 11.3.9: Specifying Boundary Layer Deformation Smoothing (in the separate User’s Guide).
Dynamic Layering Method
In prismatic (hexahedral and/or wedge) mesh zones, you can use dynamic layering to add
or remove layers of cells adjacent to a moving boundary, based on the height of the layer
adjacent to the moving surface. The dynamic mesh model in ANSYS FLUENT allows you
to specify an ideal layer height on each moving boundary. The layer of cells adjacent to
the moving boundary (layer j in Figure 3.3.7) is split or merged with the layer of cells
next to it (layer i in Figure 3.3.7) based on the height (h) of the cells in layer j.
Release 12.0 c ANSYS, Inc. January 29, 2009
3-15
Flows Using Sliding and Deforming Meshes
Figure 3.3.4: Zooming into the Mesh of the Compliant Strip Prior to Applying Boundary Layer Smoothing
3-16
Release 12.0 c ANSYS, Inc. January 29, 2009
3.3 Dynamic Mesh Theory
Figure 3.3.5: The Mesh After Applying Boundary Layer Smoothing
Release 12.0 c ANSYS, Inc. January 29, 2009
3-17
Flows Using Sliding and Deforming Meshes
Figure 3.3.6: Zooming into the Deformed Boundary Layer of the Compliant
Strip
Layer i
Layer j
h
Moving
boundary
Figure 3.3.7: Dynamic Layering
3-18
Release 12.0 c ANSYS, Inc. January 29, 2009
3.3 Dynamic Mesh Theory
If the cells in layer j are expanding, the cell heights are allowed to increase until
hmin > (1 + αs )hideal
(3.3-7)
where hmin is the minimum cell height of cell layer j, hideal is the ideal cell height, and
αs is the layer split factor. Note that ANSYS FLUENT allows you to define hideal as
either a constant value or a value that varies as a function of time or crank angle. When
the condition in Equation 3.3-7 is met, the cells are split based on the specified layering
option. This option can be height based or ratio based.
With the height-based option, the cells are split to create a layer of cells with constant
height hideal and a layer of cells of height h − hideal . With the ratio-based option, the
cells are split such that locally, the ratio of the new cell heights is exactly αs everywhere.
Figures 3.3.8 and 3.3.9 show the result of splitting a layer of cells above a valve geometry
using the height-based and ratio-based option.
Figure 3.3.8: Results of Splitting Layer with the Height-Based Option
If the cells in layer j are being compressed, they can be compressed until
hmin < αc hideal
(3.3-8)
where αc is the layer collapse factor. When this condition is met, the compressed layer
of cells is merged into the layer of cells above the compressed layer; i.e., the cells in layer
j are merged with those in layer i.
Remeshing Methods
On zones with a triangular or tetrahedral mesh, the spring-based smoothing method
(described in Section 3.3.1: Spring-Based Smoothing Method) is normally used. When
Release 12.0 c ANSYS, Inc. January 29, 2009
3-19
Flows Using Sliding and Deforming Meshes
Figure 3.3.9: Results of Splitting Layer with the Ratio-Based Option
the boundary displacement is large compared to the local cell sizes, the cell quality can
deteriorate or the cells can become degenerate. This will invalidate the mesh (e.g., result
in negative cell volumes) and consequently, will lead to convergence problems when the
solution is updated to the next time step.
To circumvent this problem, ANSYS FLUENT agglomerates cells that violate the skewness
or size criteria and locally remeshes the agglomerated cells or faces. If the new cells or
faces satisfy the skewness criterion, the mesh is locally updated with the new cells (with
the solution interpolated from the old cells). Otherwise, the new cells are discarded.
ANSYS FLUENT includes several remeshing methods that include local remeshing, local
face remeshing (for 3D flows only), face region remeshing, and 2.5D surface remeshing (for
3D flows only). The available remeshing methods in ANSYS FLUENT work for triangulartetrahedral zones and mixed zones where the non-triangular/tetrahedral elements are
skipped. The exception is the 2.5D model, where the available remeshing method only
work on wedges extruded from triangular surfaces or hex meshes.
3-20
Release 12.0 c ANSYS, Inc. January 29, 2009
3.3 Dynamic Mesh Theory
Local Remeshing Method
Using the local remeshing method, ANSYS FLUENT marks cells based on cell skewness
and minimum and maximum length scales as well as an optional sizing function.
ANSYS FLUENT evaluates each cell and marks it for remeshing if it meets one or more
of the following criteria:
• It has a skewness that is greater than a specified maximum skewness.
• It is smaller than a specified minimum length scale.
• It is larger than a specified maximum length scale.
• Its height does not meet the specified length scale (at moving face zones, e.g., above
a moving piston).
Face Region Remeshing Method
In addition to remeshing the volume mesh, ANSYS FLUENT also allows triangular and
linear faces on a deforming boundary to be remeshed. ANSYS FLUENT marks deforming
boundary faces for remeshing based on moving and deforming loops of faces.
For face region remeshing, ANSYS FLUENT marks the region of faces on the deforming
boundaries at the moving boundary based on minimum and maximum length scales.
Once marked, ANSYS FLUENT remeshes the faces and the adjacent cells to produce a very
regular mesh on the deforming boundary at the moving boundary (e.g., Figure 3.3.10).
Using this method, ANSYS FLUENT is able to remesh across multiple face zones.
For 3D simulations, ANSYS FLUENT allows remeshing with symmetric boundary conditions, and across multiple face zones which includes preserving features not only between
the different face zones, but also within a face zone. For more information, see Section 3.3.1: Feature Detection.
ANSYS FLUENT automatically extracts loops on the boundary of the face zone whose
nodes are moving or deforming. Consider a simple tetrahedral mesh of a cylinder whose
bottom wall is moving (see Figure 3.3.10). On the deforming boundary, a single loop
is generated at the bottom end of the cylinder (where the nodes are moving). ANSYS
FLUENT analyzes the height of the faces connected to the nodes on the loop and subsequently, splits or merges the faces depending on the specified maximum or minimum
length scale.
If the faces in layer j are expanding, they are allowed to expand until the maximum length
scale is reached. Conversely, if the layer is contracting, they are allowed to contract until
the minimum length scale is reached. When this condition is met, the compressed layer
of faces is merged into the layer of faces above it. The face remeshing is illustrated in
Figure 3.3.12.
Release 12.0 c ANSYS, Inc. January 29, 2009
3-21
Flows Using Sliding and Deforming Meshes
Deforming
boundary
Layer i
Layer j
h
Moving boundary
Figure 3.3.10: Remeshing at a Deforming Boundary
Local Face Remeshing Method
The local face remeshing method only applies to 3D geometries. Using this method,
ANSYS FLUENT marks the faces (and the adjacent cells) on the deforming boundaries
based on the face skewness. Using this method, ANSYS FLUENT is able to remesh locally
at deforming boundaries, however, you are not able to remesh across multiple face zones.
3-22
Release 12.0 c ANSYS, Inc. January 29, 2009
3.3 Dynamic Mesh Theory
Figure 3.3.11: Expanding Cylinder Before Region Face Remeshing
Figure 3.3.12: Expanding Cylinder After Region Face Remeshing
Release 12.0 c ANSYS, Inc. January 29, 2009
3-23
Flows Using Sliding and Deforming Meshes
2.5D Surface Remeshing Method
The 2.5D surface remeshing method only applies to extruded 3D geometries and is similar to local remeshing in two dimensions on a triangular surface mesh (not a mixed
zone). Faces on a deforming boundary are marked for remeshing based on face skewness,
minimum and maximum length scale and an optional sizing function.
Stationary Wall
Moving
Walls
Moving Walls
Figure 3.3.13: Close-Up of 2.5D Extruded Flow Meter Pump Geometry Before Remeshing and Laplacian Smoothing
3-24
Release 12.0 c ANSYS, Inc. January 29, 2009
3.3 Dynamic Mesh Theory
Remeshed Areas
Figure 3.3.14: Close-Up of 2.5D Extruded Flow Meter Pump Geometry After
Remeshing and Laplacian Smoothing
Release 12.0 c ANSYS, Inc. January 29, 2009
3-25
Flows Using Sliding and Deforming Meshes
Local Remeshing Based on Size Functions
Instead of marking cells based on minimum and maximum length scales, ANSYS FLUENT
can also mark cells based on the size distribution generated by sizing functions.
Local remeshing using size functions can be used with the following remeshing methods:
• local remeshing
• 2.5D surface remeshing
Figure 3.3.16 demonstrates the advantages of using size functions for local remeshing:
In determining the sizing function, ANSYS FLUENT draws a bounding box around the
zone that is approximately twice the size of the zone, and locates the shortest feature
length within each fluid zone. ANSYS FLUENT then subdivides the bounding box based
on the shortest feature length and the Size Function Resolution that you specify. This
allows ANSYS FLUENT to create a background mesh.
You control the resolution of the background mesh and a background mesh is created
for each fluid zone. The shortest feature length is determined by shrinking a second box
around the object, and then selecting the shortest edge on that box. The size function
is evaluated at the vertex of each individual background mesh.
As seen in Figure 3.3.17, the local value of the size function SFI is defined by
SFI =
Σ D1J ∆sJ
Σ D1J
(3.3-9)
where DJ is the distance from vertex I on the background mesh to the centroid of
boundary cell J and ∆sJ is the mesh size (length) of boundary cell J.
The size function is then smoothed using Laplacian smoothing. ANSYS FLUENT then
interpolates the value of the size function by calculating the distance LI from a given cell
centroid P to the background mesh vertices that surround the cell (see Figure 3.3.18).
The intermediate value of the size function sizeb at the centroid is computed from
sizeb =
3-26
ΣSF I L1I
Σ L1I
(3.3-10)
Release 12.0 c ANSYS, Inc. January 29, 2009
3.3 Dynamic Mesh Theory
Figure 3.3.15: Mesh at the End of a Dynamic Mesh Simulation Without Size
Functions
Figure 3.3.16: Mesh at the End of a Dynamic Mesh Simulation With Size
Functions
Release 12.0 c ANSYS, Inc. January 29, 2009
3-27
Flows Using Sliding and Deforming Meshes
Figure 3.3.17: Size Function Determination at Background Mesh Vertex I
Figure 3.3.18: Interpolating the Value of the Size Function
3-28
Release 12.0 c ANSYS, Inc. January 29, 2009
3.3 Dynamic Mesh Theory
Next, a single point Q is located within the domain (see Figure 3.3.19) that has the
largest distance dmax to the nearest boundary to it. The normalized distance db for the
given centroid P is given by
db =
dPmin
dmax
(3.3-11)
Figure 3.3.19: Determining the Normalized Distance
Using the parameters α and β (the Size Function Variation and the Size Function Rate,
respectively), you can write the final value sizeP of the size function at point P as
sizeP = sizeb × (1 + α × d1+2β
) = sizeb × γ
b
(3.3-12)
where sizeb is the intermediate value of the size function at the cell centroid.
Note that α is the size function variation. Positive values mean that the cell size increases as you move away from the boundary. Since the maximum value of db is one, the
maximum cell size becomes
sizeP,max = sizeb × (1 + α) = sizeb × γmax
(3.3-13)
thus, α is really a measure of the maximum cell size.
Release 12.0 c ANSYS, Inc. January 29, 2009
3-29
Flows Using Sliding and Deforming Meshes
The factor γ is computed from
γ = 1 + αd1+2β
b
1
1−β
γ = 1 + αdb
if α > 0
(3.3-14)
if α < 0
(3.3-15)
You can use Size Function Variation (or α) to control how large or small an interior cell
can be with respect to its closest boundary cell. α ranges from −1 to ∞, an α value of 0.5
indicates that the interior cell size can be, at most, 1.5 the size of the closest boundary
cell. Conversely, an α value of −0.5 indicates that the cell size interior of the boundary
can be half of that at the closest boundary cell. A value of 0 indicates a constant size
distribution away from the boundary.
You can use Size Function Rate (or β) to control how rapidly the cell size varies from the
boundary. The value of β should be specified such that −0.99 < β < +0.99. A positive
value indicates a slower transition from the boundary to the specified Size Function Variation value. Conversely, a negative value indicates a faster transition from the boundary
to the Size Function Variation value. A value of 0 indicates a linear variation of cell size
away from the boundary.
You can also control the resolution of the sizing function with Size Function Resolution.
The resolution determines the size of the background bins used to evaluate the size
distribution with respect to the shortest feature length of the current mesh. By default,
the Size Function Resolution is 3 in 2D problems, and 1 in 3D problems.
A set of default values (based on the current mesh) is automatically generated if you
click Use Defaults.
In summary, the sizing function is a distance-weighted average of all mesh sizes on all
boundary faces (both stationary and moving boundaries). The sizing function is based on
the sizes of the boundary cells, with the size computed from the cell volume by assuming
a perfect (equilateral) triangle in 2D and a perfect tetrahedron in 3D. You can control
the size distribution by specifying the Size Function Variation and the Size Function Rate.
If you have enabled the Sizing Function option, ANSYS FLUENT will agglomerate a cell
if
5
4
size 6∈ γsizeb , γsizeb
5
4
(3.3-16)
where γ is a factor defined by Equation 3.3-14 and Equation 3.3-15.
Note that the size function is only used for marking cells before remeshing. The size
function is not used to govern the size of the cell during remeshing.
3-30
Release 12.0 c ANSYS, Inc. January 29, 2009
3.3 Dynamic Mesh Theory
Feature Detection
For 3D simulations, ANSYS FLUENT allows you to preserve features on deforming zones
not only between the different face zones, but also within a face zone.
In the Geometry Definition tab of the Dynamic Mesh Zones dialog box, for any geometry definition, you can indicate whether you want to include features of a specific angle
by selecting Include Features under Feature Detection and setting the Feature Angle (the
zonal feature angle α) in degrees. If the angle β between adjacent faces is bigger than
the specified angle, then the feature is recognized (i.e., cos(β) < cos(α)).
3.3.2
Six DOF (6DOF) Solver Theory
The 6DOF solver in ANSYS FLUENT uses the object’s forces and moments in order to
compute the translational and angular motion of the center of gravity of an object. The
governing equation for the translational motion of the center of gravity is solved for in
the inertial coordinate system (Equation 3.3-17).
1 X−
→
−̇
ν→
fG
G =
m
(3.3-17)
→
−
where −̇
ν→
G is the translational motion of the center of gravity, m is the mass, and f G is
the force vector due to gravity.
The angular motion of the object, −̇
ω→
B , is more easily computed using body coordinates
(Equation 3.3-18).
X −→
−1
−̇
−
→
ω→
MB − −
ω→
B = L
B × LωB
(3.3-18)
−→
where L is the inertia tensor, MB is the moment vector of the body, and −
ω→
B is the rigid
body angular velocity vector.
The moments are transformed from inertial to body coordinates using
−→
−→
M B = RM G
(3.3-19)
where R is the following transformation matrix:
Cθ Cψ
Sφ Sθ Cψ − Cφ Sψ
Cφ Sθ Cψ + Sφ Sψ
Cθ Sψ
Sφ Sθ Sψ + Cφ Cψ
Cφ Sθ Sψ − Sφ Cψ
-Sθ
Sφ Cθ
Cφ Cθ
where, in generic terms, Cχ = cos(χ) and Sχ = sin(χ). The angles φ, θ, and ψ are Euler
angles that represent the following sequence of rotations:
Release 12.0 c ANSYS, Inc. January 29, 2009
3-31
Flows Using Sliding and Deforming Meshes
• rotation about the x-axis (e.g., roll for airplanes)
• rotation about the y-axis (e.g., pitch for airplanes)
• rotation about the z-axis (e.g., yaw for airplanes)
Once the angular and the translational accelerations are computed from Equation 3.3-17
and Equation 3.3-18, the rates are derived by numerical integration [328]. The angular
and translational velocities are used in the dynamic mesh calculations to update the rigid
body position.
3-32
Release 12.0 c ANSYS, Inc. January 29, 2009
Chapter 4.
Turbulence
This chapter provides theoretical background about the turbulence models available in
ANSYS FLUENT. Information is presented in the following sections:
• Section 4.1: Introduction
• Section 4.2: Choosing a Turbulence Model
• Section 4.3: Spalart-Allmaras Model
• Section 4.4: Standard, RNG, and Realizable k- Models
• Section 4.5: Standard and SST k-ω Models
• Section 4.6: k-kl-ω Transition Model
• Section 4.7: Transition SST Model
• Section 4.8: The v 2 -f Model
• Section 4.9: Reynolds Stress Model (RSM)
• Section 4.10: Detached Eddy Simulation (DES)
• Section 4.11: Large Eddy Simulation (LES) Model
• Section 4.12: Near-Wall Treatments for Wall-Bounded Turbulent Flows
For more information about using these turbulence models in ANSYS FLUENT, see Chapter 12: Modeling Turbulence in the separate User’s Guide.
4.1
Introduction
Turbulent flows are characterized by fluctuating velocity fields. These fluctuations mix
transported quantities such as momentum, energy, and species concentration, and cause
the transported quantities to fluctuate as well. Since these fluctuations can be of small
scale and high frequency, they are too computationally expensive to simulate directly in
practical engineering calculations. Instead, the instantaneous (exact) governing equations
can be time-averaged, ensemble-averaged, or otherwise manipulated to remove the resolution of small scales, resulting in a modified set of equations that are computationally
less expensive to solve. However, the modified equations contain additional unknown
Release 12.0 c ANSYS, Inc. January 29, 2009
4-1
Turbulence
variables, and turbulence models are needed to determine these variables in terms of
known quantities.
ANSYS FLUENT provides the following choices of turbulence models:
• Spalart-Allmaras model
• k- models
– Standard k- model
– Renormalization-group (RNG) k- model
– Realizable k- model
• k-ω models
– Standard k-ω model
– Shear-stress transport (SST) k-ω model
• Transition k-kl-ω model
• Transition SST model
• v 2 -f model (add-on)
• Reynolds stress models (RSM)
– Linear pressure-strain RSM model
– Quadratic pressure-strain RSM model
– Low-Re stress-omega RSM model
• Detached eddy simulation (DES) model, which includes one of the following RANS
models.
– Spalart-Allmaras RANS model
– Realizable k- RANS model
– SST k-ω RANS model
• Large eddy simulation (LES) model, which includes one of the following sub-scale
models.
– Smagorinsky-Lilly subgrid-scale model
– WALE subgrid-scale model
– Dynamic Smagorinsky model
– Kinetic-energy transport subgrid-scale model
4-2
Release 12.0 c ANSYS, Inc. January 29, 2009
4.2 Choosing a Turbulence Model
4.2
Choosing a Turbulence Model
It is an unfortunate fact that no single turbulence model is universally accepted as being superior for all classes of problems. The choice of turbulence model will depend on
considerations such as the physics encompassed in the flow, the established practice for
a specific class of problem, the level of accuracy required, the available computational
resources, and the amount of time available for the simulation. To make the most appropriate choice of model for your application, you need to understand the capabilities
and limitations of the various options.
The purpose of this section is to give an overview of issues related to the turbulence
models provided in ANSYS FLUENT. The computational effort and cost in terms of
CPU time and memory of the individual models is discussed. While it is impossible to
state categorically which model is best for a specific application, general guidelines are
presented to help you choose the appropriate turbulence model for the flow you want to
model.
Information is presented in the following sections:
• Section 4.2.1: Reynolds-Averaged Approach vs. LES
• Section 4.2.2: Reynolds (Ensemble) Averaging
• Section 4.2.3: Boussinesq Approach vs. Reynolds Stress Transport Models
4.2.1
Reynolds-Averaged Approach vs. LES
Time-dependent solutions of the Navier-Stokes equations for high Reynolds-number turbulent flows in complex geometries which set out to resolve all the way down to the
smallest scales of the motions are unlikely to be attainable for some time to come. Two
alternative methods can be employed to render the Navier-Stokes equations tractable
so that the small-scale turbulent fluctuations do not have to be directly simulated:
Reynolds-averaging (or ensemble-averaging) and filtering. Both methods introduce additional terms in the governing equations that need to be modeled in order to achieve a
“closure” for the unknowns.
The Reynolds-averaged Navier-Stokes (RANS) equations govern the transport of the averaged flow quantities, with the whole range of the scales of turbulence being modeled.
The RANS-based modeling approach therefore greatly reduces the required computational effort and resources, and is widely adopted for practical engineering applications.
An entire hierarchy of closure models are available in ANSYS FLUENT including SpalartAllmaras, k- and its variants, k-ω and its variants, and the RSM. The RANS equations
are often used to compute time-dependent flows, whose unsteadiness may be externally
imposed (e.g., time-dependent boundary conditions or sources) or self-sustained (e.g.,
vortex-shedding, flow instabilities).
Release 12.0 c ANSYS, Inc. January 29, 2009
4-3
Turbulence
LES provides an alternative approach in which large eddies are explicitly computed (resolved) in a time-dependent simulation using the “filtered” Navier-Stokes equations. The
rationale behind LES is that by modeling less of turbulence (and resolving more), the
error introduced by turbulence modeling can be reduced. It is also believed to be easier
to find a “universal” model for the small scales, since they tend to be more isotropic and
less affected by the macroscopic features like boundary conditions, than the large eddies.
Filtering is essentially a mathematical manipulation of the exact Navier-Stokes equations
to remove the eddies that are smaller than the size of the filter, which is usually taken as
the mesh size when spatial filtering is employed as in ANSYS FLUENT. Like Reynoldsaveraging, the filtering process creates additional unknown terms that must be modeled
to achieve closure. Statistics of the time-varying flow-fields such as time-averages and
r.m.s. values of the solution variables, which are generally of most engineering interest,
can be collected during the time-dependent simulation.
LES for high Reynolds number industrial flows requires a significant amount of computational resources. This is mainly because of the need to accurately resolve the energycontaining turbulent eddies in both space and time domains, which becomes most acute
in near-wall regions where the scales to be resolved become much smaller. Wall functions
in combination with a coarse near wall mesh can be employed, often with some success, to
reduce the cost of LES for wall-bounded flows. However, one needs to carefully consider
the ramification of using wall functions for the flow in question. For the same reason (to
accurately resolve the eddies), LES also requires highly accurate spatial and temporal
discretizations.
4.2.2
Reynolds (Ensemble) Averaging
In Reynolds averaging, the solution variables in the instantaneous (exact) Navier-Stokes
equations are decomposed into the mean (ensemble-averaged or time-averaged) and fluctuating components. For the velocity components:
ui = ūi + u0i
(4.2-1)
where ūi and u0i are the mean and fluctuating velocity components (i = 1, 2, 3).
Likewise, for pressure and other scalar quantities:
φ = φ̄ + φ0
(4.2-2)
where φ denotes a scalar such as pressure, energy, or species concentration.
Substituting expressions of this form for the flow variables into the instantaneous continuity and momentum equations and taking a time (or ensemble) average (and dropping
the overbar on the mean velocity, ū) yields the ensemble-averaged momentum equations.
They can be written in Cartesian tensor form as:
4-4
Release 12.0 c ANSYS, Inc. January 29, 2009
4.2 Choosing a Turbulence Model
∂ρ
∂
(ρui ) = 0
+
∂t ∂xi
"
∂
∂
∂p
∂
∂ui ∂uj
2 ∂ul
(ρui )+
(ρui uj ) = −
+
µ
+
− δij
∂t
∂xj
∂xi ∂xj
∂xj
∂xi
3 ∂xl
(4.2-3)
!#
+
∂
(−ρu0i u0j ) (4.2-4)
∂xj
Equations 4.2-3 and 4.2-4 are called Reynolds-averaged Navier-Stokes (RANS) equations.
They have the same general form as the instantaneous Navier-Stokes equations, with
the velocities and other solution variables now representing ensemble-averaged (or timeaveraged) values. Additional terms now appear that represent the effects of turbulence.
These Reynolds stresses, −ρu0i u0j , must be modeled in order to close Equation 4.2-4.
For variable-density flows, Equations 4.2-3 and 4.2-4 can be interpreted as Favre-averaged
Navier-Stokes equations [130], with the velocities representing mass-averaged values. As
such, Equations 4.2-3 and 4.2-4 can be applied to density-varying flows.
4.2.3
Boussinesq Approach vs. Reynolds Stress Transport Models
The Reynolds-averaged approach to turbulence modeling requires that the Reynolds
stresses in Equation 4.2-4 are appropriately modeled. A common method employs the
Boussinesq hypothesis [130] to relate the Reynolds stresses to the mean velocity gradients:
− ρu0i u0j = µt
∂ui ∂uj
+
∂xj
∂xi
!
!
2
∂uk
−
ρk + µt
δij
3
∂xk
(4.2-5)
The Boussinesq hypothesis is used in the Spalart-Allmaras model, the k- models, and
the k-ω models. The advantage of this approach is the relatively low computational
cost associated with the computation of the turbulent viscosity, µt . In the case of the
Spalart-Allmaras model, only one additional transport equation (representing turbulent
viscosity) is solved. In the case of the k- and k-ω models, two additional transport
equations (for the turbulence kinetic energy, k, and either the turbulence dissipation
rate, , or the specific dissipation rate, ω) are solved, and µt is computed as a function of
k and or k and ω. The disadvantage of the Boussinesq hypothesis as presented is that
it assumes µt is an isotropic scalar quantity, which is not strictly true.
The alternative approach, embodied in the RSM, is to solve transport equations for each
of the terms in the Reynolds stress tensor. An additional scale-determining equation
(normally for ) is also required. This means that five additional transport equations are
required in 2D flows and seven additional transport equations must be solved in 3D.
Release 12.0 c ANSYS, Inc. January 29, 2009
4-5
Turbulence
In many cases, models based on the Boussinesq hypothesis perform very well, and the
additional computational expense of the Reynolds stress model is not justified. However,
the RSM is clearly superior in situations where the anisotropy of turbulence has a dominant effect on the mean flow. Such cases include highly swirling flows and stress-driven
secondary flows.
4.3
Spalart-Allmaras Model
This section describes the theory behind the Spalart-Allmaras model. Information is
presented in the following sections:
• Section 4.3.1: Overview
• Section 4.3.2: Transport Equation for the Spalart-Allmaras Model
• Section 4.3.3: Modeling the Turbulent Viscosity
• Section 4.3.4: Modeling the Turbulent Production
• Section 4.3.5: Modeling the Turbulent Destruction
• Section 4.3.6: Model Constants
• Section 4.3.7: Wall Boundary Conditions
• Section 4.3.8: Convective Heat and Mass Transfer Modeling
For details about using the model in ANSYS FLUENT, see Chapter 12: Modeling Turbulence
and Section 12.5: Setting Up the Spalart-Allmaras Model in the separate User’s Guide.
4.3.1
Overview
The Spalart-Allmaras model is a relatively simple one-equation model that solves a modeled transport equation for the kinematic eddy (turbulent) viscosity. This embodies a
relatively new class of one-equation models in which it is not necessary to calculate a
length scale related to the local shear layer thickness. The Spalart-Allmaras model was
designed specifically for aerospace applications involving wall-bounded flows and has been
shown to give good results for boundary layers subjected to adverse pressure gradients.
It is also gaining popularity in the turbomachinery applications.
4-6
Release 12.0 c ANSYS, Inc. January 29, 2009
4.3 Spalart-Allmaras Model
In its original form, the Spalart-Allmaras model is effectively a low-Reynolds-number
model, requiring the viscosity-affected region of the boundary layer to be properly resolved. In ANSYS FLUENT, however, the Spalart-Allmaras model has been implemented
to use wall functions when the mesh resolution is not sufficiently fine. This might make
it the best choice for relatively crude simulations on coarse meshes where accurate turbulent flow computations are not critical. Furthermore, the near-wall gradients of the
transported variable in the model are much smaller than the gradients of the transported
variables in the k- or k-ω models. This might make the model less sensitive to numerical errors when non-layered meshes are used near walls. See Section 6.1.3: Numerical
Diffusion in the separate User’s Guide for a further discussion of the numerical errors.
On a cautionary note, however, the Spalart-Allmaras model is still relatively new, and
no claim is made regarding its suitability to all types of complex engineering flows. For
instance, it cannot be relied on to predict the decay of homogeneous, isotropic turbulence. Furthermore, one-equation models are often criticized for their inability to rapidly
accommodate changes in length scale, such as might be necessary when the flow changes
abruptly from a wall-bounded to a free shear flow.
In turbulence models that employ the Boussinesq approach, the central issue is how the
eddy viscosity is computed. The model proposed by Spalart and Allmaras [331] solves
a transport equation for a quantity that is a modified form of the turbulent kinematic
viscosity.
4.3.2
Transport Equation for the Spalart-Allmaras Model
The transported variable in the Spalart-Allmaras model, νe, is identical to the turbulent
kinematic viscosity except in the near-wall (viscosity-affected) region. The transport
equation for νe is
∂
∂
1 ∂
(ρνe) +
(ρνeui ) = Gν +
∂t
∂xi
σeν ∂xj
(
∂ νe
(µ + ρνe)
∂xj
)
∂ νe
+ Cb2 ρ
∂xj
!2
− Yν + S (4.3-1)
e
ν
where Gν is the production of turbulent viscosity, and Yν is the destruction of turbulent
viscosity that occurs in the near-wall region due to wall blocking and viscous damping.
σeν and Cb2 are the constants and ν is the molecular kinematic viscosity. Seν is a userdefined source term. Note that since the turbulence kinetic energy, k, is not calculated
in the Spalart-Allmaras model, while the last term in Equation 4.2-5 is ignored when
estimating the Reynolds stresses.
Release 12.0 c ANSYS, Inc. January 29, 2009
4-7
Turbulence
4.3.3
Modeling the Turbulent Viscosity
The turbulent viscosity, µt , is computed from
µt = ρνefv1
(4.3-2)
where the viscous damping function, fv1 , is given by
fv1 =
χ3
3
χ3 + Cv1
(4.3-3)
νe
ν
(4.3-4)
and
χ≡
4.3.4
Modeling the Turbulent Production
The production term, Gν , is modeled as
(4.3-5)
Gν = Cb1 ρSeνe
where
Se ≡ S +
νe
fv2
κ2 d2
(4.3-6)
fv2 = 1 −
χ
1 + χfv1
(4.3-7)
and
Cb1 and κ are constants, d is the distance from the wall, and S is a scalar measure of the
deformation tensor. By default in ANSYS FLUENT, as in the original model proposed by
Spalart and Allmaras, S is based on the magnitude of the vorticity:
S≡
q
2Ωij Ωij
(4.3-8)
where Ωij is the mean rate-of-rotation tensor and is defined by
1
Ωij =
2
4-8
∂ui
∂uj
−
∂xj
∂xi
!
(4.3-9)
Release 12.0 c ANSYS, Inc. January 29, 2009
4.3 Spalart-Allmaras Model
The justification for the default expression for S is that, in the wall-bounded flows that
were of most interest when the model was formulated, the turbulence production found
only where vorticity is generated near walls. However, it has since been acknowledged that
one should also take into account the effect of mean strain on the turbulence production,
and a modification to the model has been proposed [65] and incorporated into ANSYS
FLUENT.
This modification combines the measures of both vorticity and the strain tensors in the
definition of S:
S ≡ |Ωij | + Cprod min (0, |Sij | − |Ωij |)
(4.3-10)
where
Cprod = 2.0, |Ωij | ≡
q
2Ωij Ωij , |Sij | ≡
q
2Sij Sij
with the mean strain rate, Sij , defined as
1
Sij =
2
∂uj
∂ui
+
∂xi ∂xj
!
(4.3-11)
Including both the rotation and strain tensors reduces the production of eddy viscosity
and consequently reduces the eddy viscosity itself in regions where the measure of vorticity exceeds that of strain rate. One such example can be found in vortical flows, i.e., flow
near the core of a vortex subjected to a pure rotation where turbulence is known to be
suppressed. Including both the rotation and strain tensors more correctly accounts for
the effects of rotation on turbulence. The default option (including the rotation tensor
only) tends to overpredict the production of eddy viscosity and hence overpredicts the
eddy viscosity itself in certain circumstances.
You can select the modified form for calculating production in the Viscous Model dialog
box.
Release 12.0 c ANSYS, Inc. January 29, 2009
4-9
Turbulence
4.3.5
Modeling the Turbulent Destruction
The destruction term is modeled as
Yν = Cw1 ρfw
2
νe
(4.3-12)
d
where
6
1 + Cw3
fw = g 6
6
g + Cw3
"
#1/6
g = r + Cw2 r6 − r
(4.3-13)
(4.3-14)
νe
r≡ e
Sκ2 d2
(4.3-15)
Cw1 , Cw2 , and Cw3 are constants, and Se is given by Equation 4.3-6. Note that the
modification described above to include the effects of mean strain on S will also affect
the value of Se used to compute r.
4.3.6
Model Constants
The model constants Cb1 , Cb2 , σeν , Cv1 , Cw1 , Cw2 , Cw3 , and κ have the following default
values [331]:
2
Cb1 = 0.1355, Cb2 = 0.622, σeν = , Cv1 = 7.1
3
Cw1 =
4.3.7
Cb1 (1 + Cb2 )
+
, Cw2 = 0.3, Cw3 = 2.0, κ = 0.4187
κ2
σeν
Wall Boundary Conditions
At walls, the modified turbulent kinematic viscosity, νe, is set to zero.
When the mesh is fine enough to resolve the viscosity-dominated sublayer, the wall shear
stress is obtained from the laminar stress-strain relationship:
u
ρuτ y
=
uτ
µ
4-10
(4.3-16)
Release 12.0 c ANSYS, Inc. January 29, 2009
4.4 Standard, RNG, and Realizable k- Models
If the mesh is too coarse to resolve the viscous sublayer, then it is assumed that the
centroid of the wall-adjacent cell falls within the logarithmic region of the boundary
layer, and the law-of-the-wall is employed:
u
1
ρuτ y
= ln E
uτ
κ
µ
!
(4.3-17)
where u is the velocity parallel to the wall, uτ is the shear velocity, y is the distance from
the wall, κ is the von Kármán constant (0.4187), and E = 9.793.
4.3.8
Convective Heat and Mass Transfer Modeling
In ANSYS FLUENT, turbulent heat transport is modeled using the concept of the Reynolds’
analogy to turbulent momentum transfer. The “modeled” energy equation is as follows:
∂
∂
∂
(ρE) +
[ui (ρE + p)] =
∂t
∂xi
∂xj
"
c p µt
k+
Prt
#
∂T
+ ui (τij )eff + Sh
∂xj
(4.3-18)
where k, in this case, is the thermal conductivity, E is the total energy, and (τij )eff is the
deviatoric stress tensor, defined as
(τij )eff = µeff
4.4
∂uj
∂ui
+
∂xi ∂xj
!
2
∂uk
− µeff
δij
3
∂xk
Standard, RNG, and Realizable k- Models
This section describes the theory behind the Standard, RNG, and Realizable k- models.
Information is presented in the following sections:
• Section 4.4.1: Standard k- Model
• Section 4.4.2: RNG k- Model
• Section 4.4.3: Realizable k- Model
• Section 4.4.4: Modeling Turbulent Production in the k- Models
• Section 4.4.5: Effects of Buoyancy on Turbulence in the k- Models
• Section 4.4.6: Effects of Compressibility on Turbulence in the k- Models
• Section 4.4.7: Convective Heat and Mass Transfer Modeling in the k- Models
Release 12.0 c ANSYS, Inc. January 29, 2009
4-11
Turbulence
For details about using the models in ANSYS FLUENT, see Chapter 12: Modeling Turbulence
and Section 12.6: Setting Up the k- Model in the separate User’s Guide.
This section presents the standard, RNG, and realizable k- models. All three models
have similar forms, with transport equations for k and . The major differences in the
models are as follows:
• the method of calculating turbulent viscosity
• the turbulent Prandtl numbers governing the turbulent diffusion of k and
• the generation and destruction terms in the equation
The transport equations, the methods of calculating turbulent viscosity, and model constants are presented separately for each model. The features that are essentially common
to all models follow, including turbulent generation due to shear buoyancy, accounting
for the effects of compressibility, and modeling heat and mass transfer.
4.4.1
Standard k- Model
Overview
The simplest “complete models” of turbulence are the two-equation models in which the
solution of two separate transport equations allows the turbulent velocity and length
scales to be independently determined. The standard k- model in ANSYS FLUENT falls
within this class of models and has become the workhorse of practical engineering flow
calculations in the time since it was proposed by Launder and Spalding [180]. Robustness, economy, and reasonable accuracy for a wide range of turbulent flows explain its
popularity in industrial flow and heat transfer simulations. It is a semi-empirical model,
and the derivation of the model equations relies on phenomenological considerations and
empiricism.
As the strengths and weaknesses of the standard k- model have become known, improvements have been made to the model to improve its performance. Two of these
variants are available in ANSYS FLUENT: the RNG k- model [384] and the realizable
k- model [313].
The standard k- model [180] is a semi-empirical model based on model transport equations for the turbulence kinetic energy (k) and its dissipation rate (). The model transport equation for k is derived from the exact equation, while the model transport equation
for was obtained using physical reasoning and bears little resemblance to its mathematically exact counterpart.
In the derivation of the k- model, the assumption is that the flow is fully turbulent, and
the effects of molecular viscosity are negligible. The standard k- model is therefore valid
only for fully turbulent flows.
4-12
Release 12.0 c ANSYS, Inc. January 29, 2009
4.4 Standard, RNG, and Realizable k- Models
Transport Equations for the Standard k- Model
The turbulence kinetic energy, k, and its rate of dissipation, , are obtained from the
following transport equations:
∂
∂
∂
(ρk) +
(ρkui ) =
∂t
∂xi
∂xj
"
µt
µ+
σk
#
∂k
+ Gk + Gb − ρ − YM + Sk
∂xj
(4.4-1)
and
∂
∂
∂
(ρ) +
(ρui ) =
∂t
∂xi
∂xj
"
µt
µ+
σ
∂
2
+ C1 (Gk + C3 Gb ) − C2 ρ + S (4.4-2)
∂xj
k
k
#
In these equations, Gk represents the generation of turbulence kinetic energy due to the
mean velocity gradients, calculated as described in Section 4.4.4: Modeling Turbulent
Production in the k- Models. Gb is the generation of turbulence kinetic energy due
to buoyancy, calculated as described in Section 4.4.5: Effects of Buoyancy on Turbulence in the k- Models. YM represents the contribution of the fluctuating dilatation in
compressible turbulence to the overall dissipation rate, calculated as described in Section 4.4.6: Effects of Compressibility on Turbulence in the k- Models. C1 , C2 , and C3
are constants. σk and σ are the turbulent Prandtl numbers for k and , respectively. Sk
and S are user-defined source terms.
Modeling the Turbulent Viscosity
The turbulent (or eddy) viscosity, µt , is computed by combining k and as follows:
k2
µt = ρCµ
(4.4-3)
where Cµ is a constant.
Model Constants
The model constants C1 , C2 , Cµ , σk , and σ have the following default values [180]:
C1 = 1.44, C2 = 1.92, Cµ = 0.09, σk = 1.0, σ = 1.3
These default values have been determined from experiments with air and water for fundamental turbulent shear flows including homogeneous shear flows and decaying isotropic
grid turbulence. They have been found to work fairly well for a wide range of wallbounded and free shear flows.
Release 12.0 c ANSYS, Inc. January 29, 2009
4-13
Turbulence
Although the default values of the model constants are the standard ones most widely
accepted, you can change them (if needed) in the Viscous Model dialog box.
4.4.2
RNG k- Model
Overview
The RNG k- model was derived using a rigorous statistical technique (called renormalization group theory). It is similar in form to the standard k- model, but includes the
following refinements:
• The RNG model has an additional term in its equation that significantly improves
the accuracy for rapidly strained flows.
• The effect of swirl on turbulence is included in the RNG model, enhancing accuracy
for swirling flows.
• The RNG theory provides an analytical formula for turbulent Prandtl numbers,
while the standard k- model uses user-specified, constant values.
• While the standard k- model is a high-Reynolds-number model, the RNG theory
provides an analytically-derived differential formula for effective viscosity that accounts for low-Reynolds-number effects. Effective use of this feature does, however,
depend on an appropriate treatment of the near-wall region.
These features make the RNG k- model more accurate and reliable for a wider class of
flows than the standard k- model.
The RNG-based k- turbulence model is derived from the instantaneous Navier-Stokes
equations, using a mathematical technique called “renormalization group” (RNG) methods. The analytical derivation results in a model with constants different from those in
the standard k- model, and additional terms and functions in the transport equations
for k and . A more comprehensive description of RNG theory and its application to
turbulence can be found in [259].
4-14
Release 12.0 c ANSYS, Inc. January 29, 2009
4.4 Standard, RNG, and Realizable k- Models
Transport Equations for the RNG k- Model
The RNG k- model has a similar form to the standard k- model:
∂
∂
∂
(ρk) +
(ρkui ) =
∂t
∂xi
∂xj
∂k
αk µeff
∂xj
!
+ Gk + Gb − ρ − YM + Sk
(4.4-4)
and
∂
∂
∂
(ρ) +
(ρui ) =
∂t
∂xi
∂xj
∂
α µeff
∂xj
!
2
+ C1 (Gk + C3 Gb ) − C2 ρ − R + S (4.4-5)
k
k
In these equations, Gk represents the generation of turbulence kinetic energy due to the
mean velocity gradients, calculated as described in Section 4.4.4: Modeling Turbulent
Production in the k- Models. Gb is the generation of turbulence kinetic energy due
to buoyancy, calculated as described in Section 4.4.5: Effects of Buoyancy on Turbulence in the k- Models. YM represents the contribution of the fluctuating dilatation in
compressible turbulence to the overall dissipation rate, calculated as described in Section 4.4.6: Effects of Compressibility on Turbulence in the k- Models. The quantities αk
and α are the inverse effective Prandtl numbers for k and , respectively. Sk and S are
user-defined source terms.
Modeling the Effective Viscosity
The scale elimination procedure in RNG theory results in a differential equation for
turbulent viscosity:
ρ2 k
d √
µ
!
= 1.72 √
ν̂ 3
ν̂
dν̂
− 1 + Cν
(4.4-6)
where
ν̂ = µeff /µ
Cν ≈ 100
Equation 4.4-6 is integrated to obtain an accurate description of how the effective turbulent transport varies with the effective Reynolds number (or eddy scale), allowing the
model to better handle low-Reynolds-number and near-wall flows.
Release 12.0 c ANSYS, Inc. January 29, 2009
4-15
Turbulence
In the high-Reynolds-number limit, Equation 4.4-6 gives
µt = ρCµ
k2
(4.4-7)
with Cµ = 0.0845, derived using RNG theory. It is interesting to note that this value
of Cµ is very close to the empirically-determined value of 0.09 used in the standard k-
model.
In ANSYS FLUENT, by default, the effective viscosity is computed using the highReynolds-number form in Equation 4.4-7. However, there is an option available that
allows you to use the differential relation given in Equation 4.4-6 when you need to
include low-Reynolds-number effects.
RNG Swirl Modification
Turbulence, in general, is affected by rotation or swirl in the mean flow. The RNG model
in ANSYS FLUENT provides an option to account for the effects of swirl or rotation by
modifying the turbulent viscosity appropriately. The modification takes the following
functional form:
µt = µt0
k
f αs , Ω,
!
(4.4-8)
where µt0 is the value of turbulent viscosity calculated without the swirl modification
using either Equation 4.4-6 or Equation 4.4-7. Ω is a characteristic swirl number evaluated within ANSYS FLUENT, and αs is a swirl constant that assumes different values
depending on whether the flow is swirl-dominated or only mildly swirling. This swirl
modification always takes effect for axisymmetric, swirling flows and three-dimensional
flows when the RNG model is selected. For mildly swirling flows (the default in ANSYS
FLUENT), αs is set to 0.07. For strongly swirling flows, however, a higher value of αs
can be used.
Calculating the Inverse Effective Prandtl Numbers
The inverse effective Prandtl numbers, αk and α , are computed using the following
formula derived analytically by the RNG theory:
α − 1.3929
α0 − 1.3929
0.6321
α + 2.3929
α0 + 2.3929
0.3679
=
µmol
µeff
(4.4-9)
where α0 = 1.0. In the high-Reynolds-number limit (µmol /µeff 1), αk = α ≈ 1.393.
4-16
Release 12.0 c ANSYS, Inc. January 29, 2009
4.4 Standard, RNG, and Realizable k- Models
The R Term in the Equation
The main difference between the RNG and standard k- models lies in the additional
term in the equation given by
R =
Cµ ρη 3 (1 − η/η0 ) 2
1 + βη 3
k
(4.4-10)
where η ≡ Sk/, η0 = 4.38, β = 0.012.
The effects of this term in the RNG equation can be seen more clearly by rearranging
Equation 4.4-5. Using Equation 4.4-10, the third and fourth terms on the right-hand
side of Equation 4.4-5 can be merged, and the resulting equation can be rewritten as
∂
∂
∂
(ρ) +
(ρui ) =
∂t
∂xi
∂xj
∂
α µeff
∂xj
!
2
∗
+ C1 (Gk + C3 Gb ) − C2
ρ
k
k
(4.4-11)
∗
where C2
is given by
∗
C2
≡ C2 +
Cµ η 3 (1 − η/η0 )
1 + βη 3
(4.4-12)
∗
In regions where η < η0 , the R term makes a positive contribution, and C2
becomes
larger than C2 . In the logarithmic layer, for instance, it can be shown that η ≈ 3.0,
∗
giving C2
≈ 2.0, which is close in magnitude to the value of C2 in the standard k-
model (1.92). As a result, for weakly to moderately strained flows, the RNG model tends
to give results largely comparable to the standard k- model.
In regions of large strain rate (η > η0 ), however, the R term makes a negative contribu∗
tion, making the value of C2
less than C2 . In comparison with the standard k- model,
the smaller destruction of augments , reducing k and, eventually, the effective viscosity.
As a result, in rapidly strained flows, the RNG model yields a lower turbulent viscosity
than the standard k- model.
Thus, the RNG model is more responsive to the effects of rapid strain and streamline
curvature than the standard k- model, which explains the superior performance of the
RNG model for certain classes of flows.
Model Constants
The model constants C1 and C2 in Equation 4.4-5 have values derived analytically by
the RNG theory. These values, used by default in ANSYS FLUENT, are
C1 = 1.42, C2 = 1.68
Release 12.0 c ANSYS, Inc. January 29, 2009
4-17
Turbulence
4.4.3
Realizable k- Model
Overview
The realizable k- model [313] is a relatively recent development and differs from the
standard k- model in two important ways:
• The realizable k- model contains a new formulation for the turbulent viscosity.
• A new transport equation for the dissipation rate, , has been derived from an exact
equation for the transport of the mean-square vorticity fluctuation.
The term “realizable” means that the model satisfies certain mathematical constraints
on the Reynolds stresses, consistent with the physics of turbulent flows. Neither the
standard k- model nor the RNG k- model is realizable.
An immediate benefit of the realizable k- model is that it more accurately predicts
the spreading rate of both planar and round jets. It is also likely to provide superior
performance for flows involving rotation, boundary layers under strong adverse pressure
gradients, separation, and recirculation.
To understand the mathematics behind the realizable k- model, consider combining
the Boussinesq relationship (Equation 4.2-5) and the eddy viscosity definition (Equation 4.4-3) to obtain the following expression for the normal Reynolds stress in an incompressible strained mean flow:
2
∂U
u2 = k − 2 νt
3
∂x
(4.4-13)
Using Equation 4.4-3 for νt ≡ µt /ρ, one obtains the result that the normal stress, u2 ,
which by definition is a positive quantity, becomes negative, i.e., “non-realizable”, when
the strain is large enough to satisfy
k ∂U
1
>
≈ 3.7
∂x
3Cµ
(4.4-14)
Similarly, it can also be shown that the Schwarz inequality for shear stresses (uα uβ 2 ≤
u2α u2β ; no summation over α and β) can be violated when the mean strain rate is large.
The most straightforward way to ensure the realizability (positivity of normal stresses
and Schwarz inequality for shear stresses) is to make Cµ variable by sensitizing it to
the mean flow (mean deformation) and the turbulence (k, ). The notion of variable
Cµ is suggested by many modelers including Reynolds [291], and is well substantiated
by experimental evidence. For example, Cµ is found to be around 0.09 in the inertial
sublayer of equilibrium boundary layers, and 0.05 in a strong homogeneous shear flow.
4-18
Release 12.0 c ANSYS, Inc. January 29, 2009
4.4 Standard, RNG, and Realizable k- Models
Both the realizable and RNG k- models have shown substantial improvements over the
standard k- model where the flow features include strong streamline curvature, vortices,
and rotation. Since the model is still relatively new, it is not clear in exactly which
instances the realizable k- model consistently outperforms the RNG model. However,
initial studies have shown that the realizable model provides the best performance of all
the k- model versions for several validations of separated flows and flows with complex
secondary flow features.
One of the weaknesses of the standard k- model or other traditional k- models lies with
the modeled equation for the dissipation rate (). The well-known round-jet anomaly
(named based on the finding that the spreading rate in planar jets is predicted reasonably
well, but prediction of the spreading rate for axisymmetric jets is unexpectedly poor) is
considered to be mainly due to the modeled dissipation equation.
The realizable k- model proposed by Shih et al. [313] was intended to address these
deficiencies of traditional k- models by adopting the following:
• A new eddy-viscosity formula involving a variable Cµ originally proposed by
Reynolds [291].
• A new model equation for dissipation () based on the dynamic equation of the
mean-square vorticity fluctuation.
One limitation of the realizable k- model is that it produces non-physical turbulent
viscosities in situations when the computational domain contains both rotating and stationary fluid zones (e.g., multiple reference frames, rotating sliding meshes). This is due
to the fact that the realizable k- model includes the effects of mean rotation in the
definition of the turbulent viscosity (see Equations 4.4-17–4.4-19). This extra rotation
effect has been tested on single rotating reference frame systems and showed superior
behavior over the standard k- model. However, due to the nature of this modification,
its application to multiple reference frame systems should be taken with some caution.
See Section 4.4.3: Modeling the Turbulent Viscosity for information about how to include
or exclude this term from the model.
Release 12.0 c ANSYS, Inc. January 29, 2009
4-19
Turbulence
Transport Equations for the Realizable k- Model
The modeled transport equations for k and in the realizable k- model are
∂
∂
∂
(ρk) +
(ρkuj ) =
∂t
∂xj
∂xj
"
µt
µ+
σk
#
∂k
+ Gk + Gb − ρ − YM + Sk
∂xj
(4.4-15)
and
∂
∂
∂
(ρ) +
(ρuj ) =
∂t
∂xj
∂xj
"
µt
µ+
σ
∂
2
√ + C1 C3 Gb + S
+ ρ C1 S − ρ C2
∂xj
k + ν
k
(4.4-16)
#
where
"
#
η
,
C1 = max 0.43,
η+5
k
η=S ,
S=
q
2Sij Sij
In these equations, Gk represents the generation of turbulence kinetic energy due to the
mean velocity gradients, calculated as described in Section 4.4.4: Modeling Turbulent
Production in the k- Models. Gb is the generation of turbulence kinetic energy due
to buoyancy, calculated as described in Section 4.4.5: Effects of Buoyancy on Turbulence in the k- Models. YM represents the contribution of the fluctuating dilatation in
compressible turbulence to the overall dissipation rate, calculated as described in Section 4.4.6: Effects of Compressibility on Turbulence in the k- Models. C2 and C1 are
constants. σk and σ are the turbulent Prandtl numbers for k and , respectively. Sk and
S are user-defined source terms.
Note that the k equation (Equation 4.4-15) is the same as that in the standard k-
model (Equation 4.4-1) and the RNG k- model (Equation 4.4-4), except for the model
constants. However, the form of the equation is quite different from those in the
standard and RNG-based k- models (Equations 4.4-2 and 4.4-5). One of the noteworthy
features is that the production term in the equation (the second term on the right-hand
side of Equation 4.4-16) does not involve the production of k; i.e., it does not contain
the same Gk term as the other k- models. It is believed that the present form better
represents the spectral energy transfer. Another desirable feature is that the destruction
term (the next to last term on the right-hand side of Equation 4.4-16) does not have any
singularity; i.e., its denominator never vanishes, even if k vanishes or becomes smaller
than zero. This feature is contrasted with traditional k- models, which have a singularity
due to k in the denominator.
4-20
Release 12.0 c ANSYS, Inc. January 29, 2009
4.4 Standard, RNG, and Realizable k- Models
This model has been extensively validated for a wide range of flows [167, 313], including
rotating homogeneous shear flows, free flows including jets and mixing layers, channel
and boundary layer flows, and separated flows. For all these cases, the performance of
the model has been found to be substantially better than that of the standard k- model.
Especially noteworthy is the fact that the realizable k- model resolves the round-jet
anomaly; i.e., it predicts the spreading rate for axisymmetric jets as well as that for
planar jets.
Modeling the Turbulent Viscosity
As in other k- models, the eddy viscosity is computed from
k2
µt = ρCµ
(4.4-17)
The difference between the realizable k- model and the standard and RNG k- models
is that Cµ is no longer constant. It is computed from
1
∗
A0 + As kU
(4.4-18)
e Ω
e
Sij Sij + Ω
ij ij
(4.4-19)
Cµ =
where
∗
U ≡
q
and
e
Ω
ij = Ωij − 2ijk ωk
Ωij = Ωij − ijk ωk
where Ωij is the mean rate-of-rotation tensor viewed in a rotating reference frame with
the angular velocity ωk . The model constants A0 and As are given by
A0 = 4.04, As =
√
6 cos φ
where
√
1
Sij Sjk Ski e q
1
φ = cos−1 ( 6W ), W =
,
S
=
S
S
,
S
=
ij
ij
ij
3
2
Se3
Release 12.0 c ANSYS, Inc. January 29, 2009
∂uj
∂ui
+
∂xi ∂xj
!
4-21
Turbulence
It can be seen that Cµ is a function of the mean strain and rotation rates, the angular
velocity of the system rotation, and the turbulence fields (k and ). Cµ in Equation 4.4-17
can be shown to recover the standard value of 0.09 for an inertial sublayer in an equilibrium boundary layer.
i
In ANSYS FLUENT, the term −2ijk ωk is, by default, not included in
e . This is an extra rotation term that is not comthe calculation of Ω
ij
patible with cases involving sliding meshes or multiple reference frames.
If you want to include this term in the model, you can enable it by using the
define/models/viscous/turbulence-expert/rke-cmu-rotation-term?
text command and entering yes at the prompt.
Model Constants
The model constants C2 , σk , and σ have been established to ensure that the model
performs well for certain canonical flows. The model constants are
C1 = 1.44, C2 = 1.9, σk = 1.0, σ = 1.2
4.4.4
Modeling Turbulent Production in the k- Models
The term Gk , representing the production of turbulence kinetic energy, is modeled identically for the standard, RNG, and realizable k- models. From the exact equation for
the transport of k, this term may be defined as
Gk = −ρu0i u0j
∂uj
∂xi
(4.4-20)
To evaluate Gk in a manner consistent with the Boussinesq hypothesis,
G k = µt S 2
(4.4-21)
where S is the modulus of the mean rate-of-strain tensor, defined as
S≡
i
4-22
q
2Sij Sij
(4.4-22)
When using the high-Reynolds number k- versions, µeff is used in lieu of
µt in Equation 4.4-21.
Release 12.0 c ANSYS, Inc. January 29, 2009
4.4 Standard, RNG, and Realizable k- Models
4.4.5
Effects of Buoyancy on Turbulence in the k- Models
When a non-zero gravity field and temperature gradient are present simultaneously, the
k- models in ANSYS FLUENT account for the generation of k due to buoyancy (Gb in
Equations 4.4-1, 4.4-4, and 4.4-15), and the corresponding contribution to the production
of in Equations 4.4-2, 4.4-5, and 4.4-16.
The generation of turbulence due to buoyancy is given by
Gb = βgi
µt ∂T
Prt ∂xi
(4.4-23)
where Prt is the turbulent Prandtl number for energy and gi is the component of the
gravitational vector in the ith direction. For the standard and realizable k- models,
the default value of Prt is 0.85. In the case of the RNG k- model, Prt = 1/α, where
α is given by Equation 4.4-9, but with α0 = 1/Pr = k/µcp . The coefficient of thermal
expansion, β, is defined as
1
β=−
ρ
∂ρ
∂T
!
(4.4-24)
p
For ideal gases, Equation 4.4-23 reduces to
Gb = −gi
µt ∂ρ
ρPrt ∂xi
(4.4-25)
It can be seen from the transport equations for k (Equations 4.4-1, 4.4-4, and 4.4-15)
that turbulence kinetic energy tends to be augmented (Gb > 0) in unstable stratification.
For stable stratification, buoyancy tends to suppress the turbulence (Gb < 0). In ANSYS
FLUENT, the effects of buoyancy on the generation of k are always included when you
have both a non-zero gravity field and a non-zero temperature (or density) gradient.
While the buoyancy effects on the generation of k are relatively well understood, the
effect on is less clear. In ANSYS FLUENT, by default, the buoyancy effects on are
neglected simply by setting Gb to zero in the transport equation for (Equation 4.4-2,
4.4-5, or 4.4-16).
However, you can include the buoyancy effects on in the Viscous Model dialog box.
In this case, the value of Gb given by Equation 4.4-25 is used in the transport equation
for (Equation 4.4-2, 4.4-5, or 4.4-16).
The degree to which is affected by the buoyancy is determined by the constant C3 . In
ANSYS FLUENT, C3 is not specified, but is instead calculated according to the following
relation [127]:
Release 12.0 c ANSYS, Inc. January 29, 2009
4-23
Turbulence
C3 = tanh
v
u
(4.4-26)
where v is the component of the flow velocity parallel to the gravitational vector and
u is the component of the flow velocity perpendicular to the gravitational vector. In
this way, C3 will become 1 for buoyant shear layers for which the main flow direction is
aligned with the direction of gravity. For buoyant shear layers that are perpendicular to
the gravitational vector, C3 will become zero.
4.4.6
Effects of Compressibility on Turbulence in the k- Models
For high-Mach-number flows, compressibility affects turbulence through so-called “dilatation dissipation”, which is normally neglected in the modeling of incompressible
flows [379]. Neglecting the dilatation dissipation fails to predict the observed decrease in
spreading rate with increasing Mach number for compressible mixing and other free shear
layers. To account for these effects in the k- models in ANSYS FLUENT, the dilatation
dissipation term, YM , is included in the k equation. This term is modeled according to
a proposal by Sarkar [300]:
YM = 2ρM2t
(4.4-27)
where Mt is the turbulent Mach number, defined as
s
Mt =
where a (≡
√
k
a2
(4.4-28)
γRT ) is the speed of sound.
This compressibility modification always takes effect when the compressible form of the
ideal gas law is used.
4.4.7
Convective Heat and Mass Transfer Modeling in the k- Models
In ANSYS FLUENT, turbulent heat transport is modeled using the concept of Reynolds’
analogy to turbulent momentum transfer. The “modeled” energy equation is thus given
by the following:
∂
∂
∂
(ρE) +
[ui (ρE + p)] =
∂t
∂xi
∂xj
!
∂T
keff
+ ui (τij )eff + Sh
∂xj
(4.4-29)
where E is the total energy, keff is the effective thermal conductivity, and
(τij )eff is the deviatoric stress tensor, defined as
4-24
Release 12.0 c ANSYS, Inc. January 29, 2009
4.4 Standard, RNG, and Realizable k- Models
(τij )eff = µeff
∂uj
∂ui
+
∂xi ∂xj
!
∂uk
2
− µeff
δij
3
∂xk
The term involving (τij )eff represents the viscous heating, and is always computed in the
density-based solvers. It is not computed by default in the pressure-based solver, but it
can be enabled in the Viscous Model dialog box.
Additional terms may appear in the energy equation, depending on the physical models
you are using. See Section 5.2.1: Heat Transfer Theory for more details.
For the standard and realizable k- models, the effective thermal conductivity is given
by
keff = k +
c p µt
Prt
where k, in this case, is the thermal conductivity. The default value of the turbulent
Prandtl number is 0.85. You can change the value of the turbulent Prandtl number in
the Viscous Model dialog box.
For the RNG k- model, the effective thermal conductivity is
keff = αcp µeff
where α is calculated from Equation 4.4-9, but with α0 = 1/Pr = k/µcp .
The fact that α varies with µmol /µeff , as in Equation 4.4-9, is an advantage of the RNG k-
model. It is consistent with experimental evidence indicating that the turbulent Prandtl
number varies with the molecular Prandtl number and turbulence [159]. Equation 4.4-9
works well across a very broad range of molecular Prandtl numbers, from liquid metals
(Pr ≈ 10−2 ) to paraffin oils (Pr ≈ 103 ), which allows heat transfer to be calculated in
low-Reynolds-number regions. Equation 4.4-9 smoothly predicts the variation of effective
Prandtl number from the molecular value (α = 1/Pr) in the viscosity-dominated region
to the fully turbulent value (α = 1.393) in the fully turbulent regions of the flow.
Turbulent mass transfer is treated similarly. For the standard and realizable k- models,
the default turbulent Schmidt number is 0.7. This default value can be changed in the
Viscous Model dialog box. For the RNG model, the effective turbulent diffusivity for
mass transfer is calculated in a manner that is analogous to the method used for the heat
transport. The value of α0 in Equation 4.4-9 is α0 = 1/Sc, where Sc is the molecular
Schmidt number.
Release 12.0 c ANSYS, Inc. January 29, 2009
4-25
Turbulence
4.5
Standard and SST k-ω Models
This section describes the theory behind the Standard and SST k-ω model. Information
is presented in the following sections:
• Section 4.5.1: Standard k-ω Model
• Section 4.5.2: Shear-Stress Transport (SST) k-ω Model
• Section 4.5.3: Wall Boundary Conditions
For details about using the models in ANSYS FLUENT, see Chapter 12: Modeling Turbulence
and Section 12.7: Setting Up the k-ω Model in the separate User’s Guide.
This section presents the standard [379] and shear-stress transport (SST) [224] k-ω models. Both models have similar forms, with transport equations for k and ω. The major
ways in which the SST model [225] differs from the standard model are as follows:
• gradual change from the standard k-ω model in the inner region of the boundary
layer to a high-Reynolds-number version of the k- model in the outer part of the
boundary layer
• modified turbulent viscosity formulation to account for the transport effects of the
principal turbulent shear stress
The transport equations, methods of calculating turbulent viscosity, and methods of
calculating model constants and other terms are presented separately for each model.
4.5.1
Standard k-ω Model
Overview
The standard k-ω model in ANSYS FLUENT is based on the Wilcox k-ω model [379],
which incorporates modifications for low-Reynolds-number effects, compressibility, and
shear flow spreading. The Wilcox model predicts free shear flow spreading rates that are
in close agreement with measurements for far wakes, mixing layers, and plane, round,
and radial jets, and is thus applicable to wall-bounded flows and free shear flows. A
variation of the standard k-ω model called the SST k-ω model is also available in ANSYS
FLUENT, and is described in Section 4.5.2: Shear-Stress Transport (SST) k-ω Model.
The standard k-ω model is an empirical model based on model transport equations for
the turbulence kinetic energy (k) and the specific dissipation rate (ω), which can also be
thought of as the ratio of to k [379].
As the k-ω model has been modified over the years, production terms have been added
to both the k and ω equations, which have improved the accuracy of the model for
predicting free shear flows.
4-26
Release 12.0 c ANSYS, Inc. January 29, 2009
4.5 Standard and SST k-ω Models
Transport Equations for the Standard k-ω Model
The turbulence kinetic energy, k, and the specific dissipation rate, ω, are obtained from
the following transport equations:
∂
∂
∂
(ρk) +
(ρkui ) =
∂t
∂xi
∂xj
∂k
Γk
∂xj
!
∂
∂
∂
(ρω) +
(ρωui ) =
∂t
∂xi
∂xj
∂ω
Γω
∂xj
!
+ G k − Yk + S k
(4.5-1)
+ G ω − Yω + S ω
(4.5-2)
and
In these equations, Gk represents the generation of turbulence kinetic energy due to mean
velocity gradients. Gω represents the generation of ω. Γk and Γω represent the effective
diffusivity of k and ω, respectively. Yk and Yω represent the dissipation of k and ω due
to turbulence. All of the above terms are calculated as described below. Sk and Sω are
user-defined source terms.
Modeling the Effective Diffusivity
The effective diffusivities for the k-ω model are given by
µt
σk
µt
= µ+
σω
Γk = µ +
(4.5-3)
Γω
(4.5-4)
where σk and σω are the turbulent Prandtl numbers for k and ω, respectively. The
turbulent viscosity, µt , is computed by combining k and ω as follows:
µt = α ∗
Release 12.0 c ANSYS, Inc. January 29, 2009
ρk
ω
(4.5-5)
4-27
Turbulence
Low-Reynolds-Number Correction
The coefficient α∗ damps the turbulent viscosity causing a low-Reynolds-number correction. It is given by
∗
α =
∗
α∞
α0∗ + Ret /Rk
1 + Ret /Rk
!
(4.5-6)
where
ρk
µω
= 6
βi
=
3
= 0.072
Ret =
(4.5-7)
Rk
(4.5-8)
α0∗
βi
(4.5-9)
(4.5-10)
∗
Note that, in the high-Reynolds-number form of the k-ω model, α∗ = α∞
= 1.
Modeling the Turbulence Production
Production of k
The term Gk represents the production of turbulence kinetic energy. From the exact
equation for the transport of k, this term may be defined as
Gk = −ρu0i u0j
∂uj
∂xi
(4.5-11)
To evaluate Gk in a manner consistent with the Boussinesq hypothesis,
G k = µt S 2
(4.5-12)
where S is the modulus of the mean rate-of-strain tensor, defined in the same way as for
the k- model (see Equation 4.4-22).
4-28
Release 12.0 c ANSYS, Inc. January 29, 2009
4.5 Standard and SST k-ω Models
Production of ω
The production of ω is given by
ω
Gω = α Gk
k
(4.5-13)
where Gk is given by Equation 4.5-11.
The coefficient α is given by
α∞
α= ∗
α
α0 + Ret /Rω
1 + Ret /Rω
!
(4.5-14)
where Rω = 2.95. α∗ and Ret are given by Equations 4.5-6 and 4.5-7, respectively.
Note that, in the high-Reynolds-number form of the k-ω model, α = α∞ = 1.
Modeling the Turbulence Dissipation
Dissipation of k
The dissipation of k is given by
Yk = ρ β ∗ fβ ∗ k ω
(4.5-15)
where
fβ ∗ =
1
1+680χ2k
1+400χ2k
χk ≤ 0
χk > 0
(4.5-16)
where
χk ≡
1 ∂k ∂ω
ω 3 ∂xj ∂xj
(4.5-17)
and
β ∗ = βi∗ [1 + ζ ∗ F (Mt )]
!
4/15 + (Ret /Rβ )4
∗
∗
βi = β∞
1 + (Ret /Rβ )4
ζ ∗ = 1.5
Release 12.0 c ANSYS, Inc. January 29, 2009
(4.5-18)
(4.5-19)
(4.5-20)
4-29
Turbulence
Rβ = 8
∗
β∞
= 0.09
(4.5-21)
(4.5-22)
where Ret is given by Equation 4.5-7.
Dissipation of ω
The dissipation of ω is given by
Yω = ρ β fβ ω 2
(4.5-23)
where
1 + 70χω
1 + 80χω
Ωij Ωjk Ski
=
∗ ω)3
(β∞
!
1 ∂ui
∂uj
=
−
2 ∂xj
∂xi
fβ =
(4.5-24)
χω
(4.5-25)
Ωij
(4.5-26)
The strain rate tensor, Sij is defined in Equation 4.3-11. Also,
β∗
β = βi 1 − i ζ ∗ F (Mt )
βi
"
#
(4.5-27)
βi∗ and F (Mt ) are defined by Equations 4.5-19 and 4.5-28, respectively.
Compressibility Correction
The compressibility function, F (Mt ), is given by
(
F (Mt ) =
0
Mt ≤ Mt0
M2t − M2t0 Mt > Mt0
(4.5-28)
where
2k
a2
= 0.25
M2t ≡
Mt0
a =
4-30
q
γRT
(4.5-29)
(4.5-30)
(4.5-31)
Release 12.0 c ANSYS, Inc. January 29, 2009
4.5 Standard and SST k-ω Models
∗
Note that, in the high-Reynolds-number form of the k-ω model, βi∗ = β∞
. In the incompressible form, β ∗ = βi∗ .
Model Constants
1
∗
∗
= 0.09, βi = 0.072, Rβ = 8
α∞
= 1, α∞ = 0.52, α0 = , β∞
9
Rk = 6, Rω = 2.95, ζ ∗ = 1.5, Mt0 = 0.25, σk = 2.0, σω = 2.0
4.5.2
Shear-Stress Transport (SST) k-ω Model
Overview
The shear-stress transport (SST) k-ω model was developed by Menter [224] to effectively
blend the robust and accurate formulation of the k-ω model in the near-wall region with
the free-stream independence of the k- model in the far field. To achieve this, the k-
model is converted into a k-ω formulation. The SST k-ω model is similar to the standard
k-ω model, but includes the following refinements:
• The standard k-ω model and the transformed k- model are both multiplied by a
blending function and both models are added together. The blending function is
designed to be one in the near-wall region, which activates the standard k-ω model,
and zero away from the surface, which activates the transformed k- model.
• The SST model incorporates a damped cross-diffusion derivative term in the ω
equation.
• The definition of the turbulent viscosity is modified to account for the transport of
the turbulent shear stress.
• The modeling constants are different.
These features make the SST k-ω model more accurate and reliable for a wider class
of flows (e.g., adverse pressure gradient flows, airfoils, transonic shock waves) than the
standard k-ω model. Other modifications include the addition of a cross-diffusion term
in the ω equation and a blending function to ensure that the model equations behave
appropriately in both the near-wall and far-field zones.
Release 12.0 c ANSYS, Inc. January 29, 2009
4-31
Turbulence
Transport Equations for the SST k-ω Model
The SST k-ω model has a similar form to the standard k-ω model:
∂
∂
∂
(ρk) +
(ρkui ) =
∂t
∂xi
∂xj
∂k
Γk
∂xj
!
e −Y +S
+G
k
k
k
(4.5-32)
+ G ω − Y ω + Dω + S ω
(4.5-33)
and
∂
∂
∂
(ρω) +
(ρωui ) =
∂t
∂xi
∂xj
∂ω
Γω
∂xj
!
e represents the generation of turbulence kinetic energy due to
In these equations, G
k
mean velocity gradients, calculated as described in Section 4.5.1: Modeling the Turbulence Production. Gω represents the generation of ω, calculated as described in Section 4.5.1: Modeling the Turbulence Production. Γk and Γω represent the effective diffusivity of k and ω, respectively, which are calculated as described below. Yk and Yω
represent the dissipation of k and ω due to turbulence, calculated as described in Section 4.5.1: Modeling the Turbulence Dissipation. Dω represents the cross-diffusion term,
calculated as described below. Sk and Sω are user-defined source terms.
Modeling the Effective Diffusivity
The effective diffusivities for the SST k-ω model are given by
µt
σk
µt
= µ+
σω
Γk = µ +
(4.5-34)
Γω
(4.5-35)
where σk and σω are the turbulent Prandtl numbers for k and ω, respectively. The
turbulent viscosity, µt , is computed as follows:
µt =
ρk
1
h
i
ω max 1∗ , SF2
α
(4.5-36)
a1 ω
where S is the strain rate magnitude and
4-32
1
F1 /σk,1 + (1 − F1 )/σk,2
1
=
F1 /σω,1 + (1 − F1 )/σω,2
σk =
(4.5-37)
σω
(4.5-38)
Release 12.0 c ANSYS, Inc. January 29, 2009
4.5 Standard and SST k-ω Models
α∗ is defined in Equation 4.5-6. The blending functions, F1 and F2 , are given by
F1 = tanh Φ41
(4.5-39)
√
"
!
k 500µ
4ρk
, 2
,
0.09ωy ρy ω
σω,2 Dω+ y 2
"
#
1 1 ∂k ∂ω
−10
= max 2ρ
, 10
σω,2 ω ∂xj ∂xj
#
Φ1 = min max
Dω+
"
√
F2 = tanh Φ22
Φ2 = max 2
k 500µ
,
0.09ωy ρy 2 ω
(4.5-40)
(4.5-41)
(4.5-42)
#
(4.5-43)
where y is the distance to the next surface and Dω+ is the positive portion of the crossdiffusion term (see Equation 4.5-52).
Modeling the Turbulence Production
Production of k
e represents the production of turbulence kinetic energy, and is defined as:
The term G
k
e = min(G , 10ρβ ∗ kω)
G
k
k
where Gk is defined in the same manner as in the standard k-ω model.
tion 4.5.1: Modeling the Turbulence Production for details.
(4.5-44)
See Sec-
Production of ω
The term Gω represents the production of ω and is given by
Gω =
α e
Gk
νt
(4.5-45)
Note that this formulation differs from the standard k-ω model. The difference between
the two models also exists in the way the term α∞ is evaluated. In the standard k-ω
model, α∞ is defined as a constant (0.52). For the SST k-ω model, α∞ is given by
α∞ = F1 α∞,1 + (1 − F1 )α∞,2
Release 12.0 c ANSYS, Inc. January 29, 2009
(4.5-46)
4-33
Turbulence
where
α∞,1 =
βi,1
κ2
q
−
∗
∗
β∞
σw,1 β∞
(4.5-47)
α∞,2 =
βi,2
κ2
q
−
∗
∗
β∞
σw,2 β∞
(4.5-48)
where κ is 0.41.
Modeling the Turbulence Dissipation
Dissipation of k
The term Yk represents the dissipation of turbulence kinetic energy, and is defined in a
similar manner as in the standard k-ω model (see Section 4.5.1: Modeling the Turbulence
Dissipation). The difference is in the way the term fβ ∗ is evaluated. In the standard k-ω
model, fβ ∗ is defined as a piecewise function. For the SST k-ω model, fβ ∗ is a constant
equal to 1. Thus,
Yk = ρβ ∗ kω
(4.5-49)
Dissipation of ω
The term Yω represents the dissipation of ω, and is defined in a similar manner as in
the standard k-ω model (see Section 4.5.1: Modeling the Turbulence Dissipation). The
difference is in the way the terms βi and fβ are evaluated. In the standard k-ω model,
βi is defined as a constant (0.072) and fβ is defined in Equation 4.5-24. For the SST k-ω
model, fβ is a constant equal to 1. Thus,
Yk = ρβω 2
(4.5-50)
Instead of having a constant value, βi is given by
βi = F1 βi,1 + (1 − F1 )βi,2
(4.5-51)
and F1 is obtained from Equation 4.5-39.
4-34
Release 12.0 c ANSYS, Inc. January 29, 2009
4.5 Standard and SST k-ω Models
Cross-Diffusion Modification
The SST k-ω model is based on both the standard k-ω model and the standard k- model.
To blend these two models together, the standard k- model has been transformed into
equations based on k and ω, which leads to the introduction of a cross-diffusion term
(Dω in Equation 4.5-33). Dω is defined as
Dω = 2 (1 − F1 ) ρσω,2
1 ∂k ∂ω
ω ∂xj ∂xj
(4.5-52)
For details about the various k- models, see Section 4.4: Standard, RNG, and Realizable
k- Models.
Model Constants
σk,1 = 1.176, σω,1 = 2.0, σk,2 = 1.0, σω,2 = 1.168
a1 = 0.31, βi,1 = 0.075 βi,2 = 0.0828
∗
∗
All additional model constants (α∞
, α∞ , α0 , β∞
, Rβ , Rk , Rω , ζ ∗ , and Mt0 ) have the same
values as for the standard k-ω model (see Section 4.5.1: Model Constants).
4.5.3
Wall Boundary Conditions
The wall boundary conditions for the k equation in the k-ω models are treated in the
same way as the k equation is treated when enhanced wall treatments are used with
the k- models. This means that all boundary conditions for wall-function meshes will
correspond to the wall function approach, while for the fine meshes, the appropriate
low-Reynolds-number boundary conditions will be applied.
In ANSYS FLUENT the value of ω at the wall is specified as
ωw =
Release 12.0 c ANSYS, Inc. January 29, 2009
ρ (u∗ )2 +
ω
µ
(4.5-53)
4-35
Turbulence
The asymptotic value of ω + in the laminar sublayer is given by
+
ω = min
ωw+ ,
6
βi (y + )2
!
(4.5-54)
where
ωw+
=
2
50
ks+
ks+ < 25
ks+
100
ks+
(4.5-55)
≥ 25
where
ρks u∗
ks+ = max 1.0,
µ
!
(4.5-56)
and ks is the roughness height.
In the logarithmic (or turbulent) region, the value of ω + is
1 du+
turb
ω+ = q
+
∗
dy
β∞
(4.5-57)
which leads to the value of ω in the wall cell as
u∗
ω=q
∗ κy
β∞
(4.5-58)
Note that in the case of a wall cell being placed in the buffer region, ANSYS FLUENT
will blend ω + between the logarithmic and laminar sublayer values.
4-36
Release 12.0 c ANSYS, Inc. January 29, 2009
4.6 k-kl-ω Transition Model
4.6
k-kl-ω Transition Model
This section describes the theory behind the k-kl-ω Transition model. For details about
using the model in ANSYS FLUENT, see Chapter 12: Modeling Turbulence and Section 12.8: Setting Up the Transition k-kl-ω Model in the separate User’s Guide.
4.6.1
Overview
The k-kl-ω transition model [364] is used to predict boundary layer development and
calculate transition onset. This model can be used to effectively address the transition
of the boundary layer from a laminar to a turbulent regime.
4.6.2
Transport Equations for the k-kl-ω Model
The k-kl-ω model is considered to be a three-equation eddy-viscosity type, which includes
transport equations for turbulent kinetic energy (kT ), laminar kinetic energy (kL ), and
the inverse turbulent time scale (ω)
DkT
∂
= PKT + R + RN AT − ωkT − DT +
Dt
∂xj
"
αT
ν+
αk
"
DkL
∂
∂kL
= PKL − R − RN AT − DL +
ν
Dt
∂xj
∂xj
∂kT
∂xj
#
(4.6-1)
#
(4.6-2)
!
"
#
√
Dω
ω
CωR
ω
kT
∂
αT ∂ω
2
2
= Cω1 PkT +
−1
(R+RN AT )−Cω2 ω +Cω3 fω αT fW 3 +
ν+
Dt
kT
fW
kT
d
∂xj
αω ∂xj
(4.6-3)
The inclusion of the turbulent and laminar fluctuations on the mean flow and energy
equations via the eddy viscosity and total thermal diffusivity is as follows:
−ui uj = νT OT
∂Ui ∂Uj
+
∂xj
∂xi
−ui θ = αθ,T OT
!
2
− kT OT δij
3
∂θ
∂xi
(4.6-4)
(4.6-5)
The effective length is defined as
λef f = M IN (Cλ d, λT )
(4.6-6)
where λT is the turbulent length scale and is defined by
Release 12.0 c ANSYS, Inc. January 29, 2009
4-37
Turbulence
√
k
ω
λT =
(4.6-7)
and the small scale energy is defined by
kT,s = fss fW kT
fW =
"
(4.6-8)
λef f
λT
(4.6-9)
Css νΩ
fss = exp −
kT
2 #
(4.6-10)
The large scale energy is given by
kT,l = kT − kT,s
(4.6-11)
Note that the sum of Equations 4.6-8 and 4.6-11 yields the turbulent kinetic energy kT .
The turbulence production term generated by turbulent fluctuations is given by
PkT = νT,s S 2
(4.6-12)
where the small-scale turbulent viscosity is νT,s
q
νT,s = fν fIN T Cµ kT,s λef f
(4.6-13)
and
Cµ =
1
A0 + As (S/ω)
fν = 1 − exp −
q
(4.6-14)
ReT,s
Aν
(4.6-15)
A damping function defining the turbulent production due to intermittency is given by
!
fIN T = M IN
4-38
kL
,1
CIN T kT OT
(4.6-16)
Release 12.0 c ANSYS, Inc. January 29, 2009
4.6 k-kl-ω Transition Model
ReT,s =
2
fW
kT
νω
(4.6-17)
In Equation 4.6-2, PkL is the production of laminar kinetic energy by large scale turbulent
fluctuations, such that
PkL = νT,l S 2
(4.6-18)
The large-scale turbulent viscosity νT,1 is modeled as
(
νT,1
0.5(kL + kT,1 )
∗
= M IN νT,1
,
S
)
(4.6-19)
where
∗
νT,1
= fτ,1 C11
Ωλ2ef f
ν
!
q
kT,1 λef f + βT S C12 φN AT d2 Ω
(4.6-20)
The limit in Equation 4.6-19 binds the realizability such that it is not violated in the
two-dimensional developing boundary layer. The time-scale-based damping function fτ,1
is
"
fτ,1
kT,1
= 1 − exp −Cτ,1 2
λef f Ω2
#
(4.6-21)
where βT S from Equation 4.6-20 is
βT S
M AX(φN AT − CT S,crit , 0)2
= 1 − exp −
AT S
φN AT =
d2 Ω
ν
!
(4.6-22)
(4.6-23)
Near-wall dissipation is given by
Release 12.0 c ANSYS, Inc. January 29, 2009
√
√
∂ k T ∂ kT
DT = 2ν
∂xj ∂xj
(4.6-24)
√
√
∂ kL ∂ kL
DL = 2ν
∂xj ∂xj
(4.6-25)
4-39
Turbulence
In Equation 4.6-1 – 4.6-3, R represents the averaged effect of the breakdown of streamwise
fluctuations into turbulence during bypass transition:
R = CR βBP kL ω/fW
(4.6-26)
βBP , which is the threshold function controls the bypass transition process:
βBP
φBP
= 1 − exp −
ABP
"
φBP = M AX
!
(4.6-27)
!
#
kT
− CBP,crit , 0
νΩ
(4.6-28)
The breakdown to turbulence due to instabilities is considered to be a natural transition
production term, given by
RN AT = CR,N AT βN AT kL Ω
(4.6-29)
"
βN AT
M AX(φN AT − CN AT,crit /fN AT,crit , 0)
= 1 − exp −
AN AT
√
fN AT,crit = 1 − exp CN C
kL d
ν
)
(4.6-30)
!
(4.6-31)
The use of ω as the scale-determining variable can lead to a reduced intermittency effect
in the outer region of a turbulent boundary layer, and consequently an elimination of
the wake region in the velocity profile. From Equation 4.6-3, the following damping is
defined as
λef f
fω = 1 − exp −0.41
λT
!4
(4.6-32)
The total eddy viscosity and eddy diffusivity included in Equations 4.6-4 and 4.6-5 are
given by
νT OT = νT,s + νT,l
αθ,T OT = fW
kT
kT OT
!
(4.6-33)
q
νT,s
+ (1 − fW )Cα,θ kT λef f
P rθ
(4.6-34)
The turbulent scalar diffusivity in Equations 4.6-1 – 4.6-3 is defined as
4-40
Release 12.0 c ANSYS, Inc. January 29, 2009
4.7 Transition SST Model
q
αT = fν Cµ,std kT,s λef f
(4.6-35)
kT OT = kT + kL
(4.6-36)
Model Constants
The model constants for the k-kl-ω transition model are listed below [364]
A0 = 4.04, As = 2.12, Aν = 6.75, ABP = 0.6
AN AT = 200, AT S = 200, CBP,crit = 1.2, CN C = 0.1
CN AT,crit = 1250, CIN T = 0.75, CT S,crit = 1000, CR,N AT = 0.02
C11 = 3.4 × 10−6 , C12 = 1.0 × 10−10 , CR = 0.12, Cα,θ = 0.035
CSS = 1.5, Cτ,1 = 4360, Cω1 = 0.44, Cω2 = 0.92
Cω3 = 0.3, CωR = 1.5, Cλ = 2.495, Cµ,std = 0.09
P rθ = 0.85, σk = 1, σω = 1.17
4.7
Transition SST Model
This section describes the theory behind the Transition SST model. Information is
presented in the following sections:
• Section 4.7.1: Overview
• Section 4.7.2: Transport Equations for the Transition SST Model
• Section 4.7.3: Specifying Inlet Turbulence Levels
For details about using the model in ANSYS FLUENT, see Chapter 12: Modeling Turbulence
and Section 12.9: Setting Up the Transition SST Model in the separate User’s Guide.
Release 12.0 c ANSYS, Inc. January 29, 2009
4-41
Turbulence
4.7.1
Overview
The transition SST model is based on the coupling of the SST k − ω transport equations
with two other transport equations, one for the intermittency and one for the transition
onset criteria, in terms of momentum-thickness Reynolds number. An ANSYS proprietary
empirical correlation (Langtry and Menter) has been developed to cover standard bypass
transition as well as flows in low free-stream turbulence environments.
In addition, a very powerful option has been included to allow you to enter your own
user-defined empirical correlation, which can then be used to control the transition onset
momentum thickness Reynolds number equation. To learn how to set up the transition
SST model, see Section 12.9: Setting Up the Transition SST Model (in the separate User’s
Guide).
4.7.2
Transport Equations for the Transition SST Model
The transport equation for the intermittency γ is defined as:
∂(ργ) ∂(ρUj γ)
∂
+
= Pγ1 − Eγ1 + Pγ2 − Eγ2 +
∂t
∂xj
∂xj
"
µt
µ+
σγ
!
∂γ
∂xj
#
(4.7-1)
The transition sources are defined as follows:
Pγ1 = 2Flength ρS[γFonset ]cγ3
Eγ1 = Pγ1 γ
(4.7-2)
where S is the strain rate magnitude. Flength is an empirical correlation that controls the
length of the transition region. The destruction/relaminarization sources are defined as
follows:
Pγ2 = (2cγ1 )ρΩγFturb
Eγ2 = cγ2 Pγ2 γ
(4.7-3)
where Ω is the vorticity magnitude. The transition onset is controlled by the following
functions:
ReV
RT
4-42
ρy 2 S
µ
ρk
=
µω
=
(4.7-4)
Release 12.0 c ANSYS, Inc. January 29, 2009
4.7 Transition SST Model
Rev
2.193Reθc
4
= min(max(Fonset1 , Fonset1
), 2.0)
Fonset1 =
Fonset2
RT 3
= max 1 −
,0
2.5
= max(Fonset2 − Fonset3 , 0)
Fonset3
Fonset
(4.7-5)
−
Fturb = e
RT
4
!
4
(4.7-6)
Reθc is the critical Reynolds number where the intermittency first starts to increase in
g and
the boundary layer. This occurs upstream of the transition Reynolds number Re
θt
the difference between the two must be obtained from an empirical correlation. Both the
g.
Flength and Reθc correlations are functions of Re
θt
The constants for the intermittency equation are:
cγ1 = 0.03; cγ2 = 50; cγ3 = 0.5; σγ = 1.0
Separation Induced Transition Correction
The modification for separation-induced transition is:
γsep = min 2max
−
RT
20
Rev
− 1, 0 Freattch , 2 Fθt
3.235Reθc
4
Freattch = e
γef f = max(γ, γsep )
(4.7-7)
The model constants in Equation 4.7-7 have been adjusted from those of Menter et
al. [226] in order to improve the predictions of separated flow transition. The main
difference is that the constant that controls the relation between Rev and Reθc was
changed from 2.193, its value for a Blasius boundary layer, to 3.235, the value at a
separation point where the shape factor is 3.5 [226]. The boundary condition for γ at a
wall is zero normal flux, while for an inlet, γ is equal to 1.0.
g is
The transport equation for the transition momentum thickness Reynolds number Re
θt
"
g)
g)
g
∂(ρRe
∂(ρUj Re
∂
∂ Re
θt
θt
θt
+
= Pθt +
σθt (µ + µt )
∂t
∂xj
∂xj
∂xj
Release 12.0 c ANSYS, Inc. January 29, 2009
#
(4.7-8)
4-43
Turbulence
The source term is defined as follows:
ρ
g )(1.0 − F )
Pθt = cθt (Reθt − Re
θt
θt
t
500µ
t =
ρU 2
) , 1.0 − γ − 1/50
1.0 − 1/50
4
− yδ
Fθt = min max Fwake e(
gµ
Re
θt
ρU
15
δBL =
θBL
2
50Ωy
δ =
δBL
U
!2
, 1.0
(4.7-9)
(4.7-10)
θBL =
ρωy 2
µ
Reω 2
= e−( 1E+5 )
(4.7-11)
Reω =
Fwake
(4.7-12)
g equation are:
The model constants for the Re
θt
cθt = 0.03 σθt = 2.0
g at a wall is zero flux. The boundary condition for
The boundary condition for Re
θt
g at an inlet should be calculated from the empirical correlation based on the inlet
Re
θt
turbulence intensity.
The model contains three empirical correlations. ReΘt is the transition onset as observed
in experiments. This has been modified from Menter et al. [226] in order to improve the
predictions for natural transition. It is used in Equation 4.7-9. Flength is the length of the
transition zone and is substituted in Equation 4.7-2. ReΘc is the point where the model
is activated in order to match both ReΘt and Flength , and is used in Equation 4.7-5. At
present, these empirical correlations are proprietary and are not given in this manual.
ReΘt = f (T u, λ)
g )
Flength = f (Re
Θt
g )
ReΘc = f (Re
Θt
4-44
(4.7-13)
Release 12.0 c ANSYS, Inc. January 29, 2009
4.7 Transition SST Model
The first empirical correlation is a function of the local turbulence intensity, T u, and the
Thwaites’ pressure gradient coefficient λθ is defined as
λθ = (θ2 /v)dU/ds
(4.7-14)
where dU/ds is the acceleration in the streamwise direction.
Coupling the Transition Model and SST Transport Equations
The transition model interacts with the SST turbulence model, as follows:
∂
∂
f −D
g+ ∂
(ρk) +
(ρuj k) = P
k
k
∂t
∂xj
∂xj
∂k
(µ + σk µt )
∂xj
!
(4.7-15)
f =γ P
P
k
ef f k
(4.7-16)
g = min(max(γ , 0.1), 1.0)D
D
k
ef f
k
(4.7-17)
√
ρy k
Ry =
µ
−
F3 = e
Ry
120
(4.7-18)
3
Ft = max(F1orig , F3 )
(4.7-19)
(4.7-20)
where Pk and Dk are the original production and destruction terms for the SST model
and F1orig is the original SST blending function. Note that the production term in the
ω-equation is not modified. The rationale behind the above model formulation is given
in detail in Menter et al. [226].
In order to capture the laminar and transitional boundary layers correctly, the mesh must
have a y + of approximately one. If the y + is too large (i.e. > 5), then the transition
onset location moves upstream with increasing y + . It is recommended to use the bounded
second order upwind based discretization for the mean flow, turbulence and transition
equations.
Release 12.0 c ANSYS, Inc. January 29, 2009
4-45
Turbulence
4.7.3
Specifying Inlet Turbulence Levels
It has been observed that the turbulence intensity specified at an inlet can decay quite
rapidly depending on the inlet viscosity ratio (µt /µ) (and hence turbulence eddy frequency). As a result, the local turbulence intensity downstream of the inlet can be much
smaller than the inlet value (see Figure 4.7.1). Typically, the larger the inlet viscosity
ratio, the smaller the turbulent decay rate. However, if too large a viscosity ratio is specified (i.e., >100), the skin friction can deviate significantly from the laminar value. There
is experimental evidence that suggests that this effect occurs physically; however, at this
point it is not clear how accurately the transition model reproduces this behavior. For
this reason, if possible, it is desirable to have a relatively low (i.e ≈1 – 10) inlet viscosity
ratio and to estimate the inlet value of turbulence intensity such that at the leading edge
of the blade/airfoil, the turbulence intensity has decayed to the desired value. The decay
of turbulent kinetic energy can be calculated with the following analytical solution:
k = kinlet (1 + ωinlet βt)
−β ∗
β
(4.7-21)
For the SST turbulence model in the freestream the constants are:
β = 0.09, β ∗ = 0.0828
The time scale can be determined as follows:
t=
x
V
(4.7-22)
where x is the streamwise distance downstream of the inlet and V is the mean convective
velocity. The eddy viscosity is defined as:
µt =
ρk
ω
(4.7-23)
The decay of turbulent kinetic energy equation can be rewritten in terms of inlet turbulence intensity (Tuinlet ) and eddy viscosity ratio (µt /µ) as follows:
Tu = Tu2inlet
4-46
"
3ρV xβTu2inlet
1+
2µ(µt /µ)
# −β ∗
0.5
β
(4.7-24)
Release 12.0 c ANSYS, Inc. January 29, 2009
4.8 The v 2 -f Model
Figure 4.7.1: Decay of Turbulence Intensity (Tu ) as a Function of Streamwise
Distance (x)
4.8
The v 2 -f Model
The v 2 -f model is similar to the standard k- model, but incorporates near-wall turbulence anisotropy and non-local pressure-strain effects. A limitation of the v 2 -f model is
that it cannot be used to solve Eulerian multiphase problems, whereas the k- model is
typically used in such applications. The v 2 -f model is a general low-Reynolds-number
turbulence model that is valid all the way up to solid walls, and therefore does not need
to make use of wall functions. Although the model was originally developed for attached
or mildly separated boundary layers [82], it also accurately simulates flows dominated by
separation [24].
The distinguishing feature of the v 2 -f model is its use of the velocity scale, v 2 , instead
of the turbulent kinetic energy, k, for evaluating the eddy viscosity. v 2 , which can be
thought of as the velocity fluctuation normal to the streamlines, has shown to provide
the right scaling in representing the damping of turbulent transport close to the wall, a
feature that k does not provide.
For more information about the theoretical background and usage of the v 2 -f model,
please visit the User Services Center (www.fluentusers.com) .
Release 12.0 c ANSYS, Inc. January 29, 2009
4-47
Turbulence
4.9
Reynolds Stress Model (RSM)
This section describes the theory behind the Reynolds Stress model (RSM). Information
is presented in the following sections:
• Section 4.9.1: Overview
• Section 4.9.2: Reynolds Stress Transport Equations
• Section 4.9.3: Modeling Turbulent Diffusive Transport
• Section 4.9.4: Modeling the Pressure-Strain Term
• Section 4.9.5: Effects of Buoyancy on Turbulence
• Section 4.9.6: Modeling the Turbulence Kinetic Energy
• Section 4.9.7: Modeling the Dissipation Rate
• Section 4.9.8: Modeling the Turbulent Viscosity
• Section 4.9.9: Wall Boundary Conditions
• Section 4.9.10: Convective Heat and Mass Transfer Modeling
For details about using the model in ANSYS FLUENT, see Chapter 12: Modeling Turbulence
and Section 12.10: Setting Up the Reynolds Stress Model in the separate User’s Guide.
4.9.1
Overview
The Reynolds stress model (RSM) [108, 177, 178] is the most elaborate type of turbulence model that ANSYS FLUENT provides. Abandoning the isotropic eddy-viscosity
hypothesis, the RSM closes the Reynolds-averaged Navier-Stokes equations by solving
transport equations for the Reynolds stresses, together with an equation for the dissipation rate. This means that five additional transport equations are required in 2D flows,
in comparison to seven additional transport equations solved in 3D.
Since the RSM accounts for the effects of streamline curvature, swirl, rotation, and rapid
changes in strain rate in a more rigorous manner than one-equation and two-equation
models, it has greater potential to give accurate predictions for complex flows. However,
the fidelity of RSM predictions is still limited by the closure assumptions employed to
model various terms in the exact transport equations for the Reynolds stresses. The
modeling of the pressure-strain and dissipation-rate terms is particularly challenging, and
often considered to be responsible for compromising the accuracy of RSM predictions.
4-48
Release 12.0 c ANSYS, Inc. January 29, 2009
4.9 Reynolds Stress Model (RSM)
The RSM might not always yield results that are clearly superior to the simpler models
in all classes of flows to warrant the additional computational expense. However, use
of the RSM is a must when the flow features of interest are the result of anisotropy in
the Reynolds stresses. Among the examples are cyclone flows, highly swirling flows in
combustors, rotating flow passages, and the stress-induced secondary flows in ducts.
The exact form of the Reynolds stress transport equations may be derived by taking moments of the exact momentum equation. This is a process wherein the exact momentum
equations are multiplied by a fluctuating property, the product then being Reynoldsaveraged. Unfortunately, several of the terms in the exact equation are unknown and
modeling assumptions are required in order to close the equations.
4.9.2
Reynolds Stress Transport Equations
The exact transport equations for the transport of the Reynolds stresses, ρu0i u0j , may be
written as follows:
∂
∂
∂
ρ u0i u0j u0k + p δkj u0i + δik u0j
(ρ u0i u0j )
+
(ρuk u0i u0j ) = −
∂xk
∂x
|∂t {z
}
|
{z
}
| k {z
}
Local Time Derivative Cij ≡ Convection
DT,ij ≡ Turbulent Diffusion
"
+
#
∂
∂
µ
(u0 u0 )
∂xk
∂xk i j
|
{z
− ρ
}
DL,ij ≡ Molecular Diffusion
|
u0i u0k
{z
Pij ≡ Stress Production
∂u0i ∂u0j
p
+
∂xj
∂xi
+
|
∂ui
∂uj
+ u0j u0k
∂xk
∂xk
{z
!
−
}
φij ≡ Pressure Strain
−2ρΩk u0j u0m ikm + u0i u0m jkm
|
}
{z
Fij ≡ Production by System Rotation
+
!
− ρβ(gi u0j θ + gj u0i θ)
|
}
{z
}
Gij ≡ Buoyancy Production
∂u0i ∂u0j
∂x{z
k ∂xk
|
}
ij ≡ Dissipation
2µ
Suser
(4.9-1)
| {z }
User-Defined Source Term
Of the various terms in these exact equations, Cij , DL,ij , Pij , and Fij do not require any
modeling. However, DT,ij , Gij , φij , and ij need to be modeled to close the equations.
The following sections describe the modeling assumptions required to close the equation
set.
Release 12.0 c ANSYS, Inc. January 29, 2009
4-49
Turbulence
4.9.3
Modeling Turbulent Diffusive Transport
DT,ij can be modeled by the generalized gradient-diffusion model of Daly and Harlow [67]:
DT,ij
∂
ku0 u0 ∂u0 u0
= Cs
ρ k ` i j
∂xk
∂x`
!
(4.9-2)
However, this equation can result in numerical instabilities, so it has been simplified in
ANSYS FLUENT to use a scalar turbulent diffusivity as follows [194]:
DT,ij
µt ∂u0i u0j
σk ∂xk
∂
=
∂xk
!
(4.9-3)
The turbulent viscosity, µt , is computed using Equation 4.9-33.
Lien and Leschziner [194] derived a value of σk = 0.82 by applying the generalized
gradient-diffusion model, Equation 4.9-2, to the case of a planar homogeneous shear
flow. Note that this value of σk is different from that in the standard and realizable k-
models, in which σk = 1.0.
4.9.4
Modeling the Pressure-Strain Term
Linear Pressure-Strain Model
By default in ANSYS FLUENT, the pressure-strain term, φij , in Equation 4.9-1 is modeled
according to the proposals by Gibson and Launder [108], Fu et al. [104], and Launder [176,
177].
The classical approach to modeling φij uses the following decomposition:
φij = φij,1 + φij,2 + φij,w
(4.9-4)
where φij,1 is the slow pressure-strain term, also known as the return-to-isotropy term,
φij,2 is called the rapid pressure-strain term, and φij,w is the wall-reflection term.
The slow pressure-strain term, φij,1 , is modeled as
φij,1 ≡ −C1 ρ
0 0 2
u u − δij k
k i j 3
(4.9-5)
with C1 = 1.8.
The rapid pressure-strain term, φij,2 , is modeled as
4-50
Release 12.0 c ANSYS, Inc. January 29, 2009
4.9 Reynolds Stress Model (RSM)
φij,2 ≡ −C2
2
(Pij + Fij + 5/6Gij − Cij ) − δij (P + 5/6G − C)
3
(4.9-6)
where C2 = 0.60, Pij , Fij , Gij , and Cij are defined as in Equation 4.9-1, P =
G = 12 Gkk , and C = 12 Ckk .
1
P ,
2 kk
The wall-reflection term, φij,w , is responsible for the redistribution of normal stresses near
the wall. It tends to damp the normal stress perpendicular to the wall, while enhancing
the stresses parallel to the wall. This term is modeled as
φij,w
3
3
C` k 3/2
≡
u0k u0m nk nm δij − u0i u0k nj nk − u0j u0k ni nk
k
2
2
d
3/2
3
3
C
`k
+ C20 φkm,2 nk nm δij − φik,2 nj nk − φjk,2 ni nk
2
2
d
C10
(4.9-7)
where C10 = 0.5, C20 = 0.3, nk is the xk component of the unit normal to the wall, d is
the normal distance to the wall, and C` = Cµ3/4 /κ, where Cµ = 0.09 and κ is the von
Kármán constant (= 0.4187).
φij,w is included by default in the Reynolds stress model.
Low-Re Modifications to the Linear Pressure-Strain Model
When the RSM is applied to near-wall flows using the enhanced wall treatment described
in Section 4.12.4: Two-Layer Model for Enhanced Wall Treatment, the pressure-strain
model needs to be modified. The modification used in ANSYS FLUENT specifies the
values of C1 , C2 , C10 , and C20 as functions of the Reynolds stress invariants and the
turbulent Reynolds number, according to the suggestion of Launder and Shima [179]:
n
h
C1 = 1 + 2.58AA2 0.25 1 − exp −(0.0067Ret )2
√
C2 = 0.75 A
2
C10 = − C1 + 1.67
3 "
#
2
C − 16
0
3 2
C2 = max
,0
C2
io
(4.9-8)
(4.9-9)
(4.9-10)
(4.9-11)
with the turbulent Reynolds number defined as Ret = (ρk 2 /µ). The flatness parameter
A and tensor invariants, A2 and A3 , are defined as
Release 12.0 c ANSYS, Inc. January 29, 2009
4-51
Turbulence
9
A ≡ 1 − (A2 − A3 )
8
A2 ≡ aik aki
A3 ≡ aik akj aji
(4.9-12)
(4.9-13)
(4.9-14)
aij is the Reynolds-stress anisotropy tensor, defined as
−ρu0i u0j + 23 ρkδij
aij = −
ρk
!
(4.9-15)
The modifications detailed above are employed only when the enhanced wall treatment
is selected in the Viscous Model dialog box.
Quadratic Pressure-Strain Model
An optional pressure-strain model proposed by Speziale, Sarkar, and Gatski [334] is
provided in ANSYS FLUENT. This model has been demonstrated to give superior performance in a range of basic shear flows, including plane strain, rotating plane shear, and
axisymmetric expansion/contraction. This improved accuracy should be beneficial for a
wider class of complex engineering flows, particularly those with streamline curvature.
The quadratic pressure-strain model can be selected as an option in the Viscous Model
dialog box.
This model is written as follows:
φij = − (C1 ρ +
C1∗ P ) bij
q
1
+ C2 ρ bik bkj − bmn bmn δij + C3 − C3∗ bij bij ρkSij
3
2
+ C4 ρk bik Sjk + bjk Sik − bmn Smn δij + C5 ρk (bik Ωjk + bjk Ωik )
3
(4.9-16)
where bij is the Reynolds-stress anisotropy tensor defined as
−ρu0i u0j + 23 ρkδij
bij = −
2ρk
!
(4.9-17)
The mean strain rate, Sij , is defined as
1
Sij =
2
4-52
∂uj
∂ui
+
∂xi ∂xj
!
(4.9-18)
Release 12.0 c ANSYS, Inc. January 29, 2009
4.9 Reynolds Stress Model (RSM)
The mean rate-of-rotation tensor, Ωij , is defined by
1
Ωij =
2
∂ui
∂uj
−
∂xj
∂xi
!
(4.9-19)
The constants are
C1 = 3.4, C1∗ = 1.8, C2 = 4.2, C3 = 0.8, C3∗ = 1.3, C4 = 1.25, C5 = 0.4
The quadratic pressure-strain model does not require a correction to account for the
wall-reflection effect in order to obtain a satisfactory solution in the logarithmic region
of a turbulent boundary layer. It should be noted, however, that the quadratic pressurestrain model is not available when the enhanced wall treatment is selected in the Viscous
Model dialog box.
Low-Re Stress-Omega Model
The low-Re stress-omega model is a stress-transport model that is based on the omega
equations and LRR model [379]. This model is ideal for modeling flows over curved surfaces and swirling flows. The low-Re stress-omega model can be selected in the Viscous
Model dialog box and requires no treatments of wall reflections. The closure coefficients are identical to the k-ω model (Section 4.5.1: Model Constants), however, there
are additional closure coefficients, C1 and C2 , noted below.
The low-Re stress-omega model resembles the k-ω model due to its excellent predictions
for a wide range of turbulent flows. Furthermore, low Reynolds number modifications
and surface boundary conditions for rough surfaces are similar to the k-ω model.
Equation 4.9-4 can be re-written for the low-Re stress-omega model such that wall reflections are excluded:
φij = φij,1 + φij,2
(4.9-20)
Therefore,
h
i
∗
φij = −C1 ρβRSM
ω ui 0 uj 0 − 2/3δij k − αˆ0 [Pij − 1/3Pkk δij ]
− βˆ0 [Dij − 1/3Pkk δij ] − k γˆ0 [Sij − 1/3Skk δij ]
(4.9-21)
where Dij is defined as
Release 12.0 c ANSYS, Inc. January 29, 2009
4-53
Turbulence
"
Dij = −ρ ui
0u
m
0
∂um
∂um
+ u j 0 um 0
∂xj
∂xi
#
(4.9-22)
∗
The mean strain rate Sij is defined in Equation 4.9-18 and βRSM
is defined by
∗
βRSM
= β ∗ fβ ∗
(4.9-23)
where β ∗ and fβ∗ are defined in the same way as for the standard k − ω, using Equations 4.5-16 and 4.5-22, respectively. The only difference here is that the equation for fβ∗
uses a value of 640 instead of 680, as in Equation 4.5-16.
The constants are
αˆ0 =
8 + C2 ˆ
8C2 − 2
60C2 − 4
, β0 =
, γˆ0 =
11
11
55
C1 = 1.8, C2 = 0.52
The above formulation does not require viscous damping functions to resolve the nearwall sublayer. However, inclusion of the viscous damping function [379] could improve
model predictions for certain flows. This results in the following changes:
α̂ =
1 + αˆ0 ReT /Rk
1 + ReT /Rk
β̂ = β̂0
γ̂ = γ̂0
ReT /Rk
1 + ReT /Rk
0.007 + ReT /Rk
1 + ReT /Rk
"
5/3 + ReT /Rk
C1 = 1.8
1 + ReT /Rk
#
where α̂, β̂, and γ̂ would replace αˆ0 , βˆ0 , and γˆ0 in Equation 4.9-21. The constants are
Rβ = 12, Rk = 12, Rω = 6.20
Inclusion of the low-Re viscous damping is controlled by enabling Low-Re Corrections
under k-omega Options in the Viscous Model dialog box.
4-54
Release 12.0 c ANSYS, Inc. January 29, 2009
4.9 Reynolds Stress Model (RSM)
4.9.5
Effects of Buoyancy on Turbulence
The production terms due to buoyancy are modeled as
Gij = (Ji Uj + Jj Ui ) = −β(gi uj θ + gj Ui θ)
Ui θ =
µt ∂T
(
)
Prt ∂Xi
(4.9-24)
(4.9-25)
where Prt is the turbulent Prandtl number for energy, with a default value of 0.85.
Using the definition of the coefficient of thermal expansion, β, given by Equation 4.4-24,
the following expression is obtained for Gij for ideal gases:
µt
∂ρ
∂ρ
Gij = −
gi
+ gj
ρPrt
∂xj
∂xi
i
!
(4.9-26)
Note that the buoyancy effects are not included if low-Re omega based
RSM model is used.
4.9.6 Modeling the Turbulence Kinetic Energy
In general, when the turbulence kinetic energy is needed for modeling a specific term, it
is obtained by taking the trace of the Reynolds stress tensor:
1
k = u0i u0i
2
(4.9-27)
As described in Section 4.9.9: Wall Boundary Conditions, an option is available in ANSYS
FLUENT to solve a transport equation for the turbulence kinetic energy in order to obtain
boundary conditions for the Reynolds stresses. In this case, the following model equation
is used:
∂
∂
∂
(ρk) +
(ρkui ) =
∂t
∂xi
∂xj
"
µt
µ+
σk
#
∂k
1
+ (Pii + Gii ) − ρ(1 + 2M2t ) + Sk (4.9-28)
∂xj
2
where σk = 0.82 and Sk is a user-defined source term. Equation 4.9-28 is obtainable
by contracting the modeled equation for the Reynolds stresses (Equation 4.9-1). As one
might expect, it is essentially identical to Equation 4.4-1 used in the standard k- model.
Release 12.0 c ANSYS, Inc. January 29, 2009
4-55
Turbulence
Although Equation 4.9-28 is solved globally throughout the flow domain, the values of k
obtained are used only for boundary conditions. In every other case, k is obtained from
Equation 4.9-27. This is a minor point, however, since the values of k obtained with
either method should be very similar.
4.9.7
Modeling the Dissipation Rate
The dissipation tensor, ij , is modeled as
2
ij = δij (ρ + YM )
3
(4.9-29)
where YM = 2ρM2t is an additional “dilatation dissipation” term according to the model
by Sarkar [300]. The turbulent Mach number in this term is defined as
s
Mt =
k
a2
(4.9-30)
√
where a (≡ γRT ) is the speed of sound. This compressibility modification always takes
effect when the compressible form of the ideal gas law is used.
The scalar dissipation rate, , is computed with a model transport equation similar to
that used in the standard k- model:
∂
∂
∂
(ρ) +
(ρui ) =
∂t
∂xi
∂xj
"
µt
µ+
σ
∂
1
2
C1 [Pii + C3 Gii ] − C2 ρ + S (4.9-31)
∂xj
2
k
k
#
where σ = 1.0, C1 = 1.44, C2 = 1.92, C3 is evaluated as a function of the local flow
direction relative to the gravitational vector, as described in Section 4.4.5: Effects of
Buoyancy on Turbulence in the k- Models, and S is a user-defined source term.
In the case when the Reynolds Stress model is coupled with the omega equation, the
dissipation tensor ij is modeled as
∗
ij = 2/3δij ρβRSM
kω
(4.9-32)
∗
Where βRSM
is defined in Section 4.9.4: Modeling the Pressure-Strain Term and the
specific dissipation rate ω is computed in the same way as for the standard k − ω model,
using Equation 4.5-2.
4-56
Release 12.0 c ANSYS, Inc. January 29, 2009
4.9 Reynolds Stress Model (RSM)
4.9.8
Modeling the Turbulent Viscosity
The turbulent viscosity, µt , is computed similarly to the k- models:
µt = ρCµ
k2
(4.9-33)
where Cµ = 0.09.
4.9.9 Wall Boundary Conditions
The RSM model in ANSYS FLUENT requires boundary conditions for individual Reynolds
stresses, u0i u0j , and for the turbulence dissipation rate, (or ω if the low-Re stress-omega
model is used). These quantities can be input directly or derived from the turbulence
intensity and characteristic length (Section 12.14.3: Reynolds Stress Model in the separate
User’s Guide).
At walls, ANSYS FLUENT computes the near-wall values of the Reynolds stresses and
from wall functions (see Section 4.12.2: Standard Wall Functions, Section 4.12.3: NonEquilibrium Wall Functions, and Section 4.12.4: Enhanced Wall Functions). ANSYS
FLUENT applies explicit wall boundary conditions for the Reynolds stresses by using
the log-law and the assumption of equilibrium, disregarding convection and diffusion
in the transport equations for the stresses (Equation 4.9-1). Using a local coordinate
system, where τ is the tangential coordinate, η is the normal coordinate, and λ is the
binormal coordinate, the Reynolds stresses at the wall-adjacent cells (assuming standard
wall functions or non-equilibrium wall functions) are computed from
0
u0 2
u0 u0
u0τ2
u2
= 1.098, η = 0.247, λ = 0.655, − τ η = 0.255
k
k
k
k
(4.9-34)
To obtain k, ANSYS FLUENT solves the transport equation of Equation 4.9-28. For
reasons of computational convenience, the equation is solved globally, even though the
values of k thus computed are needed only near the wall; in the far field k is obtained
directly from the normal Reynolds stresses using Equation 4.9-27. By default, the values
of the Reynolds stresses near the wall are fixed using the values computed from Equation 4.9-34, and the transport equations in Equation 4.9-1 are solved only in the bulk
flow region.
Alternatively, the Reynolds stresses can be explicitly specified in terms of wall-shear
stress, instead of k:
0
u0η2
u0τ u0η
u0τ2
uλ2
=
5.1,
=
1.0,
=
2.3,
−
= 1.0
u2τ
u2τ
u2τ
u2τ
Release 12.0 c ANSYS, Inc. January 29, 2009
(4.9-35)
4-57
Turbulence
q
where uτ is the friction velocity defined by uτ ≡ τw /ρ, where τw is the wall-shear stress.
When this option is chosen, the k transport equation is not solved.
When using enhanced wall treatments as the near-wall treatment, ANSYS FLUENT applies zero flux wall boundary conditions to the Reynolds stress equations.
4.9.10
Convective Heat and Mass Transfer Modeling
With the Reynolds stress model in ANSYS FLUENT, turbulent heat transport is modeled
using the concept of Reynolds’ analogy to turbulent momentum transfer. The “modeled”
energy equation is thus given by the following:
∂
∂
∂
(ρE) +
[ui (ρE + p)] =
∂t
∂xi
∂xj
"
c p µt
k+
Prt
#
∂T
+ ui (τij )eff + Sh
∂xj
(4.9-36)
where E is the total energy and (τij )eff is the deviatoric stress tensor, defined as
(τij )eff = µeff
∂uj
∂ui
+
∂xi ∂xj
!
2
∂uk
− µeff
δij
3
∂xk
The term involving (τij )eff represents the viscous heating, and is always computed in the
density-based solvers. It is not computed by default in the pressure-based solver, but it
can be enabled in the Viscous Model dialog box. The default value of the turbulent
Prandtl number is 0.85. You can change the value of Prt in the Viscous Model dialog
box.
Turbulent mass transfer is treated similarly, with a default turbulent Schmidt number of
0.7. This default value can be changed in the Viscous Model dialog box.
4.10
Detached Eddy Simulation (DES)
This section describes the theory behind the Detached Eddy Simulation (DES) model.
Information is presented in the following sections:
• Section 4.10.1: Spalart-Allmaras Based DES Model
• Section 4.10.2: Realizable k- Based DES Model
• Section 4.10.3: SST k-ω Based DES Model
For details about using the model in ANSYS FLUENT, see Chapter 12: Modeling Turbulence
and Section 12.11: Setting Up the Detached Eddy Simulation Model in the separate User’s
Guide.
4-58
Release 12.0 c ANSYS, Inc. January 29, 2009
4.10 Detached Eddy Simulation (DES)
Overview
ANSYS FLUENT offers three different models for the detached eddy simulation: the
Spalart-Allmaras model, the realizable k- model, and the SST k-ω model.
In the DES approach, the unsteady RANS models are employed in the boundary layer,
while the LES treatment is applied to the separated regions. The LES region is normally
associated with the core turbulent region where large unsteady turbulence scales play a
dominant role. In this region, the DES models recover LES-like subgrid models. In the
near-wall region, the respective RANS models are recovered.
DES models have been specifically designed to address high Reynolds number wall
bounded flows, where the cost of a near-wall resolving Large Eddy Simulation would
be prohibitive. The difference with the LES model is that it relies only on the required
resolution in the boundary layers. The application of DES, however, may still require
significant CPU resources and therefore, as a general guideline, it is recommended that
the conventional turbulence models employing the Reynolds-averaged approach be used
for practical calculations.
The DES models, often referred to as the hybrid LES/RANS models combine RANS
modeling with LES for applications such as high-Re external aerodynamics simulations.
In ANSYS FLUENT, the DES model is based on the one-equation Spalart-Allmaras model,
the realizable k- model, and the SST k-ω model. The computational costs, when using
the DES models, is less than LES computational costs, but greater than RANS.
4.10.1
Spalart-Allmaras Based DES Model
The standard Spalart-Allmaras model uses the distance to the closest wall as the definition for the length scale d, which plays a major role in determining the level of production
and destruction of turbulent viscosity (Equations 4.3-6, 4.3-12, and 4.3-15). The DES
e
model, as proposed by Shur et al. [314] replaces d everywhere with a new length scale d,
defined as
de = min(d, Cdes ∆)
(4.10-1)
where the grid spacing, ∆, is based on the largest grid space in the x, y, or z directions
forming the computational cell. The empirical constant Cdes has a value of 0.65.
For a typical RANS grid with a high aspect ratio in the boundary layer, and where the
wall-parallel grid spacing usually exceeds δ, where δ is the size of the boundary layer,
Equation 4.10-1 will ensure that the DES model is in the RANS mode for the entire
boundary layer. However, in case of an ambiguous grid definition, where ∆ << δ, the
DES limiter can activate the LES mode inside the boundary layer, where the grid is not
fine enough to sustain resolved turbulence. Therefore, a new formulation [332] of DES
Release 12.0 c ANSYS, Inc. January 29, 2009
4-59
Turbulence
is available in ANSYS FLUENT to preserve the RANS mode throughout the boundary
layer. This is known as the delayed option or DDES for delayed DES.
The DES length scale de is re-defined according to:
de = d − fd max(0, d − Cdes ∆)
(4.10-2)
where fd is given by:
fd = 1 − tanh (8rd )3
(4.10-3)
This formulation is the default settings.
4.10.2
Realizable k- Based DES Model
This DES model is similar to the Realizable k- model discussed in Section 4.4.3: Realizable k- Model, with the exception of the dissipation term in the k equation. In the
DES model, the Realizable k- RANS dissipation term is modified such that:
3
ρk 2
Yk =
ldes
(4.10-4)
where
ldes = min(lrke , lles )
k
= Cdes ∆
lrke =
lles
(4.10-5)
3
2
(4.10-6)
(4.10-7)
where Cdes is a calibration constant used in the DES model and has a value of 0.61 and
∆ is the maximum local grid spacing (∆x, ∆y, ∆z).
For the case where ldes = lrke , you will obtain an expression for the dissipation of the k
formulation for the Realizable k- model (Section 4.4.3: Realizable k- Model):
Yk = ρ Similarly to the Spalart-Allmaras model, the delayed concept can be applied as
well to the Realizable DES model to preserve the RANS mode throughout the boundary
layer. The DES length ldes in Equation 4.10-8 is redefined such that
ldes = lrke − fd max(0, lrke − Cdes ∆)
4-60
(4.10-8)
Release 12.0 c ANSYS, Inc. January 29, 2009
4.11 Large Eddy Simulation (LES) Model
4.10.3
SST k-ω Based DES Model
The dissipation term of the turbulent kinetic energy (see Section 4.5.1: Modeling the Turbulence Dissipation) is modified for the DES turbulence model as described in Menter’s
work [225] such that
Yk = ρβ ∗ kωFDES
(4.10-9)
where FDES is expressed as
Lt
FDES = max
Cdes ∆
,1
(4.10-10)
where Cdes is a calibration constant used in the DES model and has a value of 0.61, ∆ is
the maximum local grid spacing (∆x, ∆y, ∆z).
The turbulent length scale is the parameter that defines this RANS model:
√
Lt =
k
β ∗ω
(4.10-11)
The DES-SST model also offers the option to “protect” the boundary layer from the
limiter (delayed option). This is achieved with the help of the zonal formulation of the
SST model. FDES is modified according to
Lt
FDES = max
Cdes ∆
(1 − FSST ), 1
(4.10-12)
with FSST = 0, F1 , F2 , where F1 and F2 are the blending functions of the SST model.
The default settings use F2 .
4.11
Large Eddy Simulation (LES) Model
This section describes the theory behind the Large Eddy Simulation (LES) model. Information is presented in the following sections:
• Section 4.11.1: Overview
• Section 4.11.2: Filtered Navier-Stokes Equations
• Section 4.11.3: Subgrid-Scale Models
• Section 4.11.4: Inlet Boundary Conditions for the LES Model
Release 12.0 c ANSYS, Inc. January 29, 2009
4-61
Turbulence
For details about using the model in ANSYS FLUENT, see Chapter 12: Modeling Turbulence
and Section 12.12: Setting Up the Large Eddy Simulation Model in the separate User’s
Guide.
4.11.1
Overview
Turbulent flows are characterized by eddies with a wide range of length and time scales.
The largest eddies are typically comparable in size to the characteristic length of the
mean flow. The smallest scales are responsible for the dissipation of turbulence kinetic
energy.
It is possible, in theory, to directly resolve the whole spectrum of turbulent scales using
an approach known as direct numerical simulation (DNS). No modeling is required in
DNS. However, DNS is not feasible for practical engineering problems involving high
Reynolds number flows. The cost required for DNS to resolve the entire range of scales
is proportional to Re3t , where Ret is the turbulent Reynolds number. Clearly, for high
Reynolds numbers, the cost becomes prohibitive.
In LES, large eddies are resolved directly, while small eddies are modeled. Large eddy
simulation (LES) thus falls between DNS and RANS in terms of the fraction of the
resolved scales. The rationale behind LES can be summarized as follows:
• Momentum, mass, energy, and other passive scalars are transported mostly by large
eddies.
• Large eddies are more problem-dependent. They are dictated by the geometries
and boundary conditions of the flow involved.
• Small eddies are less dependent on the geometry, tend to be more isotropic, and
are consequently more universal.
• The chance of finding a universal turbulence model is much higher for small eddies.
Resolving only the large eddies allows one to use much coarser mesh and larger timesstep sizes in LES than in DNS. However, LES still requires substantially finer meshes
than those typically used for RANS calculations. In addition, LES has to be run for
a sufficiently long flow-time to obtain stable statistics of the flow being modeled. As
a result, the computational cost involved with LES is normally orders of magnitudes
higher than that for steady RANS calculations in terms of memory (RAM) and CPU
time. Therefore, high-performance computing (e.g., parallel computing) is a necessity for
LES, especially for industrial applications.
The following sections give details of the governing equations for LES, the subgrid-scale
turbulence models, and the boundary conditions.
4-62
Release 12.0 c ANSYS, Inc. January 29, 2009
4.11 Large Eddy Simulation (LES) Model
4.11.2
Filtered Navier-Stokes Equations
The governing equations employed for LES are obtained by filtering the time-dependent
Navier-Stokes equations in either Fourier (wave-number) space or configuration (physical)
space. The filtering process effectively filters out the eddies whose scales are smaller than
the filter width or grid spacing used in the computations. The resulting equations thus
govern the dynamics of large eddies.
A filtered variable (denoted by an overbar) is defined by
φ(x) =
Z
φ(x0 )G(x, x0 )dx0
(4.11-1)
D
where D is the fluid domain, and G is the filter function that determines the scale of the
resolved eddies.
In ANSYS FLUENT, the finite-volume discretization itself implicitly provides the filtering
operation:
1 Z
φ(x) =
φ(x0 ) dx0 ,
V ν
x0 ∈ ν
(4.11-2)
where V is the volume of a computational cell. The filter function, G(x, x0 ), implied here
is then
(
0
G(x, x ) =
1/V, x0 ∈ ν
0,
x0 otherwise
(4.11-3)
The LES capability in ANSYS FLUENT is applicable to compressible flows. For the sake
of concise notation, however, the theory is presented here for incompressible flows.
Filtering the Navier-Stokes equations, one obtains
∂ρ
∂
+
(ρui ) = 0
∂t ∂xi
(4.11-4)
∂
∂
∂
∂p
∂τij
(ρui ) +
(ρui uj ) =
(σij ) −
−
∂t
∂xj
∂xj
∂xi
∂xj
(4.11-5)
and
where σij is the stress tensor due to molecular viscosity defined by
"
∂ui ∂uj
σij ≡ µ
+
∂xj
∂xi
Release 12.0 c ANSYS, Inc. January 29, 2009
!#
2 ∂ul
− µ
δij
3 ∂xl
(4.11-6)
4-63
Turbulence
and τij is the subgrid-scale stress defined by
τij ≡ ρui uj − ρui uj
4.11.3
(4.11-7)
Subgrid-Scale Models
The subgrid-scale stresses resulting from the filtering operation are unknown, and require
modeling. The subgrid-scale turbulence models in ANSYS FLUENT employ the Boussinesq hypothesis [130] as in the RANS models, computing subgrid-scale turbulent stresses
from
1
τij − τkk δij = −2µt S ij
3
(4.11-8)
where µt is the subgrid-scale turbulent viscosity. The isotropic part of the subgrid-scale
stresses τkk is not modeled, but added to the filtered static pressure term. S ij is the
rate-of-strain tensor for the resolved scale defined by
1
S ij ≡
2
∂ui ∂uj
+
∂xj
∂xi
!
(4.11-9)
For compressible flows, it is convenient to introduce the density-weighted (or Favre)
filtering operator:
φe =
ρφ
ρ
(4.11-10)
The Favre Filtered Navier-Stokes equation takes the same form as Equation 4.11-5. The
compressible form of the subgrid stress tensor is defined as:
ei u
ej
τij = ρug
i uj − ρu
(4.11-11)
This term is split into its isotropic and deviatoric parts
1
1
τij = τij − τkk δij + τkk δij
3
|
{z
}
|3 {z }
isotropic
deviatoric
(4.11-12)
The deviatoric part of the subgrid-scale stress tensor is modeled using the compressible
form of the Smagorinsky model:
1
1
τij − τkk δij = 2µt (Sij − §kk δij )
3
3
4-64
(4.11-13)
Release 12.0 c ANSYS, Inc. January 29, 2009
4.11 Large Eddy Simulation (LES) Model
As for incompressible flows, the term involving τkk can be added to the filtered pressure
or simply neglected [89]. Indeed, this term can be re-written as τkk = γM 2 sgs p where
Msgs is the subgrid Mach number. This subgrid Mach number can be expected to be
small when the turbulent Mach number of the flow is small.
ANSYS FLUENT offers four models for µt : the Smagorinsky-Lilly model, the dynamic
Smagorinsky-Lilly model, the WALE model, and the dynamic kinetic energy subgridscale model.
The subgrid-scale turbulent flux of a scalar, φ, is modeled using s subgrid-scale turbulent
Prandtl number by
qj = −
µt ∂φ
σt ∂xj
(4.11-14)
where qj is the subgrid-scale flux.
In the dynamic models, the subgrid-scale turbulent Prandtl number or Schmidt number
is obtained by applying the dynamic procedure originally proposed by Germano [106] to
the subgrid-scale flux.
Smagorinsky-Lilly Model
This simple model was first proposed by Smagorinsky [320]. In the Smagorinsky-Lilly
model, the eddy-viscosity is modeled by
µt = ρL2s S
where Ls is the mixing length for subgrid scales and S ≡
Ls is computed using
Ls = min (κd, Cs ∆)
(4.11-15)
q
2S ij S ij . In ANSYS FLUENT,
(4.11-16)
where κ is the von Kármán constant, d is the distance to the closest wall, Cs is the
Smagorinsky constant, and ∆ is the local grid scale. In ANSYS FLUENT, ∆ is computed
according to the volume of the computational cell using
∆ = V 1/3
(4.11-17)
Lilly derived a value of 0.17 for Cs for homogeneous isotropic turbulence in the inertial
subrange. However, this value was found to cause excessive damping of large-scale fluctuations in the presence of mean shear and in transitional flows as near solid boundary,
and has to be reduced in such regions. In short, Cs is not a universal constant, which
is the most serious shortcoming of this simple model. Nonetheless, a Cs value of around
Release 12.0 c ANSYS, Inc. January 29, 2009
4-65
Turbulence
0.1 has been found to yield the best results for a wide range of flows, and is the default
value in ANSYS FLUENT.
Dynamic Smagorinsky-Lilly Model
Germano et al. [106] and subsequently Lilly [197] conceived a procedure in which the
Smagorinsky model constant, Cs , is dynamically computed based on the information
provided by the resolved scales of motion. The dynamic procedure thus obviates the
need for users to specify the model constant Cs in advance.
The concept of the dynamic procedure is to apply a second filter (called the test filter) to
ˆ is equal to twice the grid filter width ∆.
the equations of motion. The new filter width ∆
Both filters produce a resolved flow field. The difference between the two resolved fields
is the contribution of the small scales whose size is in between the grid filter and the test
filter. The information related to these scales is used to compute the model constant. In
ANSYS FLUENT, the variable density formulation of the model is considered as explained
below.
At the test filtered field level, the SGS stress tensor can be expressed as:
d d b
d
Tij = ρu
i uj − (ρui ρuj /ρ)
(4.11-18)
Both Tij and τij are modeled in the same way with the Smagorinsky-Lilly model, assuming
scale similarity:
e δ )
e S
e − 1S
τij = −2Cρ∆2 S|(
kk ij
ij
3
(4.11-19)
1b
be be
b 2 |S|(
Tij = −2C ρb∆
S ij − Sekk δij )
3
(4.11-20)
In Equation 4.11-19 and Equation 4.11-20, the coefficient C is asumed to be the same
and independent of the filtering process (note that per Equation 4.11-25, C = Cs2 ). The
grid filtered SGS and the test-filtered SGS are related by the Germano identity [106] such
that:
1 dd
d
ei u
ej − (ρ
uei ρuej )
Lij = Tij − τc
ij = ρu
ρb
(4.11-21)
Where Lij is computable from the resolved large eddy field. Substituting the grid-filter
Smagorinsky-Lilly model and Equation 4.11-20 into Equation 4.11-21, the following expressions can be derived to solve for C with the contraction obtained from the least
square analysis of Lilly (1992).
4-66
Release 12.0 c ANSYS, Inc. January 29, 2009
4.11 Large Eddy Simulation (LES) Model
C=
(Lij − Lkk δij /3)
Mij Mij
(4.11-22)
With
Mij
be be
d
b 2ρ
eS
e
b |S|
= −2 ∆
S ij − ∆2 ρ |S|
ij
(4.11-23)
More details of the model implementation in ANSYS FLUENT and its validation can be
found in [165].
√
The Cs = C obtained using the dynamic Smagorinsky-Lilly model varies in time and
space over a fairly wide range. To avoid numerical instability, both the numerator and
the denominator in Equation 4.11-22 are locally averaged (or filtered) using the test-filter.
In ANSYS FLUENT, Cs is also clipped at zero and 0.23 by default.
Wall-Adapting Local Eddy-Viscosity (WALE) Model
In the WALE model [248], the eddy viscosity is modeled by
µt =
ρL2s
(Sijd Sijd )3/2
(S ij S ij )5/2 + (Sijd Sijd )5/4
(4.11-24)
where Ls and Sijd in the WALE model are defined, respectively, as
Ls = min κd, Cw V 1/3
Sijd =
1 2
1
∂ui
g ij + g 2ji − δij g 2kk , g ij =
2
3
∂xj
(4.11-25)
(4.11-26)
In ANSYS FLUENT, the default value of the WALE constant, Cw , is 0.325 and has been
found to yield satisfactory results for a wide range of flow. The rest of the notation is the
same as for the Smagorinsky-Lilly model. With this spatial operator, the WALE model
is designed to return the correct wall asymptotic (y 3 ) behavior for wall bounded flows.
Dynamic Kinetic Energy Subgrid-Scale Model
The original and dynamic Smagorinsky-Lilly models, discussed previously, are essentially
algebraic models in which subgrid-scale stresses are parameterized using the resolved velocity scales. The underlying assumption is the local equilibrium between the transferred
energy through the grid-filter scale and the dissipation of kinetic energy at small subgrid scales. The subgrid-scale turbulence can be better modeled by accounting for the
transport of the subgrid-scale turbulence kinetic energy.
Release 12.0 c ANSYS, Inc. January 29, 2009
4-67
Turbulence
The dynamic subgrid-scale kinetic energy model in ANSYS FLUENT replicates the model
proposed by Kim and Menon [168].
The subgrid-scale kinetic energy is defined as
ksgs =
1 2
uk − u2k
2
(4.11-27)
which is obtained by contracting the subgrid-scale stress in Equation 4.11-7.
The subgrid-scale eddy viscosity, µt , is computed using ksgs as
1/2
µt = Ck ksgs
∆f
(4.11-28)
where ∆f is the filter-size computed from ∆f ≡ V 1/3 .
The subgrid-scale stress can then be written as
2
1/2
τij − ksgs δij = −2Ck ksgs
∆f S ij
3
(4.11-29)
ksgs is obtained by solving its transport equation
k 3/2
∂k sgs ∂uj k sgs
∂ui
∂
+
= −τij
− Cε sgs +
∂t
∂xj
∂xj
∆f
∂xj
µt ∂ksgs
σk ∂xj
!
(4.11-30)
In the above equations, the model constants, Ck and Cε , are determined dynamically [168].
σk is hardwired to 1.0. The details of the implementation of this model in ANSYS FLUENT and its validation is given by Kim [165].
4.11.4
Inlet Boundary Conditions for the LES Model
This section describes the three algorithms available in ANSYS FLUENT to model the
fluctuating velocity at velocity inlet boundaries or pressure inlet boundaries.
No Perturbations
The stochastic components of the flow at the velocity-specified inlet boundaries are neglected if the No Perturbations option is used. In such cases, individual instantaneous
velocity components are simply set equal to their mean velocity counterparts. This option is suitable only when the level of turbulence at the inflow boundaries is negligible or
does not play a major role in the accuracy of the overall solution.
4-68
Release 12.0 c ANSYS, Inc. January 29, 2009
4.11 Large Eddy Simulation (LES) Model
Vortex Method
To generate a time-dependent inlet condition, a random 2D vortex method is considered.
With this approach, a perturbation is added on a specified mean velocity profile via a
fluctuating vorticity field (i.e. two-dimensional in the plane normal to the streamwise
direction). The vortex method is based on the Lagrangian form of the 2D evolution
equation of the vorticity and the Biot-Savart law. A particle discretization is used to
solve this equation. These particles, or “vortex points” are convected randomly and
carry information about the vorticity field. If N is the number of vortex points and A
is the area of the inlet section, the amount of vorticity carried by a given particle i is
represented by the circulation Γi and an assumed spatial distribution η:
v
u
u
Γi (x, y) = 4t
η(~x) =
πAk(x, y)
3N [2 ln(3) − 3 ln(2)]
1 −|x|2 /2σ2
2
2
2e
−
1
2e−|x| /2σ
2
2πσ
(4.11-31)
(4.11-32)
where k is the turbulence kinetic energy. The parameter σ provides control over the size
of a vortex particle. The resulting discretization for the velocity field is given by
~u(~x) =
0 2
2
N
1 X
((~xi − ~x) × ~z)(1 − e|~x−~x | /2σ )
Γi
2π i=1
|~x − ~x0i |2
(4.11-33)
Where ~z is the unit vector in the streamwise direction. Originally [311], the size of
the vortex was fixed by an ad hoc value of σ. To make the vortex method generally
applicable, a local vortex size is specified through a turbulent mixing length hypothesis. σ
is calculated from a known profile of mean turbulence kinetic energy and mean dissipation
rate at the inlet according to the following:
σ=
ck 3/2
2
(4.11-34)
where c = 0.16. To ensure that the vortex will always belong to resolved scales, the
minimum value of σ in Equation 4.11-34 is bounded by the local grid size. The sign
of the circulation of each vortex is changed randomly each characteristic time scale τ .
In the general implementation of the vortex method, this time scale represents the time
necessary for a 2D vortex convected by the bulk velocity in the boundary normal direction
to travel along n times its mean characteristic 2D size (σm ), where n is fixed equal to
100 from numerical testing. The vortex method considers only velocity fluctuations in
the plane normal to the streamwise direction.
Release 12.0 c ANSYS, Inc. January 29, 2009
4-69
Turbulence
In ANSYS FLUENT however, a simplified linear kinematic model (LKM) for the streamwise velocity fluctuations is used [219]. It is derived from a linear model that mimics
the influence of the two-dimensional vortex in the streamwise mean velocity field. If the
mean streamwise velocity U is considered as a passive scalar, the fluctuation u0 resulting
from the transport of U by the planar fluctuating velocity field v 0 is modeled by
u0 = −~v 0 · ~g
(4.11-35)
~ . When this mean
where ~g is the unit vector aligned with the mean velocity gradient ∇U
velocity gradient is equal to zero, a random perturbation can be considered instead.
Since the fluctuations are equally distributed among the velocity components, only the
prescribed kinetic energy profile can be fulfilled at the inlet of the domain. Farther
downstream, the correct fluctuation distribution is recovered [219]. However, if the distribution of the normal fluctuations is known or can be prescribed at the inlet, a rescaling
technique can be applied to the synthetic flow field in order to fulfill the normal statistic
fluctuations < uu >, < vv >, and < ww > as given at the inlet.
With the rescaling procedure, the velocity fluctuations are expressed according to:
√
< u i ui >
0∗
0
u i = ui q
(4.11-36)
2/3k
This also results in an improved representation of the turbulent flow field downstream
of the inlet. This rescaling procedure is used only if the Reynolds-Stress Components is
specified as the Reynolds-Stress Specification Method, instead of the default option K or
Turbulence Intensity.
i
Since the vortex method theory is based on the modification of the velocity
field normal to the streamwise direction, it is imperative that you create
an inlet plane normal (or as close as possible) to the streamwise velocity
direction.
Spectral Synthesizer
The spectral synthesizer provides an alternative method of generating fluctuating velocity
components. It is based on the random flow generation technique originally proposed
by Kraichnan [171] and modified by Smirnov et al. [321]. In this method, fluctuating
velocity components are computed by synthesizing a divergence-free velocity-vector field
from the summation of Fourier harmonics. In ANSYS FLUENT, the number of Fourier
harmonics is fixed to 100.
4-70
Release 12.0 c ANSYS, Inc. January 29, 2009
4.12 Near-Wall Treatments for Wall-Bounded Turbulent Flows
i
Both the vortex method and the spectral synthesizer are available for velocity inlet and pressure inlet boundary conditions. For the velocity inlet,
the fluctuations are added on the mean specified velocity. For the pressure
inlet, virtual body forces are employed in the momentum equations to add
the reconstructed turbulent fluctuations to the velocity field. These virtual
body forces are considered only in the first LES cells close to the inlet.
Both methods are also available for the DES models. However, note that
such unsteady boundary conditions are appropriate and effective mainly
for external aerodynamic flows. For internal flows, if the inlet is inside a
full RANS zone, the fluctuations generated by both methods will be rapidly
damped by the RANS turbulent eddy viscosity. Note also that whether
the inlet will be fully or partly covered by a RANS zone will depend on
the mesh and on the DES model.
Finally it should be noted that both methods require realistic inlet conditions (U,k, profiles) which can be obtained from separate RANS simulations. Unrealistic (“flat”) turbulent profiles at inlets will generate unrealistic turbulent eddies at inlets.
4.12 Near-Wall Treatments for Wall-Bounded Turbulent Flows
Information about near-wall tratments for wall-bounded turbulent flows is presented in
the following sections:
• Section 4.12.1: Overview
• Section 4.12.2: Standard Wall Functions
• Section 4.12.3: Non-Equilibrium Wall Functions
• Section 4.12.4: Enhanced Wall Treatment
• Section 4.12.5: User-Defined Wall Functions
• Section 4.12.6: LES Near-Wall Treatment
4.12.1
Overview
Turbulent flows are significantly affected by the presence of walls. Obviously, the mean
velocity field is affected through the no-slip condition that has to be satisfied at the wall.
However, the turbulence is also changed by the presence of the wall in non-trivial ways.
Very close to the wall, viscous damping reduces the tangential velocity fluctuations, while
kinematic blocking reduces the normal fluctuations. Toward the outer part of the nearwall region, however, the turbulence is rapidly augmented by the production of turbulence
kinetic energy due to the large gradients in mean velocity.
Release 12.0 c ANSYS, Inc. January 29, 2009
4-71
Turbulence
The near-wall modeling significantly impacts the fidelity of numerical solutions, inasmuch
as walls are the main source of mean vorticity and turbulence. After all, it is in the nearwall region that the solution variables have large gradients, and the momentum and other
scalar transports occur most vigorously. Therefore, accurate representation of the flow in
the near-wall region determines successful predictions of wall-bounded turbulent flows.
The k- models, the RSM, and the LES model are primarily valid for turbulent core
flows (i.e., the flow in the regions somewhat far from walls). Consideration therefore
needs to be given as to how to make these models suitable for wall-bounded flows. The
Spalart-Allmaras and k-ω models were designed to be applied throughout the boundary
layer, provided that the near-wall mesh resolution is sufficient.
Numerous experiments have shown that the near-wall region can be largely subdivided
into three layers. In the innermost layer, called the “viscous sublayer”, the flow is almost
laminar, and the (molecular) viscosity plays a dominant role in momentum and heat
or mass transfer. In the outer layer, called the fully-turbulent layer, turbulence plays
a major role. Finally, there is an interim region between the viscous sublayer and the
fully turbulent layer where the effects of molecular viscosity and turbulence are equally
important. Figure 4.12.1 illustrates these subdivisions of the near-wall region, plotted in
semi-log coordinates.
Figure 4.12.1: Subdivisions of the Near-Wall Region
In Figure 4.12.1, y + ≡ ρuτ y/µ, where uτ is the friction velocity, defined as
4-72
q
τw
.
ρ
Release 12.0 c ANSYS, Inc. January 29, 2009
4.12 Near-Wall Treatments for Wall-Bounded Turbulent Flows
Wall Functions vs. Near-Wall Model
Traditionally, there are two approaches to modeling the near-wall region. In one approach, the viscosity-affected inner region (viscous sublayer and buffer layer) is not resolved. Instead, semi-empirical formulas called “wall functions” are used to bridge the
viscosity-affected region between the wall and the fully-turbulent region. The use of wall
functions obviates the need to modify the turbulence models to account for the presence
of the wall.
In another approach, the turbulence models are modified to enable the viscosity-affected
region to be resolved with a mesh all the way to the wall, including the viscous sublayer.
For the purposes of discussion, this will be termed the “near-wall modeling” approach.
These two approaches are depicted schematically in Figure 4.12.2.
Figure 4.12.2: Near-Wall Treatments in ANSYS FLUENT
In most high-Reynolds-number flows, the wall function approach substantially saves computational resources, because the viscosity-affected near-wall region, in which the solution
variables change most rapidly, does not need to be resolved. The wall-function approach
is popular because it is economical, robust, and can be reasonably accurate. It is a
practical option for the near-wall treatments for industrial flow simulations.
The wall-function approach, however, is inadequate in situations where the low-Reynoldsnumber effects are pervasive and the assumptions underlying the wall functions cease to
be valid. Such situations require near-wall models that are valid in the viscosity-affected
region and accordingly integrable all the way to the wall.
Release 12.0 c ANSYS, Inc. January 29, 2009
4-73
Turbulence
ANSYS FLUENT provides both the wall-function approach and the near-wall modeling
approach.
Wall Functions
Wall functions are a set of semi-empirical formulas and functions that in effect “bridge”
or “link” the solution variables at the near-wall cells and the corresponding quantities
on the wall. The wall functions comprise
• laws-of-the-wall for the mean velocity and temperature (or other scalars)
• formulae for the near-wall turbulent quantities
Depending on the choice of turbulent model, ANSYS FLUENT offers three to four choices
of wall-function approaches:
• Standard Wall Functions
• Non-Equilibrium Wall Functions
• Enhanced Wall Functions (as a part of EWT)
• User-Defined Wall Functions
4.12.2
Standard Wall Functions
The standard wall functions in ANSYS FLUENT are based on the work of Launder and
Spalding [181], and have been most widely used in industrial flows. They are provided
as a default option in ANSYS FLUENT.
Momentum
The law-of-the-wall for mean velocity yields
U∗ =
1
ln(Ey ∗ )
κ
(4.12-1)
where
1/2
UP Cµ1/4 kP
U ≡
τw /ρ
∗
(4.12-2)
is the dimensionless velocity.
4-74
Release 12.0 c ANSYS, Inc. January 29, 2009
4.12 Near-Wall Treatments for Wall-Bounded Turbulent Flows
1/2
ρCµ1/4 kP yP
y ≡
µ
is the dimensionless distance from the wall.
∗
and κ
E
UP
kP
yP
µ
=
=
=
=
=
=
(4.12-3)
von Kármán constant (= 0.4187)
empirical constant (= 9.793)
mean velocity of the fluid at the near-wall node P
turbulence kinetic energy at the near-wall node P
distance from point P to the wall
dynamic viscosity of the fluid
The logarithmic law for mean velocity is known to be valid for 30 < y ∗ < 300. In ANSYS
FLUENT, the log-law is employed when y ∗ > 11.225.
When the mesh is such that y ∗ < 11.225 at the wall-adjacent cells, ANSYS FLUENT
applies the laminar stress-strain relationship that can be written as
U ∗ = y∗
(4.12-4)
It should be noted that, in ANSYS FLUENT, the laws-of-the-wall for mean velocity and
temperature are based on the wall unit, y ∗ , rather than y + (≡ ρuτ y/µ). These quantities
are approximately equal in equilibrium turbulent boundary layers.
Energy
Reynolds’ analogy between momentum and energy transport gives a similar logarithmic
law for mean temperature. As in the law-of-the-wall for mean velocity, the law-of-thewall for temperature employed in ANSYS FLUENT comprises the following two different
laws:
• linear law for the thermal conduction sublayer, or thermal viscous sublayer, where
conduction is important
• logarithmic law for the turbulent region where effects of turbulence dominate conduction
The thickness of the thermal conduction layer is, in general, different from the thickness
of the (momentum) viscous sublayer, and changes from fluid to fluid. For example, the
thickness of the thermal sublayer for a high-Prandtl-number fluid (e.g., oil) is much less
than its momentum sublayer thickness. For fluids of low Prandtl numbers (e.g., liquid
metal), on the contrary, it is much larger than the momentum sublayer thickness.
√
δ
≈ Pr
δT
Release 12.0 c ANSYS, Inc. January 29, 2009
(4.12-5)
4-75
Turbulence
In highly compressible flows, the temperature distribution in the near-wall region can
be significantly different from that of low subsonic flows, due to the heating by viscous
dissipation. In ANSYS FLUENT, the temperature wall functions include the contribution
from the viscous heating [357].
The law-of-the-wall implemented in ANSYS FLUENT has the following composite form:
1/2
(Tw − TP ) ρcp kP
T ≡
q̇
∗
1/4 1/2
C
k
Pr y ∗ + 12 ρPr µ q̇ P UP2
h
i
Pr 1 ln(Ey ∗ ) + P +
t κ
=
1/4 1/2
1 C µ kP
ρ
{Prt UP2 + (Pr − Prt )Uc2 }
q̇
2
(y ∗ < yT∗ )
(y ∗ > yT∗ )
(4.12-6)
where P is computed by using the formula given by Jayatilleke [150]:
"
P = 9.24
Pr
Prt
3/4
#
−1
h
1 + 0.28e−0.007Pr/Prt
i
(4.12-7)
and
kP
ρ
cp
q̇
TP
Tw
Pr
Prt
A
Uc
=
=
=
=
=
=
=
=
=
=
turbulent kinetic energy at the first near-wall node P
density of fluid
specific heat of fluid
wall heat flux
temperature at the first near-wall node P
temperature at the wall
molecular Prandtl number (µcp /kf )
turbulent Prandtl number (0.85 at the wall)
Van Driest constant (= 26)
mean velocity magnitude at y ∗ = yT∗
Note that, for the pressure-based solver, the terms
1/2
C 1/4 k
1
ρPr µ P UP2
2
q̇
and
1/2
o
1 Cµ1/4 kP n
ρ
Prt UP2 + (Pr − Prt )Uc2
2
q̇
will be included in Equation 4.12-6 only for compressible flow calculations.
The non-dimensional thermal sublayer thickness, yT∗ , in Equation 4.12-6 is computed as
the y ∗ value at which the linear law and the logarithmic law intersect, given the molecular
Prandtl number of the fluid being modeled.
4-76
Release 12.0 c ANSYS, Inc. January 29, 2009
4.12 Near-Wall Treatments for Wall-Bounded Turbulent Flows
The procedure of applying the law-of-the-wall for temperature is as follows. Once the
physical properties of the fluid being modeled are specified, its molecular Prandtl number
is computed. Then, given the molecular Prandtl number, the thermal sublayer thickness,
yT∗ , is computed from the intersection of the linear and logarithmic profiles, and stored.
During the iteration, depending on the y ∗ value at the near-wall cell, either the linear or
the logarithmic profile in Equation 4.12-6 is applied to compute the wall temperature Tw
or heat flux q̇ (depending on the type of the thermal boundary conditions).
The function for P given by Equation 4.12-7 is relevant for the smooth walls. For the
rough walls, however, this function is modified as follows:
Prough = 3.15Pr
0.695
1
1
−
0
E
E
0.359
E0
+
E
!0.6
P
(4.12-8)
where E 0 is the wall function constant modified for the rough walls, defined by E 0 = E/fr .
To find a description of the roughness function fr , you may refer to Equation 7.3-42 in
Section 7.3.14: Wall Roughness Effects in Turbulent Wall-Bounded Flows in the separate
User’s Guide.
Species
When using wall functions for species transport, ANSYS FLUENT assumes that species
transport behaves analogously to heat transfer. Similarly to Equation 4.12-6, the law-ofthe-wall for species can be expressed for constant property flow with no viscous dissipation
as
1/2
(Yi,w − Yi ) ρCµ1/4 kP
Y ≡
Ji,w
∗
(
=
Sc yh∗
i
Sct κ1 ln(Ey ∗ ) + Pc
(y ∗ < yc∗ )
(y ∗ > yc∗ )
(4.12-9)
where Yi is the local species mass fraction, Sc and Sct are molecular and turbulent
Schmidt numbers, and Ji,w is the diffusion flux of species i at the wall. Note that Pc and
yc∗ are calculated in a similar way as P and yT∗ , with the difference being that the Prandtl
numbers are always replaced by the corresponding Schmidt numbers.
Turbulence
In the k- models and in the RSM (if the option to obtain wall boundary conditions from
the k equation is enabled), the k equation is solved in the whole domain including the
wall-adjacent cells. The boundary condition for k imposed at the wall is
∂k
=0
∂n
Release 12.0 c ANSYS, Inc. January 29, 2009
(4.12-10)
4-77
Turbulence
where n is the local coordinate normal to the wall.
The production of kinetic energy, Gk , and its dissipation rate, , at the wall-adjacent
cells, which are the source terms in the k equation, are computed on the basis of the local
equilibrium hypothesis. Under this assumption, the production of k and its dissipation
rate are assumed to be equal in the wall-adjacent control volume.
Thus, the production of k is based on the logarithmic law and is computed from
G k ≈ τw
∂U
τw
= τw
1/2
∂y
κρkP yP
(4.12-11)
and is computed from
3/2
C 3/4 k
P = µ P
κyP
(4.12-12)
The equation is not solved at the wall-adjacent cells, but instead is computed using
Equation 4.12-12. ω and Reynolds stress equations are solved as detailed in Sections 4.5.3
and 4.9.9, respectively.
Note that, as shown here, the wall boundary conditions for the solution variables, including mean velocity, temperature, species concentration, k, and , are all taken care of
by the wall functions. Therefore, you do not need to be concerned about the boundary
conditions at the walls.
The standard wall functions described so far are provided as a default option in ANSYS
FLUENT. The standard wall functions work reasonably well for a broad range of wallbounded flows. However, they tend to become less reliable when the flow situations
depart from the ideal conditions that are assumed in their derivation. Among others,
the constant-shear and local equilibrium assumptions are the ones that most restrict the
universality of the standard wall functions. Accordingly, when the near-wall flows are
subjected to severe pressure gradients, and when the flows are in strong non-equilibrium,
the quality of the predictions is likely to be compromised.
The non-equilibrium wall functions offered as an additional option that can potentially
improve the results in such situations.
i
Standard wall functions are available with the following viscous models:
• k- models
• Reynolds Stress models
4-78
Release 12.0 c ANSYS, Inc. January 29, 2009
4.12 Near-Wall Treatments for Wall-Bounded Turbulent Flows
Scalable Wall Functions
The purpose of scalable wall functions is to force the usage of the log law in conjunction
with the standard wall functions approach. This is achieved by introducing a limiter in
the y* calculations such that
y∗e = M AX(y∗, y∗limit )
(4.12-13)
where y∗limit = 11.225. The use of Equation 4.12-13 in the context of the scalable wall
functions concept is straightforward, i.e. the y* formulation used for any standard wall
function formula is replaced by y∗e.
Scalable wall functions can be enabled only when the standard wall functions are used
and only via the following text command:
define/models/viscous/near-wall-treatment/scalable-wall-functions?
4.12.3
Non-Equilibrium Wall Functions
In addition to the standard wall function described above (which is the default near-wall
treatment) a two-layer-based, non-equilibrium wall function [166] is also available. The
key elements in the non-equilibrium wall functions are as follows:
• Launder and Spalding’s log-law for mean velocity is sensitized to pressure-gradient
effects.
• The two-layer-based concept is adopted to compute the budget of turbulence kinetic
energy (Gk ,) in the wall-neighboring cells.
The law-of-the-wall for mean temperature or species mass fraction remains the same as
in the standard wall functions described above.
The log-law for mean velocity sensitized to the pressure gradients is
Ue Cµ1/4 k 1/2
ρCµ1/4 k 1/2 y
1
= ln E
τw /ρ
κ
µ
!
(4.12-14)
where
1 dp
Ue = U −
"
yv
y
√ ln
2 dx ρκ k
yv
!
y − yv y 2
+ √ + v
µ
ρκ k
#
(4.12-15)
and yv is the physical viscous sublayer thickness, and is computed from
Release 12.0 c ANSYS, Inc. January 29, 2009
4-79
Turbulence
yv ≡
µyv∗
(4.12-16)
1/4 1/2
ρCµ kP
where yv∗ = 11.225.
The non-equilibrium wall function employs the two-layer concept in computing the budget of turbulence kinetic energy at the wall-adjacent cells, which is needed to solve the k
equation at the wall-neighboring cells. The wall-neighboring cells are assumed to consist
of a viscous sublayer and a fully turbulent layer. The following profile assumptions for
turbulence quantities are made:
(
τt =
y 2
yv
0, y < yv
k=
τw , y > yv
kP ,
kP , y < yv
=
y > yv
2νk
,
y2
3/2
k
,
C` ∗ y
y < yv
y > yv
(4.12-17)
where C` ∗ = κCµ−3/4 , and yv is the dimensional thickness of the viscous sublayer, defined
in Equation 4.12-16.
Using these profiles, the cell-averaged production of k, Gk , and the cell-averaged dissipation rate, , can be computed from the volume average of Gk and of the wall-adjacent
cells. For quadrilateral and hexahedral cells for which the volume average can be approximated with a depth-average,
!
1 Z yn ∂U
1
τw2
yn
ln
Gk ≡
τt
dy =
yn 0
∂y
κyn ρCµ1/4 kP1/2
yv
(4.12-18)
and
!
1/2
1 Z yn
1 2ν kP
yn
≡
dy =
+ ∗ ln
kP
yn 0
yn yv
C`
yv
(4.12-19)
where yn is the height of the cell (yn = 2yP ). For cells with other shapes (e.g., triangular
and tetrahedral grids), the appropriate volume averages are used.
In Equations 4.12-18 and 4.12-19, the turbulence kinetic energy budget for the wallneighboring cells is effectively depends on the proportions of the viscous sublayer and
the fully turbulent layer, which varies widely from cell to cell in highly non-equilibrium
flows. The nonequilibrium wall functions account for the effect of pressure gradients on
the distortion of the velocity profiles. In such cases the assumption of local equilibrium,
when the production of the turbulent kinetic energy is equal to the rate of its distruction,
is no longer valid. Therefore, the non-equilibrium wall functions, in effect, partly account
for the non-equilibrium effects that are neglected in the standard wall functions.
4-80
Release 12.0 c ANSYS, Inc. January 29, 2009
4.12 Near-Wall Treatments for Wall-Bounded Turbulent Flows
Standard Wall Functions vs. Non-Equilibrium Wall Functions
Because of the capability to partly account for the effects of pressure gradients, the nonequilibrium wall functions are recommended for use in complex flows involving separation,
reattachment, and impingement where the mean flow and turbulence are subjected to
pressure gradients and rapid changes. In such flows, improvements can be obtained,
particularly in the prediction of wall shear (skin-friction coefficient) and heat transfer
(Nusselt or Stanton number).
i
Non-equilibrium wall functions are available with the following turbulence
closures:
• k- models
• Reynolds Stress Transport models
Limitations of the Wall Function Approach
The standard wall functions give reasonable predictions for the majority of high-Reynoldsnumber wall-bounded flows. The non-equilibrium wall functions further extend the applicability of the wall function approach by including the effects of pressure gradient;
however, the above wall functions become less reliable when the flow conditions depart
too much from the ideal conditions underlying the wall functions. Examples are as follows:
• Pervasive low-Reynolds-number or near-wall effects (e.g., flow through a small gap
or highly viscous, low-velocity fluid flow).
• Massive transpiration through the wall (blowing/suction).
• Severe pressure gradients leading to boundary layer separations.
• Strong body forces (e.g., flow near rotating disks, buoyancy-driven flows).
• High three-dimensionality in the near-wall region (e.g., Ekman spiral flow, strongly
skewed 3D boundary layers).
If any of the above listed features prevail in the flow you are modeling, and if it is
considered critically important for the success of your simulation, you must employ the
near-wall modeling approach combined with the adequate mesh resolution in the nearwall region. ANSYS FLUENT provides the enhanced wall treatment for such situations.
This approach can be used with the k- and the RSM models.
Release 12.0 c ANSYS, Inc. January 29, 2009
4-81
Turbulence
4.12.4
Enhanced Wall Treatment
Enhanced wall treatment is a near-wall modeling method that combines a two-layer model
with so-called enhanced wall functions. If the near-wall mesh is fine enough to be able
to resolve the viscous sublayer (typically with the first near-wall node placed at y + ≈ 1),
then the enhanced wall treatment will be identical to the traditional two-layer zonal
model (see below for details). However, the restriction that the near-wall mesh must be
sufficiently fine everywhere might impose too large a computational requirement. Ideally,
one would like to have a near-wall formulation that can be used with coarse meshes
(usually referred to as wall-function meshes) as well as fine meshes (low-Reynolds-number
meshes). In addition, excessive error should not be incurred for the intermediate meshes
where the first near-wall node is placed neither in the fully turbulent region, where the
wall functions are suitable, nor in the direct vicinity of the wall at y + ≈ 1, where the
low-Reynold-number approach is adequate.
To achieve the goal of having a near-wall modeling approach that will possess the accuracy
of the standard two-layer approach for fine near-wall meshes and that, at the same time,
will not significantly reduce accuracy for wall-function meshes, ANSYS FLUENT can
combine the two-layer model with enhanced wall functions, as described in the following
sections.
Two-Layer Model for Enhanced Wall Treatment
In ANSYS FLUENT’s near-wall model, the viscosity-affected near-wall region is completely
resolved all the way to the viscous sublayer. The two-layer approach is an integral part
of the enhanced wall treatment and is used to specify both and the turbulent viscosity
in the near-wall cells. In this approach, the whole domain is subdivided into a viscosityaffected region and a fully-turbulent region. The demarcation of the two regions is
determined by a wall-distance-based, turbulent Reynolds number, Rey , defined as
√
ρy k
Rey ≡
µ
(4.12-20)
where y is the wall-normal distance calculated at the cell centers. In ANSYS FLUENT, y
is interpreted as the distance to the nearest wall:
y ≡ min k~r − ~rw k
~
rw ∈Γw
(4.12-21)
where ~r is the position vector at the field point, and ~rw is the position vector of the
wall boundary. Γw is the union of all the wall boundaries involved. This interpretation
allows y to be uniquely defined in flow domains of complex shape involving multiple
walls. Furthermore, y defined in this way is independent of the mesh topology.
4-82
Release 12.0 c ANSYS, Inc. January 29, 2009
4.12 Near-Wall Treatments for Wall-Bounded Turbulent Flows
In the fully turbulent region (Rey > Re∗y ; Re∗y = 200), the k- models or the RSM
(described in Sections 4.4 and 4.9) are employed.
In the viscosity-affected near-wall region (Rey < Re∗y ), the one-equation model of Wolfstein [382] is employed. In the one-equation model, the momentum equations and the
k equation are retained as described in Sections 4.4 and 4.9. However, the turbulent
viscosity, µt , is computed from
√
µt,2layer = ρ Cµ `µ k
(4.12-22)
where the length scale that appears in Equation 4.12-22 is computed from [51]
`µ = yC` ∗ 1 − e−Rey /Aµ
(4.12-23)
The two-layer formulation for turbulent viscosity described above is used as a part of the
enhanced wall treatment, in which the two-layer definition is smoothly blended with the
high-Reynolds-number µt definition from the outer region, as proposed by Jongen [153]:
µt,enh = λ µt + (1 − λ )µt,2layer
(4.12-24)
where µt is the high-Reynolds-number definition as described in Section 4.4: Standard,
RNG, and Realizable k- Models or 4.9 for the k- models or the RSM. A blending
function, λ , is defined in such a way that it is equal to unity away from walls and is zero
in the vicinity of the walls. The blending function has the following form:
Rey − Re∗y
1
λ =
1 + tanh
2
A
"
!#
(4.12-25)
The constant A determines the width of the blending function. By defining a width such
that the value of λ will be within 1% of its far-field value given a variation of ∆Rey , the
result is
A=
|∆Rey |
artanh(0.98)
(4.12-26)
Typically, ∆Rey would be assigned a value that is between 5% and 20% of Re∗y . The
main purpose of the blending function λ is to prevent solution convergence from being
impeded when the value of µt obtained in the outer layer does not match with the value
of µt returned by the Wolfstein model at the edge of the viscosity-affected region.
Release 12.0 c ANSYS, Inc. January 29, 2009
4-83
Turbulence
The field in the viscosity-affected region is computed from
=
k 3/2
`
(4.12-27)
The length scales that appear in Equation 4.12-27 are computed from Chen and Patel [51]:
` = yC` ∗ 1 − e−Rey /A
(4.12-28)
If the whole flow domain is inside the viscosity-affected region (Rey < 200), is not
obtained by solving the transport equation; it is instead obtained algebraically from
Equation 4.12-27. ANSYS FLUENT uses a procedure for the blending of that is similar
to the µt -blending in order to ensure a smooth transition between the algebraicallyspecified in the inner region and the obtained from solution of the transport equation
in the outer region.
The constants in Equations 4.12-23 and 4.12-28, are taken from [51] and are as follows:
C` ∗ = κCµ−3/4 ,
Aµ = 70,
A = 2C` ∗
(4.12-29)
Enhanced Wall Functions
To have a method that can extend its applicability throughout the near-wall region
(i.e., viscous sublayer, buffer region, and fully-turbulent outer region) it is necessary to
formulate the law-of-the wall as a single wall law for the entire wall region. ANSYS
FLUENT achieves this by blending the linear (laminar) and logarithmic (turbulent) lawsof-the-wall using a function suggested by Kader [155]:
1
+
Γ
u+ = eΓ u+
lam + e uturb
(4.12-30)
where the blending function is given by:
Γ=−
a(y + )4
1 + by +
(4.12-31)
where a = 0.01 and b = 5.
Similarly, the general equation for the derivative
du+
dy +
is
+
+
1 du
du+
turb
Γ dulam
Γ
=
e
+
e
dy +
dy +
dy +
4-84
(4.12-32)
Release 12.0 c ANSYS, Inc. January 29, 2009
4.12 Near-Wall Treatments for Wall-Bounded Turbulent Flows
This approach allows the fully turbulent law to be easily modified and extended to take
into account other effects such as pressure gradients or variable properties. This formula
also guarantees the correct asymptotic behavior for large and small values of y + and
reasonable representation of velocity profiles in the cases where y + falls inside the wall
buffer region (3 < y + < 10).
The enhanced wall functions were developed by smoothly blending an enhanced turbulent
wall law with the laminar wall law. The enhanced turbulent law-of-the-wall for compressible flow with heat transfer and pressure gradients has been derived by combining the
approaches of White and Cristoph [378] and Huang et al. [134]:
i
du+
1 h 0
turb
+
+ 2 1/2
=
S
(1
−
βu
−
γ(u
)
)
dy +
κy +
(4.12-33)
where
(
0
S =
1 + αy + for y + < ys+
1 + αys+ for y + ≥ ys+
(4.12-34)
and
νw dp
µ dp
=
τw u∗ dx
ρ2 (u∗ )3 dx
∗
σt qw u
σt qw
β ≡
=
cp τw Tw
ρcp u∗ Tw
σt (u∗ )2
γ ≡
2cp Tw
α ≡
(4.12-35)
(4.12-36)
(4.12-37)
where ys+ is the location at which the log-law slope is fixed. By default, ys+ = 60. The
coefficient α in Equation 4.12-33 represents the influences of pressure gradients while
the coefficients β and γ represent the thermal effects. Equation 4.12-33 is an ordinary
differential equation and ANSYS FLUENT will provide an appropriate analytical solution.
If α, β, and γ all equal 0, an analytical solution would lead to the classical turbulent
logarithmic law-of-the-wall.
The laminar law-of-the-wall is determined from the following expression:
du+
lam
= 1 + αy +
dy +
Release 12.0 c ANSYS, Inc. January 29, 2009
(4.12-38)
4-85
Turbulence
Note that the above expression only includes effects of pressure gradients through α,
while the effects of variable properties due to heat transfer and compressibility on the
laminar wall law are neglected. These effects are neglected because they are thought to be
of minor importance when they occur close to the wall. Integration of Equation 4.12-38
results in
+
u+
1+
lam = y
α +
y
2
(4.12-39)
Enhanced thermal wall functions follow the same approach developed for the profile of
u+ . The unified wall thermal formulation blends the laminar and logarithmic profiles
according to the method of Kader [155]:
T+ ≡
(Tw − TP ) ρcp uT
q̇
1
+
+
= eΓ Tlam
+ e Γ Tturb
(4.12-40)
where the notation for TP and q̇ is the same as for standard thermal wall functions (see
Equation 4.12-6). Furthermore, the blending factor Γ is defined as
Γ = −
a(Pr y + )4
1 + bPr3 y +
(4.12-41)
where Pr is the molecular Prandtl number, and the coefficients a and b are defined as in
Equation 4.12-31.
Apart from the formulation for T + in Equation 4.12-40, the enhanced thermal wall functions follow the same logic as for standard thermal wall functions (see Section 4.12.2: Energy),
resulting in the following definition for turbulent and laminar thermal wall functions:
+
Tlam
(
+
Tturb
= Prt
u+
turb
= Pr
u+
lam
ρu∗ 2
u
+
2q̇
!
(4.12-42)
ρu∗ 2
Pr
2
2
+P +
u −
− 1 (u+
c ) (u∗ )
2q̇
Prt
)
(4.12-43)
+
where the quantity u+
c is the value of u at the fictitious “crossover” between the laminar
and turbulent region. The function P is defined in the same way as for the standard wall
functions.
A similar procedure is also used for species wall functions when the enhanced wall treatment is used. In this case, the Prandtl numbers in Equations 4.12-42 and 4.12-43 are
replaced by adequate Schmidt numbers. See Section 4.12.2: Species for details about the
species wall functions.
4-86
Release 12.0 c ANSYS, Inc. January 29, 2009
4.12 Near-Wall Treatments for Wall-Bounded Turbulent Flows
The boundary conditions for the turbulence kinetic energy are similar to the ones used
with the standard wall functions (Equation 4.12-10). However, the production of turbulence kinetic energy, Gk , is computed using the velocity gradients that are consistent
with the enhanced law-of-the-wall (Equations 4.12-30 and 4.12-32), ensuring a formulation that is valid throughout the near-wall region.
i
The enhanced wall treatment is available with the following turbulence
closures:
• k- models
• Realizable k- based DES model
• Reynolds Stress Transport models
The enhanced wall functions are available with the following turbulence
models:
• Spalart-Allmaras model
• k-ω models
• k-ω based DES model
• Large Eddy Simulation
However, the enhanced wall functions are not available with SpalartAllmaras model.
4.12.5
User-Defined Wall Functions
This option is only available when one of the k- model is enabled. Selecting the UserDefined Wall Functions under Near-wall Treatment allows you to hook a Law-of-the-Wall
UDF. For more information about user-defined wall functions,
see Section 2.3.28: DEFINE WALL FUNCTIONS in the separate UDF Manual.
i
User-defined wall functions are available with the following turbulence closures:
• k- models
Release 12.0 c ANSYS, Inc. January 29, 2009
4-87
Turbulence
4.12.6
LES Near-Wall Treatment
When the mesh is fine enough to resolve the laminar sublayer, the wall shear stress is
obtained from the laminar stress-strain relationship:
u
ρuτ y
=
uτ
µ
(4.12-44)
If the mesh is too coarse to resolve the laminar sublayer, it is assumed that the centroid
of the wall-adjacent cell falls within the logarithmic region of the boundary layer, and
the law-of-the-wall is employed:
u
1
ρuτ y
= ln E
uτ
κ
µ
!
(4.12-45)
where κ is the von Kármán constant and E = 9.793. If the mesh is such that the first
near-wall point is within the buffer region, then two above laws are blended in accordance
with the Equation 4.12-30.
For the LES simulations in ANSYS FLUENT, there is an alternative near-wall approach
based on the work of Werner and Wengle [375], who proposed an analytical integration
of the power-law near-wall velocity distribution resulting in the following expressions for
the wall shear stress:
|τw | =
2µ|up |
∆z
ρ
1+B
1−B 1−B
A
2
1+B
µ
ρ∆z
+
1+B
A
B
µ
ρ∆z
|up |
2
1+B
for |up | ≤
2
µ
A 1−B
2ρ∆z
for |up | >
2
µ
1−B
A
2ρ∆z
(4.12-46)
where up is the wall-parallel velocity, A = 8.3, B = 1/7 are the constants, and ∆z is the
near-wall control volume length scale.
The Werner-Wengle wall functions can be enabled using the define/models/viscous/
near-wall-treatment/werner-wengle-wall-fn? text command.
4-88
Release 12.0 c ANSYS, Inc. January 29, 2009
Chapter 5.
Heat Transfer
This chapter describes the theory behind heat transfer in ANSYS FLUENT. Information
is provided in the following sections:
• Section 5.1: Introduction
• Section 5.2: Modeling Conductive and Convective Heat Transfer
• Section 5.3: Modeling Radiation
For more information about using heat transfer in ANSYS FLUENT, see Chapter 13: Modeling Heat Transfer in the separate User’s Guide.
5.1
Introduction
The flow of thermal energy from matter occupying one region in space to matter occupying a different region in space is known as heat transfer. Heat transfer can occur by
three main methods: conduction, convection, and radiation. Physical models involving
conduction and/or convection only are the simplest (Section 5.2: Modeling Conductive
and Convective Heat Transfer), while buoyancy-driven flow or natural convection (Section 5.2.2: Natural Convection and Buoyancy-Driven Flows Theory), and radiation models (Section 5.3: Modeling Radiation) are more complex. Depending on your problem,
ANSYS FLUENT will solve a variation of the energy equation that takes into account
the heat transfer methods you have specified. ANSYS FLUENT is also able to predict
heat transfer in periodically repeating geometries (Section 13.4: Modeling Periodic Heat
Transfer in the separate User’s Guide), thus greatly reducing the required computational
effort in certain cases.
For more information about using heat transfer models in ANSYS FLUENT, see Section 13.2: Modeling Conductive and Convective Heat Transfer, Section 13.3: Modeling
Radiation, and Section 13.4: Modeling Periodic Heat Transfer in the separate User’s
Guide.
Release 12.0 c ANSYS, Inc. January 29, 2009
5-1
Heat Transfer
5.2
Modeling Conductive and Convective Heat Transfer
ANSYS FLUENT allows you to include heat transfer within the fluid and/or solid regions
in your model. Problems ranging from thermal mixing within a fluid to conduction in
composite solids can thus be handled by ANSYS FLUENT.
When your ANSYS FLUENT model includes heat transfer you will need to activate the
relevant physical models, supply thermal boundary conditions, and input material properties that govern heat transfer and/or vary with temperature as part of the setup. For
information about setting up and using heat transfer in your ANSYS FLUENT model, see
Chapter 13: Modeling Heat Transfer in the separate User’s Guide. Information about
heat transfer theory is presented in the following subsections.
• Section 5.2.1: Heat Transfer Theory
• Section 5.2.2: Natural Convection and Buoyancy-Driven Flows Theory
5.2.1
Heat Transfer Theory
The Energy Equation
ANSYS FLUENT solves the energy equation in the following form:
X
∂
hj J~j + (τ eff · ~v ) + Sh
(ρE) + ∇ · (~v (ρE + p)) = ∇ · keff ∇T −
∂t
j
(5.2-1)
where keff is the effective conductivity (k + kt , where kt is the turbulent thermal conductivity, defined according to the turbulence model being used), and J~j is the diffusion
flux of species j. The first three terms on the right-hand side of Equation 5.2-1 represent
energy transfer due to conduction, species diffusion, and viscous dissipation, respectively.
Sh includes the heat of chemical reaction, and any other volumetric heat sources you have
defined.
In Equation 5.2-1,
E =h−
p v2
+
ρ
2
(5.2-2)
where sensible enthalpy h is defined for ideal gases as
h=
X
Yj hj
(5.2-3)
j
and for incompressible flows as
5-2
Release 12.0 c ANSYS, Inc. January 29, 2009
5.2 Modeling Conductive and Convective Heat Transfer
h=
X
Yj hj +
j
p
ρ
(5.2-4)
In Equations 5.2-3 and 5.2-4, Yj is the mass fraction of species j and
hj =
Z
T
Tref
cp,j dT
(5.2-5)
where Tref is 298.15 K.
The Energy Equation for the Non-Premixed Combustion Model
When the non-adiabatic non-premixed combustion model is enabled, ANSYS FLUENT
solves the total enthalpy form of the energy equation:
!
∂
kt
(ρH) + ∇ · (ρ~v H) = ∇ ·
∇H + Sh
∂t
cp
(5.2-6)
Under the assumption that the Lewis number (Le) = 1, the conduction and species
diffusion terms combine to give the first term on the right-hand side of the above equation
while the contribution from viscous dissipation appears in the non-conservative form as
the second term. The total enthalpy H is defined as
H=
X
Yj H j
(5.2-7)
j
where Yj is the mass fraction of species j and
Hj =
Z
T
Tref,j
cp,j dT + h0j (Tref,j )
(5.2-8)
h0j (Tref,j ) is the formation enthalpy of species j at the reference temperature Tref,j .
Inclusion of Pressure Work and Kinetic Energy Terms
Equation 5.2-1 includes pressure work and kinetic energy terms which are often negligible
in incompressible flows. For this reason, the pressure-based solver by default does not
include the pressure work or kinetic energy when you are solving incompressible flow.
If you wish to include these terms, use the define/models/energy? text command.
When asked to include pressure work in energy equation? and include kinetic
energy in energy equation?, respond by entering yes in the console window.
Pressure work and kinetic energy are always accounted for when you are modeling compressible flow or using the density-based solver.
Release 12.0 c ANSYS, Inc. January 29, 2009
5-3
Heat Transfer
Inclusion of the Viscous Dissipation Terms
Equations 5.2-1 and 5.2-6 include viscous dissipation terms, which describe the thermal
energy created by viscous shear in the flow.
When the pressure-based solver is used, ANSYS FLUENT’s default form of the energy
equation does not include them (because viscous heating is often negligible). Viscous
heating will be important when the Brinkman number, Br, approaches or exceeds unity,
where
µUe2
Br =
k∆T
(5.2-9)
and ∆T represents the temperature difference in the system.
When your problem requires inclusion of the viscous dissipation terms and you are using the pressure-based solver, you should activate the terms using the Viscous Heating
option in the Viscous Model dialog box. Compressible flows typically have Br ≥ 1.
Note, however, that when the pressure-based solver is used, ANSYS FLUENT does not
automatically activate the viscous dissipation if you have defined a compressible flow
model.
When the density-based solver is used, the viscous dissipation terms are always included
when the energy equation is solved.
Inclusion of the Species Diffusion Term
Equations 5.2-1 and 5.2-6 both include the effect of enthalpy transport due to species
diffusion.
When the pressure-based solver is used, the term
X
∇ · hj J~j
j
is included in Equation 5.2-1 by default. If you do not want to include it, you can disable
the Diffusion Energy Source option in the Species Model dialog box.
When the non-adiabatic non-premixed combustion model is being used, this term does
not explicitly appear in the energy equation, because it is included in the first term on
the right-hand side of Equation 5.2-6.
When the density-based solver is used, this term is always included in the energy equation.
5-4
Release 12.0 c ANSYS, Inc. January 29, 2009
5.2 Modeling Conductive and Convective Heat Transfer
Energy Sources Due to Reaction
Sources of energy, Sh , in Equation 5.2-1 include the source of energy due to chemical
reaction:
Sh,rxn = −
X h0j
j
Mj
Rj
(5.2-10)
where h0j is the enthalpy of formation of species j and Rj is the volumetric rate of creation
of species j.
In the energy equation used for non-adiabatic non-premixed combustion (Equation 5.2-6),
the heat of formation is included in the definition of enthalpy (see Equation 5.2-7), so
reaction sources of energy are not included in Sh .
Energy Sources Due To Radiation
When one of the radiation models is being used, Sh in Equation 5.2-1 or 5.2-6 also
includes radiation source terms. See Section 5.3: Modeling Radiation for details.
Interphase Energy Sources
It should be noted that the energy sources, Sh , also include heat transfer between the
continuous and the discrete phase. This is discussed further in Section 15.12.1: Coupling
Between the Discrete and Continuous Phases.
Energy Equation in Solid Regions
In solid regions, the energy transport equation used by ANSYS FLUENT has the following
form:
∂
(ρh) + ∇ · (~v ρh) = ∇ · (k∇T ) + Sh
∂t
where
ρ
h
k
T
Sh
(5.2-11)
= density
R
= sensible enthalpy, TTref cp dT
= conductivity
= temperature
= volumetric heat source
The second term on the left-hand side of Equation 5.2-11 represents convective energy
transfer due to rotational or translational motion of the solids. The velocity field ~v is
computed from the motion specified for the solid zone (see Section 7.2.2: Solid Conditions
in the separate User’s Guide). The terms on the right-hand side of Equation 5.2-11 are
the heat flux due to conduction and volumetric heat sources within the solid, respectively.
Release 12.0 c ANSYS, Inc. January 29, 2009
5-5
Heat Transfer
Anisotropic Conductivity in Solids
When you use the pressure-based solver, ANSYS FLUENT allows you to specify anisotropic
conductivity for solid materials. The conduction term for an anisotropic solid has the
form
∇ · (kij ∇T )
(5.2-12)
where kij is the conductivity matrix. See Section 8.5.5: Anisotropic Thermal Conductivity
for Solids in the separate User’s Guide for details on specifying anisotropic conductivity
for solid materials.
Diffusion at Inlets
The net transport of energy at inlets consists of both the convection and diffusion components. The convection component is fixed by the inlet temperature specified by you.
The diffusion component, however, depends on the gradient of the computed temperature field. Thus the diffusion component (and therefore the net inlet transport) is not
specified a priori.
In some cases, you may wish to specify the net inlet transport of energy rather than the
inlet temperature. If you are using the pressure-based solver, you can do this by disabling
inlet energy diffusion. By default, ANSYS FLUENT includes the diffusion flux of energy
at inlets. To turn off inlet diffusion, use the define/models/energy? text command
and respond no when asked to Include diffusion at inlets?
Inlet diffusion cannot be turned off if you are using the density-based solver.
5.2.2
Natural Convection and Buoyancy-Driven Flows Theory
When heat is added to a fluid and the fluid density varies with temperature, a flow can be
induced due to the force of gravity acting on the density variations. Such buoyancy-driven
flows are termed natural-convection (or mixed-convection) flows and can be modeled by
ANSYS FLUENT.
The importance of buoyancy forces in a mixed convection flow can be measured by the
ratio of the Grashof and Reynolds numbers:
gβ∆T L
Gr
2 =
v2
Re
5-6
(5.2-13)
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
When this number approaches or exceeds unity, you should expect strong buoyancy
contributions to the flow. Conversely, if it is very small, buoyancy forces may be ignored
in your simulation. In pure natural convection, the strength of the buoyancy-induced
flow is measured by the Rayleigh number:
Ra =
gβ∆T L3 ρ
µα
(5.2-14)
where β is the thermal expansion coefficient:
1
β=−
ρ
∂ρ
∂T
!
(5.2-15)
p
and α is the thermal diffusivity:
α=
k
ρcp
(5.2-16)
Rayleigh numbers less than 108 indicate a buoyancy-induced laminar flow, with transition
to turbulence occurring over the range of 108 < Ra < 1010 .
5.3
Modeling Radiation
Information about radiation modeling theory is presented in the following sections:
• Section 5.3.1: Overview and Limitations
• Section 5.3.2: Radiative Transfer Equation
• Section 5.3.3: P-1 Radiation Model Theory
• Section 5.3.4: Rosseland Radiation Model Theory
• Section 5.3.5: Discrete Transfer Radiation Model (DTRM) Theory
• Section 5.3.6: Discrete Ordinates (DO) Radiation Model Theory
• Section 5.3.7: Surface-to-Surface (S2S) Radiation Model Theory
• Section 5.3.8: Radiation in Combusting Flows
• Section 5.3.9: Choosing a Radiation Model
For information about setting up and using radiation models in ANSYS FLUENT, see
Section 13.3: Modeling Radiation in the separate User’s Guide.
Release 12.0 c ANSYS, Inc. January 29, 2009
5-7
Heat Transfer
5.3.1
Overview and Limitations
ANSYS FLUENT provides five radiation models which allow you to include radiation,
with or without a participating medium, in your heat transfer simulations.
Heating or cooling of surfaces due to radiation and/or heat sources or sinks due to
radiation within the fluid phase can be included in your model using one of the following
radiation models.
• Discrete Transfer Radiation Model (DTRM) [47, 312]
• P-1 Radiation Model [52, 315]
• Rosseland Radiation Model [315]
• Surface-to-Surface (S2S) Radiation Model [315]
• Discrete Ordinates (DO) Radiation Model [56, 282]
In addition to these radiation models, ANSYS FLUENT also provides a solar load model
that allows you to include the effects of solar radiation in your simulation.
Typical applications well suited for simulation using radiative heat transfer include the
following:
• radiative heat transfer from flames
• surface-to-surface radiant heating or cooling
• coupled radiation, convection, and/or conduction heat transfer
• radiation through windows in HVAC applications, and cabin heat transfer analysis
in automotive applications
• radiation in glass processing, glass fiber drawing, and ceramic processing
You should include radiative heat transfer in your simulation when the radiant heat flux,
4
4
Qrad = σ(Tmax
− Tmin
), is large compared to the heat transfer rate due to convection
or conduction. Typically this will occur at high temperatures where the fourth-order
dependence of the radiative heat flux on temperature implies that radiation will dominate.
5-8
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
Advantages and Limitations of the DTRM
The primary advantages of the DTRM are threefold: it is a relatively simple model, you
can increase the accuracy by increasing the number of rays, and it applies to a wide range
of optical thicknesses.
You should be aware of the following limitations when using the DTRM in ANSYS FLUENT:
• DTRM assumes that all surfaces are diffuse. This means that the reflection of
incident radiation at the surface is isotropic with respect to the solid angle.
• The effect of scattering is not included.
• The implementation assumes gray radiation.
• Solving a problem with a large number of rays is CPU-intensive.
• DTRM is not compatible with non-conformal interface or sliding meshes.
• DTRM is not compatible with parallel processing.
Advantages and Limitations of the P-1 Model
The P-1 model has several advantages over the DTRM. For the P-1 model, the RTE
(Equation 5.3-1) is a diffusion equation, which is easy to solve with little CPU demand.
The model includes the effect of scattering. For combustion applications where the optical
thickness is large, the P-1 model works reasonably well. In addition, the P-1 model can
easily be applied to complicated geometries with curvilinear coordinates.
You should be aware of the following limitations when using the P-1 radiation model:
• P-1 model assumes that all surfaces are diffuse. This means that the reflection of
incident radiation at the surface is isotropic with respect to the solid angle.
• The implementation assumes gray radiation.
• There may be a loss of accuracy, depending on the complexity of the geometry, if
the optical thickness is small.
• P-1 model tends to over-predict radiative fluxes from localized heat sources or sinks.
Release 12.0 c ANSYS, Inc. January 29, 2009
5-9
Heat Transfer
Advantages and Limitations of the Rosseland Model
The Rosseland model has two advantages over the P-1 model. Since it does not solve an
extra transport equation for the incident radiation (as the P-1 model does), the Rosseland
model is faster than the P-1 model and requires less memory.
The Rosseland model can be used only for optically thick media. It is recommended for
use when the optical thickness exceeds 3. Note also that the Rosseland model is not
available when the density-based solver is being used; it is available with the pressurebased solver, only.
Advantages and Limitations of the DO Model
The DO model spans the entire range of optical thicknesses, and allows you to solve problems ranging from surface-to-surface radiation to participating radiation in combustion
problems. It also allows the solution of radiation at semi-transparent walls. Computational cost is moderate for typical angular discretizations, and memory requirements are
modest.
The current implementation is restricted to either gray radiation or non-gray radiation
using a gray-band model. Solving a problem with a fine angular discretization may be
CPU-intensive.
The non-gray implementation in ANSYS FLUENT is intended for use with participating
media with a spectral absorption coefficient aλ that varies in a stepwise fashion across
spectral bands, but varies smoothly within the band. Glass, for example, displays banded
behavior of this type. The current implementation does not model the behavior of gases
such as carbon dioxide or water vapor, which absorb and emit energy at distinct wave
numbers [234]. The modeling of non-gray gas radiation is still an evolving field. However,
some researchers [98] have used gray-band models to model gas behavior by approximating the absorption coefficients within each band as a constant. The implementation in
ANSYS FLUENT can be used in this fashion if desired.
The non-gray implementation in ANSYS FLUENT is compatible with all the models with
which the gray implementation of the DO model can be used. Thus, it is possible to
include scattering, anisotropy, semi-transparent media, and particulate effects. However, the non-gray implementation assumes a constant absorption coefficient within each
wavelength band. The weighted-sum-of-gray-gases model (WSGGM) cannot be used to
specify the absorption coefficient in each band. The implementation allows the specification of spectral emissivity at walls. The emissivity is assumed to be constant within
each band.
5-10
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
Advantages and Limitations of the S2S Model
The surface-to-surface (S2S) radiation model is good for modeling the enclosure radiative transfer without participating media (e.g., spacecraft heat rejection systems, solar
collector systems, radiative space heaters, and automotive underhood cooling systems).
In such cases, the methods for participating radiation may not always be efficient. As
compared to the DTRM and the DO radiation models, the S2S model has a much faster
time per iteration, although the view factor calculation itself is CPU-intensive. This
increased time for view factor calculation will be especially pronounced when the emitting/absorbing surfaces are the polygonal faces of polyhedral cells.
You should be aware of the following limitations when using the S2S radiation model:
• S2S model assumes that all surfaces are diffuse.
• The implementation assumes gray radiation.
• The storage and memory requirements increase very rapidly as the number of surface faces increases. This can be minimized by using a cluster of surface faces,
although the CPU time is independent of the number of clusters that are used.
• S2S model cannot be used to model participating radiation problems.
• S2S model cannot be used if your model contains periodic boundary conditions.
• S2S model with hemicube/adaptive view factor methods cannot be used if your
model contains symmetry boundary conditions.
• S2S model does not support non-conformal interfaces, hanging nodes, or mesh
adaption.
Release 12.0 c ANSYS, Inc. January 29, 2009
5-11
Heat Transfer
5.3.2
Radiative Transfer Equation
The radiative transfer equation (RTE) for an absorbing, emitting, and scattering medium
at position ~r in the direction ~s is
dI(~r, ~s)
σT 4
σs Z 4π
+ (a + σs )I(~r, ~s) = an2
+
I(~r, ~s 0 ) Φ(~s · ~s 0 ) dΩ0
ds
π
4π 0
where ~r
~s
~s 0
s
a
n
σs
σ
I
T
Φ
Ω0
=
=
=
=
=
=
=
=
=
=
=
=
(5.3-1)
position vector
direction vector
scattering direction vector
path length
absorption coefficient
refractive index
scattering coefficient
Stefan-Boltzmann constant (5.669 × 10−8 W/m2 -K4 )
radiation intensity, which depends on position (~r) and direction (~s)
local temperature
phase function
solid angle
(a + σs )s is the optical thickness or opacity of the medium. The refractive index n is
important when considering radiation in semi-transparent media. Figure 5.3.1 illustrates
the process of radiative heat transfer.
Absorption and
scattering loss:
I (a+ σs) ds
Outgoing radiation
I + (dI/ds)ds
Incoming
radiation (I)
Gas emission:
(aσT 4/ π) ds
Scattering
addition
ds
Figure 5.3.1: Radiative Heat Transfer
5-12
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
The DTRM and the P-1, Rosseland, and DO radiation models require the absorption
coefficient a as input. a and the scattering coefficient σs can be constants, and a can also
be a function of local concentrations of H2 O and CO2 , path length, and total pressure.
ANSYS FLUENT provides the weighted-sum-of-gray-gases model (WSGGM) for computation of a variable absorption coefficient. See Section 5.3.8: Radiation in Combusting
Flows for details. The discrete ordinates implementation can model radiation in semitransparent media. The refractive index n of the medium must be provided as a part of
the calculation for this type of problem. The Rosseland model also requires you to enter
a refractive index, or use the default value of 1.
5.3.3
P-1 Radiation Model Theory
The P-1 radiation model is the simplest case of the more general P-N model, which is
based on the expansion of the radiation intensity I into an orthogonal series of spherical
harmonics [52, 315]. This section provides details about the equations used in the P-1
model. For information about setting up the model, see Section 13.3.1: Steps in Using
the Radiation Models in the separate User’s Guide.
The P-1 Model Equations
As mentioned above, the P-1 radiation model is the simplest case of the P-N model. If
only four terms in the series are used, the following equation is obtained for the radiation
flux qr :
qr = −
1
∇G
3(a + σs ) − Cσs
(5.3-2)
where a is the absorption coefficient, σs is the scattering coefficient, G is the incident
radiation, and C is the linear-anisotropic phase function coefficient, described below.
After introducing the parameter
1
(3(a + σs ) − Cσs )
(5.3-3)
qr = −Γ∇G
(5.3-4)
∇ · (Γ∇G) − aG + 4an2 σT 4 = SG
(5.3-5)
Γ=
Equation 5.3-2 simplifies to
The transport equation for G is
Release 12.0 c ANSYS, Inc. January 29, 2009
5-13
Heat Transfer
where n is the refractive index of the medium, σ is the Stefan-Boltzmann constant and
SG is a user-defined radiation source. ANSYS FLUENT solves this equation to determine
the local radiation intensity when the P-1 model is active.
Combining Equations 5.3-4 and 5.3-5 yields the following equation:
− ∇ · qr = aG − 4an2 σT 4
(5.3-6)
The expression for −∇·qr can be directly substituted into the energy equation to account
for heat sources (or sinks) due to radiation.
Anisotropic Scattering
Included in the P-1 radiation model is the capability for modeling anisotropic scattering.
ANSYS FLUENT models anisotropic scattering by means of a linear-anisotropic scattering
phase function:
Φ(~s 0 · ~s) = 1 + C~s 0 · ~s
(5.3-7)
Here, ~s is the unit vector in the direction of scattering, and ~s 0 is the unit vector in the
direction of the incident radiation. C is the linear-anisotropic phase function coefficient,
which is a property of the fluid. C ranges from −1 to 1. A positive value indicates that
more radiant energy is scattered forward than backward, and a negative value means that
more radiant energy is scattered backward than forward. A zero value defines isotropic
scattering (i.e., scattering that is equally likely in all directions), which is the default
in ANSYS FLUENT. You should modify the default value only if you are certain of the
anisotropic scattering behavior of the material in your problem.
Particulate Effects in the P-1 Model
When your ANSYS FLUENT model includes a dispersed second phase of particles, you
can include the effect of particles in the P-1 radiation model. Note that when particles
are present, ANSYS FLUENT ignores scattering in the gas phase. (That is, Equation 5.3-8
assumes that all scattering is due to particles.)
For a gray, absorbing, emitting, and scattering medium containing absorbing, emitting,
and scattering particles, the transport equation for the incident radiation can be written
as
∇ · (Γ∇G) + 4π an
2 σT
π
4
!
+ Ep − (a + ap )G = 0
(5.3-8)
where Ep is the equivalent emission of the particles, ap is the equivalent absorption
coefficient, and n is the refractive index of the medium. These are defined as follows:
5-14
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
4
σTpn
Ep = lim
pn Apn
V →0
πV
n=1
N
X
(5.3-9)
and
ap = lim
V →0
N
X
pn
n=1
Apn
V
(5.3-10)
In Equations 5.3-9 and 5.3-10, pn , Apn , and Tpn are the emissivity, projected area, and
temperature of particle n. The summation is over N particles in volume V . These
quantities are computed during particle tracking in ANSYS FLUENT.
The projected area Apn of particle n is defined as
Apn =
πd2pn
4
(5.3-11)
where dpn is the diameter of the nth particle.
The quantity Γ in Equation 5.3-8 is defined as
Γ=
1
3(a + ap + σp )
(5.3-12)
where the equivalent particle scattering factor is defined as
σp = lim
V →0
N
X
(1 − fpn )(1 − pn )
n=1
Apn
V
(5.3-13)
and is computed during particle tracking. In Equation 5.3-13, fpn is the scattering factor
associated with the nth particle.
Heat sources (sinks) due to particle radiation are included in the energy equation as
follows:
− ∇ · qr = −4π an
Release 12.0 c ANSYS, Inc. January 29, 2009
2 σT
π
4
!
+ Ep + (a + ap )G
(5.3-14)
5-15
Heat Transfer
Boundary Condition Treatment for the P-1 Model at Walls
To get the boundary condition for the incident radiation equation, the dot product of
the outward normal vector ~n and Equation 5.3-4 is computed:
qr · ~n = −Γ∇G · ~n
∂G
qr,w = −Γ
∂n
(5.3-15)
(5.3-16)
Thus the flux of the incident radiation, G, at a wall is −qr,w . The wall radiative heat
flux is computed using the following boundary condition:
Iw (~r, ~s) = fw (~r, ~s)
n2 σTw4
+ ρw I(~r, −~s)
fw (~r, ~s) = w
π
(5.3-17)
(5.3-18)
where ρw is the wall reflectivity. The Marshak boundary condition is then used to eliminate the angular dependence [262]:
Z
0
2π
Iw (~r, ~s) ~n · ~s dΩ =
Z
0
2π
fw (~r, ~s) ~n · ~s dΩ
(5.3-19)
Substituting Equations 5.3-17 and 5.3-18 into Equation 5.3-19 and performing the integrations yields
2 σT 4
w
qr,w = −
4πw n
− (1 − ρw )Gw
2(1 + ρw )
π
(5.3-20)
If it is assumed that the walls are diffuse gray surfaces, then ρw = 1 − w , and Equation 5.3-20 becomes
qr,w = −
w
4n2 σTw4 − Gw
2 (2 − w )
(5.3-21)
Equation 5.3-21 is used to compute qr,w for the energy equation and for the incident
radiation equation boundary conditions.
5-16
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
Boundary Condition Treatment for the P-1 Model at Flow Inlets and Exits
The net radiative heat flux at flow inlets and outlets is computed in the same manner as at
walls, as described above. ANSYS FLUENT assumes that the emissivity of all flow inlets
and outlets is 1.0 (black body absorption) unless you choose to redefine this boundary
treatment.
ANSYS FLUENT includes an option that allows you to use different temperatures for
radiation and convection at inlets and outlets. This can be useful when the temperature
outside the inlet or outlet differs considerably from the temperature in the enclosure. See
Section 13.3.6: Defining Boundary Conditions for Radiation in the separate User’s Guide
for details.
5.3.4
Rosseland Radiation Model Theory
The Rosseland or diffusion approximation for radiation is valid when the medium is
optically thick ((a + σs )L 1), and is recommended for use in problems where the
optical thickness is greater than 3. It can be derived from the P-1 model equations,
with some approximations. This section provides details about the equations used in the
Rosseland model. For information about setting up the model, see Section 13.3.1: Steps
in Using the Radiation Models in the separate User’s Guide.
The Rosseland Model Equations
As with the P-1 model, the radiative heat flux vector in a gray medium can be approximated by Equation 5.3-4:
qr = −Γ∇G
(5.3-22)
where Γ is given by Equation 5.3-3.
The Rosseland radiation model differs from the P-1 model in that the Rosseland model
assumes that the intensity is the black-body intensity at the gas temperature. (The P-1
model actually calculates a transport equation for G.) Thus G = 4σn2 T 4 , where n is the
refractive index. Substituting this value for G into Equation 5.3-22 yields
qr = −16σΓn2 T 3 ∇T
Release 12.0 c ANSYS, Inc. January 29, 2009
(5.3-23)
5-17
Heat Transfer
Since the radiative heat flux has the same form as the Fourier conduction law, it is
possible to write
q = qc + qr
= −(k + kr )∇T
kr = 16σΓn2 T 3
(5.3-24)
(5.3-25)
(5.3-26)
where k is the thermal conductivity and kr is the radiative conductivity. Equation 5.3-24
is used in the energy equation to compute the temperature field.
Anisotropic Scattering
The Rosseland model allows for anisotropic scattering, using the same phase function
(Equation 5.3-7) described for the P-1 model in Section 5.3.3: Anisotropic Scattering.
Boundary Condition Treatment for the Rosseland Model at Walls
Since the diffusion approximation is not valid near walls, it is necessary to use a temperature slip boundary condition. The radiative heat flux at the wall boundary, qr,w , is
defined using the slip coefficient ψ:
qr,w = −
σ Tw4 − Tg4
(5.3-27)
ψ
where Tw is the wall temperature, Tg is the temperature of the gas at the wall, and the
slip coefficient ψ is approximated by a curve fit to the plot given in [315]:
ψ=
1/2
3
2x +3x2 −12x+7
54
0
Nw < 0.01
0.01 ≤ Nw ≤ 10
Nw > 10
(5.3-28)
where Nw is the conduction to radiation parameter at the wall:
Nw =
k(a + σs )
4σTw3
(5.3-29)
and x = log10 Nw .
5-18
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
Boundary Condition Treatment for the Rosseland Model at Flow Inlets and
Exits
No special treatment is required at flow inlets and outlets for the Rosseland model. The
radiative heat flux at these boundaries can be determined using Equation 5.3-24.
5.3.5
Discrete Transfer Radiation Model (DTRM) Theory
The main assumption of the DTRM is that the radiation leaving the surface element in a
certain range of solid angles can be approximated by a single ray. This section provides
details about the equations used in the DTRM. For information about setting up the
model, see Section 13.3.2: Setting Up the DTRM in the separate User’s Guide.
The DTRM Equations
The equation for the change of radiant intensity, dI, along a path, ds, can be written as
dI
aσT 4
+ aI =
ds
π
where
a
I
T
σ
=
=
=
=
(5.3-30)
gas absorption coefficient
intensity
gas local temperature
Stefan-Boltzmann constant (5.669 × 10−8 W/m2 -K4 )
Here, the refractive index is assumed to be unity. The DTRM integrates Equation 5.3-30
along a series of rays emanating from boundary faces. If a is constant along the ray, then
I(s) can be estimated as
I(s) =
σT 4
(1 − e−as ) + I0 e−as
π
(5.3-31)
where I0 is the radiant intensity at the start of the incremental path, which is determined
by the appropriate boundary condition (see the description of boundary conditions, below). The energy source in the fluid due to radiation is then computed by summing the
change in intensity along the path of each ray that is traced through the fluid control
volume.
The “ray tracing” technique used in the DTRM can provide a prediction of radiative
heat transfer between surfaces without explicit view factor calculations. The accuracy of
the model is limited mainly by the number of rays traced and the computational mesh.
Release 12.0 c ANSYS, Inc. January 29, 2009
5-19
Heat Transfer
Ray Tracing
The ray paths are calculated and stored prior to the fluid flow calculation. At each
radiating face, rays are fired at discrete values of the polar and azimuthal angles (see
Figure 5.3.2). To cover the radiating hemisphere, θ is varied from 0 to π2 and φ from 0
to 2π. Each ray is then traced to determine the control volumes it intercepts as well as
its length within each control volume. This information is then stored in the radiation
file, which must be read in before the fluid flow calculations begin.
n
θ
φ
P
t
Figure 5.3.2: Angles θ and φ Defining the Hemispherical Solid Angle About
a Point P
Clustering
DTRM is computationally very expensive when there are too many surfaces to trace rays
from and too many volumes crossed by the rays. To reduce the computational time, the
number of radiating surfaces and absorbing cells is reduced by clustering surfaces and
cells into surface and volume “clusters”. The volume clusters are formed by starting from
a cell and simply adding its neighbors and their neighbors until a specified number of
cells per volume cluster is collected. Similarly, surface clusters are made by starting from
a face and adding its neighbors and their neighbors until a specified number of faces per
surface cluster is collected.
The incident radiation flux, qin , and the volume sources are calculated for the surface and
volume clusters respectively. These values are then distributed to the faces and cells in
the clusters to calculate the wall and cell temperatures. Since the radiation source terms
are highly non-linear (proportional to the fourth power of temperature), care must be
taken to calculate the average temperatures of surface and volume clusters and distribute
the flux and source terms appropriately among the faces and cells forming the clusters.
5-20
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
The surface and volume cluster temperatures are obtained by area and volume averaging
as shown in the following equations:
Af Tf4
P
Af
P
f
Tsc =
Vc Tc4
P
Vc
P
!1/4
!1/4
c
Tvc =
(5.3-32)
(5.3-33)
where Tsc and Tvc are the temperatures of the surface and volume clusters respectively,
Af and Tf are the area and temperature of face f , and Vc and Tc are the volume and
temperature of cell c. The summations are carried over all faces of a surface cluster and
all cells of a volume cluster.
Boundary Condition Treatment for the DTRM at Walls
The radiation intensity approaching a point on a wall surface is integrated to yield the
incident radiative heat flux, qin , as
qin =
Z
~s·~
n>0
Iin~s · ~ndΩ
(5.3-34)
where Ω is the hemispherical solid angle, Iin is the intensity of the incoming ray, ~s is the
ray direction vector, and ~n is the normal pointing out of the domain. The net radiative
heat flux from the surface, qout , is then computed as a sum of the reflected portion of qin
and the emissive power of the surface:
qout = (1 − w )qin + w σTw4
(5.3-35)
where Tw is the surface temperature of the point P on the surface and w is the wall
emissivity which you input as a boundary condition. ANSYS FLUENT incorporates the
radiative heat flux (Equation 5.3-35) in the prediction of the wall surface temperature.
Equation 5.3-35 also provides the surface boundary condition for the radiation intensity
I0 of a ray emanating from the point P , as
I0 =
Release 12.0 c ANSYS, Inc. January 29, 2009
qout
π
(5.3-36)
5-21
Heat Transfer
Boundary Condition Treatment for the DTRM at Flow Inlets and Exits
The net radiative heat flux at flow inlets and outlets is computed in the same manner as at
walls, as described above. ANSYS FLUENT assumes that the emissivity of all flow inlets
and outlets is 1.0 (black body absorption) unless you choose to redefine this boundary
treatment.
ANSYS FLUENT includes an option that allows you to use different temperatures for
radiation and convection at inlets and outlets. This can be useful when the temperature
outside the inlet or outlet differs considerably from the temperature in the enclosure. See
Section 13.3.6: Defining Boundary Conditions for Radiation in the separate User’s Guide
for details.
5.3.6
Discrete Ordinates (DO) Radiation Model Theory
The discrete ordinates (DO) radiation model solves the radiative transfer equation (RTE)
for a finite number of discrete solid angles, each associated with a vector direction ~s fixed
in the global Cartesian system (x, y, z). The fineness of the angular discretization is
controlled by you, analogous to choosing the number of rays for the DTRM. Unlike the
DTRM, however, the DO model does not perform ray tracing. Instead, the DO model
transforms Equation 5.3-1 into a transport equation for radiation intensity in the spatial
coordinates (x, y, z). The DO model solves for as many transport equations as there are
directions ~s. The solution method is identical to that used for the fluid flow and energy
equations.
Two implementations of the DO model are available in ANSYS FLUENT: uncoupled and
(energy) coupled. The uncoupled implementation is sequential in nature and uses a
conservative variant of the DO model called the finite-volume scheme [56, 282], and its
extension to unstructured meshes [242]. In the uncoupled case, the equations for the
energy and radiation intensities are solved one by one, assuming prevailing values for
other variables.
Alternatively, in the coupled ordinates method (or COMET) [220], the discrete energy
and intensity equations at each cell are solved simultaneously, assuming that spatial
neighbors are known. The advantages of using the coupled approach is that it speeds up
applications involving high optical thicknesses and/or high scattering coefficients. Such
applications slow down convergence drastically when the sequential approach is used. For
information about setting up the model, see Section 13.3.4: Setting Up the DO Model in
the separate User’s Guide.
5-22
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
The DO Model Equations
The DO model considers the radiative transfer equation (RTE) in the direction ~s as a
field equation. Thus, Equation 5.3-1 is written as
∇ · (I(~r, ~s)~s) + (a + σs )I(~r, ~s) = an2
σT 4
σs Z 4π
+
I(~r, ~s 0 ) Φ(~s · ~s 0 ) dΩ0
π
4π 0
(5.3-37)
ANSYS FLUENT also allows the modeling of non-gray radiation using a gray-band model.
The RTE for the spectral intensity Iλ (~r, ~s) can be written as
σs Z 4π
Iλ (~r, ~s 0 ) Φ(~s · ~s 0 ) dΩ0
∇ · (Iλ (~r, ~s)~s) + (aλ + σs )Iλ (~r, ~s) = aλ n Ibλ +
4π 0
2
(5.3-38)
Here λ is the wavelength, aλ is the spectral absorption coefficient, and Ibλ is the black
body intensity given by the Planck function. The scattering coefficient, the scattering
phase function, and the refractive index n are assumed independent of wavelength.
The non-gray DO implementation divides the radiation spectrum into N wavelength
bands, which need not be contiguous or equal in extent. The wavelength intervals are
supplied by you, and correspond to values in vacuum (n = 1). The RTE is integrated
over each wavelength interval, resulting in transport equations for the quantity Iλ ∆λ,
the radiant energy contained in the wavelength band ∆λ. The behavior in each band is
assumed gray. The black body emission in the wavelength band per unit solid angle is
written as
[F (0 → nλ2 T ) − F (0 → nλ1 T )]n2
σT 4
π
(5.3-39)
where F (0 → nλT ) is the fraction of radiant energy emitted by a black body [234] in the
wavelength interval from 0 to λ at temperature T in a medium of refractive index n. λ2
and λ1 are the wavelength boundaries of the band.
The total intensity I(~r, ~s) in each direction ~s at position ~r is computed using
I(~r, ~s) =
X
Iλk (~r, ~s)∆λk
(5.3-40)
k
where the summation is over the wavelength bands.
Boundary conditions for the non-gray DO model are applied on a band basis. The
treatment within a band is the same as that for the gray DO model.
Release 12.0 c ANSYS, Inc. January 29, 2009
5-23
Heat Transfer
Energy Coupling and the DO Model
The coupling between energy and radiation intensities at a cell (which is also known
as COMET) [220] accelerates the convergence of the finite volume scheme for radiative
heat transfer. This method results in significant improvement in the convergence for
applications involving optical thicknesses greater than 10. This is typically encountered
in glass-melting applications. This feature is advantageous when scattering is significant,
resulting in strong coupling between directional radiation intensities. This DO model
implementation is utilized in ANSYS FLUENT by enabling the DO/Energy Coupling option
for the DO model in the Radiation Model dialog box. The discrete energy equations for
the coupled method are presented below.
The energy equation when integrated over a control volume i, yields the discrete energy
equation:
N
X
µTij Tj − βiT Ti − αiT
j=1
where
αiT
βiT
SiT
κ
∆V
L
X
Iik ωk − SiT Sih
(5.3-41)
k=1
= κ∆Vi
= 16κσTi∗3 ∆Vi
= 12κσTi∗4 ∆Vi
= absorption coefficient
= control volume
The coefficient µTij and the source term Sih are due to the discretization of the convection
and diffusion terms as well as the non-radiative source terms.
Combining the discretized form of Equation 5.3-37 and the discretized energy equation,
Equation 5.3-41, yields [220]:
P~i ~qi + ~ri = 0
5-24
(5.3-42)
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
where
~qi =
~
Pi =
Ii1
Ii2
:
:
IiL
Ti
(5.3-43)
Mii1 + ηi11 + γi1 ω1
ηi12 + γi1 ω2
...βi1
ηi21 + γi2 ω1
Mii2 + ηi22 + γi2 ω2 ...βi2
:
:
−αiT ω1
−αiT ω2
...MiiT
PN
µlij Ijl − Si1 − SiB
:
:
PN
T
T
h
µ
T
j=1,i6=j ij j + Si + Si
j=1,i6=j
~ri =
(5.3-44)
(5.3-45)
Limitations of DO/Energy Coupling
There are some instances when using DO/Energy coupling is not recommended or is
incompatible with certain models:
• DO/Energy coupling is not recommended for cases with weak coupling between
energy and directional radiation intensities. This may result in slower convergence
of the coupled approach compared to the sequential approach.
• DO/Energy coupling is not compatible with the shell conduction model.
• DO/Energy coupling is not available when solving enthalpy equations instead of
temperature equations. Typical cases would involve combustion modeling.
To find out how to apply DO/Energy coupling, refer to Section 13.3.4: Setting Up the
DO Model in the separate User’s Guide.
Release 12.0 c ANSYS, Inc. January 29, 2009
5-25
Heat Transfer
Angular Discretization and Pixelation
Each octant of the angular space 4π at any spatial location is discretized into Nθ × Nφ
solid angles of extent ωi , called control angles. The angles θ and φ are the polar and
azimuthal angles respectively, and are measured with respect to the global Cartesian
system (x, y, z) as shown in Figure 5.3.3. The θ and φ extents of the control angle, ∆θ
and ∆φ, are constant. In two-dimensional calculations, only four octants are solved due to
symmetry, making a total of 4Nθ Nφ directions in all. In three-dimensional calculations,
a total of 8Nθ Nφ directions are solved. In the case of the non-gray model, 4Nθ Nφ or
8Nθ Nφ equations are solved for each band.
z
s
θ
φ
y
x
Figure 5.3.3: Angular Coordinate System
When Cartesian meshes are used, it is possible to align the global angular discretization
with the control volume face, as shown in Figure 5.3.4. For generalized unstructured
meshes, however, control volume faces do not in general align with the global angular
discretization, as shown in Figure 5.3.5, leading to the problem of control angle overhang [242].
Essentially, control angles can straddle the control volume faces, so that they are partially
incoming and partially outgoing to the face. Figure 5.3.6 shows a 3D example of a face
with control angle overhang.
The control volume face cuts the sphere representing the angular space at an arbitrary
angle. The line of intersection is a great circle. Control angle overhang may also occur
as a result of reflection and refraction. It is important in these cases to correctly account
for the overhanging fraction. This is done through the use of pixelation [242].
Each overhanging control angle is divided into Nθp × Nφp pixels, as shown in Figure 5.3.7.
5-26
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
incoming
directions
●
C0
n
●
C1
outgoing
directions
face f
Figure 5.3.4: Face with No Control Angle Overhang
overhanging
control angle
incoming
directions
C0
n
●
● C1
outgoing
directions
face f
Figure 5.3.5: Face with Control Angle Overhang
Release 12.0 c ANSYS, Inc. January 29, 2009
5-27
Heat Transfer
outgoing
directions
z
overhanging
control
angle
y
x
control
volume
face
incoming
directions
Figure 5.3.6: Face with Control Angle Overhang (3D)
control angle ω i
si
control
volume
face
pixel
Figure 5.3.7: Pixelation of Control Angle
5-28
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
The energy contained in each pixel is then treated as incoming or outgoing to the face.
The influence of overhang can thus be accounted for within the pixel resolution. ANSYS
FLUENT allows you to choose the pixel resolution. For problems involving gray-diffuse
radiation, the default pixelation of 1 × 1 is usually sufficient. For problems involving
symmetry, periodic, specular, or semi-transparent boundaries, a pixelation of 3 × 3 is
recommended. You should be aware, however, that increasing the pixelation adds to the
cost of computation.
Anisotropic Scattering
The DO implementation in ANSYS FLUENT admits a variety of scattering phase functions. You can choose an isotropic phase function, a linear anisotropic phase function, a
Delta-Eddington phase function, or a user-defined phase function. The linear anisotropic
phase function is described in Equation 5.3-7. The Delta-Eddington function takes the
following form:
Φ(~s · ~s 0 ) = 2f δ(~s · ~s 0 ) + (1 − f )(1 + C~s · ~s 0 )
(5.3-46)
Here, f is the forward-scattering factor and δ(~s · ~s 0 ) is the Dirac delta function. The
f term essentially cancels a fraction f of the out-scattering; thus, for f = 1, the DeltaEddington phase function will cause the intensity to behave as if there is no scattering
at all. C is the asymmetry factor. When the Delta-Eddington phase function is used,
you will specify values for f and C.
When a user-defined function is used to specify the scattering phase function, ANSYS
FLUENT assumes the phase function to be of the form
Φ(~s · ~s 0 ) = 2f δ(~s · ~s 0 ) + (1 − f )Φ∗ (~s · ~s 0 )
(5.3-47)
The user-defined function will specify Φ∗ and the forward-scattering factor f .
The scattering phase functions available for gray radiation can also be used for non-gray
radiation. However, the scattered energy is restricted to stay within the band.
Particulate Effects in the DO Model
The DO model allows you to include the effect of a discrete second phase of particulates
on radiation. In this case, ANSYS FLUENT will neglect all other sources of scattering in
the gas phase.
The contribution of the particulate phase appears in the RTE as:
∇ · (I~s) + (a + ap + σp )I(~r, ~s) = an2
Release 12.0 c ANSYS, Inc. January 29, 2009
σT 4
σp Z 4π
+ Ep +
I(~r, ~s 0 ) Φ(~s · ~s 0 ) dΩ0 (5.3-48)
π
4π 0
5-29
Heat Transfer
where ap is the equivalent absorption coefficient due to the presence of particulates, and
is given by Equation 5.3-10. The equivalent emission Ep is given by Equation 5.3-9.
The equivalent particle scattering factor σp , defined in Equation 5.3-13, is used in the
scattering terms.
For non-gray radiation, absorption, emission, and scattering due to the particulate phase
are included in each wavelength band for the radiation calculation. Particulate emission
and absorption terms are also included in the energy equation.
Boundary and Cell Zone Condition Treatment at Opaque Walls
The discrete ordinates radiation model allows the specification of opaque walls that are
interior to a domain (with adjacent fluid or solid zones on both sides of the wall), or
external to the domain (with an adjacent fluid or solid zone on one side, only). Opaque
walls are treated as gray if gray radiation is being computed, or non-gray if the non-gray
DO model is being used.
Figure 5.3.8 shows a schematic of radiation on an opaque wall in ANSYS FLUENT.
Medium a
Adjacent Fluid or Solid
q
emission
q in, a reflected, specular
q
absorbed
n
q in, a reflected, diffuse
q in, a
Figure 5.3.8: DO Radiation on Opaque Wall
The diagram in Figure 5.3.8 shows incident radiation qin,a on side a of an opaque wall.
Some of the radiant energy is reflected diffusely and specularly, depending on the diffuse
fraction fd for side a of the wall that you specify as a boundary condition.
5-30
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
Some of the incident radiation is absorbed at the surface of the wall and some radiation is
emitted from the wall surface as shown in Figure 5.3.8. The amount of incident radiation
absorbed at the wall surface and the amount emitted back depends on the emissivity of
that surface and the diffuse fraction. For non-gray DO models, you must specify internal
emissivity for each wavelength band. Radiation is not transmitted through an opaque
wall.
Radiant incident energy that impacts an opaque wall can be reflected back to the surrounding medium and absorbed by the wall. The radiation that is reflected can be
diffusely reflected and/or specularly reflected, depending on the diffuse fraction fd . If qin
is the amount of radiative energy incident on the opaque wall, then the following general
quantities are computed by ANSYS FLUENT for opaque walls:
• emission from the wall surface = n2 w σTw4
• diffusely reflected energy = fd (1 − w )qin
• specularly reflected energy = (1 − fd )(1 − w )qin
• absorption at the wall surface = w qin
where fd is the diffuse fraction, n is the refractive index of the adjacent medium, w is
the wall emissivity, σ is Boltzmann’s Constant, and Tw is the wall temperature.
Note that although ANSYS FLUENT uses emissivity in its computation of radiation quantities, it is not available for postprocessing. Absorption at the wall surface assumes that
the absorptivity is equal to the emissivity. For a purely diffused wall, fd is equal to 1 and
there is no specularly reflected energy. Similarly, for a purely specular wall, fd is equal
to 0 and there is no diffusely reflected energy. A diffuse fraction between 0 and 1 will
result in partially diffuse and partially reflected energy.
Gray Diffuse Walls
For gray diffuse radiation, the incident radiative heat flux, qin , at the wall is
qin =
Z
~s·~
n>0
Iin~s · ~ndΩ
(5.3-49)
The net radiative flux leaving the surface is given by
qout = (1 − w )qin + n2 w σTw4
(5.3-50)
where n is the refractive index of the medium next to the wall, w is the wall emissivity,
σ is Boltzmann’s Constant, and Tw is the wall temperature. This equation is also valid
for specular radiation with emissivity = 0.
Release 12.0 c ANSYS, Inc. January 29, 2009
5-31
Heat Transfer
The boundary intensity for all outgoing directions ~s at the wall is given by
I0 =
qout
π
(5.3-51)
Non-Gray Diffuse Walls
There is a special set of equations that apply uniquely to non-gray diffuse opaque walls.
These equations assume that the absorptivity is equal to the emissivity for the wall
surface. For non-gray diffuse radiation, the incident radiative heat flux qin,λ in the band
∆λ at the wall is
qin,λ = ∆λ
Z
~s·~
n>0
Iin,λ~s · ~ndΩ
(5.3-52)
The net radiative flux leaving the surface in the band ∆λ is given by
qout,λ = (1 − wλ )qin,λ + wλ [F (0 → nλ2 Tw ) − F (0 → nλ1 Tw )]n2 σTw4
(5.3-53)
where wλ is the wall emissivity in the band. F (n, λ, T ) provides the Planck distribution
function. This defines the emittance for each radiation band as a function of the temperature of the source surface. The boundary intensity for all outgoing directions ~s in
the band ∆λ at the wall is given by
I0λ =
qout,λ
π∆λ
(5.3-54)
Cell Zone and Boundary Condition Treatment at Semi-Transparent Walls
ANSYS FLUENT allows the specification of interior and exterior semi-transparent walls
for the DO model. In the case of interior semi-transparent walls, incident radiation
can pass through the wall and be transmitted to the adjacent medium (and possibly
refracted), it can be reflected back into the surrounding medium, and absorbed through
the wall thickness. Transmission and reflection can be diffuse and/or specular. You
specify the diffuse fraction for all transmitted and reflected radiation; the rest is treated
specularly. For exterior semi-transparent walls, there are two possible sources of radiation
on the boundary wall: an irradiation beam from outside the computational domain and
incident radiation from cells in adjacent fluid or solid zones.
For non-gray radiation, semi-transparent wall boundary conditions are applied on a perband basis. The radiant energy within a band is transmitted, reflected, and refracted as
in the gray case; there is no transmission, reflection, or refraction of radiant energy from
one band to another.
5-32
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
By default the DO equations are solved in all fluid zones, but not in any solid zones.
Therefore, if you have an adjacent solid zone for your thin wall, you will need to specify
the solid zone as participating in radiation in the Solid dialog box as part of the boundary
condition setup.
i
If you are interested in the detailed temperature distribution inside your
semi-transparent media, then you will need to model a semi-transparent
wall as a solid zone with adjacent fluid zone(s), and treat the solid as a
semi-transparent medium. This is discussed in a subsequent section.
Semi-Transparent Interior Walls
Figure 5.3.9 shows a schematic of an interior (two-sided) wall that is treated as semitransparent in ANSYS FLUENT and has zero thickness. Incident radiant energy depicted
by qin,a can pass through the semi-transparent wall if and only if the contiguous fluid
or solid cell zones participate in radiation, thereby allowing the radiation to be coupled.
Radiation coupling is set when a wall is specified as semi-transparent. Note that by
default, radiation is not coupled and you will need to explicitly specify radiation coupling
on the interior wall by changing the boundary condition type to semi-transparent in the
Wall dialog box (under the Radiation tab).
Medium a
Adjacent Fluid or Solid
f (for side a)
d
Medium b
Adjacent Fluid or Solid
f d (for side b)
q in, a reflected, specular
q in, a transmitted, specular, refracted
n
q in, a reflected, diffuse
(fd used is for side a)
q in, a transmitted, diffuse
(f used is for side a)
d
q in, a
na
nb
Figure 5.3.9: DO Radiation on Interior Semi-Transparent Wall
Release 12.0 c ANSYS, Inc. January 29, 2009
5-33
Heat Transfer
Incident radiant energy that is transmitted through a semi-transparent wall can be transmitted specularly and diffusely. Radiation can also be reflected at the interior wall back
to the surrounding medium if the refractive index na for the fluid zone that represents
medium a is different than the refractive index nb for medium b. Reflected radiation can
be reflected specularly and diffusely. The fraction of diffuse versus specular radiation
that is transmitted and reflected depends on the diffuse fraction for the wall. The special
cases of purely diffuse and purely specular transmission and reflection on semi-transparent
walls is presented in the following sections.
If the semi-transparent wall has thickness, then the thickness and the absorption coefficient determine the absorptivity of the ‘thin’ wall. If either the wall thickness or
absorption coefficient is set to 0, then the wall has no absorptivity. Although incident
radiation can be absorbed in a semi-transparent wall that has thickness, note that by
default the absorbed radiation flux does not affect the energy equation except where shell
conduction is used; this can result in an energy imbalance and possibly an unexpected
temperature field. The exception to this is when shell conduction is used (available in
3D only) in which case there is full correspondence between energy and radiation. If
the wall is expected to have significant absorption/emission then it may be better to
model the thickness explicitly with solid cells where practical. ANSYS FLUENT does not
include emission from the surface of semi-transparent walls (i.e. due to defined internal emissivity) except for the case when a specified temperature boundary condition is
defined.
Specular Semi-Transparent Walls
Consider the special case for a semi-transparent wall, when the diffuse fraction fd is equal
to 0 and all of the transmitted and reflected radiant energy at the semi-transparent wall
is purely specular.
Figure 5.3.10 shows a ray traveling from a semi-transparent medium a with refractive
index na to a semi-transparent medium b with a refractive index nb in the direction
~s. Surface a of the interface is the side that faces medium a; similarly, surface b faces
medium b. The interface normal ~n is assumed to point into side a. We distinguish
between the intensity Ia (~s), the intensity in the direction ~s on side a of the interface, and
the corresponding quantity on the side b, Ib (~s).
A part of the energy incident on the interface is reflected, and the rest is transmitted.
The reflection is specular, so that the direction of reflected radiation is given by
~sr = ~s − 2 (~s · ~n) ~n
5-34
(5.3-55)
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
s’
st
θb
medium b
medium a
s
θa
n
sr
n b > na
Figure 5.3.10: Reflection and Refraction of Radiation at the Interface Between Two Semi-Transparent Media
Release 12.0 c ANSYS, Inc. January 29, 2009
5-35
Heat Transfer
The radiation transmitted from medium a to medium b undergoes refraction. The direction of the transmitted energy, ~st , is given by Snell’s law:
sin θb =
na
sin θa
nb
(5.3-56)
where θa is the angle of incidence and θb is the angle of transmission, as shown in Figure 5.3.10. We also define the direction
~s 0 = ~st − 2 (~st · ~n) ~n
(5.3-57)
shown in Figure 5.3.10.
The interface reflectivity on side a [234]
1
ra (~s) =
2
na cos θb − nb cos θa
na cos θb + nb cos θa
!2
1
+
2
na cos θa − nb cos θb
na cos θa + nb cos θb
!2
(5.3-58)
represents the fraction of incident energy transferred from ~s to ~sr .
The boundary intensity Iw,a (~sr ) in the outgoing direction ~sr on side a of the interface is
determined from the reflected component of the incoming radiation and the transmission
from side b. Thus
Iw,a (~sr ) = ra (~s)Iw,a (~s) + τb (~s 0 )Iw,b (~s 0 )
(5.3-59)
where τb (~s 0 ) is the transmissivity of side b in direction ~s0 . Similarly, the outgoing intensity
in the direction ~st on side b of the interface, Iw,b (~st ), is given by
Iw,b (~st ) = rb (~s 0 )Iw,b (~s 0 ) + τa (~s)Iw,a (~s)
(5.3-60)
For the case na < nb , the energy transmitted from medium a to medium b in the incoming
solid angle 2π must be refracted into a cone of apex angle θc (see Figure 5.3.11) where
θc = sin−1
5-36
na
nb
(5.3-61)
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
medium b
medium a
θc
θb
θa
n
n b > na
Figure 5.3.11: Critical Angle θc
Similarly, the transmitted component of the radiant energy going from medium b to
medium a in the cone of apex angle θc is refracted into the outgoing solid angle 2π.
For incident angles greater than θc , total internal reflection occurs and all the incoming
energy is reflected specularly back into medium b. The equations presented above can be
applied to the general case of interior semi-transparent walls that is shown in Figure 5.3.9.
When medium b is external to the domain as in the case of an external semi-transparent
wall (Figure 5.3.12), Iw,b (~s 0 ) is given in Equation 5.3-59 as a part of the boundary
condition inputs. You supply this incoming irradiation flux in terms of its magnitude,
beam direction, and the solid angle over which the radiative flux is to be applied. Note
that the refractive index of the external medium is assumed to be 1.
Release 12.0 c ANSYS, Inc. January 29, 2009
5-37
Heat Transfer
Diffuse Semi-Transparent Walls
Consider the special case for a semi-transparent wall, when the diffuse fraction fd is equal
to 1 and all of the transmitted and reflected radiant energy at the semi-transparent wall
is purely diffuse.
In many engineering problems, the semi-transparent interface may be a diffuse reflector.
For such a case, the interfacial reflectivity r(~s) is assumed independent of ~s, and equal to
the hemispherically averaged value rd . For n = na /nb > 1, rd,a and rd,b are given by [316]
(1 − rd,b )
n2
n−1
1 (3n + 1)(n − 1) n2 (n2 − 1)2
+
+
ln
−
=
2
6(n + 1)2
(n2 + 1)3
n+1
2n3 (n2 + 2n − 1)
8n4 (n4 + 1)
+
ln(n)
(n2 + 1)(n4 − 1)
(n2 + 1)(n4 − 1)2
rd,a = 1 −
rd,b
(5.3-62)
(5.3-63)
The boundary intensity for all outgoing directions on side a of the interface is given by
Iw,a =
rd,a qin,a + τd,b qin,b
π
(5.3-64)
Iw,b =
rd,b qin,b + τd,a qin,a
π
(5.3-65)
Similarly for side b,
where
qin,a = −
qin,b =
Z
Z
4π
4π
Iw,a~s · ~ndΩ, ~s · ~n < 0
Iw,b~s · ~ndΩ, ~s · ~n ≥ 0
(5.3-66)
(5.3-67)
When medium b is external to the domain as in the case of an external semi-transparent
wall (Figure 5.3.12), qin,b is given as a part of the boundary condition inputs. You supply
this incoming irradiation flux in terms of its magnitude, beam direction, and the solid
angle over which the radiative flux is to be applied. Note that the refractive index of the
external medium is assumed to be 1.
5-38
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
Partially Diffuse Semi-Transparent Walls
When the diffuse fraction fd that you enter for a semi-transparent wall is between 0
and 1, the wall is partially diffuse and partially specular. In this case, ANSYS FLUENT
includes the reflective and transmitted radiative flux contributions from both diffuse and
specular components to the defining equations.
Semi-Transparent Exterior Walls
Figure 5.3.12 shows the general case of an irradiation beam qirrad applied to an exterior
semi-transparent wall with zero thickness and a non-zero absorption coefficient for the
material property. Refer to the previous section for the radiation effects of wall thickness
on semi-transparent walls.
Outside computational domain
q
Medium A
Adjacent Fluid or Solid Zone
irrad reflected, specular
q
q
irrad
normal
q
q
θ
irrad reflected, diffuse
q
irrad
transmitted, specular & refracted
irrad transmitted, diffuse
irrad
n
b
n
a
n a not equal to nb
Figure 5.3.12: DO Irradiation on External Semi-Transparent Wall
Release 12.0 c ANSYS, Inc. January 29, 2009
5-39
Heat Transfer
An irradiation flux passes through the semi-transparent wall from outside the computational domain (Figure 5.3.12) into the adjacent fluid or solid medium a. The transmitted
radiation can be refracted (bent) and dispersed specularly and diffusely, depending on
the refractive index and the diffuse fraction that you provide as a boundary condition
input. Note that there is a reflected component of qirrad when the refractive index of the
wall (nb ) is not equal to 1, as shown.
There is an additional flux beyond qirrad that is applied when the Mixed or Radiation
wall boundary conditions are selected in the Thermal tab. This external flux at the
semi-transparent wall is computed by ANSYS FLUENT as
4
Qext = external σTrad
(5.3-68)
The fraction of the above energy that will enter into the domain depends on the transmissivity of the semi-transparent wall under consideration. Note that this energy is
distributed across the solid angles (i.e., similar treatment as diffuse component.)
Incident radiation can also occur on external semi-transparent walls. Refer to the previous discussion on interior walls for details, since the radiation effects are the same.
The irradiation beam is defined by the magnitude, beam direction, and beam width that
you supply. The irradiation magnitude is specified in terms of an incident radiant heat
flux (W/m2 ). Beam width is specified as the solid angle over which the irradiation is
distributed (i.e., the beam θ and φ extents). The default beam width in ANSYS FLUENT
is 1e − 6 degrees which is suitable for collimated beam radiation. Beam direction is
defined by the vector of the centroid of the solid angle. If you select the feature Apply
Direct Irradiation Parallel to the Beam in the Wall boundary condition dialog box, then you
supply qirrad for irradiation (Figure 5.3.12) and ANSYS FLUENT computes and uses the
surface normal flux qirrad,normal in its radiation calculation. If this feature is not checked,
then you must supply the surface normal flux qirrad,normal for irradiation.
Figure 5.3.13 shows a schematic of the beam direction and beam width for the irradiation
beam. You provide these inputs (in addition to irradiation magnitude) as part of the
boundary conditions for a semi-transparent wall.
The irradiation beam can be refracted in medium a depending on the refractive index
that is specified for the particular fluid or solid zone material.
5-40
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
z
External Beam Irradiation
θ
y
ϕ
x
Beam Width ( ϕ )
∆ ϕ /2
y
x
−∆ ϕ /2
Beam Direction (X, Y, Z)
Beam Width ( θ )
z
y
∆ θ /2
−∆ θ /2
Beam Direction (X, Y, Z)
Figure 5.3.13: Beam Width and Direction for External Irradiation Beam
Release 12.0 c ANSYS, Inc. January 29, 2009
5-41
Heat Transfer
Limitations
Where shell conduction is not active, there is only limited support for absorbing and
emitting semi-transparent thin walls. In cases with significant emission or absorption
of radiation in a participating solid material, such as the absorption of long wavelength
radiation in a glass window, the use of semi-transparent thin walls can result in the
prediction of unphysical temperatures in the numerical solution. In a 3-dimensional
model this can be overcome by activating the shell conduction option for the respective
thin wall. Otherwise, where possible, it is advisable to represent the solid wall thickness
explicitly with one or more layers of cells across the wall thickness.
Solid Semi-Transparent Media
The discrete ordinates radiation model allows you to model a solid zone that has adjacent
fluid or solid zones on either side as a “semi-transparent” medium. This is done by
designating the solid zone to participate in radiation as part of the boundary condition
setup. Modeling a solid zone as a semi-transparent medium allows you to obtain a detailed
temperature distribution inside the semi-transparent zone since ANSYS FLUENT solves
the energy equation on a per-cell basis for the solid and provides you with the thermal
results. By default however, the DO equations are solved in fluid zones, but not in any
solid zones. Therefore, you will need to specify the solid zone as participating in radiation
in the Solid dialog box as part of the boundary condition setup.
Boundary Condition Treatment at Specular Walls and Symmetry Boundaries
At specular walls and symmetry boundaries, the direction of the reflected ray ~sr corresponding to the incoming direction ~s is given by Equation 5.3-55. Furthermore,
Iw (~sr ) = Iw (~s)
(5.3-69)
Boundary Condition Treatment at Periodic Boundaries
When rotationally periodic boundaries are used, it is important to use pixelation in order
to ensure that radiant energy is correctly transferred between the periodic and shadow
faces. A pixelation between 3 × 3 and 10 × 10 is recommended.
Boundary Condition Treatment at Flow Inlets and Exits
The treatment at flow inlets and exits is described in Section 5.3.5: Boundary Condition
Treatment for the DTRM at Flow Inlets and Exits.
5-42
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
5.3.7
Surface-to-Surface (S2S) Radiation Model Theory
The surface-to-surface radiation model can be used to account for the radiation exchange
in an enclosure of gray-diffuse surfaces. The energy exchange between two surfaces depends in part on their size, separation distance, and orientation. These parameters are
accounted for by a geometric function called a “view factor”.
The main assumption of the S2S model is that any absorption, emission, or scattering of
radiation can be ignored; therefore, only “surface-to-surface” radiation need be considered
for analysis.
For information about setting up the model, see Section 13.3.3: Setting Up the S2S Model
in the separate User’s Guide.
Gray-Diffuse Radiation
ANSYS FLUENT’s S2S radiation model assumes the surfaces to be gray and diffuse.
Emissivity and absorptivity of a gray surface are independent of the wavelength. Also,
by Kirchoff’s law [234], the emissivity equals the absorptivity ( = α). For a diffuse
surface, the reflectivity is independent of the outgoing (or incoming) directions.
The gray-diffuse model is what is used in ANSYS FLUENT. Also, as stated earlier, for
applications of interest, the exchange of radiative energy between surfaces is virtually
unaffected by the medium that separates them. Thus, according to the gray-body model,
if a certain amount of radiant energy (E) is incident on a surface, a fraction (ρE) is
reflected, a fraction (αE) is absorbed, and a fraction (τ E) is transmitted. Since for most
applications the surfaces in question are opaque to thermal radiation (in the infrared
spectrum), the surfaces can be considered opaque. The transmissivity, therefore, can
be neglected. It follows, from the conservation of energy, that α + ρ = 1, since α =
(emissivity), and ρ = 1 − .
The S2S Model Equations
The energy flux leaving a given surface is composed of directly emitted and reflected
energy. The reflected energy flux is dependent on the incident energy flux from the
surroundings, which then can be expressed in terms of the energy flux leaving all other
surfaces. The energy reflected from surface k is
qout,k = k σTk4 + ρk qin,k
(5.3-70)
where qout,k is the energy flux leaving the surface, k is the emissivity, σ is Boltzmann’s
constant, and qin,k is the energy flux incident on the surface from the surroundings.
Release 12.0 c ANSYS, Inc. January 29, 2009
5-43
Heat Transfer
The amount of incident energy upon a surface from another surface is a direct function
of the surface-to-surface “view factor,” Fjk . The view factor Fjk is the fraction of energy
leaving surface k that is incident on surface j. The incident energy flux qin,k can be
expressed in terms of the energy flux leaving all other surfaces as
Ak qin,k =
N
X
Aj qout,j Fjk
(5.3-71)
j=1
where Ak is the area of surface k and Fjk is the view factor between surface k and surface
j. For N surfaces, using the view factor reciprocity relationship gives
Aj Fjk = Ak Fkj for j = 1, 2, 3, . . . N
(5.3-72)
so that
qin,k =
N
X
Fkj qout,j
(5.3-73)
j=1
Therefore,
qout,k = k σTk4 + ρk
N
X
Fkj qout,j
(5.3-74)
j=1
which can be written as
Jk = Ek + ρk
N
X
Fkj Jj
(5.3-75)
j=1
where Jk represents the energy that is given off (or radiosity) of surface k, and Ek
represents the emissive power of surface k. This represents N equations, which can be
recast into matrix form as
KJ = E
(5.3-76)
where K is an N × N matrix, J is the radiosity vector, and E is the emissive power
vector.
5-44
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
Equation 5.3-76 is referred to as the radiosity matrix equation. The view factor between
two finite surfaces i and j is given by
1 Z Z cos θi cos θj
Fij =
δij dAi dAj
Ai Ai Aj
πr2
(5.3-77)
where δij is determined by the visibility of dAj to dAi . δij = 1 if dAj is visible to dAi
and 0 otherwise.
Clustering
The S2S radiation model is computationally very expensive when there is a large number
of radiating surfaces. To reduce the computational time as well as the storage requirement, the number of radiating surfaces is reduced by creating surface “clusters”. The
surface clusters are made by starting from a face and adding its neighbors and their
neighbors until a specified number of faces per surface cluster is collected.
An algorithm has been implemented for the creation of surface clusters which is faster
and supports non-conformal interfaces, hanging nodes, or mesh adaption. This algorithm
is now the default. If you wish to use the old algorithm, you may use the TUI command
but adaption and non-conformal interfaces will not be supported.
The radiosity, J, is calculated for the surface clusters. These values are then distributed
to the faces in the clusters to calculate the wall temperatures. Since the radiation source
terms are highly non-linear (proportional to the fourth power of temperature), care must
be taken to calculate the average temperature of the surface clusters and distribute the
flux and source terms appropriately among the faces forming the clusters.
The surface cluster temperature is obtained by area averaging as shown in the following
equation:
Af Tf4
P
Af
P
Tsc =
f
!1/4
(5.3-78)
where Tsc is the temperature of the surface cluster, and Af and Tf are the area and
temperature of face f . The summation is carried over all faces of a surface cluster.
Release 12.0 c ANSYS, Inc. January 29, 2009
5-45
Heat Transfer
Smoothing
Smoothing can be performed on the view factor matrix to enforce the reciprocity relationship and conservation.
The reciprocity relationship is represented by
Ai Fij = Aj Fji
(5.3-79)
where Ai is the area of surface i, Fij is the view factor between surfaces i and j, and Fji
is the view factor between surfaces j and i.
Once the reciprocity relationship has been enforced, a least-squares smoothing method [175]
can be used to ensure that conservation is satisfied, i.e.,
X
5.3.8
Fij = 1.0
(5.3-80)
Radiation in Combusting Flows
The Weighted-Sum-of-Gray-Gases Model
The weighted-sum-of-gray-gases model (WSGGM) is a reasonable compromise between
the oversimplified gray gas model and a complete model which takes into account particular absorption bands. The basic assumption of the WSGGM is that the total emissivity
over the distance s can be presented as
=
I
X
a,i (T )(1 − e−κi ps )
(5.3-81)
i=0
where a,i is the emissivity weighting factor for the ith fictitious gray gas, the bracketed
quantity is the ith fictitious gray gas emissivity, κi is the absorption coefficient of the ith
gray gas, p is the sum of the partial pressures of all absorbing gases, and s is the path
length. For a,i and κi ANSYS FLUENT uses values obtained from [60] and [326]. These
values depend on gas composition, and a,i also depend on temperature. When the total
pressure is not equal to 1 atm, scaling rules for κi are used (see Equation 5.3-87).
The absorption coefficient for i = 0 is assigned a value of zero to account for windows in
P
the spectrum between spectral regions of high absorption ( Ii=1 a,i < 1) and the weighting factor for i = 0 is evaluated from [326]:
a,0 = 1 −
I
X
a,i
(5.3-82)
i=1
5-46
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
The temperature dependence of a,i can be approximated by any function, but the most
common approximation is
J
X
a,i =
b,i,j T j−1
(5.3-83)
j=1
where b,i,j are the emissivity gas temperature polynomial coefficients. The coefficients
b,i,j and κi are estimated by fitting Equation 5.3-81 to the table of total emissivities,
obtained experimentally [60, 70, 326].
The absorptivity α of the radiation from the wall can be approximated in a similar
way [326], but, to simplify the problem, it is assumed that = α [233]. This assumption is
justified unless the medium is optically thin and the wall temperature differs considerably
from the gas temperature.
Since the coefficients b,i,j and κi are slowly varying functions of ps and T , they can be
assumed constant for a wide range of these parameters. In [326] these constant coefficients
are presented for different relative pressures of the CO2 and H2 O vapor, assuming that
the total pressure pT is 1 atm. The values of the coefficients shown in [326] are valid for
0.001 ≤ ps ≤ 10.0 atm-m and 600 ≤ T ≤ 2400 K. For T > 2400 K, coefficient values
suggested by [60] are used. If κi ps 1 for all i, Equation 5.3-81 simplifies to
=
I
X
a,i κi ps
(5.3-84)
i=0
Comparing Equation 5.3-84 with the gray gas model with absorption coefficient a, it can
be seen that the change of the radiation intensity over the distance s in the WSGGM is
exactly the same as in the gray gas model with the absorption coefficient
a=
I
X
a,i κi p
(5.3-85)
i=0
which does not depend on s. In the general case, a is estimated as
a=−
ln(1 − )
s
(5.3-86)
where the emissivity for the WSGGM is computed using Equation 5.3-81. a as defined
by Equation 5.3-86 depends on s, reflecting the non-gray nature of the absorption of
thermal radiation in molecular gases. In ANSYS FLUENT, Equation 5.3-85 is used when
s ≤ 10−4 m and Equation 5.3-86 is used for s > 10−4 m. Note that for s ≈ 10−4 m,
the values of a predicted by Equations 5.3-85 and 5.3-86 are practically identical (since
Equation 5.3-86 reduces to Equation 5.3-85 in the limit of small s).
Release 12.0 c ANSYS, Inc. January 29, 2009
5-47
Heat Transfer
ANSYS FLUENT allows you to specify s as the mean beam length or the characteristic
cell size. The model based on the mean beam length is the recommended approach,
especially when you have a nearly homogeneous medium and you are interested in the
radiation exchange between the walls of the enclosure. You can specify the mean beam
length or have ANSYS FLUENT compute it. If you do decide to use the WSGGM based
on the characteristic cell size, note that the predicted values of a will be mesh dependent
(this is a known limitation of the model). See Section 8.8.1: Inputs for a CompositionDependent Absorption Coefficient in the separate User’s Guide for details about setting
properties for the WSGGM.
i
The WSGGM cannot be used to specify the absorption coefficient in each
band when using the non-gray DO model. If the WSGGM is used with
the non-gray DO model, the absorption coefficient will be the same in all
bands.
When ptot 6= 1 atm
The WSGGM, as described above, assumes that ptot —the total (static) gas pressure—is
equal to 1 atm. In cases where ptot is not unity (e.g., combustion at high temperatures),
scaling rules suggested in [84] are used to introduce corrections. When ptot < 0.9 atm or
ptot > 1.1 atm, the values for κi in Equations 5.3-81 and 5.3-85 are rescaled:
κi → κi pm
tot
(5.3-87)
where m is a non-dimensional value obtained from [84], which depends on the partial
pressures and temperature T of the absorbing gases, as well as on ptot .
The Effect of Soot on the Absorption Coefficient
When soot formation is computed, ANSYS FLUENT can include the effect of the soot concentration on the radiation absorption coefficient. The generalized soot model estimates
the effect of the soot on radiative heat transfer by determining an effective absorption
coefficient for soot. The absorption coefficient of a mixture of soot and an absorbing
(radiating) gas is then calculated as the sum of the absorption coefficients of pure gas
and pure soot:
as+g = ag + as
(5.3-88)
where ag is the absorption coefficient of gas without soot (obtained from the WSGGM)
and
as = b1 ρm [1 + bT (T − 2000)]
5-48
(5.3-89)
Release 12.0 c ANSYS, Inc. January 29, 2009
5.3 Modeling Radiation
with
b1 = 1232.4 m2 /kg and bT ≈ 4.8 × 10−4 K−1
ρm is the soot density in kg/m3 .
The coefficients b1 and bT were obtained [302] by fitting Equation 5.3-89 to data based
on the Taylor-Foster approximation [348] and data based on the Smith et al. approximation [326].
See Section 8.8: Radiation Properties and Section 21.3.1: Using the Soot Models in the
separate User’s Guide for information about including the soot-radiation interaction effects.
The Effect of Particles on the Absorption Coefficient
ANSYS FLUENT can also include the effect of discrete phase particles on the radiation
absorption coefficient, provided that you are using either the P-1 or the DO model. When
the P-1 or DO model is active, radiation absorption by particles can be enabled. The
particle emissivity, reflectivity, and scattering effects are then included in the calculation
of the radiative heat transfer. See Section 23.5: Setting Material Properties for the
Discrete Phase in the separate User’s Guide for more details on the input of radiation
properties for the discrete phase.
5.3.9
Choosing a Radiation Model
For certain problems one radiation model may be more appropriate than the others.
When deciding which radiation model to use, consider the following:
• Optical thickness: The optical thickness aL is a good indicator of which model to
use in your problem. Here, L is an appropriate length scale for your domain. For
flow in a combustor, for example, L is the diameter of the combustion chamber.
If aL 1, your best alternatives are the P-1 and Rosseland models. The P-1
model should typically be used for optical thicknesses > 1. For optical thickness
> 3, the Rosseland model is cheaper and more efficient. For high optical thickness
cases, a second-order discretization scheme for the DO model is recommended. The
DTRM and the DO model work across the full range of optical thicknesses, but are
substantially more expensive to use. Consequently, you should use the “thick-limit”
models, P-1 and Rosseland, if the problem allows it. For optically thin problems
(aL < 1), the DTRM and the DO model, only, are appropriate.
• Scattering and emissivity: The P-1, Rosseland, and DO models account for scattering, while the DTRM neglects it. Since the Rosseland model uses a temperature
slip condition at walls, it is insensitive to wall emissivity.
Release 12.0 c ANSYS, Inc. January 29, 2009
5-49
Heat Transfer
• Particulate effects: Only the P-1 and DO models account for exchange of radiation
between gas and particulates (see Equation 5.3-8).
• Semi-transparent walls (interior and exterior): Only the DO model allows you to
model semi-transparent walls of various types (e.g., glass).
• Specular walls: Only the DO model allows specular reflection (e.g., for dust-free
mirror).
• Partially-specular walls: Only the DO model allows specular reflection (e.g., dusty
mirror).
• Non-gray radiation: Only the DO model allows you to compute non-gray radiation
using a gray band model.
• Localized heat sources: In problems with localized sources of heat, the P-1 model
may over-predict the radiative fluxes. The DO model is probably the best suited
for computing radiation for this case, although the DTRM, with a sufficiently large
number of rays, is also acceptable.
• Enclosure radiative transfer with non-participating media: The surface-to-surface
(S2S) model is suitable for this type of problem. The radiation models used with
participating media may, in principle, be used to compute the surface-to-surface
radiation, but they are not always efficient.
External Radiation
If you need to include radiative heat transfer from the exterior of your physical model,
you can include an external radiation boundary condition in your model (for details, see
Section 7.3.14: Thermal Boundary Conditions at Walls in the separate User’s Guide). If
you are not concerned with radiation within the domain, this boundary condition can be
used without activating one of the radiation models.
5-50
Release 12.0 c ANSYS, Inc. January 29, 2009
Chapter 6.
Heat Exchangers
Many engineering systems, including power plants, climate control, and engine cooling
systems typically contain tubular heat exchangers. However, for most engineering problems, it is impractical to model individual fins and tubes of a heat exchanger core. In
principle, heat exchanger cores introduce a pressure drop to the primary fluid stream and
transfer heat to a second fluid, a coolant, referred to here as the auxiliary fluid.
In ANSYS FLUENT, lumped-parameter models are used to account for the pressure loss
and auxiliary fluid heat rejection. ANSYS FLUENT provides two heat exchanger models:
the macro (ungrouped and grouped) models and the dual cell model. The macro model
allows you to choose between two heat transfer models, namely the simple-effectivenessmodel and the number-of-transfer-units (NTU) model. The models can be used to compute auxiliary fluid inlet temperature for a fixed heat rejection or total heat rejection for
a fixed auxiliary fluid inlet temperature. For the simple-effectiveness-model, the auxiliary
fluid may be single-phase or two-phase. The dual cell model uses the NTU method for
heat transfer calculations. This model allows the solution of auxiliary flow on a separate
mesh (other than the primary fluid mesh), unlike the macro model, where the auxiliary
flow is modeled as 1-D flow. The dual cell model also offers more flexibility as far as the
shape of the heat exchanger is concerned, and overcomes some of the major limitations
present in the macro model.
For more information about using the heat exchanger models, see Section 14: Modeling
Heat Exchangers in the separate User’s Guide.
The following sections contain information about the theory behind the heat exchanger
models:
• Section 6.1: The Macro Heat Exchanger Models
• Section 6.2: The Dual Cell Model
6.1
The Macro Heat Exchanger Models
The following sections contain information about the theory behind the macro heat exchanger models:
• Section 6.1.1: Overview and Restrictions of the Macro Heat Exchanger Models
• Section 6.1.2: Macro Heat Exchanger Model Theory
Release 12.0 c ANSYS, Inc. January 29, 2009
6-1
Heat Exchangers
6.1.1
Overview and Restrictions of the Macro Heat Exchanger Models
Overview
In a typical heat exchanger core, the auxiliary fluid temperature is stratified in the
direction of the auxiliary fluid flow. As a result, heat rejection is not constant over
the entire core. In ANSYS FLUENT, the fluid zone representing the heat exchanger
core is subdivided into macroscopic cells or macros along the auxiliary fluid path, as in
Figure 6.1.1. In this figure, the core is discretized into 3×4×2 macros. This configuration
consists of 2 passes, each pass having four rows and three columns of macros. The
auxiliary fluid inlet temperature to each macro is computed and then subsequently used
to compute the heat rejection from each macro. This approach provides a realistic heat
rejection distribution over the heat exchanger core.
To use the heat exchanger models, you must define one or more fluid zone(s) to represent
the heat exchanger core. Typically, the fluid zone is sized to the dimension of the core
itself. As part of the setup procedure, you will define the auxiliary fluid path, the number
of macros, and the physical properties and operating conditions of the core (pressure drop
parameters, heat exchanger effectiveness, auxiliary fluid flow rate, etc.).
You can also combine several fluid zones as a single heat exchanger group. In this
situation each fluid zone acts as a separate heat exchanger core, and the auxiliary fluid
mass flow rate of the heat exchanger group is divided among the zones in the ratio of the
respective volumes. For the purpose of auxiliary fluid flow, heat exchanger groups can also
be connected in series. In addition, a heat exchanger group can have an auxiliary fluid
pressure drop (e.g., for pressure dependent properties) and a supplementary auxiliary
fluid stream entering or leaving it. For more information on heat exchanger groups, see
Section 14.4: Using the Grouped Macro Heat Exchanger Model.
The heat exchanger models were designed for “compact” heat exchangers, implying that
the primary fluid side flow is unidirectional. The auxiliary fluid is assumed to flow through
a large number of parallel tubes, which can optionally double back in a serpentine pattern
to create a number of “passes”. You can independently choose the principal auxiliary fluid
flow direction, the pass-to-pass direction and the external primary fluid flow direction.
i
6-2
It is highly recommended that the free-form Tet mesh is not used in the
macro heat exchanger model. Instead, evenly distributed Hex/Wedge cells
should be used for improved accuracy and a more robust solution process.
Release 12.0 c ANSYS, Inc. January 29, 2009
6.1 The Macro Heat Exchanger Models
Coolant Passage
Macro 0
Macro 1
Macro 2
Macro 21
Macro 2 2
Macro 23
Macro 3
Macro 4
Macro 5
Macro 18
Macro 19
Macro 20
Macro 6
Macro 7
Macro 8
Macro 15
Macro 16
Macro 17
Macro 9
Macro 10
Macro 11
Macro 12
Macro 13
Macro 14
Figure 6.1.1: Core Discretized Into 3 × 4×2 Macros
Release 12.0 c ANSYS, Inc. January 29, 2009
6-3
Heat Exchangers
Restrictions
The following restrictions exist for the macro heat exchanger models:
• The core must be approximately rectangular in shape.
• The primary fluid streamwise direction (see Equation 6.1-1) must be aligned with
one of the three orthogonal axes defined by the rectangular core.
• Flow acceleration effects are neglected in calculating the pressure loss coefficient.
• For the simple-effectiveness-model, the primary fluid capacity rate must be less than
the auxiliary fluid capacity rate.
• Auxiliary fluid phase change cannot be modeled using the ntu-model.
• The macro-based method requires that an equal number of cells reside in each
macro of equal size and shape.
• Auxiliary fluid flow is assumed to be 1-D.
• The pass width has to be uniform.
• Accuracy is not guaranteed when the mesh is not structured or layered.
• Accuracy is not guaranteed when there is upstream diffusion of temperature at the
inlet/outlet of the core.
• Non-conformal meshes cannot be attached to the inlet/outlet of the core. An extra
layer has to be created to avoid it.
6.1.2
Macro Heat Exchanger Model Theory
In ANSYS FLUENT, the heat exchanger core is treated as a fluid zone with momentum
and heat transfer. Pressure loss is modeled as a momentum sink in the momentum
equation, and heat transfer is modeled as a heat source in the energy equation.
ANSYS FLUENT provides two heat transfer models: the default ntu-model and the simpleeffectiveness-model. The simple-effectiveness-model interpolates the effectiveness from the
velocity vs effectiveness curve that you provide. For the ntu-model, ANSYS FLUENT
calculates the effectiveness, , from the NTU value that is calculated by ANSYS FLUENT
from the heat transfer data provided by the user in tabular format. ANSYS FLUENT will
automatically convert this heat transfer data to a primary fluid mass flow rate vs NTU
curve (this curve will be piecewise linear). This curve will be used by ANSYS FLUENT
to calculate the NTU for macros based on their size and primary fluid flow rate.
6-4
Release 12.0 c ANSYS, Inc. January 29, 2009
6.1 The Macro Heat Exchanger Models
The ntu-model provides the following features:
• The model can be used to check the heat capacity for both the primary and the
auxiliary fluid, and takes the lesser of the two for the calculation of heat transfer.
• The model can be used to model heat transfer to the primary fluid from the auxiliary
fluid and vice versa.
• The model can be used to model primary fluid-side reverse flow.
• The model can be used with variable density of the primary fluid.
• The model can be used in either the serial or parallel ANSYS FLUENT solvers.
• Transient profiles can be used for the auxiliary fluid inlet temperature and for total
heat rejection.
• Transient profiles can be used for auxiliary mass flow rates.
The simple-effectiveness-model provides the following features:
• The model can be used to model heat transfer from the auxiliary fluid to the
primary fluid.
• The auxiliary fluid properties can be a function of pressure and temperature, thus
allowing phase change of the auxiliary fluid.
• The model can be used by serial as well as parallel solvers.
• The model can be used to make a network of heat exchangers using a heat exchanger
group (Section 14.4: Using the Grouped Macro Heat Exchanger Model).
• Transient profiles can be used for the auxiliary fluid inlet temperature and for total
heat rejection.
• Transient profiles can be used for auxiliary mass flow rates.
Release 12.0 c ANSYS, Inc. January 29, 2009
6-5
Heat Exchangers
Streamwise Pressure Drop
In both heat transfer models, pressure loss is modeled using the porous media model in
ANSYS FLUENT. For the dual cell model (Section 6.2: The Dual Cell Model), pressure
loss is used for both streams, while for the macro model, it is used only for the primary
side.
The loss coefficients of the porous media model are computed using curve fitting of the
pressure-versus-flow rate data outside of ANSYS FLUENT, which you will specify for the
cell zone conditions. However, in some cases, the data for curve-fitting is not available.
The macro model provides an additional means of getting the coefficients if the data is
not available. The coefficients can also be automatically computed (and updated) using
a known pressure loss coefficient as a function of some geometric parameters, the theory
of which is defined below:
1
∆p = f ρm UA2 min
2
(6.1-1)
where
∆p
f
ρm
UAmin
= streamwise pressure drop
= streamwise pressure loss coefficient
= mean primary fluid density
= primary fluid velocity at the minimum flow area
The pressure loss coefficient is computed from
νe
νe
A νm
f = (Kc + 1 − σ ) − (1 − σ − Ke ) + 2
− 1 + fc
νi
νi
Ac νi
2
2
(6.1-2)
where
σ
Kc
Ke
A
Ac
fc
νe
νi
νm
6-6
=
=
=
=
=
=
=
=
=
minimum flow to face area ratio
entrance loss coefficient
exit loss coefficient
primary fluid-side surface area
minimum cross-sectional flow area
core friction factor
specific volume at the exit
specific volume at the inlet
mean specific volume ≡ 12 (νe + νi )
Release 12.0 c ANSYS, Inc. January 29, 2009
6.1 The Macro Heat Exchanger Models
Kc and Ke are empirical quantities obtained from experimental data. You will need to
specify these parameters based on graphs that are closest to the heat exchanger configuration that you are setting up [160], [158]. These parameters are used to set up large
resistances in the two non-streamwise directions, effectively forcing the primary fluid flow
through the core to be unidirectional.
In Equation 6.1-2, the core friction factor is defined as
fc = aRebmin
(6.1-3)
where
a
b
Remin
= core friction coefficient
= core friction exponent
= Reynolds number for velocity at the minimum flow area
a and b are empirical quantities obtained from experimental data. You will need to
specify the core friction coefficient and exponent based on graphs that are closest to the
heat exchanger models that you set up [160], [158].
The Reynolds number in Equation 6.1-3 is defined as
Remin =
ρm UAmin Dh
µm
(6.1-4)
where
ρm
µm
Dh
UAmin
= mean primary fluid density
= mean primary fluid viscosity
= hydraulic diameter
= primary fluid velocity at the minimum flow area
For a heat exchanger core, the hydraulic diameter can be defined as
Ac
Dh = 4L
A
(6.1-5)
where L is the flow length of the heat exchanger. If the tubes are normal to the primary
fluid flow, then L is the length in the primary fluid flow direction. Note that UAmin can
be calculated from
UAmin =
U
σ
(6.1-6)
where U is the primary fluid velocity and σ is the minimum flow to face area ratio.
Release 12.0 c ANSYS, Inc. January 29, 2009
6-7
Heat Exchangers
Heat Transfer Effectiveness
For the simple-effectiveness-model, the heat-exchanger effectiveness, , is defined as the
ratio of actual rate of heat transfer from the hot to cold fluid to the maximum possible
rate of heat transfer. The maximum possible heat transfer is given by
qmax = Cmin (Tin,hot − Tin,cold )
(6.1-7)
where Tin,hot and Tin,cold are the inlet temperatures of the hot and cold fluids and
Cmin = min[(ṁcp )hot , (ṁcp )cold ]
(6.1-8)
Thus, the actual rate of heat transfer, q, is defined as
q = Cmin (Tin,hot − Tin,cold )
(6.1-9)
The value of depends on the heat exchanger geometry and flow pattern (parallel flow,
counter flow, cross flow, etc.). Even though the effectiveness of the primary fluid is
computed using uniform conditions on the entire heat exchanger core, it is being applied
to a small portion of the core represented by a computational cell. This can make it less
accurate for some heat exchanger cores, where there is a strong variation in the primary
flow. For a core with a strong primary flow variation, the NTU model must be used.
For the ntu-model, given the heat exchanger performance data (total heat rejection versus
primary flow rate) based on uniform test conditions, ANSYS FLUENT calculates the
effectiveness of the entire heat exchanger from the ratio of heat capacity and the number
of transfer units using the relation
1 0.22
0.78
= 1 − exp − Ntu
(1 − e−Cr Ntu )
Cr
(6.1-10)
where Cr is the ratio of Cmin to Cmax .
The heat exchanger performance data should be specified for a number of auxiliary flow
rates so that ANSYS FLUENT can compute the number of transfer units versus the
primary fluid flow rate for a number of auxiliary fluid flow rates. This NTU, which is
based on the full heat exchanger and uniform conditions, is scaled for each macro using
the ratio of their volumes and minimum heat capacities.
For each macro, the primary fluid inlet temperature is calculated using the mass average
of the incoming primary fluid temperatures at the boundaries. This automatically takes
into account any reverse flow of the primary fluid at the boundaries.
6-8
Release 12.0 c ANSYS, Inc. January 29, 2009
6.1 The Macro Heat Exchanger Models
Heat Rejection
Heat rejection is computed for each cell within a macro and added as a source term to the
energy equation for the primary fluid flow. Note that heat rejection from the auxiliary
fluid to primary fluid can be either positive or negative.
For the simple-effectiveness-model, the heat transfer for a given cell is computed from
qcell = (ṁcp )g (Tin,auxiliary − Tcell )
(6.1-11)
where
(ṁcp )g
Tin,auxiliary
Tcell
=
=
=
=
heat exchanger effectiveness
primary fluid capacity rate (flow rate × specific heat)
auxiliary fluid inlet temperature of macro containing the cell
cell temperature
For the simple-effectiveness-model, the heat rejection from a macro is calculated by summing the heat transfer of all the cells contained within the macro
qmacro =
X
qcell
(6.1-12)
all cells in macro
For the ntu-model, the heat transfer for a macro is calculated from
qmacro = Cmin (Tin,auxiliary − Tin,primary )
(6.1-13)
where
Tin,auxiliary
Tin,primary
= macro effectiveness
= macro auxiliary fluid inlet temperature
= macro primary fluid inlet temperature
For the ntu-model, the heat transfer for a given cell is computed from
qcell = qmacro
Release 12.0 c ANSYS, Inc. January 29, 2009
Vcell
Vmacro
(6.1-14)
6-9
Heat Exchangers
For both heat exchanger models, the total heat rejection from the heat exchanger core is
computed as the sum of the heat rejection from all the macros:
qtotal =
X
qmacro
(6.1-15)
all macros
The auxiliary fluid inlet temperature to each macro (Tin,auxiliary in Equations 6.1-11 and
6.1-13) is computed based on the energy balance of the auxiliary fluid at a previous macro
computation. For a given macro,
qmacro = (ṁ)auxiliary (hout − hin )
(6.1-16)
where hin and hout are the inlet and outlet enthalpies of the auxiliary fluid in the macro.
The auxiliary fluid outlet temperature from the macro is calculated as
Tout =
hout
cp,auxiliary
constant specific heat method
(6.1-17)
f (hout , p) UDF method
where
f
p
= user-defined function
= auxiliary fluid pressure
The values of hout and Tout then become the inlet conditions to the next macro.
The first row of macros (Macros 0, 1, and 2 in Figure 6.1.1) are assumed to be where the
auxiliary fluid enters the heat exchanger core. When the fixed total heat rejection from
the heat exchanger core is specified, the inlet temperature to the first row of macros is
iteratively computed, so that all of the equations are satisfied simultaneously. When a
fixed auxiliary fluid inlet temperature is specified, the heat transfer for the first row of
macros are used to calculate their exit enthalpy, which becomes the inlet condition for
the next row macros. At the end of each pass, the outlet enthalpy of each macro (in the
last row) is mass averaged to obtain the inlet condition for the next pass macros.
6-10
Release 12.0 c ANSYS, Inc. January 29, 2009
6.1 The Macro Heat Exchanger Models
Macro Heat Exchanger Group Connectivity
If the optional macro heat exchanger group is used, a single heat exchanger may be
consist of multiple fluid zones. In this case, the auxiliary fluid is assumed to flow through
these zones in parallel. Thus, after taking into account any auxiliary stream effects, the
auxiliary fluid inlet mass flow rate is automatically apportioned to each zone in the group
as follows:
!
P
ṁi =
Vi,k
ṁ
P P
i
k Vi,k
k
(6.1-18)
where ṁi is the total auxiliary mass flow rate for the heat exchanger group. Vi,k refers
to the volume of the kth finite volume cell within the ith fluid zone. Within each zone,
the auxiliary fluid flows through each macro in series as usual.
At the outlet end of the group, the parallel auxiliary fluid streams through the individual
zones are recombined, and the outlet auxiliary fluid enthalpy is calculated on a massaveraged basis:
P
h̄ =
ṁi hi
P
i ṁi
!
i
(6.1-19)
With user-defined functions, the simple-effectiveness-model allows you to simulate twophase auxiliary fluid flows and other complex auxiliary fluid enthalpy relationships of the
form
h = h(T, p, x)
(6.1-20)
where p is the absolute pressure and x is the quality (mass fraction of vapor) of a twophase vapor-liquid mixture. When pressure-dependent auxiliary fluid properties are used,
the mean pressure within each macro is calculated and passed to the user-defined function
as
p̄j = pin + j +
1 ∆p
2 N
(6.1-21)
where
j
pin
∆p
N
=
=
=
=
macro row index
inlet auxiliary fluid pressure
overall pressure drop across a heat exchanger group
number of rows per pass × number of passes.
To learn how to use the macro heat exchanger models, refer to Section 14.3: Using the
Ungrouped Macro Heat Exchanger Model and Section 14.4: Using the Grouped Macro
Heat Exchanger Model in the separate User’s Guide.
Release 12.0 c ANSYS, Inc. January 29, 2009
6-11
Heat Exchangers
6.2
The Dual Cell Model
The following sections contain information about the theory behind the dual cell heat
exchanger model:
• Section 6.2.1: Overview and Restrictions of the Dual Cell Model
• Section 6.2.2: Dual Cell Model Theory
6.2.1
Overview and Restrictions of the Dual Cell Model
Overview
The Macro Model is quite suitable for thin rectangular heat exchanger cores, where
the pass-to-pass is perpendicular to the primary flow direction and the auxiliary flow is
uniform. Moreover, the mesh should be uniform and structured. However, many practical
heat exchangers have a non-rectangular core and the auxiliary fluid, before reaching the
core, may pass through arbitrary shaped inlet tanks, which make them highly nonuniform. It is quite possible that due to the complex shape of the core and or ease of
meshing, the structured mesh may not be the obvious choice. These shortcomings of the
macro model can be easily overcome by using the dual cell heat exchanger model. This
model allows the solution of both the primary and auxiliary flow on separate co-located
meshes and couples the two flows only through heat transfer at the heat exchanger core.
Restrictions
The following restrictions exist for the dual cell heat exchanger models:
• Heat transfer calculations are based on the NTU method only.
• Multipass heat exchangers cannot be modeled. This will require hooking a UDF.
• In the case of a heat exchanger core with non-matching meshes, the total cell count
for the primary and auxiliary core should approximately be the same.
6-12
Release 12.0 c ANSYS, Inc. January 29, 2009
6.2 The Dual Cell Model
6.2.2
Dual Cell Model Theory
The dual cell heat exchanger consists of two porous fluid zones, namely a primary zone
and an auxiliary zone. The two zones are solved simultaneously and are coupled only
through heat transfer. The common region in each zone, where heat transfer takes place,
represents the heat exchanger core. The cores for both primary and auxiliary zones
occupy the same physical space, as shown in Figure 6.2.1. The cells in the two cores
should overlap completely in the physical space to ensure conservative heat transfer.
Heat transfer occurs between cells in close proximity based on the cell centroid. In other
words, a primary zone cell exchanges heat with one, and only one, auxiliary zone cell
and vice versa. Therefore, if one of the core (say primary) mesh is too coarse or fine
relative to the other core (say auxiliary) conservation of heat transfer is not ensured.
Heat transfer calculations in the dual cell model are based on the NTU method.
NTU Relations
In a cross-flow pattern, the NTU values are calculated as in Equation 6.1-10. The equation is solved iteratively using the Newton-Raphson. For parallel flow, the NTU value is
calculated as follows:
NTU =
−ln(1 − − Cr )
(Cr + 1)
(6.2-1)
and for counter flow, the following equation is used:
N T UCr =1 =
1−
(6.2-2)
Otherwise,
"
(1 − )
1
ln
NTU =
(Cr − 1)
(1 − Cr )
#
(6.2-3)
where Cr is the heat capacity ratio and is the effectiveness.
Release 12.0 c ANSYS, Inc. January 29, 2009
6-13
Heat Exchangers
Figure 6.2.1: Core with Matching Quad Meshes for Primary and Auxiliary
Zones in a Cross-Flow Pattern
6-14
Release 12.0 c ANSYS, Inc. January 29, 2009
6.2 The Dual Cell Model
Heat Rejection
Heat rejection is computed for each cell in the two cores (primary and auxiliary) and
added as a source term to the energy equation for the respective flows. This is illustrated
in Figure 6.2.2 and the following equations:
Figure 6.2.2: Core with Primary and Auxiliary Zones with Possible Overlap
of Cells
ṁscaled,A = ρcell,A V~cell,A Ainlet,A
(6.2-4)
ṁscaled,P = ρcell,P V~cell,P Ainlet,P
(6.2-5)
Cmin,scaled = min[(Cp,cell ṁscale )|P , (Cp,cell ṁscale )|A ]
(6.2-6)
Release 12.0 c ANSYS, Inc. January 29, 2009
6-15
Heat Exchangers
N T Uscaled = [N T Uf ull (ṁscaled,P , ṁscaled,A )]bilinearinterpolation
(6.2-7)
(U A)scaled = N T Uscaled Cmin,scaled
(6.2-8)
dq = qcell =
where
Tcell,A
Tcell,P
U
A
Cmin,scaled
=
=
=
=
=
(U A)scaled (Tcell,A − Tcell,P )
V olumecell
(6.2-9)
auxiliary cell temperature
primary cell temperature
overall heat transfer coefficient
total heat transfer area
scaled minimum heat capacity rate
You can supply the NTU values, or it can be calculated using the supplied raw data and
the effectiveness-NTU relation that you specify.
To learn how to use the dual cell heat exchanges model, refer to Section 14.5: Using the
Dual Cell Heat Exchanger Model in the separate User’s Guide.
6-16
Release 12.0 c ANSYS, Inc. January 29, 2009
Chapter 7.
Species Transport and Finite-Rate Chemistry
ANSYS FLUENT can model the mixing and transport of chemical species by solving
conservation equations describing convection, diffusion, and reaction sources for each
component species. Multiple simultaneous chemical reactions can be modeled, with reactions occurring in the bulk phase (volumetric reactions) and/or on wall or particle
surfaces, and in the porous region. Species transport modeling capabilities, both with
and without reactions, are described in this chapter.
Note that you may also want to consider modeling your turbulent reacting flame using
the mixture fraction approach (for non-premixed systems, described in Chapter 8: NonPremixed Combustion), the reaction progress variable approach (for premixed systems,
described in Chapter 9: Premixed Combustion), the partially premixed approach (described in Chapter 10: Partially Premixed Combustion), or the composition PDF Transport approach (described in Chapter 11: Composition PDF Transport). Modeling multiphase species transport and finite-rate chemistry can be found in Chapter 16: Multiphase
Flows.
Information is divided into the following sections:
• Section 7.1: Volumetric Reactions
• Section 7.2: Wall Surface Reactions and Chemical Vapor Deposition
• Section 7.3: Particle Surface Reactions
For more information about using these models in ANSYS FLUENT, see Chapter 15: Modeling Species Transport and Finite-Rate Chemistry in the separate User’s Guide.
7.1
Volumetric Reactions
Theoretical information about species transport and finite-rate chemistry as related to
volumetric reactions is presented in this section. Additional information can be found in
the following sections:
• Section 7.1.1: Species Transport Equations
• Section 7.1.2: The Generalized Finite-Rate Formulation for Reaction Modeling
For more information about using species transport and finite-rate chemistry as related
to volumetric reactions, see Section 15.1: Volumetric Reactions in the separate User’s
Guide.
Release 12.0 c ANSYS, Inc. January 29, 2009
7-1
Species Transport and Finite-Rate Chemistry
7.1.1
Species Transport Equations
When you choose to solve conservation equations for chemical species, ANSYS FLUENT
predicts the local mass fraction of each species, Yi , through the solution of a convectiondiffusion equation for the ith species. This conservation equation takes the following
general form:
∂
(ρYi ) + ∇ · (ρ~v Yi ) = −∇ · J~i + Ri + Si
∂t
(7.1-1)
where Ri is the net rate of production of species i by chemical reaction (described later
in this section) and Si is the rate of creation by addition from the dispersed phase plus
any user-defined sources. An equation of this form will be solved for N − 1 species where
N is the total number of fluid phase chemical species present in the system. Since the
mass fraction of the species must sum to unity, the N th mass fraction is determined as
one minus the sum of the N − 1 solved mass fractions. To minimize numerical error,
the N th species should be selected as that species with the overall largest mass fraction,
such as N2 when the oxidizer is air.
Mass Diffusion in Laminar Flows
In Equation 7.1-1, J~i is the diffusion flux of species i, which arises due to gradients of
concentration and temperature. By default, ANSYS FLUENT uses the dilute approximation (also called Fick’s law) to model mass diffusion due to concentration gradients,
under which the diffusion flux can be written as
∇T
J~i = −ρDi,m ∇Yi − DT,i
T
(7.1-2)
Here Di,m is the mass diffusion coefficient for species i in the mixture, and DT,i is the
thermal (Soret) diffusion coefficient.
For certain laminar flows, the dilute approximation may not be acceptable, and full
multicomponent diffusion is required. In such cases, the Maxwell-Stefan equations can
be solved; see Section 8.9.2: Full Multicomponent Diffusion in the separate User’s Guide
for details.
7-2
Release 12.0 c ANSYS, Inc. January 29, 2009
7.1 Volumetric Reactions
Mass Diffusion in Turbulent Flows
In turbulent flows, ANSYS FLUENT computes the mass diffusion in the following form:
µt
∇T
J~i = − ρDi,m +
∇Yi − DT,i
Sct
T
(7.1-3)
µt
where Sct is the turbulent Schmidt number ( ρD
where µt is the turbulent viscosity
t
and Dt is the turbulent diffusivity). The default Sct is 0.7. Note that turbulent diffusion
generally overwhelms laminar diffusion, and the specification of detailed laminar diffusion
properties in turbulent flows is generally not necessary.
Treatment of Species Transport in the Energy Equation
For many multicomponent mixing flows, the transport of enthalpy due to species diffusion
"
∇·
n
X
#
hi J~i
i=1
can have a significant effect on the enthalpy field and should not be neglected. In particular, when the Lewis number
Lei =
k
ρcp Di,m
(7.1-4)
for any species is far from unity, neglecting this term can lead to significant errors.
ANSYS FLUENT will include this term by default. In Equation 7.1-4, k is the thermal
conductivity.
Diffusion at Inlets
For the pressure-based solver in ANSYS FLUENT, the net transport of species at inlets
consists of both convection and diffusion components. (For the density-based solvers,
only the convection component is included.) The convection component is fixed by the
inlet species mass fraction specified by you. The diffusion component, however, depends
on the gradient of the computed species field at the inlet. Thus the diffusion component
(and therefore the net inlet transport) is not specified a priori. For information about
specifying the net inlet transport of species, see Section 15.1.5: Defining Cell Zone and
Boundary Conditions for Species in the separate User’s Guide.
Release 12.0 c ANSYS, Inc. January 29, 2009
7-3
Species Transport and Finite-Rate Chemistry
7.1.2
The Generalized Finite-Rate Formulation for Reaction Modeling
The reaction rates that appear as source terms in Equation 7.1-1 are computed in ANSYS
FLUENT, for turbulent flows, by one of three models:
• Laminar finite-rate model: The effect of turbulent fluctuations are ignored, and
reaction rates are determined by Arrhenius kinetic expressions.
• Eddy-dissipation model: Reaction rates are assumed to be controlled by the turbulence, so expensive Arrhenius chemical kinetic calculations can be avoided. The
model is computationally cheap, but, for realistic results, only one or two step
heat-release mechanisms should be used.
• Eddy-dissipation-concept (EDC) model: Detailed Arrhenius chemical kinetics can
be incorporated in turbulent flames. Note that detailed chemical kinetic calculations are computationally expensive.
The generalized finite-rate formulation is suitable for a wide range of applications including laminar or turbulent reaction systems, and combustion systems with premixed,
non-premixed, or partially-premixed flames.
The Laminar Finite-Rate Model
The laminar finite-rate model computes the chemical source terms using Arrhenius expressions, and ignores the effects of turbulent fluctuations. The model is exact for laminar
flames, but is generally inaccurate for turbulent flames due to highly non-linear Arrhenius
chemical kinetics. The laminar model may, however, be acceptable for combustion with
relatively slow chemistry and small turbulence-chemistry interaction, such as supersonic
flames.
The net source of chemical species i due to reaction is computed as the sum of the
Arrhenius reaction sources over the NR reactions that the species participate in:
NR
X
Ri = Mw,i
R̂i,r
(7.1-5)
r=1
where Mw,i is the molecular weight of species i and R̂i,r is the Arrhenius molar rate of
creation/destruction of species i in reaction r. Reaction may occur in the continuous
phase at wall surfaces.
Consider the rth reaction written in general form as follows:
N
X
i=1
7-4
N
kf,r X
0
νi,r
Mi *
)
kb,r
00
νi,r
Mi
(7.1-6)
i=1
Release 12.0 c ANSYS, Inc. January 29, 2009
7.1 Volumetric Reactions
where
N
0
νi,r
00
νi,r
Mi
kf,r
kb,r
=
=
=
=
=
=
number of chemical species in the system
stoichiometric coefficient for reactant i in reaction r
stoichiometric coefficient for product i in reaction r
symbol denoting species i
forward rate constant for reaction r
backward rate constant for reaction r
Equation 7.1-6 is valid for both reversible and non-reversible reactions. (Reactions in ANSYS FLUENT are non-reversible by default.) For non-reversible reactions, the backward
rate constant, kb,r , is simply omitted.
The summations in Equation 7.1-6 are for all chemical species in the system, but only
species that appear as reactants or products will have non-zero stoichiometric coefficients.
Hence, species that are not involved will drop out of the equation.
For a non-reversible reaction (that is, the Include Backward Reaction button is disabled),
the molar rate of creation/destruction of species i in reaction r (R̂i,r in Equation 7.1-5)
is given by
R̂i,r = Γ
00
νi,r
−
0
νi,r
kf,r
N
Y
0 +η 00 )
(ηj,r
j,r
[Cj,r ]
(7.1-7)
j=1
where
Cj,r
0
ηj,r
00
ηj,r
= molar concentration of species j in reaction r (kgmol/m3 )
= rate exponent for reactant species j in reaction r
= rate exponent for product species j in reaction r
For a reversible reaction, the molar rate of creation/destruction of species i in reaction r
is given by
00
0
kf,r
R̂i,r = Γ νi,r
− νi,r
N
Y
[Cj,r ]
0
ηj,r
j=1
− kb,r
N
Y
00
νj,r
[Cj,r ]
(7.1-8)
j=1
Note that the rate exponent for the reverse reaction part in Equation 7.1-8 is always the
00
).
product species stoichiometric coefficient (νj,r
For information about inputting the stoichiometric coefficients and rate exponents for
both global forward (non-reversible) reactions and elementary (reversible) reactions, see
Section 15.1.3: Inputs for Reaction Definition in the separate User’s Guide.
Γ represents the net effect of third bodies on the reaction rate. This term is given by
Γ=
N
X
γj,r Cj
(7.1-9)
j
Release 12.0 c ANSYS, Inc. January 29, 2009
7-5
Species Transport and Finite-Rate Chemistry
where γj,r is the third-body efficiency of the jth species in the rth reaction. By default,
ANSYS FLUENT does not include third-body effects in the reaction rate calculation. You
can, however, opt to include the effect of third-body efficiencies if you have data for them.
The forward rate constant for reaction r, kf,r , is computed using the Arrhenius expression
kf,r = Ar T βr e−Er /RT
(7.1-10)
where
Ar
βr
Er
R
=
=
=
=
pre-exponential factor (consistent units)
temperature exponent (dimensionless)
activation energy for the reaction (J/kgmol)
universal gas constant (J/kgmol-K)
0
00
0
00
You (or the database) will provide values for νi,r
, νi,r
, ηj,r
, ηj,r
, βr , Ar , Er , and, optionally,
γj,r during the problem definition in ANSYS FLUENT.
If the reaction is reversible, the backward rate constant for reaction r, kb,r , is computed
from the forward rate constant using the following relation:
kb,r =
kf,r
Kr
(7.1-11)
where Kr is the equilibrium constant for the rth reaction, computed from
N
X
∆Sr0 ∆Hr0
Kr = exp
−
R
RT
!
patm
RT
00
0
(νi,r
− νi,r
)
i=1
(7.1-12)
where patm denotes atmospheric pressure (101325 Pa). The term within the exponential
function represents the change in Gibbs free energy, and its components are computed
as follows:
N
S0
∆Sr0 X
i
00
0
=
νi,r
− νi,r
R
R
i=1
(7.1-13)
N
h0
∆Hr0 X
i
00
0
=
νi,r − νi,r
RT
RT
i=1
(7.1-14)
where Si0 and h0i are the standard-state entropy and standard-state enthalpy (heat of
formation). These values are specified in ANSYS FLUENT as properties of the mixture
material.
7-6
Release 12.0 c ANSYS, Inc. January 29, 2009
7.1 Volumetric Reactions
Pressure-Dependent Reactions
ANSYS FLUENT can use one of three methods to represent the rate expression in pressuredependent (or pressure fall-off) reactions. A “fall-off” reaction is one in which the temperature and pressure are such that the reaction occurs between Arrhenius high-pressure
and low-pressure limits, and thus is no longer solely dependent on temperature.
There are three methods of representing the rate expressions in this fall-off region. The
simplest one is the Lindemann [198] form. There are also two other related methods, the
Troe method [111] and the SRI method [339], that provide a more accurate description
of the fall-off region.
Arrhenius rate parameters are required for both the high- and low-pressure limits. The
rate coefficients for these two limits are then blended to produce a smooth pressuredependent rate expression. In Arrhenius form, the parameters for the high-pressure limit
(k) and the low-pressure limit (klow ) are as follows:
k = AT β e−E/RT
klow = Alow T βlow e−Elow /RT
(7.1-15)
(7.1-16)
The net rate constant at any pressure is then taken to be
!
knet
pr
=k
F
1 + pr
(7.1-17)
klow [M ]
k
(7.1-18)
where pr is defined as
pr =
and [M ] is the concentration of the bath gas, which can include third-body efficiencies.
If the function F in Equation 7.1-17 is unity, then this is the Lindemann form. ANSYS
FLUENT provides two other forms to describe F , namely the Troe method and the SRI
method.
In the Troe method, F is given by
#2 −1
log pr + c
log Fcent
log F = 1 +
n − d(log pr + c)
Release 12.0 c ANSYS, Inc. January 29, 2009
"
(7.1-19)
7-7
Species Transport and Finite-Rate Chemistry
where
c = −0.4 − 0.67 log Fcent
n =
0.75 − 1.27 log Fcent
d =
0.14
(7.1-20)
(7.1-21)
(7.1-22)
Fcent = (1 − α)e−T /T1 + αe−T /T2 + e−T3 /T
(7.1-23)
and
The parameters α, T3 , T2 , and T1 are specified as inputs.
In the SRI method, the blending function F is approximated as
"
!
−b
−T
F = d a exp
+ exp
T
c
# X
Te
(7.1-24)
where
X=
1
1 + log2 pr
(7.1-25)
In addition to the three Arrhenius parameters for the low-pressure limit (klow ) expression,
you must also supply the parameters a, b, c, d, and e in the F expression.
i
Chemical kinetic mechanisms usually contain a wide range of time scales
and form a set of highly non-linear, stiff coupled equations. For solution
procedure guidelines, see Section 15.1.7: Solution Procedures for Chemical
Mixing and Finite-Rate Chemistry in the separate User’s Guide. Also,
if you have a chemical mechanism in CHEMKIN [161] format, you can
import this mechanism into ANSYS FLUENT (see Section 15.1.9: Importing
a Volumetric Kinetic Mechanism in CHEMKIN Format in the separate
User’s Guide).
The Eddy-Dissipation Model
Most fuels are fast burning, and the overall rate of reaction is controlled by turbulent
mixing. In non-premixed flames, turbulence slowly convects/mixes fuel and oxidizer into
the reaction zones where they burn quickly. In premixed flames, the turbulence slowly
convects/mixes cold reactants and hot products into the reaction zones, where reaction
7-8
Release 12.0 c ANSYS, Inc. January 29, 2009
7.1 Volumetric Reactions
occurs rapidly. In such cases, the combustion is said to be mixing-limited, and the
complex, and often unknown, chemical kinetic rates can be safely neglected.
ANSYS FLUENT provides a turbulence-chemistry interaction model, based on the work
of Magnussen and Hjertager [216], called the eddy-dissipation model. The net rate of
production of species i due to reaction r, Ri,r , is given by the smaller (i.e., limiting value)
of the two expressions below:
Ri,r =
0
νi,r
Mw,i Aρ
Ri,r =
where
YP
YR
A
B
is
is
is
is
YR
min 0
R
k
νR,r Mw,R
0
νi,r
Mw,i ABρ
k
!
(7.1-26)
P
P YP
00
j νj,r Mw,j
PN
(7.1-27)
the mass fraction of any product species, P
the mass fraction of a particular reactant, R
an empirical constant equal to 4.0
an empirical constant equal to 0.5
In Equations 7.1-26 and 7.1-27, the chemical reaction rate is governed by the large-eddy
mixing time scale, k/, as in the eddy-breakup model of Spalding [333]. Combustion
proceeds whenever turbulence is present (k/ > 0), and an ignition source is not required to initiate combustion. This is usually acceptable for non-premixed flames, but
in premixed flames, the reactants will burn as soon as they enter the computational
domain, upstream of the flame stabilizer. To remedy this, ANSYS FLUENT provides
the finite-rate/eddy-dissipation model, where both the Arrhenius (Equation 7.1-8), and
eddy-dissipation (Equations 7.1-26 and 7.1-27) reaction rates are calculated. The net
reaction rate is taken as the minimum of these two rates. In practice, the Arrhenius rate
acts as a kinetic “switch”, preventing reaction before the flame holder. Once the flame
is ignited, the eddy-dissipation rate is generally smaller than the Arrhenius rate, and
reactions are mixing-limited.
i
Although ANSYS FLUENT allows multi-step reaction mechanisms (number
of reactions > 2) with the eddy-dissipation and finite-rate/eddy-dissipation
models, these will likely produce incorrect solutions. The reason is that
multi-step chemical mechanisms are based on Arrhenius rates, which differ for each reaction. In the eddy-dissipation model, every reaction has
the same, turbulent rate, and therefore the model should be used only
for one-step (reactant → product), or two-step (reactant → intermediate, intermediate → product) global reactions. The model cannot predict
kinetically controlled species such as radicals. To incorporate multi-step
chemical kinetic mechanisms in turbulent flows, use the EDC model (described below).
Release 12.0 c ANSYS, Inc. January 29, 2009
7-9
Species Transport and Finite-Rate Chemistry
i
The eddy-dissipation model requires products to initiate reaction (see
Equation 7.1-27). When you initialize the solution for steady flows, ANSYS
FLUENT sets all species mass fractions to a maximum of the user specified initial value and 0.01. This is usually sufficient to start the reaction.
However, if you converge a mixing solution first, where all product mass
fractions are zero, you may then have to patch products into the reaction zone to ignite the flame. For details, see Section 15.1.7: Ignition in
Combustion Simulations in the separate User’s Guide.
The Eddy-Dissipation Model for LES
When the LES turbulence model is used, the turbulent mixing rate, /k in Equations 7.1-26 and 7.1-27, is replaced by the subgrid-scale mixing rate. This is calculated
as
−1
τsgs
=
q
2Sij Sij
(7.1-28)
where
−1
τsgs
Sij
−1
= subgrid-scale
mixing rate (s )
∂ui
j
= 21 ∂x
+ ∂u
= strain rate tensor (s−1 )
∂xi
j
The Eddy-Dissipation-Concept (EDC) Model
The eddy-dissipation-concept (EDC) model is an extension of the eddy-dissipation model
to include detailed chemical mechanisms in turbulent flows [215]. It assumes that reaction
occurs in small turbulent structures, called the fine scales. The length fraction of the fine
scales is modeled as [115]
∗
ξ = Cξ
where
Cξ
ν
∗
ν
k2
1/4
(7.1-29)
denotes fine-scale quantities and
=
=
volume fraction constant = 2.1377
kinematic viscosity
The volume fraction of the fine scales is calculated as ξ ∗ 3 . Species are assumed to react
in the fine structures over a time scale
∗
τ = Cτ
1/2
ν
(7.1-30)
where Cτ is a time scale constant equal to 0.4082.
7-10
Release 12.0 c ANSYS, Inc. January 29, 2009
7.2 Wall Surface Reactions and Chemical Vapor Deposition
In ANSYS FLUENT, combustion at the fine scales is assumed to occur as a constant
pressure reactor, with initial conditions taken as the current species and temperature in
the cell. Reactions proceed over the time scale τ ∗ , governed by the Arrhenius rates of
Equation 7.1-8, and are integrated numerically using the ISAT algorithm [277]. ISAT
can accelerate the chemistry calculations by two to three orders of magnitude, offering
substantial reductions in run-times. Details about the ISAT algorithm may be found
in Sections 11.3.3 and 11.3.4. ISAT is very powerful, but requires some care. See Section 19.6.2: Using ISAT Efficiently in the separate User’s Guide for details on using ISAT
efficiently.
The source term in the conservation equation for the mean species i, Equation 7.1-1, is
modeled as
ρ(ξ ∗ )2
Ri = ∗
(Yi∗ − Yi )
τ [1 − (ξ ∗ )3 ]
(7.1-31)
where Yi∗ is the fine-scale species mass fraction after reacting over the time τ ∗ .
The EDC model can incorporate detailed chemical mechanisms into turbulent reacting
flows. However, typical mechanisms are invariably stiff and their numerical integration
is computationally costly. Hence, the model should be used only when the assumption
of fast chemistry is invalid, such as modeling the slow CO burnout in rapidly quenched
flames, or the NO conversion in selective non-catalytic reduction (SNCR).
For guidelines on obtaining a solution using the EDC model, see Section 15.1.7: Solution
of Stiff Laminar Chemistry Systems in the separate User’s Guide.
7.2
Wall Surface Reactions and Chemical Vapor Deposition
For gas-phase reactions, the reaction rate is defined on a volumetric basis and the rate
of creation and destruction of chemical species becomes a source term in the species
conservation equations. For surface reactions, the rate of adsorption and desorption is
governed by both chemical kinetics and diffusion to and from the surface. Wall surface
reactions thus create sources and sinks of chemical species in the gas phase, as well as on
the reacting surface.
Theoretical information about wall surface reactions and chemical vapor deposition is
presented in this section. Information can be found in the following sections:
• Section 7.2.1: Surface Coverage Reaction Rate Modification
• Section 7.2.2: Reaction-Diffusion Balance for Surface Chemistry
• Section 7.2.3: Slip Boundary Formulation for Low-Pressure Gas Systems
Release 12.0 c ANSYS, Inc. January 29, 2009
7-11
Species Transport and Finite-Rate Chemistry
For more information about using wall surface reactions and chemical vapor deposition,
see Section 15.2: Wall Surface Reactions and Chemical Vapor Deposition in the separate
User’s Guide.
Consider the rth wall surface reaction written in general form as follows:
Ng
X
i=1
0
gi,r
Gi
+
Nb
X
b0i,r Bi
+
i=1
Ns
X
Kr
s0i,r Si *
)
i=1
Ng
X
00
gi,r
Gi +
i=1
Nb
X
b00i,r Bi +
i=1
Ns
X
s00i,r Si
(7.2-1)
i=1
where Gi , Bi , and Si represent the gas phase species, the bulk (or solid) species, and the
surface-adsorbed (or site) species, respectively. Ng , Nb , and Ns are the total numbers of
0
these species. gi,r
, b0i,r , and s0i,r are the stoichiometric coefficients for each reactant species
00
i, and gi,r
, b00i,r , and s00i,r are the stoichiometric coefficients for each product species i. Kr
is the overall forward reaction rate constant. Note that ANSYS FLUENT cannot model
reversible surface reactions.
The summations in Equation 7.2-1 are for all chemical species in the system, but only
species involved as reactants or products will have non-zero stoichiometric coefficients.
Hence, species that are not involved will drop out of the equation.
The rate of the rth reaction is
Rr =
Ng
Y
Ns
0
0
Y
ηi,g,r
ηj,s,r
kf,r [Ci ]wall
[Sj ]wall
j=1
i=1
(7.2-2)
0
where [ ]wall represents molar concentrations of surface-adsorbed species on the wall. ηi,g,r
th
0
is the rate exponent for the i gaseous species as reactant in the reaction and ηj,s,r is the
rate exponent for the j th site species as reactant in the reaction. It is assumed that the
reaction rate does not depend on concentrations of the bulk (solid) species. From this,
the net molar rate of production or consumption of each species i is given by
R̂i,gas =
R̂i,bulk =
R̂i,site =
N
rxn
X
r=1
N
rxn
X
r=1
N
rxn
X
0
00
(gi,r
− gi,r
)Rr
i = 1, 2, 3, . . . , Ng
(7.2-3)
(b00i,r − b0i,r )Rr
i = 1, 2, 3, . . . , Nb
(7.2-4)
(s00i,r − s0i,r )Rr
i = 1, 2, 3, . . . , Ns
(7.2-5)
r=1
The forward rate constant for reaction r (kf,r ) is computed using the Arrhenius expression,
7-12
Release 12.0 c ANSYS, Inc. January 29, 2009
7.2 Wall Surface Reactions and Chemical Vapor Deposition
kf,r = Ar T βr e−Er /RT
where
Ar
βr
Er
R
=
=
=
=
(7.2-6)
pre-exponential factor (consistent units)
temperature exponent (dimensionless)
activation energy for the reaction (J/kgmol)
universal gas constant (J/kgmol-K)
0
00
You (or the database) will provide values for gi,r
, gi,r
, b0i,r , b00i,r , s0i,r , s00i,r , βr , Ar , and Er .
To include the mass transfer effects and model heat release, refer to Section 15.2.3: Including Mass Transfer To Surfaces in Continuity, Section 15.2.4: Wall Surface Mass Transfer
Effects in the Energy Equation, and Section 15.2.5: Modeling the Heat Release Due to
Wall Surface Reactions in the separate User’s Guide
7.2.1
Surface Coverage Reaction Rate Modification
ANSYS FLUENT has the option to modify the surface reaction rate as a function of
species site coverages. In such cases, the forward rate constant for the rth reaction is
evaluated as,
kf,r = Ar T βr e−Er /RT
Y
10Zk ηk,r (Zk µk,r ) e−k,r Zk /RT
(7.2-7)
ksite
In Equation 7.2-7, the three surface coverage rate modification parameters for specie k in
reaction r are ηk,r , µk,r and k,r . These parameters default to zero for reaction species that
are not surface rate modifying. The surface (coverage) site fraction, Zk is the fraction of
surface sites covered by specie k, and is defined as,
Zk = [Sk ]/ρsite
(7.2-8)
where [Sk ] is the surface site concentration and ρsite is the surface site density (see Equation 7.2-13).
Release 12.0 c ANSYS, Inc. January 29, 2009
7-13
Species Transport and Finite-Rate Chemistry
7.2.2
Reaction-Diffusion Balance for Surface Chemistry
Reactions at surfaces change gas-phase, surface-adsorbed (site) and bulk (solid) species.
On reacting surfaces, the mass flux of each gas specie due to diffusion and convection
to/from the surface is balanced with its rate of consumption/production on the surface,
ρwall Di
∂Yi,wall
− ṁdep Yi,wall = Mw,i R̂i,gas
∂n
∂ [Si ]wall
= R̂i,site
∂t
i = 1, 2, 3, . . . , Ng
(7.2-9)
i = 1, 2, 3, . . . , Ns
(7.2-10)
The wall mass fraction Yi,wall is related to concentration by
[Gi ]wall =
ρwall Yi,wall
Mw,i
(7.2-11)
ṁdep is the net rate of mass deposition or etching as a result of surface reaction; i.e.,
ṁdep =
Nb
X
Mw,i R̂i,bulk
(7.2-12)
i=1
[Si ]wall is the site species concentration at the wall, and is defined as
[Si ]wall = ρsite Zi
(7.2-13)
where ρsite is the site density and Zi is the site coverage of species i.
Equations 7.2-9 and 7.2-10 are solved for the dependent variables Yi,wall and Zi using a
point-by-point coupled Newton solver. The effective gas-phase reaction source terms are
then available for solution of the gas-phase species transport Equation 7.1-1.
7-14
Release 12.0 c ANSYS, Inc. January 29, 2009
7.2 Wall Surface Reactions and Chemical Vapor Deposition
7.2.3
Slip Boundary Formulation for Low-Pressure Gas Systems
Most semiconductor fabrication devices operate far below atmospheric pressure, typically
only a few millitorrs. At such low pressures, the fluid flow is in the slip regime and the
normally used no-slip boundary conditions for velocity and temperature are no longer
valid.
The Knudsen number, denoted Kn, and defined as the ratio of mean free path to a
characteristic length scale of the system, is used to quantify continuum flow regimes.
Since the mean free path increases as the pressure is lowered, the high end of Kn values
represents free molecular flow and the low end the continuum regime. The range in
between these two extremes is called the slip regime (0.01 < Kn < 0.1) [28] In the slip
regime, the gas-phase velocity at a solid surface differs from the velocity at which the
wall moves, and the gas temperature at the surface differs from the wall temperature.
Maxwell’s models are adopted for these physical phenomena in ANSYS FLUENT for their
simplicity and effectiveness.
• velocity slip
2 − αv
∂U
2 − αv
Uw − Ug =
Kn
≈
αv
∂n
αv
Vg ≡ (V~ · ~n)g = Vw
λ
(Ug − Uc )
δ
(7.2-14)
(7.2-15)
Here, U and V represents the velocity component that is parallel and normal to
the wall, respectively. The subscripts g, w and c indicate gas, wall and cell-center
velocities. δ is the distance from cell center to the wall. αv is the momentum
accommodation coefficient of the gas mixture and its value is calculated as massfraction weighted average of each gas species in the system.
αv =
Ng
X
Yi αi
(7.2-16)
i=1
The mean free path, λ, is computed as follows:
kB T
λ = √
2πσ 2 p
σ =
Ng
X
Yi σi
(7.2-17)
(7.2-18)
i=1
σi is the Lennard-Jones characteristic length of species i. kB is the Boltzmann
constant, 1.38066 × 10−23 J/K.
Release 12.0 c ANSYS, Inc. January 29, 2009
7-15
Species Transport and Finite-Rate Chemistry
Equations 7.2-14 and 7.2-15 indicate that while the gas velocity component normal
to the wall is the same as the wall normal velocity, the tangential components slip.
The values lie somewhere between the cell-center and the wall values. These two
equations can be combined to give a generalized formulation:
V~w + kδ [(V~w · ~n)~n + V~c − (V~c · ~n)~n]
~
Vg =
1 + kδ
(7.2-19)
where
2 − αv
k≡λ
αv
(7.2-20)
• temperature jump
2 − αT
Tw − Tg = 2
αT
∂T
2 − αT
Kn
≈2
∂n
αT
λ
(Tg − Tc )
δ
(7.2-21)
or equivalently
Tg =
Tw + βTc
1+β
(7.2-22)
β=
2(2 − αT )
αT δ
(7.2-23)
where
αT is the thermal accommodation coefficient of the gas mixture and is calculated
P
as αT = Yi αT,i .
i
7-16
The low-pressure slip boundary formulation is available only with the
pressure-based solver.
Release 12.0 c ANSYS, Inc. January 29, 2009
7.3 Particle Surface Reactions
7.3
Particle Surface Reactions
As described in Section 15.4.5: The Multiple Surface Reactions Model, it is possible to
define multiple particle surface reactions to model the surface combustion of a combusting discrete-phase particle. This section provides theoretical background about particle
surface reactions. Information can be found in the following sections:
• Section 7.3.1: General Description
• Section 7.3.2: ANSYS FLUENT Model Formulation
• Section 7.3.3: Extension for Stoichiometries with Multiple Gas Phase Reactants
• Section 7.3.4: Solid-Solid Reactions
• Section 7.3.5: Solid Decomposition Reactions
• Section 7.3.6: Solid Deposition Reactions
• Section 7.3.7: Gaseous Solid Catalyzed Reactions on the Particle Surface
For more information about using particle surface reactions, see Section 15.3: Particle
Surface Reactions in the separate User’s Guide.
7.3.1
General Description
The relationships for calculating char particle burning rates are presented and discussed
in detail by Smith [324]. The particle reaction rate, R (kg/m2 -s), can be expressed as
R = D0 (Cg − Cs ) = Rc (Cs )N
(7.3-1)
where
D0
Cg
Cs
Rc
N
=
=
=
=
=
bulk diffusion coefficient (m/s)
mean reacting gas species concentration in the bulk (kg/m3 )
mean reacting gas species concentration at the particle surface (kg/m3 )
chemical reaction rate coefficient (units vary)
apparent reaction order (dimensionless)
In Equation 7.3-1, the concentration at the particle surface, Cs , is not known, so it should
be eliminated, and the expression is recast as follows:
R
R = Rc Cg −
D0
Release 12.0 c ANSYS, Inc. January 29, 2009
N
(7.3-2)
7-17
Species Transport and Finite-Rate Chemistry
This equation has to be solved by an iterative procedure, with the exception of the cases
when N = 1 or N = 0. When N = 1, Equation 7.3-2 can be written as
R=
Cg Rc D0
D0 + R c
(7.3-3)
In the case of N = 0, if there is a finite concentration of reactant at the particle surface,
the solid depletion rate is equal to the chemical reaction rate. If there is no reactant
at the surface, the solid depletion rate changes abruptly to the diffusion-controlled rate.
In this case, however, ANSYS FLUENT will always use the chemical reaction rate for
stability reasons.
7.3.2 ANSYS FLUENT Model Formulation
A particle undergoing an exothermic reaction in the gas phase is shown schematically in
Figure 7.3.1. Tp and T∞ are the temperatures in Equation 15.4-78.
Cd,b
Tp
Ck
T∞
Temperature
Concentration
Cd,s
Distance
Figure 7.3.1: A Reacting Particle in the Multiple Surface Reactions Model
Based on the analysis above, ANSYS FLUENT uses the following equation to describe
the rate of reaction r of a particle surface species j with the gas phase species n. The
reaction stoichiometry of reaction r in this case is described by
particle species j(s) + gas phase species n → products
and the rate of reaction is given as
Rj,r = Ap ηr Yj Rj,r
7-18
(7.3-4)
Release 12.0 c ANSYS, Inc. January 29, 2009
7.3 Particle Surface Reactions
Rj,r = Rkin,r
Rj,r
pn −
D0,r
!N
(7.3-5)
where
Rj,r
Ap
Yj
ηr
Rj,r
pn
D0,r
Rkin,r
Nr
=
=
=
=
=
=
=
=
=
rate of particle surface species depletion (kg/s)
particle surface area (m2 )
mass fraction of surface species j in the particle
effectiveness factor (dimensionless)
rate of particle surface species reaction per unit area (kg/m2 -s)
bulk partial pressure of the gas phase species (Pa)
diffusion rate coefficient for reaction r
kinetic rate of reaction r (units vary)
apparent order of reaction r
The effectiveness factor, ηr , is related to the surface area, and can be used in each reaction
in the case of multiple reactions. D0,r is given by
D0,r = C1,r
[(Tp + T∞ )/2]0.75
dp
(7.3-6)
The kinetic rate of reaction r is defined as
Rkin,r = Ar Tp βr e−(Er /RTp )
(7.3-7)
The rate of the particle surface species depletion for reaction order Nr = 1 is given by
Rj,r = Ap ηr Yj pn
Rkin,r D0,r
D0,r + Rkin,r
(7.3-8)
For reaction order Nr = 0,
Rj,r = Ap ηr Yj Rkin,r
Release 12.0 c ANSYS, Inc. January 29, 2009
(7.3-9)
7-19
Species Transport and Finite-Rate Chemistry
7.3.3
Extension for Stoichiometries with Multiple Gas Phase Reactants
When more than one gas phase reactant takes part in the reaction, the reaction stoichiometry must be extended to account for this case:
particle species j(s) + gas phase species 1 + gas phase species 2 + . . .
+ gas phase species nmax → products
To describe the rate of reaction r of a particle surface species j in the presence of nmax
gas phase species n, it is necessary to define the diffusion-limited species for each solid
particle reaction, i.e., the species for which the concentration gradient between the bulk
and the particle surface is the largest. For the rest of the species, the surface and the
bulk concentrations are assumed to be equal. The concentration of the diffusion-limited
species is shown as Cd,b and Cd,s in Figure 7.3.1, and the concentrations of all other
species are denoted as Ck . For stoichiometries with multiple gas phase reactants, the
bulk partial pressure pn in Equations 7.3-4 and 7.3-8 is the bulk partial pressure of the
diffusion-limited species, pr,d for reaction r.
The kinetic rate of reaction r is then defined as
Rkin,r =
max
Ar T βr e−(Er /RT ) nY
r,n
pN
n
(pr,d )Nr,d
n=1
(7.3-10)
where
pn
Nr,n
= bulk partial pressure of gas species n
= reaction order in species n
When this model is enabled, the constant C1,r (Equation 7.3-6) and the effectiveness
factor ηr (Equation 7.3-4) are entered in the Reactions dialog box (see Section 15.3.1: User
Inputs for Particle Surface Reactions in the separate User’s Guide).
7.3.4
Solid-Solid Reactions
Reactions involving only particle surface reactants can be modeled, provided that the
particle surface reactants and products exist on the same particle.
particle species 1(s) + particle species 2(s) + . . . → products
The reaction rate for this case is given by Equation 7.3-9.
7-20
Release 12.0 c ANSYS, Inc. January 29, 2009
7.3 Particle Surface Reactions
7.3.5
Solid Decomposition Reactions
The decomposition reactions of particle surface species can be modeled.
particle species 1(s) + particle species 2(s) + . . . + particle species nmax (s) →
gas species j + products
The reaction rate for this case is given by Equations 7.3-4–7.3-10, where the diffusionlimited species is now the gaseous product of the reaction. If there are more than one
gaseous product species in the reaction, it is necessary to define the diffusion-limited
species for the particle reaction as the species for which the concentration gradient between the bulk and the particle surface is the largest.
7.3.6
Solid Deposition Reactions
The deposition reaction of a solid species on a particle can be modeled with the following
assumptions:
gas species 1 + gas species 2 + . . . + gas species nmax → solid species j(s) + products
The theoretical analysis and Equations 7.3-4–7.3-10 are applied for the surface reaction
rate calculation, with the mass fraction of the surface species set to unity in Equations 7.3-4, 7.3-8, and 7.3-9.
In ANSYS FLUENT, for the particle surface species to be deposited on a particle, a finite
mass of the species must already exist in the particle. This allows for activation of the
deposition reaction selectively to particular injection particles. It follows that, to initiate
the solid species deposition reaction on a particle, the particle must be defined in the
Set Injection Properties dialog box (or Set Multiple Injection Properties dialog
box) to contain a small mass fraction of the solid species to be deposited. For details on
defining the particle surface species mass fractions, see Section 15.3.3: Using the Multiple
Surface Reactions Model for Discrete-Phase Particle Combustion in the separate User’s
Guide.
7.3.7
Gaseous Solid Catalyzed Reactions on the Particle Surface
Reactions of gaseous species catalyzed on the particle surface can also be modeled following Equations 7.3-4–7.3-10 for the surface reaction rate calculation, with the mass
fraction of the surface species set to unity in Equations 7.3-4, 7.3-8, and 7.3-9. To apply
this type of reaction, see Section 15.3.2: Modeling Gaseous Solid Catalyzed Reactions in
the separate User’s Guide. For details on defining the particle surface species mass fractions, see Section 15.3.3: Using the Multiple Surface Reactions Model for Discrete-Phase
Particle Combustion in the separate User’s Guide.
Release 12.0 c ANSYS, Inc. January 29, 2009
7-21
Species Transport and Finite-Rate Chemistry
7-22
Release 12.0 c ANSYS, Inc. January 29, 2009
Chapter 8.
Non-Premixed Combustion
In non-premixed combustion, fuel and oxidizer enter the reaction zone in distinct streams.
This is in contrast to premixed systems, in which reactants are mixed at the molecular
level before burning. Examples of non-premixed combustion include pulverized coal
furnaces, diesel internal-combustion engines and pool fires.
Under certain assumptions, the thermochemistry can be reduced to a single parameter:
the mixture fraction. The mixture fraction, denoted by f , is the mass fraction that
originated from the fuel stream. In other words, it is the local mass fraction of burnt
and unburnt fuel stream elements (C, H, etc.) in all the species (CO2 , H2 O, O2 , etc.).
The approach is elegant because atomic elements are conserved in chemical reactions.
In turn, the mixture fraction is a conserved scalar quantity, and therefore its governing
transport equation does not have a source term. Combustion is simplified to a mixing
problem, and the difficulties associated with closing non-linear mean reaction rates are
avoided. Once mixed, the chemistry can be modeled as being in chemical equilibrium
with the Equilibrium model, being near chemical equilibrium with the Steady Laminar
Flamelet model, or significantly departing from chemical equilibrium with the Unsteady
Laminar Flamelet model.
For more information about using the non-premixed combustion model, see Chapter 16: Modeling Non-Premixed Combustion in the separate User’s Guide. Theoretical information
about the non-premixed combustion model is presented in the following sections:
• Section 8.1: Introduction
• Section 8.2: Non-Premixed Combustion and Mixture Fraction Theory
• Section 8.3: Restrictions and Special Cases for Using the Non-Premixed Model
• Section 8.4: The Laminar Flamelet Models Theory
• Section 8.5: The Steady Laminar Flamelet Model Theory
• Section 8.6: The Unsteady Laminar Flamelet Model Theory
Release 12.0 c ANSYS, Inc. January 29, 2009
8-1
Non-Premixed Combustion
8.1
Introduction
Non-premixed modeling involves the solution of transport equations for one or two conserved scalars (the mixture fractions). Equations for individual species are not solved.
Instead, species concentrations are derived from the predicted mixture fraction fields. The
thermochemistry calculations are preprocessed and then tabulated for look-up in ANSYS
FLUENT. Interaction of turbulence and chemistry is accounted for with an assumed-shape
Probability Density Function (PDF).
8.2
Non-Premixed Combustion and Mixture Fraction Theory
Information about non-premixed combustion and mixture fraction theory are presented
in the following sections:
• Section 8.2.1: Mixture Fraction Theory
• Section 8.2.2: Modeling of Turbulence-Chemistry Interaction
• Section 8.2.3: Non-Adiabatic Extensions of the Non-Premixed Model
• Section 8.2.4: Chemistry Tabulation
8.2.1
Mixture Fraction Theory
Definition of the Mixture Fraction
The basis of the non-premixed modeling approach is that under a certain set of simplifying
assumptions, the instantaneous thermochemical state of the fluid is related to a conserved
scalar quantity known as the mixture fraction, f . The mixture fraction can be written
in terms of the atomic mass fraction as [319]
f=
Zi − Zi,ox
Zi,fuel − Zi,ox
(8.2-1)
where Zi is the elemental mass fraction for element, i. The subscript ox denotes the value
at the oxidizer stream inlet and the subscript fuel denotes the value at the fuel stream
inlet. If the diffusion coefficients for all species are equal, then Equation 8.2-1 is identical
for all elements, and the mixture fraction definition is unique. The mixture fraction is
thus the elemental mass fraction that originated from the fuel stream.
8-2
Release 12.0 c ANSYS, Inc. January 29, 2009
8.2 Non-Premixed Combustion and Mixture Fraction Theory
If a secondary stream (another fuel or oxidant, or a non-reacting stream) is included,
the fuel and secondary mixture fractions are simply the elemental mass fractions of the
fuel and secondary streams, respectively. The sum of all three mixture fractions in the
system (fuel, secondary stream, and oxidizer) is always equal to 1:
ffuel + fsec + fox = 1
(8.2-2)
This indicates that only points on the plane ABC (shown in Figure 8.2.1) in the mixture
fraction space are valid. Consequently, the two mixture fractions, ffuel and fsec , cannot
vary independently; their values are valid only if they are both within the triangle OBC
shown in Figure 8.2.1.
fox
1
fsec
A
1
C
O
0
B
1
ffuel
Figure 8.2.1: Relationship of ffuel , fsec , and fox
ANSYS FLUENT discretizes the triangle OBC as shown in Figure 8.2.2. Essentially, the
primary mixture fraction, ffuel , is allowed to vary between zero and one, as for the single
mixture fraction case, while the secondary mixture fraction lies on lines with the following
equation:
fsec = psec × (1 − ffuel )
(8.2-3)
where psec is the normalized secondary mixture fraction and is the value at the intersection
of a line with the secondary mixture fraction axis. Note that unlike fsec , psec is bounded
between zero and one, regardless of the ffuel value.
Release 12.0 c ANSYS, Inc. January 29, 2009
8-3
Non-Premixed Combustion
C
1
p
sec
f sec
B
O
0
f fuel
1
Figure 8.2.2: Relationship of ffuel , fsec , and psec
8-4
Release 12.0 c ANSYS, Inc. January 29, 2009
8.2 Non-Premixed Combustion and Mixture Fraction Theory
An important characteristic of the normalized secondary mixture fraction, psec , is its
assumed statistical independence from the fuel mixture fraction, ffuel . Note that unlike
fsec , psec is not a conserved scalar. This normalized mixture fraction definition, psec ,
is used everywhere in ANSYS FLUENT when prompted for Secondary Mixture Fraction
except when defining the rich limit for a secondary fuel stream, which is defined in terms
of fsec .
Transport Equations for the Mixture Fraction
Under the assumption of equal diffusivities, the species equations can be reduced to a
single equation for the mixture fraction, f . The reaction source terms in the species
equations cancel (since elements are conserved in chemical reactions), and thus f is a
conserved quantity. While the assumption of equal diffusivities is problematic for laminar
flows, it is generally acceptable for turbulent flows where turbulent convection overwhelms
molecular diffusion. The Favre mean (density-averaged) mixture fraction equation is
µt
∂
∇f + Sm + Suser
(ρf ) + ∇ · (ρ~v f ) = ∇ ·
σt
∂t
(8.2-4)
The source term Sm is due solely to transfer of mass into the gas phase from liquid fuel
droplets or reacting particles (e.g., coal). Suser is any user-defined source term.
In addition to solving for the Favre mean mixture fraction, ANSYS FLUENT solves a
conservation equation for the mixture fraction variance, f 0 2 [152]:
2
∂ 02
µt
ρf + ∇ · ρ~v f 0 2 = ∇ ·
∇f 0 2 + Cg µt ∇f − Cd ρ f 0 2 + Suser
∂t
σt
k
(8.2-5)
where f 0 = f − f . The default values for the constants σt , Cg , and Cd are 0.85, 2.86, and
2.0, respectively, and Suser is any user-defined source term.
The mixture fraction variance is used in the closure model describing turbulence-chemistry
interactions (see Section 8.2.2: Modeling of Turbulence-Chemistry Interaction).
0
2
For a two-mixture-fraction problem, ffuel and ffuel
are obtained from Equations 8.2-4 and
02
02
8.2-5 by substituting ffuel for f and ffuel for f . fsec is obtained from Equation 8.2-4 by
2 is obtained
substituting fsec for f . psec is then calculated using Equation 8.2-3, and p0sec
by solving Equation 8.2-5 with psec substituted for f . To a first-order approximation, the
variances in psec and fsec are relatively insensitive to ffuel , and therefore the equation for
2 is essentially the same as f 0 2 .
p0sec
sec
i
2 instead of f 0 2 is valid when the mass flow rate of
The equation for p0sec
sec
the secondary stream is relatively small compared with the total mass flow
rate.
Release 12.0 c ANSYS, Inc. January 29, 2009
8-5
Non-Premixed Combustion
The Non-Premixed Model for LES
For Large Eddy Simulations, ransport equation is not solved for the mixture fraction
variance. Instead, it is modeled as
2
f 0 2 = Cvar L2s |∇f |
(8.2-6)
where
Cvar
Ls
=
=
constant
subgrid length scale (see Equation 4.11-16)
The constant Cvar is computed dynamically when the Dynamic Stress option is enabled
in the Viscous dialog box, else a constant value (with a default of 0.5) is used.
If the Dynamic Scalar Flux option is enabled, the turbulent Sc (σt in Equation 8.2-4) is
computed dynamically.
Mixture Fraction vs. Equivalence Ratio
The mixture fraction definition can be understood in relation to common measures of
reacting systems. Consider a simple combustion system involving a fuel stream (F), an
oxidant stream (O), and a product stream (P) symbolically represented at stoichiometric
conditions as
F + r O → (1 + r) P
(8.2-7)
where r is the air-to-fuel ratio on a mass basis. Denoting the equivalence ratio as φ,
where
φ=
(fuel/air)actual
(fuel/air)stoichiometric
(8.2-8)
the reaction in Equation 8.2-7, under more general mixture conditions, can then be
written as
φ F + r O → (φ + r) P
(8.2-9)
Looking at the left side of this equation, the mixture fraction for the system as a whole
can then be deduced to be
f=
8-6
φ
φ+r
(8.2-10)
Release 12.0 c ANSYS, Inc. January 29, 2009
8.2 Non-Premixed Combustion and Mixture Fraction Theory
Equation 8.2-10 allows the computation of the mixture fraction at stoichiometric conditions (φ = 1) or at fuel-rich conditions (e.g., φ > 1), or fuel-lean conditions (e.g.,
φ < 1).
Relationship of f to Species Mass Fraction, Density, and Temperature
The power of the mixture fraction modeling approach is that the chemistry is reduced to
one or two conserved mixture fractions. Under the assumption of chemical equilibrium,
all thermochemical scalars (species fractions, density, and temperature) are uniquely
related to the mixture fraction(s).
For a single mixture fraction in an adiabatic system, the instantaneous values of mass
fractions, density, and temperature depend solely on the instantaneous mixture fraction,
f:
φi = φi (f )
(8.2-11)
If a secondary stream is included, the instantaneous values will depend on the instantaneous fuel mixture fraction, ffuel , and the secondary partial fraction, psec :
φi = φi (ffuel , psec )
(8.2-12)
In Equations 8.2-11 and 8.2-12, φi represents the instantaneous species mass fraction,
density, or temperature. In the case of non-adiabatic systems, the effect of heat loss/gain
is parameterized as
φi = φi (f, H)
(8.2-13)
for a single mixture fraction system, where H is the instantaneous enthalpy (see Equation 5.2-7).
If a secondary stream is included,
φi = φi (ffuel , psec , H)
(8.2-14)
Examples of non-adiabatic flows include systems with radiation, heat transfer through
walls, heat transfer to/from discrete phase particles or droplets, and multiple inlets at
different temperatures. Additional detail about the mixture fraction approach in such
non-adiabatic systems is provided in Section 8.2.3: Non-Adiabatic Extensions of the NonPremixed Model.
In many reacting systems, the combustion is not in chemical equilibrium. ANSYS FLUENT offers several approaches to model chemical non-equilibrium, including the finiterate (see Section 7.1.2: The Generalized Finite-Rate Formulation for Reaction Modeling),
Release 12.0 c ANSYS, Inc. January 29, 2009
8-7
Non-Premixed Combustion
EDC (see Section 7.1.2: The Eddy-Dissipation-Concept (EDC) Model), and PDF transport (see Chapter 11: Composition PDF Transport) models, where detailed kinetic mechanisms can be incorporated.
There are three approaches in the non-premixed combustion model to simulate chemical
non-equilibrium. The first is to use the Rich Flammability Limit (RFL) option in the
Equilibrium model, where rich regions are modeled as a mixed-but-unburnt mixture of
pure fuel and a leaner equilibrium burnt mixture (see Section 16.2.5: Enabling the Rich
Flammability Limit (RFL) Option in the separate User’s Guide). The second approach
is the Steady Laminar Flamelet model, where chemical non-equilibrium due to diffusion
flame stretching by turbulence can be modeled. The third approach is the Unsteady
Laminar Flamelet model where slow-forming product species that are far from chemical
equilibrium can be modeled. See Sections 8.4 and 8.6 for details about the Steady and
Unsteady Laminar Flamelet models in ANSYS FLUENT.
8.2.2
Modeling of Turbulence-Chemistry Interaction
Equations 8.2-11 through 8.2-14 describe the instantaneous relationships between mixture
fraction and species fractions, density, and temperature under the assumption of chemical
equilibrium. The ANSYS FLUENT prediction of the turbulent reacting flow, however,
is concerned with prediction of the averaged values of these fluctuating scalars. How
these averaged values are related to the instantaneous values depends on the turbulencechemistry interaction model. ANSYS FLUENT applies the assumed-shape probability
density function (PDF) approach as its closure model when the non-premixed model is
used. The assumed shape PDF closure model is described in this section.
Description of the Probability Density Function
The Probability Density Function, written as p(f ), can be thought of as the fraction of
time that the fluid spends in the vicinity of the state f . Figure 8.2.3 plots the time trace
of mixture fraction at a point in the flow (right-hand side) and the probability density
function of f (left-hand side). The fluctuating value of f , plotted on the right side of the
figure, spends some fraction of time in the range denoted as ∆f . p(f ), plotted on the left
side of the figure, takes on values such that the area under its curve in the band denoted,
∆f , is equal to the fraction of time that f spends in this range. Written mathematically,
1X
τi
T →∞ T
i
p(f ) ∆f = lim
(8.2-15)
where T is the time scale and τi is the amount of time that f spends in the ∆f band. The
shape of the function p(f ) depends on the nature of the turbulent fluctuations in f . In
practice, p(f ) is unknown and is modeled as a mathematical function that approximates
the actual PDF shapes that have been observed experimentally.
8-8
Release 12.0 c ANSYS, Inc. January 29, 2009
8.2 Non-Premixed Combustion and Mixture Fraction Theory
Figure 8.2.3: Graphical Description of the Probability Density Function,
p(f )
Derivation of Mean Scalar Values from the Instantaneous Mixture Fraction
The probability density function p(f ), describing the temporal fluctuations of f in the
turbulent flow, can be used to compute averaged values of variables that depend on
f . Density-weighted mean species mass fractions and temperature can be computed (in
adiabatic systems) as
φi =
Z
0
1
p(f )φi (f )df
(8.2-16)
for a single-mixture-fraction system. When a secondary stream exists, mean values are
calculated as
φi =
Z
1
Z
0
0
1
p1 (ffuel )p2 (psec )φi (ffuel , psec )dffuel dpsec
(8.2-17)
where p1 is the PDF of ffuel and p2 is the PDF of psec . Here, statistical independence of
ffuel and psec is assumed, so that p(ffuel , psec ) = p1 (ffuel )p2 (psec ).
Release 12.0 c ANSYS, Inc. January 29, 2009
8-9
Non-Premixed Combustion
Similarly, the mean time-averaged fluid density, ρ, can be computed as
1 Z 1 p(f )
=
df
ρ
0 ρ(f )
(8.2-18)
for a single-mixture-fraction system, and
1 Z 1 Z 1 p1 (ffuel )p2 (psec )
dffuel dpsec
=
ρ(ffuel , psec )
ρ
0
0
(8.2-19)
when a secondary stream exists. ρ(f ) or ρ(ffuel , psec ) is the instantaneous density obtained
using the instantaneous species mass fractions and temperature in the ideal gas law
equation.
Using Equations 8.2-16 and 8.2-18 (or Equations 8.2-17 and 8.2-19), it remains only to
specify the shape of the function p(f ) (or p1 (ffuel ) and p2 (psec )) in order to determine the
local mean fluid state at all points in the flow field.
The Assumed-Shape PDF
The shape of the assumed PDF, p(f ), is described in ANSYS FLUENT by one of two
mathematical functions:
• the double-delta function (two-mixture-fraction cases only)
• the β-function (single- and two-mixture-fraction cases)
The double-delta function is the most easily computed, while the β-function most closely
represents experimentally observed PDFs. The shape produced by this function depends
solely on the mean mixture fraction, f , and its variance, f 0 2 . A detailed description of
each function follows.
The Double Delta Function PDF
The double delta function is given by
0.5,
p(f ) = 0.5,
0,
q
f = f − qf 0 2
f = f + f 02
elsewhere
(8.2-20)
with suitable bounding near f = 1 and f = 0. One example of the double delta function
is illustrated in Figure 8.2.4. As noted above, the double delta function PDF is very easy
to compute but is invariably less accurate than the alternate β-function PDF because it
8-10
Release 12.0 c ANSYS, Inc. January 29, 2009
8.2 Non-Premixed Combustion and Mixture Fraction Theory
assumes that only two states occur in the turbulent flow. For this reason, it is available
only for two-mixture-fraction simulations where the savings in computational cost is
significant.
p(f)
0.5
0
f
0
f
Figure 8.2.4: Example of the Double Delta Function PDF Shape
The β-Function PDF
The β-function PDF shape is given by the following function of f and f 0 2 :
p(f ) = R
f α−1 (1 − f )β−1
f α−1 (1 − f )β−1 df
(8.2-21)
where
#
"
f (1 − f )
α=f
−1
f 02
(8.2-22)
and
"
#
f (1 − f )
−1
β = (1 − f )
f 02
(8.2-23)
Importantly, the PDF shape p(f ) is a function of only its first two moments, namely
the mean mixture fraction, f , and the mixture fraction variance, f 0 2 . Thus, given ANSYS FLUENT’s prediction of f and f 0 2 at each point in the flow field (Equations 8.2-4
and 8.2-5), the assumed PDF shape can be computed and used as the weighting function
to determine the mean values of species mass fractions, density, and temperature using,
Release 12.0 c ANSYS, Inc. January 29, 2009
8-11
Non-Premixed Combustion
Equations 8.2-16 and 8.2-18 (or, for a system with a secondary stream, Equations 8.2-17
and 8.2-19).
This logical dependence is depicted visually in Figure 8.2.5 for a single mixture fraction.
PDF Shape
p(f ) = p (f , f ’ 2 )
Chemistry Model
φ i (f )
1
φ i = ∫ p(f ) φ i (f ) df
o
Look-up Table φi = φi (f , f
’2)
Figure 8.2.5: Logical Dependence of Averaged Scalars φi on f , f 0 2 , and
the Chemistry Model (Adiabatic, Single-Mixture-Fraction Systems)
8.2.3 Non-Adiabatic Extensions of the Non-Premixed Model
Many reacting systems involve heat transfer through wall boundaries, droplets, and/or
particles. In such flows the local thermochemical state is no longer related only to f ,
but also to the enthalpy, H. The system enthalpy impacts the chemical equilibrium
calculation and the temperature and species of the reacting flow. Consequently, changes
in enthalpy due to heat loss must be considered when computing scalars from the mixture
fraction, as in Equation 8.2-13.
In such non-adiabatic systems, turbulent fluctuations should be accounted for by means
of a joint PDF, p(f, H). The computation of p(f, H), however, is not practical for
most engineering applications. The problem can be simplified significantly by assuming
that the enthalpy fluctuations are independent of the enthalpy level (i.e., heat losses
do not significantly impact the turbulent enthalpy fluctuations). With this assumption,
p(f, H) = p(f )δ(H − H) and mean scalars are calculated as
φi =
8-12
Z
0
1
φi (f, H)p(f )df
(8.2-24)
Release 12.0 c ANSYS, Inc. January 29, 2009
8.2 Non-Premixed Combustion and Mixture Fraction Theory
Determination of φi in the non-adiabatic system thus requires solution of the modeled
transport equation for mean enthalpy:
!
∂
kt
(ρH) + ∇ · (ρ~v H) = ∇ ·
∇H + Sh
∂t
cp
(8.2-25)
where Sh accounts for source terms due to radiation, heat transfer to wall boundaries,
and heat exchange with the dispersed phase.
Figure 8.2.6 depicts the logical dependence of mean scalar values (species mass fraction,
density, and temperature) on ANSYS FLUENT’s prediction of f , f 0 2 , and H in nonadiabatic single-mixture-fraction systems.
Figure 8.2.6: Logical Dependence of Averaged Scalars φi on f , f 0 2 , H, and
the Chemistry Model (Non-Adiabatic, Single-Mixture-Fraction
Systems)
When a secondary stream is included, the mean values are calculated from
φi =
Z
0
1
Z
1
0
Release 12.0 c ANSYS, Inc. January 29, 2009
φi (ffuel , psec , H)p1 (ffuel )p2 (psec )dffuel dpsec
(8.2-26)
8-13
Non-Premixed Combustion
As noted above, the non-adiabatic extensions to the PDF model are required in systems
involving heat transfer to walls and in systems with radiation included. In addition, the
non-adiabatic model is required in systems that include multiple fuel or oxidizer inlets
with different inlet temperatures. Finally, the non-adiabatic model is required in particleladen flows (e.g., liquid fuel systems or coal combustion systems) when such flows include
heat transfer to the dispersed phase. Figure 8.2.7 illustrates several systems that must
include the non-adiabatic form of the PDF model.
Q wall or Q radiation
Fuel
Oxidant
f=1
f=0
(a) Heat Transfer to Domain Boundaries and/or
Radiation Heat Transfer
Oxidant
T = T1
Fuel
Oxidant
T = T2
(b) Multiple Fuel or Oxidant Inlets at Different
Temperatures
Oxidant
Liquid Fuel or
Pulverized Coal
(c) Dispersed Phase Heat or Mass Transfer (e.g.,
Liquid Fuel or Coal Combustion)
Figure 8.2.7: Reacting Systems Requiring Non-Adiabatic Non-Premixed
Model Approach
8-14
Release 12.0 c ANSYS, Inc. January 29, 2009
8.2 Non-Premixed Combustion and Mixture Fraction Theory
8.2.4
Chemistry Tabulation
Look-Up Tables for Adiabatic Systems
For an equilibrium, adiabatic, single-mixture-fraction case, the mean temperature, density, and species fraction are functions of the f and f 02 only (see Equations 8.2-16 and
8.2-21). Significant computational time can be saved by computing these integrals once,
storing them in a look-up table, and retrieving them during the ANSYS FLUENT simulation.
Figure 8.2.8 illustrates the concept of the look-up tables generated for a single-mixturefraction system. Given ANSYS FLUENT’s predicted value for f and f 0 2 at a point in the
flow domain, the mean value of mass fractions, density, or temperature (φi ) at that point
can be obtained by table interpolation.
The table, Figure 8.2.8, is the mathematical result of the integration of Equation 8.2-16.
There is one look-up table of this type for each scalar of interest (species mass fractions,
density, and temperature). In adiabatic systems, where the instantaneous enthalpy is
a function of only the instantaneous mixture fraction, a two-dimensional look-up table,
like that in Figure 8.2.8, is all that is required.
Scalar
Value
Scaled
Variance
Mean
Mixture
Fraction
Figure 8.2.8: Visual Representation of a Look-Up Table for the Scalar φi as
a Function of f and f 0 2 in Adiabatic Single-Mixture-Fraction
Systems
For systems with two mixture fractions, the creation and interpolation costs of fourdimensional look-up tables are computationally expensive. By default, the instantaneous properties φi are tabulated as a function of the fuel mixture fraction ffuel and
the secondary partial fraction psec (see Equation 8.2-12), and the PDF integrations (see
Equation 8.2-14) are performed at run-time. This two-dimensional table is illustrated in
Figure 8.2.9. Alternatively, 4D look-up tables can be created before the simulation and
Release 12.0 c ANSYS, Inc. January 29, 2009
8-15
Non-Premixed Combustion
interpolated at run time (see Section 16.7.1: Full Tabulation of the Two-Mixture-Fraction
Model in the separate User’s Guide).
Instantaneous
Scalar
Value
Secondary
Partial
Fraction
Fuel
Mixture
Fraction
Figure 8.2.9: Visual Representation of a Look-Up Table for the Scalar φi as
a Function of ffuel and psec in Adiabatic Two-Mixture-Fraction
Systems
3D Look-Up Tables for Non-Adiabatic Systems
In non-adiabatic systems, where the enthalpy is not linearly related to the mixture fraction, but depends also on wall heat transfer and/or radiation, a look-up table is required
for each possible enthalpy value in the system. The result, for single mixture fraction
systems, is a three-dimensional look-up table, as illustrated in Figure 8.2.10, which consists of layers of two-dimensional tables, each one corresponding to a normalized heat loss
or gain. The first slice corresponds to the maximum heat loss from the system, the last
slice corresponds to the maximum heat gain to the system, and the zero heat loss/gain
slice corresponds to the adiabatic table. Slices interpolated between the adiabatic and
maximum slices correspond to heat gain, and those interpolated between the adiabatic
and minimum slices correspond to heat loss.
The three-dimensional look-up table allows ANSYS FLUENT to determine the value of
each mass fraction, density, and temperature from calculated values of f , f 0 2 , and H.
This three-dimensional table in Figure 8.2.10 is the visual representation of the integral
in Equation 8.2-24.
8-16
Release 12.0 c ANSYS, Inc. January 29, 2009
8.2 Non-Premixed Combustion and Mixture Fraction Theory
normalized
heat loss/gain
n+1
normalized
heat loss/gainn
normalized
heat loss/gainn-1
Scalar
Value
Scaled
Variance
Mean
Mixture
Fraction
Figure 8.2.10: Visual Representation of a Look-Up Table for the Scalar φi as
a Function of f and f 0 2 and Normalized Heat Loss/Gain in
Non-Adiabatic Single-Mixture-Fraction Systems
For non-adiabatic, two-mixture-fraction problems, it is very expensive to tabulate and
retrieve Equation 8.2-26 since five-dimensional tables are required. By default, 3D lookup tables of the instantaneous state relationship given by Equation 8.2-14 are created.
The 3D table in Figure 8.2.11 is the visual representation of Equation 8.2-14. The mean
density during the ANSYS FLUENT solution is calculated by integrating the instantaneous density over the fuel and secondary mixture fraction space (see Equation 8.2-26).
Alternatively, 5D look-up tables can be created before the simulation and interpolated
at run time (see Section 16.7.1: Full Tabulation of the Two-Mixture-Fraction Model in
the separate User’s Guide). The one-time pre-generation the 5D look-up table is very
expensive, but, once built, interpolating the table during ANSYS FLUENT solution is
usually significantly faster than performing the integrations at run-time. This is especially true for cases with a large number of cells that require many iteration or time-steps
to converge.
Release 12.0 c ANSYS, Inc. January 29, 2009
8-17
Non-Premixed Combustion
i
Note that the computation time in ANSYS FLUENT for a two-mixturefraction case will be much greater than for a single-mixture-fraction problem. This expense should be carefully considered before choosing the
two-mixture-fraction model. Also, it is usually expedient to start a twomixture-fraction simulation from a converged single-mixture-fraction solution.
normalized
heat loss/gain
Instantaneous
Scalar
Value
n+1
normalized
heat loss/gain n
normalized
heat loss/gain
n-1
Secondary
Partial
Fraction
Fuel
Mixture
Fraction
Figure 8.2.11: Visual Representation of a Look-Up Table for the Scalar φi
as a Function of ffuel , psec , and Normalized Heat Loss/Gain in
Non-Adiabatic Two-Mixture-Fraction Systems
8-18
Release 12.0 c ANSYS, Inc. January 29, 2009
8.3 Restrictions and Special Cases for Using the Non-Premixed Model
8.3
Restrictions and Special Cases for Using the Non-Premixed Model
8.3.1
Restrictions on the Mixture Fraction Approach
The unique dependence of φi (species mass fractions, density, or temperature) on f
(Equation 8.2-11 or 8.2-13) requires that the reacting system meet the following conditions:
• The chemical system must be of the diffusion type with discrete fuel and oxidizer
inlets (spray combustion and pulverized fuel flames may also fall into this category).
• The Lewis number must be unity. (This implies that the diffusion coefficients for
all species and enthalpy are equal, a good approximation in turbulent flow).
• When a single mixture fraction is used, the following conditions must be met:
– Only one type of fuel is involved. The fuel may be made up of a burnt mixture
of reacting species (e.g., 90% CH4 and 10% CO) and you may include multiple
fuel inlets. The multiple fuel inlets must have the same composition; two or
more fuel inlets with different fuel composition are not allowed (e.g., one inlet
of CH4 and one inlet of CO). Similarly, in spray combustion systems or in
systems involving reacting particles, only one off-gas is permitted.
– Only one type of oxidizer is involved. The oxidizer may consist of a mixture of
species (e.g., 21% O2 and 79% N2 ) and you may have multiple oxidizer inlets.
The multiple oxidizer inlets must, however, have the same composition. Two
or more oxidizer inlets with different compositions are not allowed (e.g., one
inlet of air and a second inlet of pure oxygen).
• When two mixture fractions are used, three streams can be involved in the system.
Valid systems are as follows:
– Two fuel streams with different compositions and one oxidizer stream. Each
fuel stream may be made up of a mixture of reacting species (e.g., 90% CH4
and 10% CO). You may include multiple inlets of each fuel stream, but each
fuel inlet must have one of the two defined compositions (e.g., one inlet of CH4
and one inlet of CO).
– Mixed fuel systems including gas-liquid, gas-coal, or liquid-coal fuel mixtures
with a single oxidizer. In systems with a gas-coal or liquid-coal fuel mixture,
the coal volatiles and char can be treated as a single composite fuel stream
and the secondary stream can represent another fuel. Alternatively, for coal
combustion, the volatile and char off-gases are tracked separately as distinct
fuel streams.
Release 12.0 c ANSYS, Inc. January 29, 2009
8-19
Non-Premixed Combustion
– Two oxidizer streams with different compositions and one fuel stream. Each
oxidizer stream may consist of a mixture of species (e.g. 21% O2 and 79%
N2 ). You may have multiple inlets of each oxidizer stream, but each oxidizer
inlet must have one of the two defined compositions (e.g., one inlet of air and
a second inlet of pure oxygen).
– A fuel stream, an oxidizer stream, and a non-reacting secondary stream.
• The flow must be turbulent.
It is important to emphasize that these restrictions eliminate the use of the non-premixed
approach for directly modeling premixed combustion. This is because the unburned premixed stream is far from chemical equilibrium. Note, however, that an extended mixture
fraction formulation, the partially premixed model (see Chapter 10: Partially Premixed
Combustion), can be applied to non-premixed (with mixed-but-unburnt regions), as well
as partially premixed flames.
Figures 8.3.1 and 8.3.2 illustrate typical reacting system configurations that can be handled by the non-premixed model in ANSYS FLUENT. Figure 8.3.3 shows a premixed
configuration that cannot be modeled using the non-premixed model.
8.3.2
Using the Non-Premixed Model for Liquid Fuel or Coal Combustion
You can use the non-premixed model if your ANSYS FLUENT simulation includes liquid
droplets and/or coal particles. In this case, fuel enters the gas phase within the computational domain at a rate determined by the evaporation, devolatilization, and char
combustion laws governing the dispersed phase. In the case of coal, the volatiles and
the products of char can be defined as two different types of fuel (using two mixture
fractions) or as a single composite off-gas (using one mixture fraction), as described in
Section 16.4.5: Modeling Coal Combustion Using the Non-Premixed Model in the separate User’s Guide.
8-20
Release 12.0 c ANSYS, Inc. January 29, 2009
8.3 Restrictions and Special Cases for Using the Non-Premixed Model
60% CH4
40% CO
f=1
21% O2
79% N2
f=0
(a) Simple Fuel/Oxidant Diffusion Flame
35% O 2
65% N 2
f=0
60% CH 4
40% CO
35% O2
f=1
f=0
65% N 2
(b) Diffusion System Using Multiple Oxidant Inlets
60% CH 4
20% CO
10% C3H8
10% CO2
f=1
21% O2
79% N2
f=0
60% CH 4
20% CO
10% C3H8
10% CO2
f=1
(c) System Using Multiple Fuel Inlets
Figure 8.3.1: Chemical Systems That Can Be Modeled Using a Single Mixture Fraction
Release 12.0 c ANSYS, Inc. January 29, 2009
8-21
Non-Premixed Combustion
CH 4/CO/C 3H 8
Oxidant
CH 4/C 3H
8
(a) System Containing Two Dissimilar Fuel Inlets
21% O2
Fuel
35% O2
(b) System Containing Two Dissimilar Oxidant Inlets
Figure 8.3.2: Chemical System Configurations That Can Be Modeled Using
Two Mixture Fractions
CH
4
O
2
N
2
Figure 8.3.3: Premixed Systems That Cannot Be Modeled Using the NonPremixed Model
8-22
Release 12.0 c ANSYS, Inc. January 29, 2009
8.3 Restrictions and Special Cases for Using the Non-Premixed Model
8.3.3
Using the Non-Premixed Model with Flue Gas Recycle
While most problems you solve using the non-premixed model will involve inlets that
contain either pure oxidant or pure fuel (f = 0 or 1), you can include an inlet that has
an intermediate value of mixture fraction (0 < f < 1) provided that this inlet represents
a completely reacted mixture. Such cases arise when there is flue gas recirculation, as
depicted schematically in Figure 8.3.4. Since f is a conserved quantity, the mixture
fraction at the flue gas recycle inlet can be computed as
ṁfuel + ṁrecyc fexit = (ṁfuel + ṁox + ṁrecyc )fexit
(8.3-1)
or
fexit =
ṁfuel
ṁfuel + ṁox
(8.3-2)
where fexit is the exit mixture fraction (and the mixture fraction at the flue gas recycle
inlet), ṁox is the mass flow rate of the oxidizer inlet, ṁfuel is the mass flow rate of the
fuel inlet, ṁrecyc is the mass flow rate of the recycle inlet.
If a secondary stream is included,
ffuel,exit =
ṁfuel
ṁfuel
+ ṁsec + ṁox
(8.3-3)
and
psec,exit =
ṁsec
ṁsec + ṁox
(8.3-4)
.
m
R
fexit
.
m
F
f=1
.
m
O
f=0
fexit
Figure 8.3.4: Using the Non-Premixed Model with Flue Gas Recycle
Release 12.0 c ANSYS, Inc. January 29, 2009
8-23
Non-Premixed Combustion
8.3.4
Using the Non-Premixed Model with the Inert Model
To model the effect of dilution on combustion without the expense of using two mixture
fractions, ANSYS FLUENT allows the introduction of an inert stream into the domain.
Unlike a secondary mixture fraction, the inert does not chemically equilibrate with the
primary fuel and oxidizer - instead, its composition remains constant after mixing. However the inert stream does affect the solution due to its influence on enthalpy, specific
heat, and density of the mixture. The equation for conservation of inert is written as:
∂ρYI
µt
+ ∇ · (~v ρYI ) = ∇ ·
∇ (YI )
∂t
Sct
(8.3-5)
where
YI
Sct
µt
ρ
=
=
=
=
inert stream tracer
turbulent Schmidt number
turbulent viscosity
density
Equation 8.3-5 has no sources or sinks, because the problem is reduced to tracking a
conserved scalar when it is assumed that the inert components have the same turbulent
diffusivities.
Mixture Composition
The mixture properties are computed from the mean (f¯) and variance (f¯0 ) of the mixture
fraction in the cell, the reaction progress variable (c, when the partially premixed model
is enabled), the cell enthalpy (H, for non-adiabatic flows), and the inert tracer (YI ). The
mixture is modeled as a blend of inert and active species, but the PDF tables need to be
accessed with conditioned variables. Conditioning is necessary to take into account the
volume taken up by the inert fraction, yet still be able to utilize previously built tables
by straightforward lookup. The mean mixture fraction and mixture fraction variance
used to access the PDF table is given by:
f¯
1 − YI
f¯02
=
(1 − YI )2
f¯I =
(8.3-6)
f¯I02
(8.3-7)
The reaction progress variable c is not conditioned, however the cell enthalpy must be
conditioned to account for the inert enthalpy. The inert enthalpy and active enthalpy
are obtained from the following relationships:
H(T ) = (1 − YI )H pdf (T ) + YI H I (T )
8-24
(8.3-8)
Release 12.0 c ANSYS, Inc. January 29, 2009
8.3 Restrictions and Special Cases for Using the Non-Premixed Model
where H is the enthalpy of the cell at temperature T , H pdf is the enthalpy of the active
mixture-fraction stream and H I is the enthalpy of the inert stream. Here it is assumed
that the inert and the active streams have the same temperature, but different enthalpies.
To calculate the temperature in the cell, Equation 8.3-8 is solved for the temperature and
for H pdf , which gives the partitioning of the energy between the inert and active streams.
The inert enthalpy is defined as
H I (T ) =
NI
X
i=0
Yi
Z
T
T0
Cpi dT
(8.3-9)
where Yi refers to the mass fraction of specie i defined in the inert stream, T0 is the
reference temperature, Cpi the specific heat of specie i, and NI is the number of inert
species.
The inert and PDF enthalpies are defined further in Equation 31.4-13 in the separate
User’s Guide.
Property Evaluation
The specific heat of the mixture is evaluated by mixing the inert and active streams in
the following way:
Cp (T ) = (1 − YI )Cppdf (T ) + YI CpI (T )
(8.3-10)
The density of the mixture is calculated by using a harmonic average of the densities of
the active and inert streams, weighted by the inert tracer:
"
(1 − YI )
YI
ρ(T ) =
+ I
pdf
ρ (T )
ρ (T )
#−1
(8.3-11)
Here, the inert density (ρI ) is calculated from the ideal gas law.
For information on how to set up the inert model, see Section 16.7.5: Setting Up the
Inert Model in the separate User’s Guide.
Release 12.0 c ANSYS, Inc. January 29, 2009
8-25
Non-Premixed Combustion
8.4
The Laminar Flamelet Models Theory
Information about the flamelet models are presented in the following sections:
• Section 8.4.1: Restrictions and Assumptions
• Section 8.4.2: The Flamelet Concept
• Section 8.4.3: Flamelet Generation
• Section 8.4.4: Flamelet Import
8.4.1
Restrictions and Assumptions
The following restrictions apply to all flamelet models in ANSYS FLUENT:
• Only a single mixture fraction can be modeled; two-mixture-fraction flamelet models are not allowed.
• The mixture fraction is assumed to follow the β-function PDF, and scalar dissipation fluctuations are ignored.
• Empirically-based streams cannot be used with the flamelet model.
8.4.2
The Flamelet Concept
Overview
The flamelet concept views the turbulent flame as an ensemble of thin, laminar, locally
one-dimensional flamelet structures embedded within the turbulent flow field [36, 267,
268] (see Figure 8.4.1).
A common laminar flame type used to represent a flamelet in a turbulent flow is the
counterflow diffusion flame. This geometry consists of opposed, axisymmetric fuel and
oxidizer jets. As the distance between the jets is decreased and/or the velocity of the
jets increased, the flame is strained and increasingly departs from chemical equilibrium
until it is eventually extinguished. The species mass fraction and temperature fields can
be measured in laminar counterflow diffusion flame experiments, or, most commonly,
calculated. For the latter, a self-similar solution exists, and the governing equations can
be simplified to one dimension along the axis of the fuel and oxidizer jets, where complex
chemistry calculations can be affordably performed.
8-26
Release 12.0 c ANSYS, Inc. January 29, 2009
8.4 The Laminar Flamelet Models Theory
turbulent flame
laminar flamelet structure
(see detail below)
flame
oxidizer
fuel
x
velocity (u fuel )
velocity (u ox )
velocity
gradient (a fuel )
velocity
gradient (a ox )
temperature (T fuel )
temperature (Tox )
fuel composition
oxidizer composition
fuel-oxidizer distance
Figure 8.4.1: Laminar Opposed-Flow Diffusion Flamelet
Release 12.0 c ANSYS, Inc. January 29, 2009
8-27
Non-Premixed Combustion
In the laminar counterflow flame, the mixture fraction, f , (see Section 8.2.1: Definition
of the Mixture Fraction for definition) decreases monotonically from unity at the fuel
jet to zero at the oxidizer jet. If the species mass fraction and temperature along the
axis are mapped from physical space to mixture fraction space, they can be uniquely
described by two parameters: the mixture fraction and the strain rate (or, equivalently,
the scalar dissipation, χ, defined in Equation 8.4-2). Hence, the chemistry is reduced and
completely described by the two quantities, f and χ.
This reduction of the complex chemistry to two variables allows the flamelet calculations to be preprocessed, and stored in look-up tables. By preprocessing the chemistry,
computational costs are reduced considerably.
The balance equations, solution methods, and sample calculations of the counterflow
laminar diffusion flame can be found in several references. Comprehensive reviews and
analyses are presented in the works of Bray and Peters, and Dixon-Lewis [36, 72].
Strain Rate and Scalar Dissipation
A characteristic strain rate for a counterflow diffusion flamelet can be defined as as =
v/2d, where v is the relative speed of the fuel and oxidizer jets, and d is the distance
between the jet nozzles.
Instead of using the strain rate to quantify the departure from equilibrium, it is expedient
to use the scalar dissipation, denoted by χ. The scalar dissipation is defined as
χ = 2D|∇f |2
(8.4-1)
where D is a representative diffusion coefficient.
Note that the scalar dissipation, χ, varies along the axis of the flamelet. For the counterflow geometry, the flamelet strain rate as can be related to the scalar dissipation at
the position where f is stoichiometric by [267]:
χst =
as exp −2[erfc−1 (2fst )]2
π
(8.4-2)
where
χst
as
fst
erfc−1
8-28
=
=
=
=
scalar dissipation at f = fst
characteristic strain rate
stoichiometric mixture fraction
inverse complementary error function
Release 12.0 c ANSYS, Inc. January 29, 2009
8.4 The Laminar Flamelet Models Theory
Physically, as the flame is strained, the width of the reaction zone diminishes, and the
gradient of f at the stoichiometric position f = fst increases. The instantaneous stoichiometric scalar dissipation, χst , is used as the essential non-equilibrium parameter. It
has the dimensions s−1 and may be interpreted as the inverse of a characteristic diffusion
time. In the limit χst → 0 the chemistry tends to equilibrium, and as χst increases due
to aerodynamic straining, the non-equilibrium increases. Local quenching of the flamelet
occurs when χst exceeds a critical value.
Embedding Laminar Flamelets in Turbulent Flames
A turbulent flame brush is modeled as an ensemble of discrete laminar flamelets. Since,
for adiabatic systems, the species mass fraction and temperature in the laminar flamelets
are completely parameterized by f and χst , density-weighted mean species mass fractions
and temperature in the turbulent flame can be determined from the PDF of f and χst as
φ=
Z Z
φ(f, χst )p(f, χst ) df dχst
(8.4-3)
where φ represents species mass fractions and temperature.
In ANSYS FLUENT, f and χst are assumed to be statistically independent, so the joint
PDF p(f, χst ) can be simplified as pf (f )pχ (χst ). A β PDF shape is assumed for pf , and
transport equations for f and f 0 2 are solved in ANSYS FLUENT to specify pf . Fluctuations in χst are ignored so that the PDF of χ is a delta function: pχ = δ(χ − χ). The
first moment, namely the mean scalar dissipation, χst , is modeled in ANSYS FLUENT as
χst =
Cχ f 0 2
k
(8.4-4)
where Cχ is a constant with a default value of 2.
For LES, the mean scalar dissipation is modeled as
χst = Cχ
(µt + µ)
2
|∇f |
ρσt
(8.4-5)
To avoid the PDF convolutions at ANSYS FLUENT run-time, the integrations in Equation 8.4-3 are preprocessed and stored in look-up tables. For adiabatic flows, flamelet
tables have three dimensions: f , f 0 2 and χst .
For non-adiabatic steady laminar flamelets, the additional parameter of enthalpy is required. However, the computational cost of modeling steady flamelets over a range of
enthalpies is prohibitive, so some approximations are made. Heat gain/loss to the system
is assumed to have a negligible effect on the species mass fractions, and adiabatic mass
fractions are used [27, 240]. The temperature is then calculated from Equation 5.2-7
Release 12.0 c ANSYS, Inc. January 29, 2009
8-29
Non-Premixed Combustion
for a range of mean enthalpy gain/loss, H. Accordingly, mean temperature and density
PDF tables have an extra dimension of mean enthalpy. The approximation of constant
adiabatic species mass fractions is, however, not applied for the case corresponding to a
scalar dissipation of zero. Such a case is represented by the non-adiabatic equilibrium
solution. For χst = 0, the species mass fractions are computed as functions of f , f 0 2 , and
H.
In ANSYS FLUENT, you can either generate your own flamelets, or import them as
flamelet files calculated with other stand-alone packages. Such stand-alone codes include
OPPDIF [210], CFX-RIF [15, 16, 272] and RUN-1DL [270]. ANSYS FLUENT can import
flamelet files in OPPDIF format or standard flamelet file format.
Instructions for generating and importing flamelets are provided in Section 8.4.3: Flamelet
Generation and Section 8.4.4: Flamelet Import.
8.4.3
Flamelet Generation
The laminar counterflow diffusion flame equations can be transformed from physical
space (with x as the independent variable) to mixture fraction space (with f as the
independent variable) [273]. In ANSYS FLUENT, a simplified set of the mixture fraction
space equations are solved [272]. Here, N equations are solved for the species mass
fractions, Yi ,
ρ
1 ∂ 2 Yi
∂Yi
= ρχ 2 + Si
∂t
2 ∂f
(8.4-6)
and one equation for temperature:
∂T
1 ∂2T
1 X
1
∂cp X
∂Yi ∂T
= ρχ 2 −
H i Si +
ρχ
+
cp,i
ρ
∂t
2 ∂f
cp i
2cp
∂f
∂f ∂f
i
"
#
(8.4-7)
The notation in Equations 8.4-6 and 8.4-7 is as follows: Yi , T , ρ, and f are the ith species
mass fraction, temperature, density, and mixture fraction, respectively. cp,i and cp are
the ith species specific heat and mixture-averaged specific heat, respectively. Si is the
ith species reaction rate, and Hi is the specific enthalpy of the ith species.
The scalar dissipation, χ, must be modeled across the flamelet. An extension of Equation 8.4-2 to variable density is used [163]:
q
2
as 3( ρ∞ /ρ + 1)
q
χ(f ) =
exp −2[erfc−1 (2f )]2
4π 2 ρ∞ /ρ + 1
(8.4-8)
where ρ∞ is the density of the oxidizer stream.
8-30
Release 12.0 c ANSYS, Inc. January 29, 2009
8.4 The Laminar Flamelet Models Theory
8.4.4
Flamelet Import
ANSYS FLUENT can import one or more flamelet files, convolute these flamelets with the
assumed-shape PDFs (see Equation 8.4-3), and construct look-up tables. The flamelet
files can be generated in ANSYS FLUENT, or with separate stand-alone computer codes.
Three types of flamelet files can be imported into ANSYS FLUENT: binary files generated
by the OPPDIF code [210], ASCII files generated by the CFX-RIF code [15, 16, 272], and
standard format files described in Section 16.7.4: Standard Flamelet Files in the separate
User’s Guide and in Peters and Rogg [270].
When flamelets are generated in physical space (such as with OPPDIF), the species and
temperature vary in one spatial dimension. The species and temperature must then be
mapped from physical space to mixture fraction space. If the diffusion coefficients of
all species are equal, a unique definition of the mixture fraction exists. However, with
differential diffusion, the mixture fraction can be defined in a number of ways.
ANSYS FLUENT provides four methods of computing the mixture fraction profile along
the laminar flamelet:
• Average of C and H: Following the work of Drake and Blint [77], the mixture
fraction is calculated as the mean value of fC and fH , where fC and f H are the
mixture fraction values based on the carbon and hydrogen elements.
• Hydrocarbon formula: Following the work of Bilger et al. [26], the mixture fraction
is calculated as
b − box
bfuel − box
(8.4-9)
YC
YH
YO
+ 0.5
−
Mw,C
Mw,H Mw,O
(8.4-10)
f=
where
b=2
YC , YH , and YO are the mass fractions of carbon, hydrogen, and oxygen atoms, and
Mw,C , Mw,H , and Mw,O are the molecular weights. box and bfuel are the values of b
at the oxidizer and fuel inlets.
• Nitrogen method: The mixture fraction is computed in terms of the mass fraction
of the nitrogen species:
f=
YN − YN,ox
YN,fuel − YN,ox
(8.4-11)
where YN is the elemental mass fraction of nitrogen along the flamelet, YN,ox is the
mass fraction of nitrogen at the oxidizer inlet, and YN,fuel is the mass fraction of
nitrogen at the fuel inlet.
Release 12.0 c ANSYS, Inc. January 29, 2009
8-31
Non-Premixed Combustion
• Read from a file (standard format files only): This option is for flamelets solved in
mixture fraction space. If you choose this method, ANSYS FLUENT will search for
the mixture fraction keyword Z, as specified in Peter and Roggs’s work [270], and
retrieve the data. If ANSYS FLUENT does not find mixture fraction data in the
flamelet file, it will instead use the hydrocarbon formula method described above.
The flamelet profiles in the multiple-flamelet data set should vary only in the strain rate
imposed; the species and the boundary conditions should be the same. In addition, it is
recommended that an extinguished flamelet is excluded from the multiple-flamelet data
set. The formats for multiple flamelets are as follows:
• OPPDIF format: The multiple-flamelet OPPDIF files should be produced using the
CNTN keyword in the OPPDIF script. Alternatively, you can use ANSYS FLUENT
to merge a number of single-flamelet OPPDIF files into a multiple-flamelet file.
• Standard format: If you have a set of standard format flamelet files, you can import
them all at the same time, and ANSYS FLUENT will merge them internally into a
multiple-flamelet file. When you import the set of flamelet files, ANSYS FLUENT
will search for and count the occurrences of the HEADER keyword to determine the
number of flamelets in the file.
• CFX-RIF format: A CFX-RIF flamelet file contains multiple flamelets at various
strains and the file should not be modified manually. Only one CFX-RIF flamelet
file should be imported.
For either type of file, ANSYS FLUENT will determine the number of flamelet profiles
and sort them in ascending strain-rate order. For flamelets generated in physical space,
you can select one of the four methods available for the calculation of mixture fraction.
The scalar dissipation will be calculated from the strain rate using Equation 8.4-2.
8.5
The Steady Laminar Flamelet Model Theory
The steady laminar flamelet approach models a turbulent flame brush as an ensemble of
discrete, steady laminar flames, called flamelets. The individual flamelets are assumed
to have the same structure as laminar flames in simple configurations, and are obtained
by experiments or calculations. Using detailed chemical mechanisms, ANSYS FLUENT
can calculate laminar opposed-flow diffusion flamelets for non-premixed combustion. The
laminar flamelets are then embedded in a turbulent flame using statistical PDF methods.
The advantage of the laminar flamelet approach is that realistic chemical kinetic effects
can be incorporated into turbulent flames. The chemistry can then be preprocessed
and tabulated, offering tremendous computational savings. However, the steady laminar
flamelet model is limited to modeling combustion with relatively fast chemistry. The
flame is assumed to respond instantaneously to the aerodynamic strain, and thus the
8-32
Release 12.0 c ANSYS, Inc. January 29, 2009
8.5 The Steady Laminar Flamelet Model Theory
model cannot capture deep non-equilibrium effects such as ignition, extinction, and slow
chemistry (like NOx ).
Information pertaining strictly to the steady flamelet model is presented in the following
sections:
• Section 8.5.1: Overview
• Section 8.5.2: Multiple Steady Flamelet Libraries
• Section 8.5.3: Steady Laminar Flamelet Automated Grid Refinement
• Section 8.5.4: Non-Adiabatic Steady Laminar Flamelets
For general information about the mixture fraction model, see Section 8.1: Introduction.
8.5.1
Overview
In a diffusion flame, at the molecular level, fuel and oxidizer diffuse into the reaction
zone. Here, they encounter high temperatures and radical species and ignite. More heat
and radicals are generated in the reaction zone and some diffuse out. In near-equilibrium
flames, the reaction rate is much faster than the diffusion rate. However, as the flame
is stretched and strained by the turbulence, species and temperature gradients increase,
and radicals and heat diffuse more quickly out of the flame. The species have less time
to reach chemical equilibrium, and the degree of local non-equilibrium increases.
The steady laminar flamelet model is suited to predict chemical non-equilibrium due
to aerodynamic straining of the flame by the turbulence. The chemistry, however, is
assumed to respond rapidly to this strain, so as the strain relaxes to zero, the chemistry
tends to equilibrium.
When the chemical time-scale is comparable to the fluid mixing time-scale, the species
can be considered to be in global chemical non-equilibrium. Such cases include NOx
formation and low-temperature CO oxidation. The steady laminar flamelet model is not
suitable for such slow-chemistry flames. Instead, you can model slow chemistry using one
of the following:
• the Unsteady Laminar Flamelet model (see Section 8.6: The Unsteady Laminar
Flamelet Model Theory)
• the trace species assumption in the NOx model (see Chapter 13: Pollutant Formation)
• the Laminar Finite-Rate model (see Section 7.1.2: The Generalized Finite-Rate
Formulation for Reaction Modeling), where the turbulence-chemistry interaction is
ignored.
Release 12.0 c ANSYS, Inc. January 29, 2009
8-33
Non-Premixed Combustion
• the EDC model (see Section 7.1.2: The Eddy-Dissipation-Concept (EDC) Model)
• the PDF transport model (see Chapter 11: Composition PDF Transport).
8.5.2
Multiple Steady Flamelet Libraries
ANSYS FLUENT can generate multiple steady flamelets over a range of strain rates to account for the varying strain field in your multi-dimensional simulation. If you specify the
number of flamelets to be greater than one, flamelets are generated at scalar dissipation
values as determined by Equation 8.5-1.
χi =
10χi−1
for χi−1 < 1 s−1
(8.5-1)
χi−1 + ∆χ for χi−1 ≥ 1 s
−1
where i ranges from 1 up to the specified maximum number of flamelets, χ0 is the
initial scalar dissipation, and ∆χ is the scalar dissipation step. Flamelets are generated
until either the maximum number of flamelets is reached, or the flamelet extinguishes.
Extinguished flamelets are excluded from the flamelet library.
8.5.3
Steady Laminar Flamelet Automated Grid Refinement
By default, 1D flamelet grids are discretized by clustering a fixed number of points
about the stoichiometric mixture fraction, which is approximated as the location of peak
temperature. ANSYS FLUENT also has the option for Automated Grid Refinement of
steady flamelets, where an adaptive algorithm inserts grid points so that the change of
values, as well as the change of slopes, between successive grid points is less than user
specified tolerances.
When using automated grid refinement, a steady solution is calculated on a coarse grid
with a user specified Initial Number of Grid Points in Flamelet (default of 8). At convergence, a new grid point is inserted midway between a point i and its neighbor i + 1
if,
|vi − vi+1 | > v (vmax − vmin )
(8.5-2)
where vi is the value for each temperature and species mass fraction at grid point i, v is
a user specified Maximum Change in Value Ratio (default of 0.5), and vmax (vmin ) are the
maximum (minimum) values over all grid points.
In addition a grid point is added if,
|si − si+1 | > s (smax − smin )
8-34
(8.5-3)
Release 12.0 c ANSYS, Inc. January 29, 2009
8.5 The Steady Laminar Flamelet Model Theory
where the slope si is defined as,
si =
vi+1 − vi
fi+1 − fi
(8.5-4)
In Equations 8.5-3 and 8.5-4, s is a user specified Maximum Change in Slope Ratio (default
of 0.5), smax (smin ) are the maximum (minimum) slopes over all grid points, and fi is
the mixture fraction value of grid point i.
The refined flamelet is reconverged, and the refinement process is repeated until no further
grid points are added by Equations 8.5-2 and 8.5-3, or the user specified Maximum Number
of Grid Points in Flamelet (default of 64) is exceeded.
8.5.4
Non-Adiabatic Steady Laminar Flamelets
For non-adiabatic steady flamelets, ANSYS FLUENT follows the approach of [27, 240]
and assumes that flamelet species profiles are unaffected by heat loss/gain from the
flamelet. No special non-adiabatic flamelet profiles need to be generated, avoiding a very
cumbersome preprocessing step. In addition, the compatibility of ANSYS FLUENT with
external steady flamelet generation packages (e.g., OPPDIF, CFX-RIF, RUN-1DL) is
retained. The disadvantage to this model is that the effect of the heat losses on the
species mass fractions is not taken into account. Also, the effect of the heat loss on the
extinction limits is not taken into account.
After flamelet generation, the flamelet profiles are convoluted with the assumed-shape
PDFs as in Equation 8.4-3, and then tabulated for look-up in ANSYS FLUENT. The
non-adiabatic PDF tables have the following dimensions:
T (f , f 0 2 , H, χ)
Yi (f , f 0 2 , H) for χ = 0 (i.e., equilibrium solution)
Yi (f , f 0 2 , χ) for χ 6= 0
ρ(f , f 0 2 , H, χ)
During the ANSYS FLUENT solution, the equations for the mean mixture fraction, mixture fraction variance, and mean enthalpy are solved. The scalar dissipation field is
calculated from the turbulence field and the mixture fraction variance (Equation 8.4-4).
The mean values of cell temperature, density, and species mass fraction are obtained
from the PDF look-up table.
Release 12.0 c ANSYS, Inc. January 29, 2009
8-35
Non-Premixed Combustion
8.6
The Unsteady Laminar Flamelet Model Theory
The steady laminar flamelet model, described in Sections 8.4 and 8.5, models local chemical non-equilibrium due to the straining effect of turbulence. In many combustors the
strain is small at the outlet and the steady flamelet model predicts all species, including
slow-forming species like NOx , to be near equilibrium, which is often inaccurate. The
cause of this inaccuracy is the disparity between the flamelet time-scale, which is the
inverse of the scalar dissipation, and the slow-forming species time-scale, which is the
residence time since the species started accumulating after mixing in the combustor.
The unsteady laminar flamelet model in ANSYS FLUENT can predict slow-forming species,
such as gaseous pollutants or product yields in liquid reactors, more accurately than
the steady laminar flamelet model. Computationally expensive chemical kinetics are
reduced to one dimension and the model is significantly faster than the laminar-finiterate, EDC or PDF Transport models where kinetics are calculated in two or three dimensions. There are two variants of the unsteady laminar flamelet model, namely an
Eulerian unsteady flamelet model (described in Section 8.6.1: The Eulerian Unsteady
Laminar Flamelet Model) and a diesel unsteady flamelet model for predicting combustion in compression-ignition engines (described in Section 8.6.2: The Diesel Unsteady
Laminar Flamelet Model).
Information pertaining strictly to the unsteady flamelet model is presented in the following sections:
• Section 8.6.1: The Eulerian Unsteady Laminar Flamelet Model
• Section 8.6.2: The Diesel Unsteady Laminar Flamelet Model
8.6.1
The Eulerian Unsteady Laminar Flamelet Model
The Eulerian unsteady laminar flamelet model can be used to predict slow-forming intermediate and product species which are not in chemical equilibrium. Typical examples of
slow-forming species are gas-phase pollutants like NOx , and product compounds in liquid reactors. By reducing the chemistry computation to one dimension, detailed kinetics
with multiple species and stiff reactions can be economically simulated in complex 3D
geometries.
The model, following the work of Barths et al. [16], postprocesses an unsteady marker
probability equation on a steady-state, converged flow field. In ANSYS FLUENT, the
steady flow solution must be computed with the steady laminar flamelet model (see
Section 8.5: The Steady Laminar Flamelet Model Theory). Since the unsteady flamelet
equations are postprocessed on a steady-state, steady flamelet solution, the effect of the
unsteady flamelet species on the flow-field are neglected.
8-36
Release 12.0 c ANSYS, Inc. January 29, 2009
8.6 The Unsteady Laminar Flamelet Model Theory
The transport equation for the unsteady flamelet marker probability, I, is
∂
µt
∇I
(ρI) + ∇ · (ρ~v I) = ∇ ·
∂t
σt
(8.6-1)
Equation 8.6-1 is always solved unsteady, and is initialized as
I=
1 for f ≥ finit
(8.6-2)
0 for f < finit
where f is the mean mixture fraction and finit is a user supplied constant, which should
be set greater than the stoichiometric mixture fraction. At inlet boundaries, ANSYS
FLUENT always sets I toward zero, and hence the I field decreases to zero with time as
I is convected and diffused out of the domain (for cases with outlet boundaries).
The unsteady flamelet species equations (Equation 8.4-6) are integrated simultaneously
with the marker probability equation, I. For liquid-phase chemistry, the initial flamelet
field is the mixed-but-unburnt flamelet, as liquid reactions are assumed to proceed immediately upon mixing. However, gas-phase chemistry invariably requires ignition, so
the initial flamelet field is calculated from a steady flamelet solution. All slow-forming
species, such as NOx , are zeroed in this initial flamelet profile since, at ignition, little
time has elapsed for any significant formation. The slow-forming species are identified
by the user before solution of the unsteady flamelet equations.
The scalar dissipation at stoichiometric mixture fraction (χst ) is required by the flamelet
species equation. This is calculated from the steady-state ANSYS FLUENT field at each
time step as a probability-weighted volume integral:
R
χst (t) = RV
V
I(~x, t) ρ(~x) χst 3/2 (~x) dV
I(~x, t) ρ(~x) χst 1/2 (~x) dV
(8.6-3)
where χst is defined in Equation 8.6-3, and V denotes the fluid volume. ANSYS FLUENT
provides the option of limiting χst to a user-specified maximum value, which should
be approximately equal to the flamelet extinction scalar dissipation (the steady flamelet
solver can be used to calculate this extinction scalar dissipation in a separate simulation).
Release 12.0 c ANSYS, Inc. January 29, 2009
8-37
Non-Premixed Combustion
The unsteady flamelet energy equation is not solved in order to avoid flamelet extinction for high scalar dissipation, and to account for non-adiabatic heat loss or gain. For
adiabatic cases, the flamelet temperature T ad (f, t) is calculated at each time step from
the steady flamelet library at the probability-weighted scalar dissipation χst from Equation 8.6-3. For non-adiabatic cases, the flamelet temperature at time t is calculated
from
T (f, t) = T ad (f, t) ξ(f, t)
(8.6-4)
where
R
ξ(f, t) =
V
I ρ T (~x|f )/Tad (f, t) dV
R
V I ρ dV
(8.6-5)
In Equation 8.6-5, T (~x|f ) denotes the ANSYS FLUENT steady-state mean cell temperature conditioned on the local cell mixture fraction.
Unsteady flamelet mean species mass fractions in each cell are accumulated over time as
Rt
Yk
uf la
=
0
Iρ
hR
1
0
i
Yk (f, t) P (f ) df dt
Rt
0
I ρ dt
(8.6-6)
where Yk (f, t) is the k’th species unsteady flamelet mass fraction, and P (f ) denotes the
Beta PDF.
The probability marker equation (Equation 8.6-1) and the flamelet species equation
(Equation 8.4-6) are advanced together in time until the probability marker has substantially convected and diffused out of the domain. The unsteady flamelet mean species,
calculated from Equation 8.6-5, reaches steady-state as the probability marker I vanishes.
Liquid Reactions
Liquid reactors are typically characterized by:
• Near constant density and temperature.
• Relatively slow reactions and species far from chemical equilibrium.
• High Schmidt number (Sc) and hence reduced molecular diffusion.
The Eulerian unsteady laminar flamelet model can be used to model liquid reactions.
When the Liquid Micro-Mixing model is enabled, ANSYS FLUENT uses the volume-weightedmixing-law formula to calculate the density.
8-38
Release 12.0 c ANSYS, Inc. January 29, 2009
8.6 The Unsteady Laminar Flamelet Model Theory
The effect of high Sc is to decrease mixing at the smallest (micro) scales and increase
the mixture fraction variance, which is modeled with the Turbulent Mixer Model [11].
0
Three transport equations are solved for the inertial-convective (fic2 ), viscous-convective
0
02
(fvc
), and viscous-diffusive (fvd2 ) subranges of the turbulent scalar spectrum,
2
∂ 02
µt
0
0
0
ρfic + ∇ · ρ~v fic2 = ∇ ·
∇fic2 + C1 µt ∇f − C2 ρ fic2
∂t
σt
k
(8.6-7)
∂ 02
µt
0
02
02
02
ρfvc + ∇ · ρ~v fvc
=∇·
∇fvc
+ C2 ρ fic2 − C3 ρ
f
∂t
σt
k
ν vc
(8.6-8)
r
µt
C5
∂ 02
0
0
0
02
ρfvd + ∇ · ρ~v fvd2 = ∇ ·
∇fvd2 + C3 ρ
fvc
− C4 +
fvd2
∂t
σt
ν
Sc
r
(8.6-9)
where the constants C1 through C5 have values of 2, 1.86, 0.058, 0.303, and 17050,
0
0
02
and fvd2 .
respectively. The total mixture fraction variance is the sum of fic2 , fvc
In Equation 8.6-9, the cell Schmidt number, Sc, is calculated as Sc = µ/ρD where µ
is the viscosity, ρ the density, and D the mass diffusivity as defined for the pdf-mixture
material.
8.6.2
The Diesel Unsteady Laminar Flamelet Model
In diesel engines, fuel sprayed into the cylinder evaporates, mixes with the surrounding
gases, and then auto-ignites as compression raises the temperature and pressure. The
diesel unsteady laminar flamelet model, based on the work of Pitsch et al. and Barths
et al. [272, 15], models the chemistry in a single, one-dimensional laminar flamelet. By
reducing the costly chemical kinetic calculation to 1D, substantial savings in run-time
can be achieved over the laminar-finite-rate, EDC or PDF Transport models.
The flamelet species and energy equations (Equations 8.4-6 and 8.4-7) are solved simultaneously with the flow. The flamelet equations are advanced for a fractional step using
properties from the flow, and then the flow is advanced for the same fractional time-step
using properties from the flamelet.
The initial flamelet condition at the start of the diesel simulation is a mixed-but-unburnt
distribution. For the flamelet fractional time-step, the volume-averaged scalar dissipation
and pressure, as well as the fuel and oxidizer temperatures, are passed from the flow solver
to the flamelet solver. To account for temperature rise during compression, the flamelet
energy equation (Equation 8.4-7) has an additional term on the right-hand side as
q̇ =
Release 12.0 c ANSYS, Inc. January 29, 2009
1 ∂p
cp ∂t
(8.6-10)
8-39
Non-Premixed Combustion
where cp is a the specific heat and p is the volume-averaged pressure in the cylinder.
This rise in flamelet temperature due to compression eventually leads to ignition of the
flamelet.
After the flamelet equations have been advanced for the fractional time-step, the PDF Table is created as a Non-Adiabatic Steady Flamelet table (see Section 8.5.4: Non-Adiabatic
Steady Laminar Flamelets). Using the properties of this table, the CFD flow field is then
advanced for the same fractional time-step.
The diesel unsteady flamelet approach can model ignition as well as formation of product, intermediate and pollutant species. Enabling the Diesel Unsteady Flamelet model is
described in Section 16.3.6: Using the Diesel Unsteady Laminar Flamelet Model in the
separate User’s Guide.
8-40
Release 12.0 c ANSYS, Inc. January 29, 2009
Chapter 9.
Premixed Combustion
ANSYS FLUENT has premixed turbulent combustion models based on the reactionprogress variable approach. For more information about using the premixed turbulent
combustion model, see Chapter 17: Modeling Premixed Combustion in the separate User’s
Guide. Theoretical information about this model is provided in the following sections:
• Section 9.1: Overview and Limitations
• Section 9.2: Zimont Turbulent Flame Closure Theory
• Section 9.3: Extended Coherent Flamelet Model Theory
• Section 9.4: Calculation of Temperature
• Section 9.5: Calculation of Density
9.1
Overview and Limitations
9.1.1
Overview
In premixed combustion, fuel and oxidizer are mixed at the molecular level prior to
ignition. Combustion occurs as a flame front propagating into the unburnt reactants.
Examples of premixed combustion include aspirated internal combustion engines, leanpremixed gas turbine combustors, and gas-leak explosions.
Premixed combustion is much more difficult to model than non-premixed combustion.
The reason for this is that premixed combustion usually occurs as a thin, propagating
flame that is stretched and contorted by turbulence. For subsonic flows, the overall
rate of propagation of the flame is determined by both the laminar flame speed and the
turbulent eddies. The laminar flame speed is determined by the rate that species and
heat diffuse upstream into the reactants and burn. To capture the laminar flame speed,
the internal flame structure would need to be resolved, as well as the detailed chemical
kinetics and molecular diffusion processes. Since practical laminar flame thicknesses are
of the order of millimeters or smaller, resolution requirements are usually unaffordable.
The effect of turbulence is to wrinkle and stretch the propagating laminar flame sheet,
increasing the sheet area and, in turn, the effective flame speed. The large turbulent
eddies tend to wrinkle and corrugate the flame sheet, while the small turbulent eddies,
if they are smaller than the laminar flame thickness, may penetrate the flame sheet and
modify the laminar flame structure.
Release 12.0 c ANSYS, Inc. January 29, 2009
9-1
Premixed Combustion
Non-premixed combustion, in comparison, can be greatly simplified to a mixing problem
(see the mixture fraction approach in Section 8.1: Introduction). The essence of premixed
combustion modeling lies in capturing the turbulent flame speed, which is influenced by
both the laminar flame speed and the turbulence.
In premixed flames, the fuel and oxidizer are intimately mixed before they enter the combustion device. Reaction then takes place in a combustion zone that separates unburnt
reactants and burnt combustion products. Partially premixed flames exhibit the properties of both premixed and diffusion flames. They occur when an additional oxidizer or
fuel stream enters a premixed system, or when a diffusion flame becomes lifted off the
burner so that some premixing takes place prior to combustion.
Premixed and partially premixed flames can be modeled using ANSYS FLUENT’s finiterate/eddy-dissipation formulation (see Chapter 7: Species Transport and Finite-Rate
Chemistry). If finite-rate chemical kinetic effects are important, the Laminar FiniteRate model (see Section 7.1.2: The Laminar Finite-Rate Model), the EDC model (see
Section 7.1.2: The Eddy-Dissipation-Concept (EDC) Model) or the composition PDF
transport model (see Chapter 11: Composition PDF Transport) can be used. For information about ANSYS FLUENT’s partially premixed combustion model, see Chapter 10: Partially Premixed Combustion. If the flame is perfectly premixed (all streams
entering the combustor have the same equivalence ratio), it is possible to use the premixed
combustion model, as described in this chapter.
9.1.2
Limitations
The following limitations apply to the premixed combustion model:
• You must use the pressure-based solver. The premixed combustion model is not
available with either of the density-based solvers.
• The premixed combustion model is valid only for turbulent, subsonic flows. These
types of flames are called deflagrations. Explosions, also called detonations, where
the combustible mixture is ignited by the heat behind a shock wave, can be modeled
with the finite-rate model using the density-based solver. See Chapter 7: Species
Transport and Finite-Rate Chemistry for information about the finite-rate model.
• The premixed combustion model cannot be used in conjunction with the pollutant (i.e., soot and NOx ) models. However, a perfectly premixed system can be
modeled with the partially premixed model (see Chapter 10: Partially Premixed
Combustion), which can be used with the pollutant models.
• You cannot use the premixed combustion model to simulate reacting discrete-phase
particles, since these would result in a partially premixed system. Only inert particles can be used with the premixed combustion model.
9-2
Release 12.0 c ANSYS, Inc. January 29, 2009
9.2 Zimont Turbulent Flame Closure Theory
9.2
Zimont Turbulent Flame Closure Theory
The turbulent premixed combustion model, based on work by Zimont et al. [390, 391,
393], involves the solution of a transport equation for the reaction progress variable. The
closure of this equation is based on the definition of the turbulent flame speed.
Information in this section is provided in the following sections:
• Section 9.2.1: Propagation of the Flame Front
• Section 9.2.2: Turbulent Flame Speed
9.2.1
Propagation of the Flame Front
In many industrial premixed systems, combustion takes place in a thin flame sheet.
As the flame front moves, combustion of unburnt reactants occurs, converting unburnt
premixed reactants to burnt products. The premixed combustion model thus considers
the reacting flow field to be divided into regions of burnt and unburnt species, separated
by the flame sheet.
The flame front propagation is modeled by solving a transport equation for the densityweighted mean reaction progress variable, denoted by c:
∂
µt
(ρc) + ∇ · (ρ~v c) = ∇ ·
∇c + ρSc
∂t
Sct
(9.2-1)
where
c
Sct
Sc
=
=
=
mean reaction progress variable
turbulent Schmidt number
reaction progress source term (s−1 )
The progress variable is defined as a normalized sum of the product species,
n
X
c=
Yi
i=1
n
X
(9.2-2)
Yi,eq
i=1
where
n
Yi
Yi,eq
= number of products
= mass fraction of product species i
= equilibrium mass fraction of product species i
Release 12.0 c ANSYS, Inc. January 29, 2009
9-3
Premixed Combustion
Based on this definition, c = 0 where the mixture is unburnt and c = 1 where the mixture
is burnt:
• c = 0: unburnt mixture
• c = 1: burnt mixture
The value of c is defined as a boundary condition at all flow inlets. It is usually specified
as either 0 (unburnt) or 1 (burnt).
The mean reaction rate in Equation 9.2-1 is modeled as [391]
ρSc = ρu Ut |∇c|
(9.2-3)
where
ρu
Ut
= density of unburnt mixture
= turbulent flame speed
Many other models for turbulent flame speed exist [36], and can be specified using userdefined functions. More information about user-defined functions can be found in the
separate UDF Manual.
9.2.2
Turbulent Flame Speed
The key to the premixed combustion model is the prediction of Ut , the turbulent flame
speed normal to the mean surface of the flame. The turbulent flame speed is influenced
by the following:
• laminar flame speed, which is, in turn, determined by the fuel concentration, temperature, and molecular diffusion properties, as well as the detailed chemical kinetics
• flame front wrinkling and stretching by large eddies, and flame thickening by small
eddies
In ANSYS FLUENT, the Zimont turbulent flame speed closure is computed using a model
for wrinkled and thickened flame fronts [391]:
1/2
1/4
Ut = A(u0 )3/4 Ul α−1/4 `t
1/4
τt
0
= Au
τc
9-4
(9.2-4)
(9.2-5)
Release 12.0 c ANSYS, Inc. January 29, 2009
9.2 Zimont Turbulent Flame Closure Theory
where
A
u0
Ul
α = k/ρcp
`t
τt = `t /u0
τc = α/Ul2
=
=
=
=
model constant
RMS (root-mean-square) velocity (m/s)
laminar flame speed (m/s)
molecular heat transfer coefficient of unburnt
mixture (thermal diffusivity) (m2 /s)
= turbulence length scale (m)
= turbulence time scale (s)
= chemical time scale (s)
The turbulence length scale, `t , is computed from
`t = CD
(u0 )3
(9.2-6)
where is the turbulence dissipation rate.
The model is based on the assumption of equilibrium small-scale turbulence inside the
laminar flame, resulting in a turbulent flame speed expression that is purely in terms
of the large-scale turbulent parameters. The default value of 0.52 for A is recommended [391], and is suitable for most premixed flames. The default value of 0.37 for CD
should also be suitable for most premixed flames.
The model is strictly applicable when the smallest turbulent eddies in the flow (the
Kolmogorov scales) are smaller than the flame thickness, and penetrate into the flame
zone. This is called the thin reaction zone combustion region, and can be quantified by
Karlovitz numbers, Ka, greater than unity. Ka is defined as
Ka =
v2
tl
= η2
tη
Ul
(9.2-7)
where
tl
tη
vη = (ν)1/4
ν
= characteristic flame time scale
= smallest (Kolmogorov) turbulence time scale
= Kolmogorov velocity
= kinematic viscosity
Lastly, the model is valid for premixed systems where the flame brush width increases in
time, as occurs in most industrial combustors. Flames that propagate for a long period
of time equilibrate to a constant flame width, which cannot be captured in this model.
Release 12.0 c ANSYS, Inc. January 29, 2009
9-5
Premixed Combustion
Turbulent Flame Speed for LES
For simulations that use the LES turbulence model, the Reynolds-averaged quantities in
the turbulent flame speed expression (Equation 9.2-4) are replaced by their equivalent
subgrid quantities. In particular, the large eddy length scale `t is modeled as
(9.2-8)
`t = Cs ∆
where Cs is the Smagorinsky constant and ∆ is the cell characteristic length.
The RMS velocity in Equation 9.2-4 is replaced by the subgrid velocity fluctuation,
calculated as
−1
u0 = `t τsgs
(9.2-9)
−1
where τsgs
is the subgrid scale mixing rate (inverse of the subgrid scale time scale), given
in Equation 7.1-28.
Laminar Flame Speed
The laminar flame speed (Ul in Equation 9.2.1) can be specified as constant, or as a
user-defined function. A third option appears for non-adiabatic premixed and partiallypremixed flames and is based on the correlation proposed by Meghalchi and Keck [227],
Ul = Ul,ref
Tu
Tu,ref
!γ
pu
!β
(9.2-10)
pu,ref
In Equation 9.2-10, Tu and pu are the unburnt reactant temperature and pressure ahead
of the flame, Tu,ref = 298K and pu,ref = 1atm.
The reference laminar flame speed, Ul,ref , is calculated from
Ul,ref = C1 + C2 (φ − C3 )2
(9.2-11)
where φ is the equivalence ratio ahead of the flame front, and C1 , C2 and C3 are fuelspecific constants. The exponents γ and β are calculated from,
γ = 2.18 − 0.8(φ − 1)
β = −0.16 + 0.22(φ − 1)
(9.2-12)
The Meghalchi-Keck laminar flame speeds are available for fuel-air mixtures of methane,
methanol, propane, iso-octane and indolene fuels.
9-6
Release 12.0 c ANSYS, Inc. January 29, 2009
9.2 Zimont Turbulent Flame Closure Theory
Unburnt Density and Thermal Diffusivity
The unburnt density (ρu in Equation 9.2.1) and unburnt thermal diffusivity (α in Equation 9.2-5) are specified constants that are set in the Materials dialog box. However, for
compressible cases, such as in-cylinder combustion, these can change significantly in time
and/or space. When the ideal gas model is selected for density, the unburnt density and
thermal diffusivity are calculated as volume averages ahead of the flame front.
Flame Stretch Effect
Since industrial low-emission combustors often operate near lean blow-off, flame stretching will have a significant effect on the mean turbulent heat release intensity. To take
this flame stretching into account, the source term for the progress variable (ρSc in Equation 9.2-1) is multiplied by a stretch factor, G [393]. This stretch factor represents the
probability that the stretching will not quench the flame; if there is no stretching (G = 1),
the probability that the flame will be unquenched is 100%.
The stretch factor, G, is obtained by integrating the log-normal distribution of the turbulence dissipation rate, :
s
1
1
cr
σ
ln
+
G = erfc −
2
2σ
2
(9.2-13)
where erfc is the complementary error function, and σ and cr are defined below.
σ is the standard deviation of the distribution of :
L
σ = µstr ln
η
!
(9.2-14)
where µstr is the stretch factor coefficient for dissipation pulsation, L is the turbulent
integral length scale, and η is the Kolmogorov micro-scale. The default value of 0.26 for
µstr (measured in turbulent non-reacting flows) is recommended by [391], and is suitable
for most premixed flames.
cr is the turbulence dissipation rate at the critical rate of strain [391]:
2
cr = 15νgcr
Release 12.0 c ANSYS, Inc. January 29, 2009
(9.2-15)
9-7
Premixed Combustion
By default, gcr is set to a very high value (1 × 108 ) so no flame stretching occurs. To
include flame stretching effects, the critical rate of strain gcr should be adjusted based on
experimental data for the burner. Numerical models can suggest a range of physically
plausible values [391], or an appropriate value can be determined from experimental data.
A reasonable model for the critical rate of strain gcr is
gcr =
BUl2
α
(9.2-16)
where B is a constant (typically 0.5) and α is the unburnt thermal diffusivity. Equation 9.2-16 can be implemented in ANSYS FLUENTusing a property user-defined function.
More information about user-defined functions can be found in the separate UDF Manual.
Gradient Diffusion
Volume expansion at the flame front can cause counter-gradient diffusion. This effect
becomes more pronounced when the ratio of the reactant density to the product density is large, and the turbulence intensity is small. It can be quantified by the ratio
(ρu /ρb )(Ul /I), where ρu , ρb , Ul , and I are the unburnt and burnt densities, laminar flame
speed, and turbulence intensity, respectively. Values of this ratio greater than one indicate a tendency for counter-gradient diffusion, and the premixed combustion model may
be inappropriate. Recent arguments for the validity of the turbulent-flame-speed model
in such regimes can be found in Zimont et al. [392].
Wall Damping
High turbulent kinetic energy levels at the walls in some problems can cause an unphysical
acceleration of the flame along the wall. In reality, radical quenching close to walls
decreases reaction rates and thus the flame speed, but is not included in the model. To
approximate this effect, ANSYS FLUENT includes a constant multiplier for the turbulent
flame speed, αw , which modifies the flame speed in the vicinity of wall boundaries:
τt
Ut = αw A
τc
1/4
(9.2-17)
The default for this constant is 1 which does not change the flame speed. Values of αw
larger than 1 increase the flame speed, while values less than 1 decrease the flame speed
in the cells next to the wall boundary.
9-8
Release 12.0 c ANSYS, Inc. January 29, 2009
9.3 Extended Coherent Flamelet Model Theory
ANSYS FLUENT will solve the transport equation for the reaction progress variable c
(Equation 9.2-1), computing the source term, ρSc , based on the theory outlined above:
1/4
ρSc = AGρu I 3/4 [Ul (λlp )]1/2 [α(λlp )]−1/4 `t |∇c|
"
= AGρu I
9.3
τt
τc (λlp )
(9.2-18)
#1/4
|∇c|
(9.2-19)
Extended Coherent Flamelet Model Theory
The Extended Coherent Flamelet Model (ECFM) [274] is a more refined premixed combustion model than the Zimont Turbulent Flame Closure. It has theoretically greater
accuracy, but is less robust and requires greater computational effort to converge.
Information in this section is provided in the following sections:
• Section 9.3.1: Closure for ECFM Source Terms
• Section 9.3.2: Turbulent Flame Speed in ECFM
The ECFM model solves an additional equation for the flame area density, denoted Σ,
which is ultimately used to model the mean reaction rate in Equation 9.2-1. The model
assumes that the smallest turbulence length scales (Kolmogorov eddies) are larger than
the laminar flame thickness, so the effect of turbulence is to wrinkle the laminar flame
sheet, however the internal laminar flame profile is not distorted. The increased surface
area of the flame results in increased net fuel consumption and an increased flame speed.
The range of applicability of the ECFM model is illustrated on the Borghi diagram in
Figure 9.3.1, where the wrinkled flamelets regime is indicated below the Da = 1 line.
Typical Internal Combustion (IC) engines typically operate in this wrinkled flamelet
range.
An expression for the transport of the net flame area per unit volume, or flame area
density, Σ, can be derived based on these assumptions [44]:
∂Σ
µt
Σ
+ ∇ · (~v Σ) = ∇ ·
∇
∂t
Sct
ρ
Release 12.0 c ANSYS, Inc. January 29, 2009
!!
+ (P1 + P2 + P3 ) Σ − D
(9.3-1)
9-9
Premixed Combustion
u0 /Ul
6
Thickened
Flames
Ka = 100
Thickened
Flamelets
Da = 1
10
@
@
@Ret = 1
@
@
@
@
1
'$
Ka = 1
&%
@
@
IC
Engines
@
Wrinkled
Flamelets
@
@
@
@
@
Laminar
Combustion
-
@
1
10
100
1000
lt /δl
Figure 9.3.1: Borghi diagram for turbulent combustion
where
Σ
Sct
µt
ρ
P1
P2
P3
D
=
=
=
=
=
=
=
=
mean flame area density
turbulent Schmidt number
turbulent viscosity
density
Source due to turbulence interaction
Source due to dilatation in the flame
Source due to expansion of burned gas
Dissipation of flame area
Equation 9.3-1 requires closure terms for the production and destruction terms for flame
area density. Several families of closure terms have been put forth in the literature [274].
ANSYS FLUENT uses the closure described in the following section.
9-10
Release 12.0 c ANSYS, Inc. January 29, 2009
9.3 Extended Coherent Flamelet Model Theory
9.3.1
Closure for ECFM Source Terms
P1 represents the production of flame area density by turbulent flame stretching, and is
modeled as
P1 = α1 Kt = α1 [(1 − α0 ) + α0 ΓK ]
k
(9.3-2)
where Kt is a turbulent time scale and α1 is a constant with a default value of 1.6. The
constant α0 (default of 1) is a user-specified linear blending between the Intermediate
Turbulent Net Flame Stretch (ITNFS) term, ΓK , for low turbulence levels at α0 = 1, and
a straightforward turbulent time scale source when α0 = 0 for high turbulence levels.
The ITNFS term, ΓK , can be specified either as a constant or calculated as a function
of the two parameters u0 /Ul and lt /δL0 , where u0 is the turbulent velocity fluctuation, Ul
is the laminar flame speed, lt is the integral turbulent length scale and δL0 is the laminar
flame thickness.
The expression for ΓK is given by:
1
u0
log10 (ΓK ) = −
exp (−(s + 0.4)) + (1 − exp (−(s + 0.4))) σ1
s − 0.11
(s + 0.4)
Ul
(9.3-3)
!
!
where s is defined as
s = log10
lt
δl0
!
(9.3-4)
and σ1 is
σ1
u0
Ul
!
2
1
u0
= 1 − exp −
3
2
Ul
! 1
3
(9.3-5)
The ITNFS term, ΓK , is sensitive to the laminar flame thickness. ANSYS FLUENT
provides several options for the calculation of this quantity:
• Constant (user-specified) value
• Meneveau Flame Thickness [223]
The laminar flame thickness is calculated as
δl0 =
Release 12.0 c ANSYS, Inc. January 29, 2009
2α
Ul
(9.3-6)
9-11
Premixed Combustion
where α is the local unburnt thermal diffusivity.
• Poinsot Flame Thickness [274]
The flame thickness is evaluated as in Equation 9.3-6 but an additional term, Γp is
added to ΓK . Γp is calculated as
3 lt Ul
1
Γp = −
log
0
2 δl u
1 − pq
!
(9.3-7)
where
pq
b
gl
s
=
=
=
=
− 12 (1 + tanh (b3 /|b|))
[log10 (u0 /Ul ) − gl ] /0.04s
(0.7 + es ) e−s + (1 + e−s ) (1 + 0.36s)
log10 (lt Ul /α)
• Blint Correction Flame Thickness [30]
This includes a correction due to rapid expansion of the gas:
δl0
Tb
=2
Tu
0.7
α
Ul
(9.3-8)
where Tu is the unburned temperature, and Tb denotes the burned temperature.
The term P2 in Equation 9.3-1 models the influence of dilatation on the production of
flame area density. The term is given by
2
P2 = α2 ∇ · (ρ~u)
3
(9.3-9)
where the constant α2 has a default of 1.
The term P3 models the effect of thermal expansion of the burned gas on the flame area
density, and is given by
P3 = α3
ρu 1 − c
Ul
Σ
ρb
c
(9.3-10)
where α3 is 1 by default.
The flame area destruction term D is modeled as
D = βUl
9-12
Σ2
1−c
(9.3-11)
Release 12.0 c ANSYS, Inc. January 29, 2009
9.4 Calculation of Temperature
where β is a constant with a default value of 1.
As formulated, the model can become singular for c = 0 and c = 1, which is handled by
limiting c. Further, the production terms P1 and P2 can be non-zero in regions where
the mixture is outside the flammability limits, which is unphysical. Accordingly, ANSYS
FLUENT sets the production terms to zero when the laminar flame speed is less than a
very small value. The stability of the solution is enhanced by ensuring that the laminar
flame speed in the destruction term is always greater than a small, finite value. Inspection
of the function for ΓK shows that a singularity exists in Equation 9.3-3 for s = -0.4 which
can occur when the turbulent integral length scale is small compared to the laminar flame
thickness. To prevent the singularity, the quantity (s + 0.4) is limited to a small positive
number. This results in a small net turbulent flame stretch term in laminar zones. These
numerical limiting constants can be adjusted in the TUI.
9.3.2
Turbulent Flame Speed in ECFM
The mean reaction rate term in the reaction progress variable Equation 9.2-1 is closed as
ρSc = ρu Ul Σ
(9.3-12)
which is the product of the unburnt density, ρu , laminar flame speed, Ul , and flame
surface area density, Σ.
9.4
Calculation of Temperature
The calculation method for temperature will depend on whether the model is adiabatic
or non-adiabatic.
9.4.1
Adiabatic Temperature Calculation
For the adiabatic premixed combustion model, the temperature is assumed to be a linear
function of reaction progress between the lowset temperature of the unburnt mixture,
Tu , and the highest adiabatic burnt temperature Tad :
T = (1 − c)Tu + cTad
9.4.2
(9.4-1)
Non-Adiabatic Temperature Calculation
For the non-adiabatic premixed combustion model, ANSYS FLUENT solves an energy
transport equation in order to account for any heat losses or gains within the system.
The energy equation in terms of sensible enthalpy, h, for the fully premixed fuel (see
Equation 5.2-3) is as follows:
Release 12.0 c ANSYS, Inc. January 29, 2009
9-13
Premixed Combustion
!
∂
k + kt
(ρh) + ∇ · (ρ~v h) = ∇ ·
∇h + Sh,chem + Sh,rad
∂t
cp
(9.4-2)
Sh,rad represents the heat losses due to radiation and Sh,chem represents the heat gains
due to chemical reaction:
Sh,chem = ρSc Hcomb Yfuel
(9.4-3)
where
Sc
Hcomb
Yfuel
9.5
=
=
=
normalized average rate of product formation (s−1 )
heat of combustion for burning 1 kg of fuel (J/kg)
fuel mass fraction of unburnt mixture
Calculation of Density
ANSYS FLUENT calculates the premxed density using the ideal gas law. For the adiabatic
model, pressure variations are neglected and the mean molecular weight is assumed to
be constant. The burnt gas density is then calculated from the following relation:
ρb Tb = ρu Tu
(9.5-1)
where the subscript u refers to the unburnt cold mixture, and the subscript b refers to
the burnt hot mixture. The required inputs are the unburnt density (ρu ), the unburnt
temperature (Tu ), and the burnt adiabatic flame temperature (Tb ).
For the non-adiabatic model, you can choose to either include or exclude pressure variations in the ideal gas equation of state. If you choose to ignore pressure fluctuations,
ANSYS FLUENT calculates the density from
ρT = ρu Tu
(9.5-2)
where T is computed from the energy transport equation, Equation 9.4-2. The required
inputs are the unburnt density (ρu ) and the unburnt temperature (Tu ). Note that, from
the incompressible ideal gas equation, the expression ρu RTu /pop may be considered to
be the effective molecular weight of the gas, where R is the gas constant and pop is the
operating pressure.
If you want to include pressure fluctuations for a compressible gas, you will need to input
the effective molecular weight of the gas, and the density will be calculated from the ideal
gas equation of state.
9-14
Release 12.0 c ANSYS, Inc. January 29, 2009
Chapter 10.
Partially Premixed Combustion
ANSYS FLUENT provides a partially premixed combustion model that is based on the
non-premixed combustion model described in Chapter 8: Non-Premixed Combustion and
the premixed combustion model described in Chapter 9: Premixed Combustion. For information about using the partially premixed combustion model, see Chapter 18: Modeling Partially Premixed Combustion in the separate User’s Guide. Information about
the theory behind the partially premixed combustion model is presented in the following
sections:
• Section 10.1: Overview and Limitations
• Section 10.2: Partially Premixed Combustion Theory
10.1
Overview and Limitations
10.1.1
Overview
Partially premixed combustion systems are premixed flames with non-uniform fuel-oxidizer
mixtures (equivalence ratios). Such flames include premixed jets discharging into a quiescent atmosphere, lean premixed combustors with diffusion pilot flames and/or cooling
air jets, and imperfectly premixed inlets.
The partially premixed model in ANSYS FLUENT is a simple combination of the nonpremixed model (Chapter 8: Non-Premixed Combustion) and the premixed model (Chapter 9: Premixed Combustion). The premixed reaction-progress variable, c, determines the
position of the flame front. Behind the flame front (c = 1), the mixture is burnt and
the equilibrium or laminar flamelet mixture fraction solution is used. Ahead of the flame
front (c = 0), the species mass fractions, temperature, and density are calculated from the
mixed but unburnt mixture fraction. Within the flame (0 < c < 1), a linear combination
of the unburnt and burnt mixtures is used.
10.1.2
Limitations
The underlying theory, assumptions, and limitations of the non-premixed and premixed
models apply directly to the partially premixed model. In particular, the single-mixturefraction approach is limited to two inlet streams, which may be pure fuel, pure oxidizer,
or a mixture of fuel and oxidizer. The two-mixture-fraction model extends the number
of inlet streams to three, but incurs a major computational overhead. See Sections 9.1.2
for additional limitations.
Release 12.0 c ANSYS, Inc. January 29, 2009
10-1
Partially Premixed Combustion
10.2
Partially Premixed Combustion Theory
The partially premixed model solves a transport equation for the mean reaction progress
variable, c (to determine the position of the flame front), as well as the mean mixture
fraction, f and the mixture fraction variance, f 0 2 . Ahead of the flame (c = 0), the fuel
and oxidizer are mixed but unburnt, and behind the flame (c = 1), the mixture is burnt.
10.2.1
Calculation of Scalar Quantities
Density weighted mean scalars (such as species fractions and temperature), denoted by
φ, are calculated from the probability density function (PDF) of f and c as
φ=
Z
0
1
Z
1
φ(f, c)p(f, c) df dc
(10.2-1)
0
Under the assumption of thin flames, so that only unburnt reactants and burnt products
exist, the mean scalars are determined from
φ=c
Z
0
1
φb (f )p(f ) df + (1 − c)
Z
0
1
φu (f )p(f ) df
(10.2-2)
where the subscripts b and u denote burnt and unburnt, respectively.
The burnt scalars, φb , are functions of the mixture fraction and are calculated by mixing
a mass f of fuel with a mass (1 − f ) of oxidizer and allowing the mixture to equilibrate.
When non-adiabatic mixtures and/or laminar flamelets are considered, φb is also a function of enthalpy and/or strain, but this does not alter the basic formulation. The unburnt
scalars, φu , are calculated similarly by mixing a mass f of fuel with a mass (1 − f ) of
oxidizer, but the mixture is not reacted.
Just as in the non-premixed model, the chemistry calculations and PDF integrations for
the burnt mixture are performed in ANSYS FLUENT, and look-up tables are constructed.
Turbulent fluctuations are neglected for the unburnt mixture, so the mean unburnt
scalars, φu , are functions of f only. The unburnt density, temperature, specific heat,
and thermal diffusivity are fitted in ANSYS FLUENT to third-order polynomials of f
using linear least squares:
φu =
3
X
cn f
n
(10.2-3)
n=0
Since the unburnt scalars are smooth and slowly-varying functions of f , these polynomial
fits are generally accurate. Access to polynomials is provided in case you want to modify
them.
10-2
Release 12.0 c ANSYS, Inc. January 29, 2009
10.2 Partially Premixed Combustion Theory
10.2.2
Laminar Flame Speed
The premixed models require the laminar flame speed (see Equation 9.2-4), which depends strongly on the composition, temperature, and pressure of the unburnt mixture.
For adiabatic perfectly premixed systems as in Chapter 9: Premixed Combustion, the
reactant stream has one composition, and the laminar flame speed is constant throughout the domain. However, in partially premixed systems, the laminar flame speed will
change as the reactant composition (equivalence ratio) changes, and this must be taken
into account.
Accurate laminar flame speeds are difficult to determine analytically, and are usually
measured from experiments or computed from 1D simulations. ANSYS FLUENT uses
fitted curves obtained from numerical simulations of the laminar flame speed [114]. These
curves were determined for hydrogen (H2 ), methane (CH4 ), acetylene (C2 H2 ), ethylene
(C2 H4 ), ethane (C2 H6 ), and propane (C3 H8 ) fuels. They are valid for inlet compositions
ranging from the lean limit through unity equivalence ratio (stoichiometric), for unburnt
temperatures from 298 K to 800 K, and for pressures from 1 bar to 40 bars.
ANSYS FLUENT fits these curves to a piecewise-linear polynomial. Mixtures leaner than
the lean limit or richer than the rich limit will not burn, and have zero flame speed. The
required inputs are values for the laminar flame speed at ten mixture fraction (f ) points.
The first (minimum) and last (maximum) f inputs are the flammability limits of the
mixture and the laminar flame speed is zero outside these value.
i
These flame speed fits are accurate for air mixtures with pure fuels of H2 ,
CH4 , C2 H2 , C2 H4 , C2 H6 , and C3 H8 . If an oxidizer other than air or a
different fuel is used, or if the unburnt temperature or pressure is outside
the range of validity, then the curve fits will be incorrect. Although ANSYS FLUENT defaults to a methane-air mixture, the laminar flame speed
polynomial and the rich and lean limits are most likely incorrect for your
specified fuel/oxidizer and unburnt temperature/pressure conditions. The
laminar flame speed polynomial should be determined from other sources,
such as measurements from the relevant literature or detailed 1D simulations, and then input into ANSYS FLUENT.
Release 12.0 c ANSYS, Inc. January 29, 2009
10-3
Partially Premixed Combustion
10-4
Release 12.0 c ANSYS, Inc. January 29, 2009
Chapter 11.
Composition PDF Transport
ANSYS FLUENT provides a composition PDF transport model for modeling finite-rate
chemistry effects in turbulent flames. For information about using the composition PDF
transport model, see Chapter 19: Modeling a Composition PDF Transport Problem in
the separate User’s Guide. Information about the theory behind this model is presented
in the following sections:
• Section 11.1: Overview and Limitations
• Section 11.2: Composition PDF Transport Theory
• Section 11.3: The Lagrangian Solution Method
• Section 11.4: The Eulerian Solution Method
11.1
Overview and Limitations
The composition PDF transport model, like the Laminar Finite-Rate (see Section 7.1.2: The
Laminar Finite-Rate Model) and EDC model (see Section 7.1.2: The Eddy-DissipationConcept (EDC) Model), should be used when you are interested in simulating finite-rate
chemical kinetic effects in turbulent reacting flows. With an appropriate chemical mechanism, kinetically-controlled species such as CO and NOx , as well as flame extinction and
ignition, can be predicted. PDF transport simulations are computationally expensive,
and it is recommended that you start your modeling with small meshes, and preferably
in 2D.
A limitation that applies to the composition PDF transport model is that you must use
the pressure-based solver as the model is not available with the density-based solver.
ANSYS FLUENT has two different discretizations of the composition PDF transport equation, namely Lagrangian and Eulerian. The Lagrangian method is strictly more accurate
than the Eulerian method, but requires significantly longer run time to converge.
Release 12.0 c ANSYS, Inc. January 29, 2009
11-1
Composition PDF Transport
11.2
Composition PDF Transport Theory
Turbulent combustion is governed by the reacting Navier-Stokes equations. While this
equation set is accurate, its direct solution (where all turbulent scales are resolved) is far
too expensive for practical turbulent flows. In Chapter 7: Species Transport and FiniteRate Chemistry, the species equations are Reynolds-averaged, which leads to unknown
terms for the turbulent scalar flux and the mean reaction rate. The turbulent scalar flux
is modeled in ANSYS FLUENT by gradient diffusion, treating turbulent convection as
enhanced diffusion. The mean reaction rate can be modeled with the Laminar, EddyDissipation or EDC Finite-Rate chemistry models. Since the reaction rate is invariably
highly non-linear, modeling the mean reaction rate in a turbulent flow is difficult and
prone to error.
An alternative to Reynolds-averaging the species and energy equations is to derive a
transport equation for their single-point, joint probability density function (PDF). This
PDF, denoted by P , can be considered to represent the fraction of the time that the
fluid spends at each species, temperature and pressure state. P has N + 2 dimensions
for the N species, temperature and pressure spaces. From the PDF, any single-point
thermo-chemical moment (e.g., mean or RMS temperature, mean reaction rate) can be
calculated. The composition PDF transport equation is derived from the Navier-Stokes
equations as [276]:
" *
+ #
i
∂
∂
∂
∂ h 00
∂
1 ∂Ji,k
(ρP ) +
(ρui P ) +
(ρSk P ) = −
ρhui |ψiP +
ρ
ψ P
∂t
∂xi
∂ψk
∂xi
∂ψk
ρ ∂xi
(11.2-1)
where
P
ρ
ui
Sk
ψ
00
ui
Ji,k
=
=
=
=
=
=
=
Favre joint PDF of composition
mean fluid density
Favre mean fluid velocity vector
reaction rate for specie k
composition space vector
fluid velocity fluctuation vector
molecular diffusion flux vector
The notation of h. . .i denotes expectations, and hA|Bi is the conditional probability of
event A, given that event B occurs.
11-2
Release 12.0 c ANSYS, Inc. January 29, 2009
11.3 The Lagrangian Solution Method
In Equation 11.2-1, the terms on the left-hand side are closed, while those on the righthand side are not and require modeling. The first term on the left-hand side is the
unsteady rate of change of the PDF, the second term is the change of the PDF due to
convection by the mean velocity field, and the third term is the change due to chemical
reactions. The principal strength of the PDF transport approach is that the highly-nonlinear reaction term is completely closed and requires no modeling. The two terms on
the right-hand side represent the PDF change due to scalar convection by turbulence
(turbulent scalar flux), and molecular mixing/diffusion, respectively.
The turbulent scalar flux term is unclosed, and is modeled in ANSYS FLUENT by the
gradient-diffusion assumption
i
∂ h 00
∂
−
ρhui |ψiP =
∂xi
∂xi
ρµt ∂P
Sct ∂xi
!
(11.2-2)
where µt is the turbulent viscosity and Sct is the turbulent Schmidt number. A turbulence
model, as described in Chapter 4: Turbulence, is required for composition PDF transport
simulations, and this determines µt .
Since single-point PDFs are described, information about neighboring points is missing
and all gradient terms, such as molecular mixing, are unclosed and must be modeled. The
mixing model is critical because combustion occurs at the smallest molecular scales when
reactants and heat diffuse together. Modeling mixing in PDF methods is not straightforward, and is the weakest link in the PDF transport approach. See Section 11.3.2: Particle
Mixing for a description of the mixing models.
11.3 The Lagrangian Solution Method
A Lagrangian Monte Carlo method is used to solve for the N + 1 dimensional PDF
Transport equation. Monte Carlo methods are appropriate for high-dimensional equations since the computational cost increases linearly with the number of dimensions.
The disadvantage is that statistical errors are introduced, and these must be carefully
controlled.
To solve the modeled PDF transport equation, an analogy is made with a stochastic
differential equation (SDE) which has identical solutions. The Monte Carlo algorithm
involves notional particles which move randomly through physical space due to particle
convection, and also through composition space due to molecular mixing and reaction.
The particles have mass and, on average, the sum of the particle masses in a cell equals
the cell mass (cell density times cell volume). Since practical meshes have large changes
in cell volumes, the particle masses are adjusted so that the number of particles in a cell
is controlled to be approximately constant and uniform.
Release 12.0 c ANSYS, Inc. January 29, 2009
11-3
Composition PDF Transport
The processes of convection, diffusion, and reaction are treated in fractional steps as
described in the sections that follow. For information on the fractional step method,
refer to [45].
Information about this method is described in the following sections:
• Section 11.3.1: Particle Convection
• Section 11.3.2: Particle Mixing
• Section 11.3.3: Particle Reaction
• Section 11.3.4: The ISAT Algorithm
11.3.1
Particle Convection
A spatially second-order-accurate Lagrangian method is used in ANSYS FLUENT, consisting of two steps. At the first convection step, particles are advanced to a new position
1/2
xi
1
= x0i + u0i ∆t
2
(11.3-1)
where
xi =
ui =
∆t =
particle position vector
Favre mean fluid-velocity vector at the particle position
particle time step
For unsteady flows, the particle time step is the physical time step. For steady-state
flows, local time steps are calculated for each cell as
∆t = min(∆tconv , ∆tdiff , ∆tmix )
(11.3-2)
where
∆tconv
∆tdiff
∆tmix
∆x
= convection number × ∆x / (cell fluid velocity)
= diffusion number × (∆x)2 / (cell turbulent diffusivity)
= mixing number × turbulent time scale
= characteristic cell length = volume1/D where D is the problem dimension
After the first convection step, all other sub-processes, including diffusion and reaction
are treated. Finally, the second convection step is calculated as
s
x1i
=
1/2
xi
+ ∆t
1/2
ui
1
1 ∂µt
2µt
− u0i +
+ ξi
2
ρSct ∂xi
ρ∆tSct
!
(11.3-3)
where
11-4
Release 12.0 c ANSYS, Inc. January 29, 2009
11.3 The Lagrangian Solution Method
ρ
ui
µt
Sct
ξi
= mean cell fluid density
= mean fluid-velocity vector at the particle position
= turbulent viscosity
= turbulent Schmidt number
= standardized normal random vector
11.3.2
Particle Mixing
Molecular mixing of species and heat must be modeled and is usually the source of the
largest modeling error in the PDF transport approach. ANSYS FLUENT provides three
models for molecular diffusion: the Modified Curl model [147, 250], the IEM model
(which is sometimes called the LSME model) [75] and the EMST model [340].
The Modified Curl Model
For the Modified Curl model, a few particle pairs are selected at random from all the
particles in a cell, and their individual compositions are moved toward their mean composition. For the special case of equal particle mass, the number of particle pairs selected
is calculated as
Npair =
1.5Cφ N ∆t
τt
(11.3-4)
where
N
Cφ
τt
=
=
=
total number of particles in the cell
mixing constant (default = 2)
turbulent time scale (for the k- model this is k/)
The algorithm in [250] is used for the general case of variable particle mass.
For each particle pair, a uniform random number ξ is selected and each particle’s composition φ is moved toward the pair’s mean composition by a factor proportional to ξ:
(φ0i mi + φ0j mj )
= (1 −
+ξ
(mi + mj )
0
(φ mi + φ0j mj )
φ1j = (1 − ξ)φ0j + ξ i
(mi + mj )
φ1i
ξ)φ0i
(11.3-5)
where φi and φj are the composition vectors of particles i and j, and mi and mj are the
masses of particles i and j.
Release 12.0 c ANSYS, Inc. January 29, 2009
11-5
Composition PDF Transport
The IEM Model
For the Interaction by Exchange with the Mean (IEM) model, the composition of all
particles in a cell are moved a small distance toward the mean composition:
φ1 = φ0 − 1 − e−0.5Cφ /τt
φ0 − φ̃
(11.3-6)
where φ0 is the composition before mixing, φ1 is the composition after mixing, and φ̃ is
the Favre mean-composition vector at the particle’s location.
The EMST Model
Physically, mixing occurs between fluid particles that are adjacent to each other. The
Modified Curl and IEM mixing models take no account of this localness, which can be a
source of error. The Euclidean Minimum Spanning Tree (EMST) model mixes particle
pairs that are close to each other in composition space. Since scalar fields are locally
smooth, particles that are close in composition space are likely to be close in physical
space. The particle pairing is determined by a Euclidean Minimum Spanning Tree, which
is the minimum length of the set of edges connecting one particle to at least one other
particle. The EMST mixing model is more accurate than the Modified Curl and IEM
mixing models, but incurs a slightly greater computational expense. Details on the EMST
model can be found in reference [340].
Liquid Reactions
Reactions in liquids often occur at low turbulence levels (small Re), among reactants
with low diffusivities (large Sc). For such flows, the mixing constant default of Cφ = 2
overestimates the mixing rate. The Liquid Micro-Mixing option interpolates Cφ from
model turbulence [278] and scalar [103] spectra.
11.3.3
Particle Reaction
The particle composition vector is represented as
φ = (Y1 , Y2 , . . . , YN , T, p)
(11.3-7)
where Yk is the kth specie mass fraction, T is the temperature and p the pressure.
For the reaction fractional step, the reaction source term is integrated as
φ1 = φ0 +
Z
∆t
Sdt
(11.3-8)
0
11-6
Release 12.0 c ANSYS, Inc. January 29, 2009
11.3 The Lagrangian Solution Method
where S is the chemical source term. Most realistic chemical mechanisms consist of
tens of species and hundreds of reactions. Typically, a reaction does not occur until
an ignition temperature is reached, but then proceeds very quickly until reactants are
consumed. Hence, some reactions have very fast time scales, in the order of 10−10 s, while
others have much slower time scales, on the order of 1 s. This time-scale disparity results
in numerical stiffness, which means that extensive computational work is required to
integrate the chemical source term in Equation 11.3-8. In ANSYS FLUENT, the reaction
step (i.e., the calculation of φ1 ) can be performed either by Direct Integration or by
In-Situ Adaptive Tabulation (ISAT), as described in the following paragraphs.
A typical steady-state PDF transport simulation in ANSYS FLUENT may have 50000
cells, with 20 particles per cell, and requires 1000 iterations to converge. Hence, at least
109 stiff ODE integrations are required. Since each integration typically takes tens or
hundreds of milliseconds, on average, the direct integration of the chemistry is extremely
CPU-demanding.
For a given reaction mechanism, Equation 11.3-8 may be considered as a mapping. With
an initial composition vector φ0 , the final state φ1 depends only on φ0 and the mapping
time ∆t. In theory, if a table could be built before the simulation, covering all realizable
φ0 states and time steps, the integrations could be avoided by table look-ups. In practice,
this a priori tabulation is not feasible since a full table in N + 3 dimensions (N species,
temperature, pressure and time-step) is required. To illustrate this, consider a structured
table with M points in each dimension. The required table size is M N +3 , and for a
conservative estimate of M = 10 discretization points and N = 7 species, the table
would contain 1010 entries.
On closer examination, the full storage of the entire realizable space is very wasteful
because most regions are never accessed. For example, it would be unrealistic to find a
composition of YOH = 1 and T = 300K in a real combustor. In fact, for steady-state, 3D
laminar simulations, the chemistry can be parameterized by the spatial position vector.
Thus, mappings must lie on a three dimensional manifold within the N + 3 dimensional
composition space. It is, hence, sufficient to tabulate only this accessed region of the
composition space.
The accessed region, however, depends on the particular chemical mechanism, molecular
transport properties, flow geometry, and boundary conditions. For this reason, the accessed region is not known before the simulation and the table cannot be preprocessed.
Instead, the table must be built during the simulation, and this is referred to as in-situ
tabulation. ANSYS FLUENT employs ISAT [277] to dynamically tabulate the chemistry
mappings and accelerate the time to solution. ISAT is a method to tabulate the accessed
composition space region “on the fly” (in-situ) with error control (adaptive tabulation).
When ISAT is used correctly, accelerations of two to three orders of magnitude are typical.
However, it is important to understand how ISAT works in order to use it optimally.
Release 12.0 c ANSYS, Inc. January 29, 2009
11-7
Composition PDF Transport
11.3.4
The ISAT Algorithm
ISAT is a powerful tool that enables realistic chemistry to be incorporated in multidimensional flow simulations by accelerating the chemistry calculations. Typical speedups of 100-fold are common. This power is apparent if one considers that with a 100-fold
speed-up, a simulation that would take three months without ISAT can be run in one
day.
At the start of an ANSYS FLUENT simulation using ISAT, the ISAT table is empty. For
the first reaction step, Equation 11.3-8 is integrated with a stiff ODE solver. This is
called Direct Integration (DI). The first table entry is created and consists of:
• the initial composition φ0
• the mapping φ1
• the mapping gradient matrix A = ∂φ1 /∂φ0
• a hyper-ellipsoid of accuracy
The next reaction mapping is calculated as follows: The initial composition vector for
this particle is denoted φ0q , where the subscript q denotes a query. The existing table
(consisting of one entry at this stage) is queried by interpolating the new mapping as
φ1q = φ1 + A(φ0q − φ0 )
(11.3-9)
The mapping gradient is hence used to linearly interpolate the table when queried. The
ellipsoid of accuracy (EOA) is the elliptical space around the table point φ0 where the
linear approximation to the mapping is accurate to the specified tolerance, tol .
If the query point φ1q is within the EOA, then the linear interpolation by Equation 11.3-9
is sufficiently accurate, and the mapping is retrieved. Otherwise, a direct integration (DI)
is performed and the mapping error = |B(φ1DI − φ1q )| is calculated (here, B is a scaling
matrix). If this error is smaller than the specified error tolerance ( < tol ), then the
original interpolation φ1q is accurate and the EOA is grown so as to include φ0q . If not, a
new table entry is added.
Table entries are stored as leaves in a binary tree. When a new table entry is added,
the original leaf becomes a node with two leaves—the original leaf and the new entry.
A cutting hyper-plane is created at the new node, so that the two leaves are on either
side of this cutting plane. A composition vector φ0q will hence lie on either side of this
hyper-plane.
11-8
Release 12.0 c ANSYS, Inc. January 29, 2009
11.4 The Eulerian Solution Method
The ISAT algorithm is summarized as follows:
1. The ISAT table is queried for every composition vector during the reaction step.
2. For each query φ0q the table is traversed to identify a leaf whose composition φ0 is
close to φ0q .
3. If the query composition φ0q lies within the EOA of the leaf, then the mapping φ1q
is retrieved using interpolation by Equation 11.3-9. Otherwise, Direct Integration
(DI) is performed and the error between the DI and the linear interpolation is
measured.
4. If the error is less than the tolerance, then the ellipsoid of accuracy is grown and
the DI result is returned. Otherwise, a new table entry is added.
At the start of the simulation, most operations are adds and grows. Later, as more of
the composition space is tabulated, retrieves become frequent. Since adds and grows are
very slow whereas retrieves are relatively quick, initial ANSYS FLUENT iterations are
slow but accelerate as the table is built.
11.4
The Eulerian Solution Method
The Lagrangian solution method solves the composition PDF transport equation by
stochastically tracking Lagrangian particles through the domain. It is computationally
expensive since a large number of particles are required to represent the PDF, and a
large number of iterations are necessary to reduce statistical errors and explicitly convect
the particles through the domain. The Eulerian PDF transport model overcomes these
limitations by assuming a shape for the PDF, which allows Eulerian transport equations
to be derived. Stochastic errors are eliminated and the transport equations are solved
implicitly, which is computationally economical. The multi-dimensional PDF shape is
assumed as a product of delta functions. As with the Lagrangian PDF model, the
highly non-linear chemical source term is closed. However, the turbulent scalar flux and
molecular mixing terms must be modeled, and are closed with the gradient diffusion and
the IEM models, respectively.
The composition PDF of Ns + 1 dimension (Ns species and enthalpy) is represented as a
collection of Ne delta functions (or modes). This presumed PDF has the following form:
P (ψ; ~x, t) =
Ne
X
n=1
pn (~x, t)
Ns
Y
δ[ψk − < φk >n (~x, t)]
(11.4-1)
k=1
where pn is the probability in each mode, < φk >n is the conditional mean composition
of specie k in the nth mode, ψk is the composition space variable of specie k, and δ(. . .)
is the delta function.
Release 12.0 c ANSYS, Inc. January 29, 2009
11-9
Composition PDF Transport
The Eulerian PDF transport equations are derived by substituting Equation 11.4-1 into
the closed composition PDF transport equation (Equation 11.2-1 with Equations 11.2-2
and 11.3-6). The unknown terms, pn and < φk >n , are determined by forcing lower
moments of this transported PDF to match the RANS lower moment transport equations,
using the Direct Quadrature Method of Moments (DQMOM) approach [103, 218]. The
resulting transport equations are:
• Probability (magnitude of the nth delta function):
∂ρpn
∂
+
(ρui pn ) = ∇(ρΓ∇pn )
∂t
∂xi
(11.4-2)
• Probability weighted conditional mean of composition k:
∂ρsk,n
∂
+
(ρui sk,n ) = ∇(ρΓ∇sk,n ) + ρ(Mk,n + Sk,n + Ck,n )
∂t
∂xi
(11.4-3)
where pn is the probability of the nth mode, and sk,n = pn < φk >n is the kth specie
probability weighted conditional mean composition of the nth mode. Γ = µl + µt /Sct
is the effective turbulent diffusivity. The terms Mk,n , Sk,n and Ck,n represent mixing,
reaction and correction terms respectively. Note that only Ne − 1 probability equations
are solved and the N th probability is calculated as one minus the sum of the Ne − 1
solved probabilities.
Reaction
The reaction source term Sk,n in Equation 11.4-3 for the kth composition and the nth
mode is calculated as,
Sk,n = pn S(< φk >n )k
(11.4-4)
where S()k is the net reaction rate for the kth component.
Mixing
The micro-mixing term Mk,n is modeled with the IEM mixing model:
Mk,n =
Cφ
(< φk >n −ψk )
τ
(11.4-5)
where τ is the turbulence time-scale and Cφ is the mixing constant.
Hence, for the two-mode DQMOM-IEM model, the mixing terms for component k are,
11-10
Release 12.0 c ANSYS, Inc. January 29, 2009
11.4 The Eulerian Solution Method
Cφ
(p1 sk,2 − p2 sk,1 )
τ
Cφ
=
(p2 sk,1 − p1 sk,2 )
τ
Mk,1 =
Mk,2
(11.4-6)
The default value of Cφ is 2, which is appropriate for gas-phase combustion. For reactions
in liquids, where the diffusivities are much smaller than gases, the Liquid Micro-Mixing
option interpolates Cφ from model turbulence [278] and scalar [103] spectra.
Correction
Using assumptions to ensure realizability and boundedness, the correction terms Ck,n in
Equation 11.4-3 for the kth composition are determined from the linear system,
Ne
X
k −1
< φk >m
Ck,n =
n
n=1
Ne
X
k −2
(mk − 1) < φk >m
pn ck,n
n
(11.4-7)
n=1
where mk are the non-negative integer lower moments (1..Ne ) for each component k.
Note that the condition of the matrix decreases with increasing mk , which reduces the
stability of higher mode simulations.
The dissipation term ck,n in Equation 11.4-7 is calculated as,
ck,n = Γ∇(< φk >n ) · ∇(< φk >n )
(11.4-8)
For the two-mode DQMOM-IEM model, the correction terms for the kth component are,
Γ
p1 (∇ < φk >1 )2 + p2 (∇ < φk >2 )2
< φk >1 − < φk >2
= −Ck,1
Ck,1 =
Ck,2
(11.4-9)
Calculation of Composition Mean and Variance
The mean composition (specie k or energy) is calculated as,
φk =
Ne
X
sk,n
(11.4-10)
n=1
and its variance is calculated as
0
φk2 = (
Ne
X
sk,n < φk >n ) − φk
2
(11.4-11)
n=1
Release 12.0 c ANSYS, Inc. January 29, 2009
11-11
Composition PDF Transport
11-12
Release 12.0 c ANSYS, Inc. January 29, 2009
Chapter 12.
Engine Ignition
This chapter discusses the theory behind the engine ignition models available in ANSYS
FLUENT. Information can be found in the following sections.
• Section 12.1: Spark Model
• Section 12.2: Autoignition Models
• Section 12.3: Crevice Model
For information about using these ignition models, see Chapter 20: Modeling Engine
Ignition in the separate User’s Guide.
12.1
Spark Model
The spark model in ANSYS FLUENT will be described in the context of the premixed turbulent combustion model. For information about using this model, see Section 20.1: Spark
Model in the separate User’s Guide. Information regarding the theory behind this model
is detailed in the following sections:
• Section 12.1.1: Overview and Limitations
• Section 12.1.2: Spark Model Theory
12.1.1
Overview and Limitations
Initiation of combustion at a desired time and location in a combustion chamber can be
accomplished by sending a high voltage across two narrowly separated wires, creating
a spark. The spark event in typical engines happens very quickly relative to the main
combustion in the engine. The physical description of this simple event is very involved
and complex, making it difficult to accurately model the spark in the context of a multidimensional engine simulation. Additionally, the energy from the spark event is several
orders of magnitude less than the chemical energy release from the fuel. Despite the
amount of research devoted to spark ignition physics and ignition devices, the ignition
of a mixture at a point in the domain is more dependent on the local composition than
on the spark energy (see Heywood [128]). Thus, for situations in which ANSYS FLUENT
is utilized for combustion engine modeling, including internal combustion engines, the
Release 12.0 c ANSYS, Inc. January 29, 2009
12-1
Engine Ignition
spark event does not need to be modeled in great detail, but simply as the initiation of
combustion over a duration, which you will set.
Since spark ignition is inherently transient, the spark model is only available in the
transient solver. Additionally, the spark model requires chemical reactions to be solved.
The spark model is available for all of the combustion models, however, it may be most
applicable to the premixed and partially premixed combustion models.
The Spark Model used in ANSYS FLUENT is based on a one-dimensional analysis by Lipatnikov [203]. The model is sensitive to perturbations and can be subject to instabilities
when used in multi-dimensional simulations. The instabilities are inherent to the model
and can be dependent on the mesh, especially near the beginning of the spark event
when the model reduces diffusion to simulate the initial laminar spark kernel growth.
The instability is susceptible to numerical errors which are increased when the mesh is
not aligned with the flame propagation. As the spark kernel grows and the model allows
turbulent mixing to occur, the effect of the instability decreases.
12.1.2
Spark Model Theory
The spark model in ANSYS FLUENT is based on the work done by Lipatnikov [203] and
extended to other combustion models. The derivation of the model can be done in the
context of the Zimont premixed combustion model.
Zimont Premixed Flame Model
The transport equation for the mean reaction progress variable, c, is given by Equation 12.1-1
∂ρc
+ ∇ · (ρ~v c) = ∇ · (Dt ∇c) + ρu Ut |∇c|
∂t
(12.1-1)
where Dt is the turbulent diffusivity, ρu is the density of the unburned mixture and Ut
is the turbulent flame speed. Since the spark is often very small compared to the mesh
size of the model and is often laminar in nature, the Zimont model is modified such that
∂ρc
+ ∇ · (ρ~v c) = ∇ · ((κ + Dtt )∇c) + ρu Ut |∇c|
∂t
(12.1-2)
where κ is the laminar thermal diffusivity and the effective diffusivity Dtt is given by
(
Dtt =
Dt 1 − exp
Dt
−ttd
τ0
if ttd ≥ 0
if ttd < 0
(12.1-3)
where is ttd = t−tig and tig denotes the time at which the spark is initiated. Additionally,
τ 0 is an effective diffusion time, which you can set.
12-2
Release 12.0 c ANSYS, Inc. January 29, 2009
12.2 Autoignition Models
Only turbulent scales that are smaller than the spark radius can contribute to turbulent
spark diffusion, so the expression for the effective turbulent diffusivity, Dtt , is ramped up
as the spark grows. This creates higher temperatures at the location of the spark and
can cause convergence difficulties. In addition to convergence difficulties, small changes
in the diffusion time can change the result significantly. Because of these issues, the
diffusion time can be controlled by the you, and has a default value of 1e-5 seconds.
Other Combustion Models
The spark model is compatible with all combustion models in ANSYS FLUENT. However,
the premixed and partially premixed models differ in that the progress variable inside
the spark region is set equal to 1, a burned state, for the duration of the spark event.
Other combustion models have the energy input into the cell. If the temperature exceeds
2500 K or the spark duration is exceeded, no energy from the spark model will be added
to the spark cells.
The spark model can be used in models other than the premixed and partially premixed
combustion models, however, you must balance energy input and diffusivity to produce a
high enough temperature to initiate combustion, which can be a nontrivial undertaking.
The model’s use has been extended to be compatible with the other models, however,
in some cases it simply creates a high temperature region and does not guarantee the
initiation of combustion.
12.2
Autoignition Models
Autoignition phenomena in engines are due to the effects of chemical kinetics of the
reacting flow inside the cylinder. There are two types of autoignition models considered
in ANSYS FLUENT:
• knock model in spark-ignited (SI) engines
• ignition delay model in diesel engines
For information regarding using autoignition models, see Section 20.2: Autoignition
Models in the separate User’s Guide. The theory behind the autoignition models is
described in the following sections:
• Section 12.2.1: Overview and Limitations
• Section 12.2.2: Ignition Model Theory
Release 12.0 c ANSYS, Inc. January 29, 2009
12-3
Engine Ignition
12.2.1
Overview and Limitations
Overview
The concept of knock has been studied extensively in the context of premixed engines,
as it defines a limit in terms of efficiency and power production of that type of engine.
As the compression ratio increases, the efficiency of the engine as a function of the work
extracted from the fuel increases.
However, as the compression ratio increases, the temperature and pressure of the air/fuel
mixture in the cylinder also increase during the cycle compressions. The temperature
and pressure increase can be large enough for the mixture to spontaneously ignite and
release its heat before the spark plug fires. The premature release of all of the energy
in the air/fuel charge is almost never desirable, as this results in the spark event no
longer controlling the combustion. As a result of the premature release of the energy,
catastrophic damage to the engine components can occur. The sudden, sharp rise in
pressure inside the engine can be heard clearly through the engine block as a knocking
sound, hence the term “knock”. For commonly available gasoline pumps, knock usually
limits the highest practical compression ratio to less than 11:1 for premium fuels and
around 9:1 for less expensive fuels.
By comparison, ignition delay in diesel engines has not been as extensively studied as
SI engines, mainly because it does not have such a sharply defining impact on engine
efficiency. Ignition delay in diesel engines refers to the time between when the fuel is
injected into the combustion chamber and when the pressure starts to increase as the
fuel releases its energy. The fuel is injected into a gas which is usually air, however, it can
have a considerable amount of exhaust gas mixed in (or EGR) to reduce nitrogen oxide
emissions (NOx). Ignition delay depends on the composition of the gas in the cylinder,
the temperature of the gas, the turbulence level, and other factors. Since ignition delay
changes the combustion phasing, which in turn impacts efficiency and emissions, it is
important to account for it in a diesel engine simulation.
Model Limitations
The main difference between the knock model and the ignition delay model is the manner
in which the model is coupled with the chemistry. The knock model always releases
energy from the fuel while the ignition delay model prevents energy from being released
prematurely.
The knock model in ANSYS FLUENT is compatible with the premixed and partially
premixed combustion models. The autoignition model is compatible with any volumetric
combustion model, with the exception of the purely premixed models. The autoignition
models are inherently transient and so are not available with steady simulations.
12-4
Release 12.0 c ANSYS, Inc. January 29, 2009
12.2 Autoignition Models
The autoignition models in general require adjustment of parameters to reproduce engine
data and are likely to require tuning to improve accuracy. Once the model is calibrated to
a particular engine configuration, then different engine speeds and loads can be reasonably
well represented. Detailed chemical kinetics may be more applicable over a wider range of
conditions, though are more expensive to solve. The single equation autoignition models
are appropriate for the situation where geometric fidelity or resolution of particular flow
details is more important than chemical effects on the simulation.
12.2.2 Ignition Model Theory
Both the knock and the ignition delay models are treated similarly in ANSYS FLUENT,
in that they share the same infrastructure. These models belong to the family of single equation autoignition models and use correlations to account for complex chemical
kinetics. They differ from the eight step reaction models, such as Halstead’s “Shell”
model [121], in that only a single transport equation is solved. The source term in the
transport equation is typically not stiff, thus making the equation relatively inexpensive
to solve.
This approach is appropriate for large simulations where geometric accuracy is more important than fully resolved chemical kinetics. The model can be used on less resolved
meshes to explore a range of designs quickly, and to obtain trends before utilizing more
expensive and presumably more accurate chemical mechanisms in multidimensional simulations.
Transport of Ignition Species
Autoignition is modeled using the transport equation for an Ignition Species, Yig , which
is given by
∂ρYig
µt
+ ∇ · (ρ~v Yig ) = ∇ ·
∇Yig + ρSig
∂t
Sct
(12.2-1)
where Yig is a “mass fraction” of a passive species representing radicals which form when
the fuel in the domain breaks down. Sct is the turbulent Schmidt number. The term Sig
is the source term for the ignition species which has a form
Sig =
Z
t
t=t0
dt
τig
where t0 corresponds to the time at which fuel is introduced into the domain. The τig
term is a correlation of ignition delay with the units of time. Ignition has occurred when
the ignition species reaches a value of 1 in the domain. It is assumed that all the radical
species represented by Yig diffuse at the same rate as the mean flow.
Release 12.0 c ANSYS, Inc. January 29, 2009
12-5
Engine Ignition
Note that the source term for these radical species is treated differently for knock and
ignition delay. Furthermore, the form of the correlation of ignition delay differs between
the two models. Details of how the source term is treated are covered in the following
sections.
Knock Modeling
When modeling knock or ignition delay, chemical energy in the fuel is released when
the ignition species reaches a value of 1 in the domain. For the knock model, two
correlations are built into ANSYS FLUENT. One is given by Douaud [76], while the other
is a generalized model which reproduces several correlations, given by Heywood [128].
Modeling of the Source Term
In order to model knock in a physically realistic manner, the source term is accumulated under appropriate conditions in a cell. Consider the one dimensional flame in
Figure 12.2.1. Here, the flame is propagating from left to right, and the temperature is
relatively low in front of the flame and high behind the flame. In this figure, Tb and Tu
represent the temperatures at the burned and unburned states, respectively. The ignition
species accumulates only when there is fuel. In the premixed model, the fuel is defined
as f uel = 1 − c, where c is the progress variable. If the progress variable has a value of
zero, the mixture is considered unburned. If the progress variable is 1, then the mixture
is considered burned.
T
6
Tb
fuel = 0
Sig = 0
Tu
fuel > 0
Sig > 0
-
X
Figure 12.2.1: Flame Front Showing Accumulation of Source Terms for the
Knock Model
When the ignition species reaches a value of 1 in the domain, knock has occurred at that
point. The value of the ignition species can exceed unity. In fact, values well above that
can be obtained in a short time. The ignition species will continue to accumulate until
there is no more fuel present.
12-6
Release 12.0 c ANSYS, Inc. January 29, 2009
12.2 Autoignition Models
Correlations
An extensively tested correlation for knock in SI engines is given by Douaud and Eyzat [76]:
ON
τ = 0.01768
100
3.402
p
−1.7
3800
exp
T
(12.2-2)
where ON is the octane number of the fuel, p is the absolute pressure in atmospheres
and T is the temperature in Kelvin.
A generalized expression for τ is also available which can reproduce many existing Arrhenius correlations. The form of the correlation is
τ =A
ON
100
a
pb T c RPMd Φd exp
−Ea
RT
(12.2-3)
where A is the pre-exponential (with units in seconds), RPM is the engine speed in cycles
per minute and Φ is the fuel/air equivalence ratio.
Energy Release
Once ignition has occurred in the domain, the knock event is modeled by releasing the
remaining fuel energy with a single-step Arrhenius reaction. An additional source term,
which burns the remaining fuel in that cell, is added to the rate term in the premixed
model. The reaction rate is given by
ω̇ = A0 exp
−Ea
RT
(12.2-4)
where A0 = 8.6 × 109 , and Ea = −15078. These values are chosen to reflect single-step
reaction rates appropriate for propane as described in Amsden [4]. The rate at which the
fuel is consumed is limited such that a completely unburned cell will burn during three of
the current time steps. Limiting the reaction rate is done purely for numerical stability.
Ignition Delay Modeling
When modeling ignition delay in diesel engines, chemical reactions are allowed to occur
when the ignition species reaches a value of 1 in the domain. For the ignition delay model,
two correlations are built into ANSYS FLUENT, one given by Hardenburg and Hase [125]
and the other, a generalized model which reproduces several Arrhenius correlations from
the literature.
Release 12.0 c ANSYS, Inc. January 29, 2009
12-7
Engine Ignition
If the ignition species is less than 1 when using the ignition delay model, the chemical
source term is suppressed by not activating the combustion model at that particular time
step; thus, the energy release is delayed. This approach is reasonable if you have a good
high-temperature chemical model, but does not wish to solve for typically expensive low
temperature chemistry.
Modeling of the Source Term
In order to model ignition in a physically realistic manner, the source term is accumulated
under appropriate conditions in a cell. Consider the one dimensional spray in Figure
12.2.2. Here, the spray is propagating from left to right and the fuel mass fraction is
Yf uel 6
fuel > 0
Sig > 0
fuel = 0
Sig = 0
-
X
Figure 12.2.2: Propagating Fuel Cloud Showing Accumulation of Source
Terms for the Ignition Delay Model
relatively low in front of the spray and high behind the spray. If there is no fuel in the
cell, the model will set the local source term to zero, nevertheless, the value of Yig can
be nonzero due to convection and diffusion.
Correlations
If fuel is present in the cell, there are two built-in options in ANSYS FLUENT to calculate
the local source term. The first correlation was done by Hardenburg and Hase and was
developed at Daimler Chrysler for heavy duty diesel engines. The correlation works over
a reasonably wide range of conditions and is given by
!
τid =
12-8
"
!
C1 + 0.22S p
1
1
21.2
exp Ea
−
+
6N
RT
17, 190
p − 12.4
!ep #
(12.2-5)
Release 12.0 c ANSYS, Inc. January 29, 2009
12.3 Crevice Model
where τid is in seconds, C1 is 0.36, N is engine speed in revolutions per minute, Ea is
the effective activation energy and ep is the pressure exponent. The expression for the
effective activation energy is given by
Ea =
Ehh
CN + 25
(12.2-6)
where CN is the cetane number. The activation energy, Ehh , pre-exponential, C1 , pressure exponent, ep , and cetane number, CN , are accessible from the GUI. The default
values of these variables are listed in the table below.
Table 12.2.1: Default Values of the Variables in the Hardenburg Correlation
Variable
Default
Ehh
618,840
CN
25
C1
0.36
ep
0.63
The second correlation, which is the generalized correlation, is given by Equation 12.2-3
and is available for ignition delay calculations.
Energy Release
If the ignition species is greater than or equal to 1 anywhere in the domain, ignition has
occurred and combustion is no longer delayed. The ignition species acts as a switch to
turn on the volumetric reactions in the domain. Note that the ignition species “mass
fraction” can exceed 1 in the domain, therefore, it is not truly a mass fraction, but rather
a passive scalar which represents the integrated correlation as a function of time.
12.3
Crevice Model
This section describes the theory behind the crevice model. Information can be found in
the following sections:
• Section 12.3.1: Overview
• Section 12.3.2: Limitations
• Section 12.3.3: Crevice Model Theory
For information regarding using the crevice model, see Section 20.3: Crevice Model in
the separate User’s Guide.
Release 12.0 c ANSYS, Inc. January 29, 2009
12-9
Engine Ignition
12.3.1
Overview
The crevice model implemented in ANSYS FLUENT is a zero-dimensional ring-flow model
based on the model outlined in Namazian and Heywood [245] and Roberts and Matthews [295].
The model is geared toward in-cylinder specific flows, and more specifically, directinjection (DI) diesel engines, and thus is available only for time-dependent simulations.
The model takes mass, momentum, and energy from cells adjoining two boundaries and
accounts for the storage of mass in the volumes of the crevices in the piston. Detailed
geometric information regarding the ring and piston—typically a ring pack around the
bore of an engine—is necessary to use the crevice model. An example representation is
shown in Figures 12.3.1–12.3.3.
Cylinder
wall
Land length
1
p
0
Ring spacing
2
3
Piston to bore
clearance
1: Top gap
2: Middle gap
3: Bottom gap
p
6
Figure 12.3.1: Crevice Model Geometry (Piston)
Wr
Tr
Figure 12.3.2: Crevice Model Geometry (Ring)
12-10
Release 12.0 c ANSYS, Inc. January 29, 2009
12.3 Crevice Model
Ring 1
Ring 2
Ring 3
p
1•
p•
3
p•
5
p = cylinder pressure
• 0
• p2
• p4
• p = crankcase pressure
6
Figure 12.3.3: Crevice Model “Network” Representation
Model Parameters
• The piston to bore clearance is the distance between the piston and the bore. Typical values are 2 to 5 mil (80 to 120 µm) in a spark engine (SI) and 4 to 7 mil
(100 to 240 µm) in some diesel engines (DI).
• The ring thickness is the variable Tr in Figure 12.3.2. Typical values range from
1 to 3 mm for SI engines and 2 to 4 mm for DI engines.
• The ring width is the variable Wr in Figure 12.3.2. Typical values range from 3 to
3.5 mm for SI engines and 4 to 6 mm for DI diesel engines.
• The ring spacing is the distance between the bottom of one ring land and the top of
the next ring land. Typical values of the ring spacing are 3 to 5 mm for SI engines
and 4 to 8 mm for DI diesel engines.
• The land length is the depth of the ring land (i.e., the cutout into the piston);
always deeper than the width of the ring by about 1 mm. Typical values are 4 to
4.5 mm for SI engines and 5 to 7 mm for DI diesel engines.
• The top gap is the clearance between the ring land and the top of the ring (40 to
80 µm).
• The middle gap is the distance between the ring and the bore (10 to 40 µm).
• The bottom gap is the clearance between the ring land and the bottom of the ring
(40 to 80 µm).
• The shared boundary and leaking wall is the piston (e.g., wall-8) and the cylinder
wall (e.g., wall.1) in most in-cylinder simulations. Cells that share a boundary
with the top of the piston and the cylinder wall are defined as the crevice cells.
Release 12.0 c ANSYS, Inc. January 29, 2009
12-11
Engine Ignition
The ring pack is the set of rings that seal the piston in the cylinder bore. As the piston
moves upward in the cylinder when the valves are closed (e.g., during the compression
stroke in a four-stroke cycle engine), the pressure in the cylinder rises and flow begins to
move past the rings. The pressure distribution in the ring pack is modeled by assuming
either fully-developed compressible flow through the spaces between the rings and the
piston, or choked compressible flow between the rings and the cylinder wall.
Since the temperature in the ring pack is fixed and the geometry is known, once a
pressure distribution is calculated, the mass in each volume can be found using the ideal
gas equation of state. The overall mass flow out of the ring pack (i.e., the flow past
the last ring specified) is also calculated at each discrete step in the ANSYS FLUENT
solution.
12.3.2 Limitations
The limitations of the crevice model are that it is zero dimensional, transient, and currently limited to two threads that share a boundary.
A zero-dimensional approach is used because it is difficult to accurately predict lateral
diffusion of species in the crevice. If the lateral diffusion of species is important in
the simulation, as in when a spray plume in a DI engine is in close proximity to the
boundary and the net mass flow is into the crevice, it is recommended that the full
multidimensional crevice geometry be simulated in ANSYS FLUENT using a nonconformal
mesh. Additionally, this approach does not specifically track individual species, as any
individual species would be instantly distributed over the entire ring pack. The mass
flux into the domain from the crevice is assumed to have the same composition as the
cell into which mass is flowing.
The formulation of the crevice flow equations is inherently transient and is solved using
ANSYS FLUENT’s stiff-equation solver. A steady problem with leakage flow can be solved
by running the transient problem to steady state. Additional limitations of the crevice
model in its current form are that only a single crevice is allowed and only one thread
can have leakage. Ring dynamics are not explicitly accounted for, although ring positions
can be set during the simulation.
In this context, the crevice model solution is a stiff initial boundary-value problem. The
stiffness increases as the pressure difference between the ring crevices increases and also as
the overall pressure difference across the ring pack increases. Thus, if the initial conditions
are very far from the solution during a time step, the ODE solver may not be able to
integrate the equations successfully. One solution to this problem is to decrease the flow
time step for several iterations. Another solution is to start with initial conditions that
are closer to the solution at the end of the time step.
12-12
Release 12.0 c ANSYS, Inc. January 29, 2009
12.3 Crevice Model
12.3.3
Crevice Model Theory
ANSYS FLUENT solves the equations for mass conservation in the crevice geometry by
assuming laminar compressible flow in the region between the piston and the top and
bottom faces of the ring, and by assuming an orifice flow between the ring and the
cylinder wall. The equation for the mass flow through the ring end gaps is of the form
ṁij = Cd Aij ρcηij
(12.3-1)
where Cd is the discharge coefficient, Aij is the gap area, ρ is the gas density, c is the
local speed of sound, and ηij is a compressibility factor given by
ηij =
"
2
γ−1
pi
pj
2
γ
−
pi
pj
γ−1
#0.5
pi
pj
γ
> 0.52
(12.3-2)
2
γ−1
γ+1
2(γ−1)
pi
pj
≤ 0.52
where γ is the ratio of specific heats, pi the upstream pressure and pj the downstream
pressure. The equation for the mass flow through the top and bottom faces of the ring
(i.e., into and out of the volume behind the piston ring) is given by
ṁij =
h2ij p2i − p2j Aij
24Wr µgas RT
(12.3-3)
where hij is the cross-sectional area of the gap, Wr is the width of the ring along which
the gas is flowing, µgas is the local gas viscosity, T is the temperature of the gas and R
is the universal gas constant. The system of equations for a set of three rings is of the
following form:
dp1
dt
dp2
dt
dp3
dt
dp4
dt
dp5
dt
Release 12.0 c ANSYS, Inc. January 29, 2009
=
=
=
=
=
p1
m1
p2
m2
p3
m3
p4
m4
p5
m5
(ṁ01 − ṁ12 )
(12.3-4)
(ṁ02 + ṁ12 − ṁ23 − ṁ24 )
(12.3-5)
(ṁ23 − ṁ34 )
(12.3-6)
(ṁ24 + ṁ34 − ṁ45 − ṁ46 )
(12.3-7)
(ṁ45 − ṁ56 )
(12.3-8)
12-13
Engine Ignition
where p0 is the average pressure in the crevice cells and p6 is the crankcase pressure input
from the text interface. The expressions for the mass flows for numerically adjacent zones
(e.g., 0-1, 1-2, 2-3, etc.) are given by Equation 12.3-3 and expressions for the mass flows
for zones separated by two integers (e.g., 0-2, 2-4, 4-6) are given by Equations 12.3-1
and 12.3-2. Thus, there are 2nr − 1 equations needed for the solution to the ring-pack
equations, where nr is the number of rings in the simulation.
12-14
Release 12.0 c ANSYS, Inc. January 29, 2009
Chapter 13.
Pollutant Formation
This chapter discusses the theory behind the models available in ANSYS FLUENT for
modeling pollutant formation.
Information is presented in the following sections:
• Section 13.1: NOx Formation
• Section 13.2: SOx Formation
• Section 13.3: Soot Formation
For information about using the models in ANSYS FLUENT, see Chapter 21: Modeling
Pollutant Formation in the separate User’s Guide.
13.1
NOx Formation
The following sections present the theoretical background of NOx prediction. For information about using the NOx models in ANSYS FLUENT, see Section 21.1.1: Using the
NOx Model in the separate User’s Guide.
• Section 13.1.1: Overview
• Section 13.1.2: Governing Equations for NOx Transport
• Section 13.1.3: Thermal NOx Formation
• Section 13.1.4: Prompt NOx Formation
• Section 13.1.5: Fuel NOx Formation
• Section 13.1.6: NOx Formation from Intermediate N2 O
• Section 13.1.7: NOx Reduction by Reburning
• Section 13.1.8: NOx Reduction by SNCR
• Section 13.1.9: NOx Formation in Turbulent Flows
Release 12.0 c ANSYS, Inc. January 29, 2009
13-1
Pollutant Formation
13.1.1
Overview
NOx emission consists of mostly nitric oxide (NO), and to a lesser degree nitrogen dioxide
(NO2 ) and nitrous oxide (N2 O). NOx is a precursor for photochemical smog, contributes
to acid rain, and causes ozone depletion. Thus, NOx is a pollutant. The ANSYS FLUENT
NOx model provides a tool to understand the sources of NOx production and to aid in
the design of NOx control measures.
NOx Modeling in ANSYS FLUENT
The ANSYS FLUENT NOx model provides the capability to model thermal, prompt, and
fuel NOx formation as well as NOx consumption due to reburning in combustion systems.
It uses rate models developed at the Department of Fuel and Energy at The University
of Leeds in England as well as from the open literature. NOx reduction using reagent
injection, such as selective noncatalytic reduction (SNCR), can be modeled in ANSYS
FLUENT along with an N2 O intermediate model which has also been incorporated.
To predict NOx emissions, ANSYS FLUENT solves a transport equation for nitric oxide
(NO) concentration. When fuel NOx sources are present, ANSYS FLUENT solves additional transport equations for intermediate species (HCN and/or NH3 ). When the N2 O
intermediate model is activated, an additional transport equation for N2 O will be solved.
The NOx transport equations are solved based on a given flow field and combustion solution. In other words, NOx is postprocessed from a combustion simulation. It is thus
evident that an accurate combustion solution becomes a prerequisite of NOx prediction.
For example, thermal NOx production doubles for every 90 K temperature increase when
the flame temperature is about 2200 K. Great care must be exercised to provide accurate thermophysical data and boundary condition inputs for the combustion model.
Appropriate turbulence, chemistry, radiation and other submodels must be employed.
To be realistic, one can only expect results to be as accurate as the input data and the
selected physical models. Under most circumstances, NOx variation trends can be accurately predicted but the NOx quantity itself cannot be pinpointed. Accurate prediction
of NOx parametric trends can cut down on the number of laboratory tests, allow more
design variations to be studied, shorten the design cycle, and reduce product development cost. That is truly the power of the ANSYS FLUENT NOx model and, in fact, the
power of CFD in general.
13-2
Release 12.0 c ANSYS, Inc. January 29, 2009
13.1 NOx Formation
NOx Formation and Reduction in Flames
In laminar flames, and at the molecular level within turbulent flames, the formation of
NOx can be attributed to four distinct chemical kinetic processes: thermal NOx formation, prompt NOx formation, fuel NOx formation, and intermediate N2 O. Thermal NOx
is formed by the oxidation of atmospheric nitrogen present in the combustion air. Prompt
NOx is produced by high-speed reactions at the flame front, and fuel NOx is produced by
oxidation of nitrogen contained in the fuel. At elevated pressures and oxygen-rich conditions, NOx may also be formed from molecular nitrogen (N2 ) via N2 O. The reburning
and SNCR mechanisms reduce the total NOx formation by accounting for the reaction
of NO with hydrocarbons and ammonia, respectively.
i
13.1.2
The NOx models cannot be used in conjunction with the premixed combustion model.
Governing Equations for NOx Transport
ANSYS FLUENT solves the mass transport equation for the NO species, taking into
account convection, diffusion, production and consumption of NO and related species.
This approach is completely general, being derived from the fundamental principle of
mass conservation. The effect of residence time in NOx mechanisms, a Lagrangian reference frame concept, is included through the convection terms in the governing equations
written in the Eulerian reference frame. For thermal and prompt NOx mechanisms, only
the NO species transport equation is needed:
∂
(ρYNO ) + ∇ · (ρ~v YNO ) = ∇ · (ρD∇YNO ) + SNO
∂t
(13.1-1)
As discussed in Section 13.1.5: Fuel NOx Formation, the fuel NOx mechanisms are more
involved. The tracking of nitrogen-containing intermediate species is important. ANSYS
FLUENT solves a transport equation for the HCN, NH3 or N2 O species in addition to the
NO species:
∂
(ρYHCN ) + ∇ · (ρ~v YHCN ) = ∇ · (ρDYHCN ) + SHCN
∂t
(13.1-2)
∂
(ρYNH3 ) + ∇ · (ρ~v YNH3 ) = ∇ · (ρDYNH3 ) + SNH3
∂t
(13.1-3)
∂
(ρYN2 O ) + ∇ · (ρ~v YN2 O ) = ∇ · (ρDYN2 O ) + SN2 O
∂t
(13.1-4)
Release 12.0 c ANSYS, Inc. January 29, 2009
13-3
Pollutant Formation
where YHCN , YNH3 , YN2 O , and YNO are mass fractions of HCN, NH3 , N2 O, and NO in
the gas phase, and D is the effective diffusion coefficient. The source terms SHCN , SNH3 ,
SN2 O , and SNO are to be determined next for different NOx mechanisms.
13.1.3
Thermal NOx Formation
The formation of thermal NOx is determined by a set of highly temperature-dependent
chemical reactions known as the extended Zeldovich mechanism. The principal reactions
governing the formation of thermal NOx from molecular nitrogen are as follows:
O + N2 *
) N + NO
N + O2 *
) O + NO
(13.1-5)
(13.1-6)
A third reaction has been shown to contribute to the formation of thermal NOx , particularly at near-stoichiometric conditions and in fuel-rich mixtures:
N + OH *
) H + NO
(13.1-7)
Thermal NOx Reaction Rates
The rate constants for these reactions have been measured in numerous experimental
studies [29, 102, 236], and the data obtained from these studies have been critically
evaluated by Baulch et al. [18] and Hanson and Salimian [124]. The expressions for the
rate coefficients for Equations 13.1-5–13.1-7 used in the NOx model are given below.
These were selected based on the evaluation of Hanson and Salimian [124].
kf,1
kf,2
kf,3
= 1.8 × 108 e−38370/T
= 1.8 × 104 T e−4680/T
= 7.1 × 107 e−450/T
kr,1
kr,2
kr,3
= 3.8 × 107 e−425/T
= 3.81 × 103 T e−20820/T
= 1.7 × 108 e−24560/T
In the above expressions, kf,1 , kf,2 , and kf,3 are the rate constants for the forward reactions
13.1-5–13.1-7, respectively, and kr,1 , kr,2 , and kr,3 are the corresponding reverse rate
constants. All of these rate constants have units of m3 /gmol-s.
The net rate of formation of NO via Reactions 13.1-5–13.1-7 is given by
d[NO]
= kf,1 [O][N2 ] + kf,2 [N][O2 ] + kf,3 [N][OH] − kr,1 [NO][N] − kr,2 [NO][O] − kr,3 [NO][H]
dt
(13.1-8)
where all concentrations have units of gmol/m3 .
To calculate the formation rates of NO and N, the concentrations of O, H, and OH are
required.
13-4
Release 12.0 c ANSYS, Inc. January 29, 2009
13.1 NOx Formation
The Quasi-Steady Assumption for [N]
The rate of formation of NOx is significant only at high temperatures (greater than
1800 K) because fixation of nitrogen requires the breaking of the strong N2 triple bond
(dissociation energy of 941 kJ/gmol). This effect is represented by the high activation
energy of reaction 13.1-5, which makes it the rate-limiting step of the extended Zeldovich
mechanism. However, the activation energy for oxidation of N atoms is small. When
there is sufficient oxygen, as in a fuel-lean flame, the rate of consumption of free nitrogen
atoms becomes equal to the rate of its formation and therefore a quasi-steady state can
be established. This assumption is valid for most combustion cases except in extremely
fuel-rich combustion conditions. Hence the NO formation rate becomes
kr,1 kr,2 [NO]2
kf,1 [N2 ]kf,2 [O2 ]
kr,1 [NO]
kf,2 [O2 ]+kf,3 [OH]
1−
d[NO]
= 2kf,1 [O][N2 ]
dt
1+
(gmol/m3 -s)
(13.1-9)
Thermal NOx Temperature Sensitivity
From Equation 13.1-9 it is clear that the rate of formation of NO will increase with
increasing oxygen concentration. It also appears that thermal NO formation should be
highly dependent on temperature but independent of fuel type. In fact, based on the
limiting rate described by kf,1 , the thermal NOx production rate doubles for every 90 K
temperature increase beyond 2200 K.
Decoupled Thermal NOx Calculations
To solve Equation 13.1-9, the concentration of O atoms and the free radical OH will
be required, in addition to the concentration of stable species (i.e., O2 , N2 ). Following
the suggestion by Zeldovich, the thermal NOx formation mechanism can be decoupled
from the main combustion process, by assuming equilibrium values of temperature, stable species, O atoms, and OH radicals. However, radical concentrations, O atoms in
particular, are observed to be more abundant than their equilibrium levels. The effect of
partial equilibrium O atoms on NOx formation rate has been investigated [232] during
laminar methane-air combustion. The results of these investigations indicate that the
level of NOx emission can be underpredicted by as much as 28% in the flame zone, when
assuming equilibrium O-atom concentrations.
Release 12.0 c ANSYS, Inc. January 29, 2009
13-5
Pollutant Formation
Approaches for Determining O Radical Concentration
There has been little detailed study of radical concentration in industrial turbulent flames,
but work [79] has demonstrated the existence of this phenomenon in turbulent diffusion
flames. Presently, there is no definitive conclusion as to the effect of partial equilibrium
on NOx formation rates in turbulent flames. Peters and Donnerhack [269] suggest that
partial equilibrium radicals can account for no more than a 25% increase in thermal NOx
and that fluid dynamics has the dominant effect on NOx formation rate. Bilger et al. [25]
suggest that in turbulent diffusion flames, the effect of O atom overshoot on the NOx
formation rate is very important.
To overcome this possible inaccuracy, one approach would be to couple the extended Zeldovich mechanism with a detailed hydrocarbon combustion mechanism involving many
reactions, species, and steps. This approach has been used previously for research purposes [229]. However, long computer processing time has made the method economically
unattractive and its extension to turbulent flows difficult.
To determine the O radical concentration, ANSYS FLUENT uses one of three approaches—
the equilibrium approach, the partial equilibrium approach, and the predicted concentration approach—in recognition of the ongoing controversy discussed above.
Method 1: Equilibrium Approach
The kinetics of the thermal NOx formation rate is much slower than the main hydrocarbon oxidation rate, and so most of the thermal NOx is formed after completion of
combustion. Therefore, the thermal NOx formation process can often be decoupled from
the main combustion reaction mechanism and the NOx formation rate can be calculated
by assuming equilibration of the combustion reactions. Using this approach, the calculation of the thermal NOx formation rate is considerably simplified. The assumption of
equilibrium can be justified by a reduction in the importance of radical overshoots at
higher flame temperature [78]. According to Westenberg [377], the equilibrium O-atom
concentration can be obtained from the expression
[O] = kp [O2 ]1/2
(13.1-10)
With kp included, this expression becomes
[O] = 3.97 × 105 T −1/2 [O2 ]1/2 e−31090/T
gmol/m3
(13.1-11)
where T is in Kelvin.
13-6
Release 12.0 c ANSYS, Inc. January 29, 2009
13.1 NOx Formation
Method 2: Partial Equilibrium Approach
An improvement to method 1 can be made by accounting for third-body reactions in the
O2 dissociation-recombination process:
O2 + M *
)O+O+M
(13.1-12)
Equation 13.1-11 is then replaced by the following expression [367]:
[O] = 36.64T 1/2 [O2 ]1/2 e−27123/T
gmol/m3
(13.1-13)
which generally leads to a higher partial O-atom concentration.
Method 3: Predicted O Approach
When the O-atom concentration is well predicted using an advanced chemistry model
(such as the flamelet submodel of the non-premixed model), [O] can be taken simply
from the local O-species mass fraction.
Approaches for Determining OH Radical Concentration
ANSYS FLUENT uses one of three approaches to determine the OH radical concentration:
the exclusion of OH from the thermal NOx calculation approach, the partial equilibrium
approach, and the use of the predicted OH concentration approach.
Method 1: Exclusion of OH Approach
In this approach, the third reaction in the extended Zeldovich mechanism (Equation 13.1-7)
is assumed to be negligible through the following observation:
k2 [O2 ]eq k3 [OH]eq
This assumption is justified for lean fuel conditions and is a reasonable assumption for
most cases.
Method 2: Partial Equilibrium Approach
In this approach, the concentration of OH in the third reaction in the extended Zeldovich
mechanism (Equation 13.1-7) is given by [19, 376]
[OH] = 2.129 × 102 T −0.57 e−4595/T [O]1/2 [H2 O]1/2 gmol/m3
Release 12.0 c ANSYS, Inc. January 29, 2009
(13.1-14)
13-7
Pollutant Formation
Method 3: Predicted OH Approach
As in the predicted O approach, when the OH radical concentration is well predicted using
an advanced chemistry model such as the flamelet model, [OH] can be taken directly from
the local OH species mass fraction.
Summary
To summarize, thermal NOx formation rate is predicted by Equation 13.1-9. The
O-atom concentration needed in Equation 13.1-9 is computed using Equation 13.1-11
for the equilibrium assumption, using Equation 13.1-13 for a partial equilibrium assumption, or using the local O-species mass fraction. You will make the choice during problem
setup. In terms of the transport equation for NO (Equation 13.1-1), the NO source term
due to thermal NOx mechanisms is
Sthermal,NO = Mw,NO
d[NO]
dt
(13.1-15)
where Mw,NO is the molecular weight of NO (kg/gmol), and d[NO]/dt is computed from
Equation 13.1-9.
13.1.4
Prompt NOx Formation
It is known that during combustion of hydrocarbon fuels, the NOx formation rate can
exceed that produced from direct oxidation of nitrogen molecules (i.e., thermal NOx ).
Prompt NOx Combustion Environments
The presence of a second mechanism leading to NOx formation was first identified by
Fenimore [91] and was termed “prompt NOx ”. There is good evidence that prompt NOx
can be formed in a significant quantity in some combustion environments, such as in lowtemperature, fuel-rich conditions and where residence times are short. Surface burners,
staged combustion systems, and gas turbines can create such conditions [13].
At present the prompt NOx contribution to total NOx from stationary combustors is
small. However, as NOx emissions are reduced to very low levels by employing new
strategies (burner design or furnace geometry modification), the relative importance of
the prompt NOx can be expected to increase.
13-8
Release 12.0 c ANSYS, Inc. January 29, 2009
13.1 NOx Formation
Prompt NOx Mechanism
Prompt NOx is most prevalent in rich flames. The actual formation involves a complex
series of reactions and many possible intermediate species. The route now accepted is as
follows:
CH + N2
N + O2
HCN + OH
CN + O2
*
)
*
)
*
)
*
)
HCN + N
NO + O
CN + H2 O
NO + CO
(13.1-16)
(13.1-17)
(13.1-18)
(13.1-19)
A number of species resulting from fuel fragmentation have been suggested as the source
of prompt NOx in hydrocarbon flames (e.g., CH, CH2 , C, C2 H), but the major contribution is from CH (Equation 13.1-16) and CH2 , via
CH2 + N2 *
) HCN + NH
(13.1-20)
The products of these reactions could lead to formation of amines and cyano compounds
that subsequently react to form NO by reactions similar to those occurring in oxidation
of fuel nitrogen, for example:
HCN + N *
) N2 + ...
(13.1-21)
Prompt NOx Formation Factors
Prompt NOx formation is proportional to the number of carbon atoms present per unit
volume and is independent of the parent hydrocarbon identity. The quantity of HCN
formed increases with the concentration of hydrocarbon radicals, which in turn increases
with equivalence ratio. As the equivalence ratio increases, prompt NOx production increases at first, then passes a peak, and finally decreases due to a deficiency in oxygen.
Primary Reaction
Reaction 13.1-16 is of primary importance. In recent studies [304], comparison of probability density distributions for the location of the peak NOx with those obtained for the
peak CH have shown close correspondence, indicating that the majority of the NOx at the
flame base is prompt NOx formed by the CH reaction. Assuming that Reaction 13.1-16
controls the prompt NOx formation rate,
d[NO]
= k0 [CH][N2 ]
dt
Release 12.0 c ANSYS, Inc. January 29, 2009
(13.1-22)
13-9
Pollutant Formation
Modeling Strategy
There are, however, uncertainties about the rate data for the above reaction. From Reactions 13.1-16–13.1-20, it can be concluded that the prediction of prompt NOx formation
within the flame requires coupling of the NOx kinetics to an actual hydrocarbon combustion mechanism. Hydrocarbon combustion mechanisms involve many steps and, as
mentioned previously, are extremely complex and costly to compute. In the present NOx
model, a global kinetic parameter derived by De Soete [69] is used. De Soete compared
the experimental values of total NOx formation rate with the rate of formation calculated
by numerical integration of the empirical overall reaction rates of NOx and N2 formation.
He showed that overall prompt formation rate can be predicted from the expression
d[NO]
= (overall prompt NOx formation rate) − (overall prompt N2 formation rate)
dt
(13.1-23)
In the early stages of the flame, where prompt NOx is formed under fuel-rich conditions,
the O concentration is high and the N radical almost exclusively forms NOx rather than
nitrogen. Therefore, the prompt NOx formation rate will be approximately equal to the
overall prompt NOx formation rate:
d[NO]
= kpr [O2 ]a [N2 ][FUEL]e−Ea /RT
dt
(13.1-24)
For C2 H4 (ethylene)-air flames,
kpr = 1.2 × 107 (RT /p)a+1 ;
Ea = 251151 J/gmol
where a is the oxygen reaction order, R is the universal gas constant, and p is pressure
(all in SI units). The rate of prompt NOx formation is found to be of the first order with
respect to nitrogen and fuel concentration, but the oxygen reaction order, a, depends on
experimental conditions.
13-10
Release 12.0 c ANSYS, Inc. January 29, 2009
13.1 NOx Formation
Rate for Most Hydrocarbon Fuels
Equation 13.1-24 was tested against the experimental data obtained by Backmier et
al. [9] for different mixture strengths and fuel types. The predicted results indicated that
the model performance declined significantly under fuel-rich conditions and for higher
hydrocarbon fuels. To reduce this error and predict the prompt NOx adequately in
all conditions, the De Soete model was modified using the available experimental data.
A correction factor, f , was developed, which incorporates the effect of fuel type, i.e.,
number of carbon atoms, and air-to-fuel ratio for gaseous aliphatic hydrocarbons. Equation 13.1-24 now becomes
d[NO]
0
0
= f kpr
[O2 ]a [N2 ][FUEL]e−Ea /RT
dt
(13.1-25)
so that the source term due to prompt NOx mechanism is
Sprompt,NO = Mw,NO
d[NO]
dt
(13.1-26)
In the above equations,
f = 4.75 + 0.0819 n − 23.2φ + 32φ2 − 12.2φ3
0
kpr
= 6.4 × 106 (RT /p)a+1 ;
(13.1-27)
Ea0 = 303474.125 J/gmol
n is the number of carbon atoms per molecule for the hydrocarbon fuel, and φ is the
equivalence ratio. The correction factor is a curve fit for experimental data, valid for
aliphatic alkane hydrocarbon fuels (Cn H2n+2 ) and for equivalence ratios between 0.6 and
0
1.6. For values outside the range, the appropriate limit should be used. Values of kpr
and
0
Ea were developed at the Department of Fuel and Energy at The University of Leeds in
England.
Here the concept of equivalence ratio refers to an overall equivalence ratio for the flame,
rather than any spatially varying quantity in the flow domain. In complex geometries with
multiple burners this may lead to some uncertainty in the specification of φ. However,
since the contribution of prompt NOx to the total NOx emission is often very small,
results are not likely to be significantly biased.
Release 12.0 c ANSYS, Inc. January 29, 2009
13-11
Pollutant Formation
Oxygen Reaction Order
Oxygen reaction order depends on flame conditions. According to De Soete [69], oxygen
reaction order is uniquely related to oxygen mole fraction in the flame:
XO2 ≤ 4.1 × 10−3
−3
≤ XO2 ≤ 1.11 × 10−2
O2 , 4.1 × 10
−0.35 − 0.1 ln XO2 , 1.11 × 10−2 < XO2 < 0.03
0,
XO2 ≥ 0.03
1.0,
−3.95 − 0.9 ln X
a=
13.1.5
(13.1-28)
Fuel NOx Formation
Fuel-Bound Nitrogen
It is well known that nitrogen-containing organic compounds present in liquid or solid
fossil fuel can contribute to the total NOx formed during the combustion process. This
fuel nitrogen is a particularly important source of nitrogen oxide emissions for residual fuel
oil and coal, which typically contain 0.3–2% nitrogen by weight. Studies have shown that
most of the nitrogen in heavy fuel oils is in the form of heterocycles and it is thought that
the nitrogen components of coal are similar [154]. It is believed that pyridine, quinoline,
and amine type heterocyclic ring structures are of importance.
Reaction Pathways
The extent of conversion of fuel nitrogen to NOx is dependent on the local combustion
characteristics and the initial concentration of nitrogen-bound compounds. Fuel-bound
compounds that contain nitrogen are released into the gas phase when the fuel droplets or
particles are heated during the devolatilization stage. From the thermal decomposition
of these compounds, (aniline, pyridine, pyrroles, etc.) in the reaction zone, radicals
such as HCN, NH3 , N, CN, and NH can be formed and converted to NOx . The above
free radicals (i.e., secondary intermediate nitrogen compounds) are subject to a double
competitive reaction path. This chemical mechanism has been subject to several detailed
investigations [230]. Although the route leading to fuel NOx formation and destruction
is still not completely understood, different investigators seem to agree on a simplified
model:
NO
O
2
ion
dat
oxi
Fuel Nitrogen
Nitrogen Intermediates
red
uct
ion
NO
N2
13-12
Release 12.0 c ANSYS, Inc. January 29, 2009
13.1 NOx Formation
Recent investigations [133] have shown that hydrogen cyanide appears to be the principal
product if fuel nitrogen is present in aromatic or cyclic form. However, when fuel nitrogen
is present in the form of aliphatic amines, ammonia becomes the principal product of
fuel nitrogen conversion.
In the ANSYS FLUENT NOx model, sources of NOx emission for gaseous, liquid and coal
fuels are considered separately. The nitrogen-containing intermediates are grouped as
HCN, NH3 , or a combination of both. Transport equations (13.1-1 and 13.1-2 or 13.1-3)
are solved, after which the source terms SHCN , SNH3 , and SNO are determined for different
fuel types. Discussions to follow refer to fuel NOx sources for SNO and intermediate HCN,
NH3 sources for SHCN and SNH3 . Contributions from thermal and prompt mechanisms
have been discussed in previous sections.
Fuel NOx from Gaseous and Liquid Fuels
The fuel NOx mechanisms for gaseous and liquid fuels are based on different physics but
the same chemical reaction pathways.
Fuel NOx from Intermediate Hydrogen Cyanide (HCN)
When HCN is used as the intermediate species:
2
1: O
NO
ion
dat
oxi
Fuel Nitrogen
HCN
red
uct
ion
2: N
O
N2
The source terms in the transport equations can be written as follows:
SHCN = Spl,HCN + SHCN−1 + SHCN−2
SNO = SNO−1 + SNO−2
Release 12.0 c ANSYS, Inc. January 29, 2009
(13.1-29)
(13.1-30)
13-13
Pollutant Formation
HCN Production in a Gaseous Fuel
The rate of HCN production is equivalent to the rate of combustion of the fuel:
Spl,HCN =
where
Spl,HCN
Rcf
YN,fuel
Rcf YN,fuel Mw,HCN
Mw,N
(13.1-31)
= source of HCN (kg/m3 -s)
= mean limiting reaction rate of fuel (kg/m3 -s)
= mass fraction of nitrogen in the fuel
The mean limiting reaction rate of fuel, Rcf , is calculated from the Magnussen combustion
model, so the gaseous fuel NOx option is available only when the generalized finite-rate
model is used.
HCN Production in a Liquid Fuel
The rate of HCN production is equivalent to the rate of fuel release into the gas phase
through droplet evaporation:
Spl,HCN =
where
Spl,HCN
Sfuel
YN,fuel
V
Sfuel YN,fuel Mw,HCN
Mw,N V
(13.1-32)
= source of HCN (kg/m3 -s)
= rate of fuel release from the liquid droplets to the gas (kg/s)
= mass fraction of nitrogen in the fuel
= cell volume (m3 )
HCN Consumption
The HCN depletion rates from reactions (1) and (2) in the above mechanism are the
same for both gaseous and liquid fuels, and are given by De Soete [69] as
R1 = A1 XHCN XOa 2 e−E1 /RT
(13.1-33)
−E2 /RT
(13.1-34)
R2 = A2 XHCN XNO e
where
13-14
R1 , R2
T
X
A1
A2
E1
E2
=
=
=
=
=
=
=
conversion rates of HCN (s−1 )
instantaneous temperature (K)
mole fractions
1.0 ×1010 s−1
3.0 ×1012 s−1
280451.95 J/gmol
251151 J/gmol
Release 12.0 c ANSYS, Inc. January 29, 2009
13.1 NOx Formation
The oxygen reaction order, a, is calculated from Equation 13.1-28.
Since mole fraction is related to mass fraction through molecular weights of the species
(Mw,i ) and the mixture (Mw,m ),
Mw,m
Yi
=
Xi = Yi
Mw,i
Mw,i
ρRT
p
!
(13.1-35)
HCN Sources in the Transport Equation
The mass consumption rates of HCN which appear in Equation 13.1-29 are calculated as
where
SHCN−1
SHCN−2
p
T
R
SHCN−1 = −R1
Mw,HCN p
RT
(13.1-36)
SHCN−2 = −R2
Mw,HCN p
RT
(13.1-37)
=
consumption rates of HCN in
reactions 1 and 2 respectively (kg/m3 -s)
= pressure (Pa)
= mean temperature (K)
= universal gas constant
NOx Sources in the Transport Equation
NOx is produced in reaction 1 but destroyed in reaction 2. The sources for Equation 13.1-30 are the same for a gaseous as for a liquid fuel, and are evaluated as follows:
Mw,NO
Mw,NO p
= R1
Mw,HCN
RT
(13.1-38)
Mw,NO
Mw,NO p
= −R2
Mw,HCN
RT
(13.1-39)
SNO−1 = −SHCN−1
SNO−2 = SHCN−2
Release 12.0 c ANSYS, Inc. January 29, 2009
13-15
Pollutant Formation
Fuel NOx from Intermediate Ammonia (NH3 )
When NH3 is used as the intermediate species:
2
1: O
NO
ion
dat
oxi
Fuel Nitrogen
NH 3
red
uct
ion
2: N
O
N2
The source terms in the transport equations can be written as follows:
SNH3 = Spl,NH3 + SNH3 −1 + SNH3 −2
SNO = SNO−1 + SNO−2
(13.1-40)
(13.1-41)
NH3 Production in a Gaseous Fuel
The rate of NH3 production is equivalent to the rate of combustion of the fuel:
Spl,NH3 =
where
Spl,NH3
Rcf
YN,fuel
Rcf YN,fuel Mw,NH3
Mw,N
(13.1-42)
= source of NH3 (kg/m3 -s)
= mean limiting reaction rate of fuel (kg/m3 -s)
= mass fraction of nitrogen in the fuel
The mean limiting reaction rate of fuel, Rcf , is calculated from the Magnussen combustion
model, so the gaseous fuel NOx option is available only when the generalized finite-rate
model is used.
13-16
Release 12.0 c ANSYS, Inc. January 29, 2009
13.1 NOx Formation
NH3 Production in a Liquid Fuel
The rate of NH3 production is equivalent to the rate of fuel release into the gas phase
through droplet evaporation:
Spl,NH3 =
where
Spl,NH3
Sfuel
YN,fuel
V
=
=
=
=
Sfuel YN,fuel Mw,NH3
Mw,N V
(13.1-43)
source of NH3 (kg/m3 -s)
rate of fuel release from the liquid droplets to the gas (kg/s)
mass fraction of nitrogen in the fuel
cell volume (m3 )
NH3 Consumption
The NH3 depletion rates from reactions (1) and (2) in the above mechanism are the same
for both gaseous and liquid fuels, and are given by De Soete [69] as
R1 = A1 XNH3 XOa 2 e−E1 /RT
(13.1-44)
−E2 /RT
(13.1-45)
R2 = A2 XNH3 XNO e
where
R1 , R2
T
X
A1
A2
E1
E2
=
=
=
=
=
=
=
conversion rates of NH3 (s−1 )
instantaneous temperature (K)
mole fractions
4.0 ×106 s−1
1.8 ×108 s−1
133947.2 J/gmol
113017.95 J/gmol
The oxygen reaction order, a, is calculated from Equation 13.1-28.
Since mole fraction is related to mass fraction through molecular weights of the species
(Mw,i ) and the mixture (Mw,m ), Xi can be calculated using Equation 13.1-35.
Release 12.0 c ANSYS, Inc. January 29, 2009
13-17
Pollutant Formation
NH3 Sources in the Transport Equation
The mass consumption rates of NH3 which appear in Equation 13.1-40 are calculated as
where
SNH3 −1
SNH3 −2
p
T
R
SNH3 −1 = −R1
Mw,NH3 p
RT
(13.1-46)
SNH3 −2 = −R2
Mw,NH3 p
RT
(13.1-47)
= consumption rates of NH3 in
reactions 1 and 2 respectively (kg/m3 -s)
= pressure (Pa)
= mean temperature (K)
= universal gas constant
NOx Sources in the Transport Equation
NOx is produced in reaction 1 but destroyed in reaction 2. The sources for Equation 13.1-41 are the same for a gaseous as for a liquid fuel, and are evaluated as follows:
Mw,NO
Mw,NO p
= R1
Mw,NH3
RT
(13.1-48)
Mw,NO
Mw,NO p
= −R2
Mw,NH3
RT
(13.1-49)
SNO−1 = −SNH3 −1
SNO−2 = SNH3 −2
Fuel NOx from Coal
Nitrogen in Char and in Volatiles
For the coal it is assumed that fuel nitrogen is distributed between the volatiles and
the char. Since there is no reason to assume that N is equally distributed between the
volatiles and the char the fraction of N in the volatiles and the char should be specified
separately.
When HCN is used as the intermediate species, two variations of fuel NOx mechanisms
for coal are included. When NH3 is used as the intermediate species, two variations of fuel
NOx mechanisms for coal are included, much like in the calculation of NOx production
from the coal via HCN. It is assumed that fuel nitrogen is distributed between the volatiles
and the char.
13-18
Release 12.0 c ANSYS, Inc. January 29, 2009
13.1 NOx Formation
Coal Fuel NOx Scheme A
The first HCN mechanism assumes that all char N converts to HCN which is then converted partially to NO [327]. The reaction pathway is described as follows:
Char N
Volatile N
1: O 2
HCN
3: Char
NO
N2
2: NO
N2
With the first scheme, all char-bound nitrogen converts to HCN. Thus,
Sc YN,char Mw,HCN
Mw,N V
= 0
Schar,HCN =
Schar,NO
where
Sc
YN,char
V
(13.1-50)
(13.1-51)
= char burnout rate (kg/s)
= mass fraction of nitrogen in char
= cell volume (m3 )
Coal Fuel NOx Scheme B
The second HCN mechanism assumes that all char N converts to NO directly [207]. The
reaction pathway is described as follows:
Char N
Volatile N
1: O 2
HCN
3: Char
NO
N2
2: NO
N2
Release 12.0 c ANSYS, Inc. January 29, 2009
13-19
Pollutant Formation
According to Lockwood [207], the char nitrogen is released to the gas phase as NO directly,
mainly as a desorption product from oxidized char nitrogen atoms. If this approach is
followed, then
Schar,HCN = 0
Sc YN,char Mw,NO
Schar,NO =
Mw,N V
(13.1-52)
(13.1-53)
HCN Scheme Selection
The second HCN mechanism tends to produce more NOx emission than the first. In
general, however, it is difficult to say which one outperforms the other.
The source terms for the transport equations are
SHCN = Spvc,HCN + SHCN−1 + SHCN−2
SNO = Schar,NO + SNO−1 + SNO−2 + SNO−3
(13.1-54)
(13.1-55)
Source contributions SHCN−1 , SHCN−2 , SNO−1 , and SNO−2 are described previously. Therefore, only the heterogeneous reaction source, SNO−3 , the char NOx source, Schar,NO , and
the HCN production source, Spvc,HCN , need to be considered.
NOx Reduction on Char Surface
The heterogeneous reaction of NO reduction on the char surface has been modeled according to the following [190]:
R3 = A3 e−E3 /RT pNO
where
R3
pNO
E3
A3
T
=
=
=
=
=
(13.1-56)
rate of NO reduction (gmol/m2BET -s)
mean NO partial pressure (atm)
142737.485 J/gmol
230 gmol/m2BET -s-atm
mean temperature (K)
The partial pressure pNO is calculated using Dalton’s law:
pNO = pXNO
13-20
Release 12.0 c ANSYS, Inc. January 29, 2009
13.1 NOx Formation
The rate of NO consumption due to reaction 3 will then be
SNO−3 = cs ABET Mw,NO R3
where
ABET
cs
SNO−3
= BET surface area (m2 /kg)
= concentration of particles (kg/m3 )
= NO consumption (kg/m3 -s)
BET Surface Area
The heterogeneous reaction involving char is mainly an adsorption process whose rate is
directly proportional to the pore surface area. The pore surface area is also known as the
BET surface area due to the researchers who pioneered the adsorption theory (Brunauer,
Emmett and Teller [42]). For commercial adsorbents, the pore (BET) surface areas range
from 100,000 to 2 million square meters per kilogram, depending on the microscopic
structure. For coal, the BET area is typically 25,000 m2 /kg which is used as the default
in ANSYS FLUENT. The overall source of HCN (Spvc,HCN ) is a combination of volatile
contribution (Svol,HCN ) and char contribution (Schar,HCN ):
Spvc,HCN = Svol,HCN + Schar,HCN
HCN from Volatiles
The source of HCN from the volatiles is related to the rate of volatile release:
Svol,HCN =
where
Svol
YN,vol
V
Svol YN,vol Mw,HCN
Mw,N V
= source of volatiles originating from
the coal particles into the gas phase (kg/s)
= mass fraction of nitrogen in the volatiles
= cell volume (m3 )
Calculation of sources related to char-bound nitrogen depends on the fuel NOx scheme
selection.
Release 12.0 c ANSYS, Inc. January 29, 2009
13-21
Pollutant Formation
Coal Fuel NOx Scheme C
The first NH3 mechanism assumes that all char N converts to NH3 which is then converted
partially to NO [327]. The reaction pathway is described as follows:
Char N
Volatile N
1: O 2
NH 3
3: Char
NO
N2
2: NO
N2
In this scheme, all char-bound nitrogen converts to NH3 . Thus,
Sc YN,char Mw,NH3
Mw,N V
= 0
(13.1-57)
Schar,NH3 =
Schar,NO
where
Sc
YN,char
V
(13.1-58)
= char burnout rate (kg/s)
= mass fraction of nitrogen in char
= cell volume (m3 )
Coal Fuel NOx Scheme D
The second NH3 mechanism assumes that all char N converts to NO directly [207]. The
reaction pathway is described as follows:
Char N
Volatile N
1: O 2
NH 3
3: Char
NO
N2
2: NO
N2
13-22
Release 12.0 c ANSYS, Inc. January 29, 2009
13.1 NOx Formation
According to Lockwood [207], the char nitrogen is released to the gas phase as NO directly,
mainly as a desorption product from oxidized char nitrogen atoms. If this approach is
followed, then
Schar,NH3 = 0
Sc YN,char Mw,NO
Schar,NO =
Mw,N V
(13.1-59)
(13.1-60)
NH3 Scheme Selection
The second NH3 mechanism tends to produce more NOx emission than the first. In
general, however, it is difficult to say which one outperforms the other.
The source terms for the transport equations are
SNH3 = Spvc,NH3 + SNH3 −1 + SNH3 −2
SNO = Schar,NO + SNO−1 + SNO−2 + SNO−3
(13.1-61)
(13.1-62)
Source contributions SNH3 −1 , SNH3 −2 , SNO−1 , SNO−2 , SNO−3 , Schar,NO are described previously. Therefore, only the NH3 production source, Spvc,NH3 , needs to be considered.
The overall production source of NH3 is a combination of volatile contribution (Svol,NH3 ),
and char contribution (Schar,NH3 ):
Spvc,NH3 = Svol,NH3 + Schar,NH3
(13.1-63)
NH3 from Volatiles
The source of NH3 from the volatiles is related to the rate of volatile release:
Svol,NH3 =
where
Svol
YN,vol
V
Svol YN,vol Mw,NH3
Mw,N V
= source of volatiles originating from
the coal particles into the gas phase (kg/s)
= mass fraction of nitrogen in the volatiles
= cell volume (m3 )
Calculation of sources related to char-bound nitrogen depends on the fuel NOx scheme
selection.
Release 12.0 c ANSYS, Inc. January 29, 2009
13-23
Pollutant Formation
Fuel Nitrogen Partitioning for HCN and NH3 Intermediates
In certain cases, especially when the fuel is a solid, both HCN and NH3 can be generated
as intermediates at high enough temperatures [247]. In particular, low-ranking (lignite)
coal has been shown to produce 10 times more NH3 compared to the level of HCN,
whereas higher-ranking (bituminous) coal has been shown to produce only HCN [246].
Studies by Winter et al. [381] have shown that for bituminous coal, using an HCN/NH3
partition ratio of 9:1 gave better NOx predictions when compared to measurements than
specifying only a single intermediate species. Liu and Gibbs [206] work with woodybiomass (pine wood chips), on the other hand, has suggested an HCN/NH3 ratio of 1:9
due to the younger age of the fuel.
In total, the above work suggests the importance of being able to specify that portions
of the fuel nitrogen will be converted to both HCN and NH3 intermediates at the same
time. In ANSYS FLUENT, fuel nitrogen partitioning can be used whenever HCN or NH3
are intermediates for NOx production, though it is mainly applicable to solid fuels such
as coal and biomass. The reaction pathways and source terms for HCN and NH3 were
discussed in previous sections.
13.1.6
NOx Formation from Intermediate N2 O
Melte and Pratt [222] proposed the first intermediate mechanism for NOx formation from
molecular nitrogen (N2 ) via nitrous oxide (N2 O). Nitrogen enters combustion systems
mainly as a component of the combustion and dilution air. Under favorable conditions,
which are elevated pressures and oxygen-rich conditions, this intermediate mechanism
can contribute as much as 90% of the NOx formed during combustion. This makes
it particularly important in equipment such as gas turbines and compression-ignition
engines. Because these devices are operated at increasingly low temperatures to prevent
NOx formation via the thermal NOx mechanism, the relative importance of the N2 Ointermediate mechanism is increasing. It has been observed that about 30% of the NOx
formed in these systems can be attributed to the N2 O-intermediate mechanism.
The N2 O-intermediate mechanism may also be of importance in systems operated in
flameless mode (e.g., diluted combustion, flameless combustion, flameless oxidation, and
FLOX systems). In a flameless mode, fuel and oxygen are highly diluted in inert gases so
that the combustion reactions and resulting heat release are carried out in the diffuse zone.
As a consequence, elevated peaks of temperature are avoided, which prevents thermal
NOx . Research suggests that the N2 O-intermediate mechanism may contribute about
90% of the NOx formed in flameless mode, and that the remainder can be attributed
to the prompt NOx mechanism. The relevance of NOx formation from N2 O has been
observed indirectly, and theoretically speculated for a number of combustion systems
and by a number of researchers [12, 61, 112, 338, 344].
13-24
Release 12.0 c ANSYS, Inc. January 29, 2009
13.1 NOx Formation
N2 O-Intermediate NOx Mechanism
The simplest form of the mechanism [222] takes into account two reversible elementary
reactions:
* N2 O + M
N2 + O + M )
N2 O + O *
) 2NO
(13.1-64)
(13.1-65)
Here, M is a general third body. Because the first reaction involves third bodies, the
mechanism is favored at elevated pressures. Both reactions involve the oxygen radical
O, which makes the mechanism favored at oxygen-rich conditions. While not always
justified, it is often assumed that the radical O atoms originate solely from the dissociation
of molecular oxygen,
1
O2 *
)O
2
(13.1-66)
According to the kinetic rate laws, the rate of NOx formation via the N2 O-intermediate
mechanism is
d[NO]
= 2 kf,2 [N2 O][O] − kr,2 [NO]2
dt
gmol/m3 -s
(13.1-67)
To solve Equation 13.1-67, you will need to have first calculated [O] and [N2 O].
It is often assumed that N2 O is at quasi-steady-state (i.e., d[N2 O]/dt = 0), which implies
[N2 O] =
kf,1 [N2 ][O][M] + kr,2 [NO]2
kr,1 [M] + kf,2 [O]
(13.1-68)
The system of Equations 13.1-67–13.1-68 can be solved for the rate of NOx formation
when the concentration of N2 , O2 , and M, the kinetic rate constants for Equations 13.1-64
and 13.1-65, and the equilibrium constant of Equation 13.1-66 are known. The appearance of NO in Equation 13.1-65 entails that coupling of the N2 O mechanism with the
thermal NOx mechanism (and other NOx mechanisms).
kf,1
kf,2
= 4.44 × 1032 T −8.358 e−28234/T
= 2.90 × 107 e−11651/T
kr,1
kr,2
= 4.00 × 108 e−28234/T
= 1.45 × 10−29 T 9.259 e−11651/T
In the above expressions, kf,1 and kf,2 are the forward rate constants of Equations 13.1-64
and 13.1-65, and kr,1 and kr,2 are the corresponding reverse rate constants. The units for
kf,2 , kr,1 , and kr,2 are m3 /gmol-s, while kf,1 has units of m6 /gmol2 -s.
Release 12.0 c ANSYS, Inc. January 29, 2009
13-25
Pollutant Formation
13.1.7
NOx Reduction by Reburning
The design of complex combustion systems for utility boilers, based on air- and fuelstaging technologies, involves many parameters and their mutual interdependence. These
parameters include local stoichiometry, temperature and chemical concentration field,
residence time distribution, velocity field, and mixing pattern. A successful application
of the in-furnace reduction techniques requires control of these parameters in an optimum
manner so as to avoid impairing the boiler performance. In the mid 1990s, global models
describing the kinetics of NOx destruction in the reburn zone of a staged combustion
system became available. Two of these models are described below.
Instantaneous Approach
The instantaneous NOx reburning mechanism is a pathway whereby NO reacts with
hydrocarbons and is subsequently reduced. In general:
CHi + NO → HCN + products
(13.1-69)
Three reburn reactions are modeled by ANSYS FLUENT for 1600 ≤ T ≤ 2100:
CH + NO →1 HCN + O
k
(13.1-70)
k2
CH2 + NO → HCN + OH
(13.1-71)
k3
(13.1-72)
CH3 + NO → HCN + H2 O
i
If the temperature is outside of this range, NO reburn will not be computed.
The rate constants for these reactions are taken from Bowman [32] and have units of
m3 /gmol-s:
k1 = 1 × 108 ;
k2 = 1.4 × 106 e−550/T ; k3 = 2 × 105
The NO depletion rate due to reburn is expressed as
d[NO]
= −k1 [CH][NO] − k2 [CH2 ][NO] − k3 [CH3 ][NO]
dt
13-26
(13.1-73)
Release 12.0 c ANSYS, Inc. January 29, 2009
13.1 NOx Formation
and the source term for the reburning mechanism in the NO transport equation can be
calculated as
Sreburn,NO = −Mw,NO
i
d[NO]
dt
(13.1-74)
To calculate the NO depletion rate due to reburning, ANSYS FLUENT will
obtain the concentrations of CH, CH2 , and CH3 from the species mass
fraction results of the combustion calculation. When you use this method,
you must be sure to include the species CH, CH2 , and CH3 in your problem
definition.
Partial Equilibrium Approach
The partial equilibrium approach is based on the model proposed by Kandamby et
al. [156] and [7]. The model adds a reduction path to De Soete’s global model [69]
that describes the NOx formation/destruction mechanism in a pulverized coal flame.
The additional reduction path accounts for the NOx destruction in the fuel-rich reburn
zone by CH radicals (see Figure 13.1.1).
CH i
(4)
O2
(3)
Fuel N
(1)
NO
CH i
(5)
Products
HCN
NO
(2)
N2
Figure 13.1.1: De Soete’s Global NOx Mechanism with Additional Reduction
Path
This model can be used in conjunction with the eddy-dissipation combustion model and
does not require the specification of CH radical concentrations, since they are computed
based on the CH-radical partial equilibrium. The reburn fuel itself can be an equivalent of
CH4 , CH3 , CH2 , or CH. How this equivalent fuel is determined is open for debate and an
approximate guide would be to consider the C/H ratio of the fuel itself. A multiplicative
constant of 4.0 × 10−4 has been developed for the partial equilibrium of CH radicals
to reduce the rates of HCN and NO in the reburn model. This value was obtained by
researchers, who developed the model, by way of predicting NOx values for a number of
test cases for which experimental data exists.
Release 12.0 c ANSYS, Inc. January 29, 2009
13-27
Pollutant Formation
NOx Reduction Mechanism
In the fuel-rich reburn zone, the HCN oxidation is suppressed and the amount of NO
formed in the primary combustion zone is decreased by the reduction reaction from HCN
to N2 . However, the NO concentration may also decrease due to reactions with CH
radicals, which are available in significant amounts in the reburn zone. The following are
considered to be the most important reactions of NO reduction by CH radicals:
NO + CH2 −→ HCN + OH
NO + CH −→ HCN + O
NO + C −→ CN + O
(13.1-75)
(13.1-76)
(13.1-77)
These reactions may be globally described by the addition of pathways (4) and (5) in
Figure 13.1.1, leading respectively to the formation of HCN and of minor intermediate
nitrogen radicals. Assuming that methane is the reburning gas, the global NO reduction
rates are then expressed as
R4 = (ka χ1 + kb χ21 )[CH4 ][NO]
R5 = kc χ31 χ2 [CH4 ][NO]
(13.1-78)
(13.1-79)
where
χ1 =
[H]
;
[H2 ]
χ2 =
[OH]
[H2 O]
Therefore, the additional source terms of the HCN and NO transport equations due to
reburn reactions are given by
d[HCN]
= 4 × 10−4 R4
dt
d[NO]
= −4 × 10−4 (R4 + R5 )
dt
13-28
(13.1-80)
(13.1-81)
Release 12.0 c ANSYS, Inc. January 29, 2009
13.1 NOx Formation
Certain assumptions are required to evaluate the rate constants ka , kb , and kc and the
factors χ1 and χ2 . For hydrocarbon diffusion flames, the following reaction set can be
reasonably considered to be in partial equilibrium:
CH4 + H
CH3 + OH
CH2 + H
CH + H
*
)
*
)
*
)
*
)
CH3 + H2
CH2 + H2 O
CH + H2
C + H2
(13.1-82)
(13.1-83)
(13.1-84)
(13.1-85)
Thus, the rate constants may be computed as
ka = k 1
kf,4 kf,5
;
kr,4 kr,5
kb = k2
kf,4 kf,5 kf,6
;
kr,4 kr,5 kr,6
kc = k3
kf,4 kf,5 kf,6 kf,7
kr,4 kr,5 kr,6 kr,7
where k1 , k2 , and k3 are the rate constants for Equations 13.1-75–13.1-77. The forward
and reverse rate constants for Equations 13.1-82–13.1-85 are kf,4 –kf,7 and kr,4 –kr,7 , respectively. In addition, it is assumed that χ1 = 1, because the H-radical concentration
in the post-flame region of a hydrocarbon diffusion flame has been observed to be of the
same order as [H2 ]. Finally, the OH-radical concentration is estimated by considering the
reaction
OH + H2 *
) H2 O + H
(13.1-86)
to be partially equilibrated, leading to the relationship
χ2 =
kr,8
kf,8
Values for the rate constants ka , kb , and kc for different equivalent fuel types are given
in Arrhenius form (AT b e−E/RT ) in Table 13.1.1 [189]. All rate constants have units of
m3 /gmol-s, and all values of E have units of J/gmol.
Release 12.0 c ANSYS, Inc. January 29, 2009
13-29
Pollutant Formation
Table 13.1.1: Rate Constants for Different Reburn Fuels
Equivalent
Fuel Type
CH4
CH3
CH2
CH
A
5.30 × 109
0.37 × 109
0.23 × 107
0.0
ka
b
E
-1.54 27977
-1.54 27977
-1.54 27977
0.0
0.0
A
3.31 × 1013
0.23 × 1013
0.14 × 1011
0.63 × 108
kb
b
-3.33
-3.33
-3.33
-3.33
E
15090
15090
15090
15090
A
3.06 × 1011
0.21 × 1011
0.13 × 109
0.58 × 106
kc
b
-2.64
-2.64
-2.64
-2.64
For Equation 13.1-86,
kf,8 = 1.02 × 105 T 1.60 e−13802/RT ; kr,8 = 4.52 × 105 T 1.60 e−80815/RT
13.1.8
NOx Reduction by SNCR
The selective noncatalytic reduction of NOx (SNCR), first described by Lyon [212], is a
method to reduce the emission of NOx from combustion by injecting a selective reductant
such as ammonia (NH3 ) or urea (CO(NH2 )2 ) into the furnace, where it can react with NO
in the flue gas to form N2 . However, the reductant can be oxidized as well to form NOx .
The selectivity for the reductive reactions decreases with increasing temperature [228]
while the rate of the initiation reaction simultaneously increases. This limits the SNCR
process to a narrow temperature interval, or window, where the lower temperature limit
for the interval is determined by the residence time.
Ammonia Injection
Several investigators have modeled the process using a large number of elementary reactions. A simple empirical model has been proposed by Fenimore [92], which is based on
experimental measurements. However, the model was found to be unsuitable for practical
applications. Ostberg and Dam-Johansen [260] proposed a two-step scheme describing
the SNCR process as shown in Figure 13.1.2, which is a single initiation step followed
by two parallel reaction pathways: one leading to NO reduction, and the other to NO
formation.
13-30
Release 12.0 c ANSYS, Inc. January 29, 2009
E
77077
77077
77077
77077
13.1 NOx Formation
OH
NO
NO
N2
OH
NH
3
NH
2
Figure 13.1.2: Simplified Reaction Mechanism for the SNCR Process
1
3
NO + NH3 + O2 −→ N2 + H2 O
4
2
5
3
NH3 + O2 −→ NO + H2 O
4
2
(13.1-87)
(13.1-88)
The reaction orders of NO and NH3 at 4% volume O2 and the empirical rate constants
kr and kox for Equations 13.1-87 and 13.1-88, respectively, have been estimated from
work done by Brouwer et al. [40]. The reaction order of NO was found to be 1 for
Equation 13.1-87 and the order of NH3 was found to be 1 for both reactions. As such,
the following reaction rates for NO and NH3 , at 4% volume O2 , were proposed:
RNO = −kr [NO][NH3 ] + kox [NH3 ][O2 ]
RNH3 = −kr [NO][NH3 ] − kox [NH3 ][O2 ]
(13.1-89)
(13.1-90)
The rate constants kr and kox have units of m3 /gmol-s, and are defined as
kr = 4.24 × 102 T 5.30 e−Er /RT ; kox = 3.50 × 10−1 T 7.65 e−Eox /RT
where Er = 349937.06 J/gmol and Eox = 524487.005 J/gmol.
Release 12.0 c ANSYS, Inc. January 29, 2009
13-31
Pollutant Formation
This model has been shown to give reasonable predictions of the SNCR process in pulverized coal and fluidized bed combustion applications. The model also captures the
influence of the most significant parameters for SNCR, which are the temperature of the
flue gas at the injection position, the residence time in the relevant temperature interval,
the NH3 to NO molar ratio, and the effect of combustible additives. This model overestimates the NO reduction for temperatures above the optimum temperature by an amount
similar to that of the detailed kinetic model of Miller and Bowman [228].
i
The SNCR process naturally occurs when NH3 is present in the flame as
a fuel N intermediate. For this reason, even if the SNCR model is not
activated and there is no reagent injection, the natural SNCR process may
still occur in the flame. The temperature range or “window” at which
SNCR may occur is 1073 K < T < 1373 K. To model your case without
using the natural SNCR process, please contact your support engineer for
information on how to deactivate it.
Urea Injection
Urea as a reagent for the SNCR process is similar to that of injecting ammonia and has
been used in the power station combustors to reduce NO emissions successfully. However,
both reagents, ammonia and urea, have major limitations as a NOx reducing agent. The
narrow temperature “window” of effectiveness and mixing limitations are difficult factors
to handle in a large combustor. The use of urea instead of ammonia as the reducing
agent is attractive because of the ease of storage and handling of the reagent.
The SNCR process using urea is a combination of Thermal DeNOx (SNCR with ammonia) and RAPRENOx (SNCR using cyanuric acid that, under heating, sublimes and
decomposes into isocyanic acid) since urea most probably decomposes into ammonia and
isocyanic acid [228].
One problem of SNCR processes using urea is that slow decay of HNCO as well as
the reaction channels leading to N2O and CO can significantly increase the emission
of pollutants other than NO. Urea seems to involve a significant emission of carboncontaining pollutants, such as CO and HNCO.
Also, some experimental observations [297] show that SNCR using urea is effective in a
narrow temperature window that is shifted toward higher temperatures when compared
to Thermal DeNOx processes at the same value of the ratio of nitrogen in the reducing
agent and in NO in the feed, β. The effect of increasing the β value is to increase the
efficiency of abatement, while the effect of increasing O2 concentration depends on the
temperature considered.
13-32
Release 12.0 c ANSYS, Inc. January 29, 2009
13.1 NOx Formation
The model described here is proposed by Brouwer et al. [40] and is a seven-step reduced
kinetic mechanism. Brouwer et al. [40] assumes that the breakdown of urea is instantaneous and 1 mole of urea is assumed to produce 1.1 moles of N H3 and 0.9 moles of
HNCO. The work of Rota et al. [297] proposed a finite rate two-step mechanism for the
breakdown of urea into ammonia and HNCO.
The seven-step reduced mechanism is given in Table 13.1.2 and the two-step urea breakdown mechanism is given in Table 13.1.3.
Table 13.1.2: Seven-Step Reduced Mechanism for SNCR with Urea
Reaction
N H3 + N O → N2 + H 2 O + H
N H3 + O2 → N O + H 2 O + H
HN CO + M → H + N CO + M
N CO + N O → N 2 O + CO
N CO + OH → N O + CO + H
N 2 O + OH → N2 + O2 + H
N 2 O + M → N2 + O + M
A
4.24E+02
3.500E-01
2.400E+08
1.000E+07
1.000E+07
2.000E+06
6.900E+17
b
5.30
7.65
0.85
0.00
0.00
0.00
-2.5
E
349937.06
524487.005
284637.8
-1632.4815
0
41858.5
271075.646
Table 13.1.3: Two-Step Urea Breakdown Process
Reaction
CO(N H 2 )2 → N H3 + HN CO
CO(N H 2 )2 + H 2 O → 2N H3 + CO2
A
1.27E+04
6.13E+04
b
0
0
E
65048.109
87819.133
where the units of A, in Tables 13.1.2 and 13.1.3, are m-gmol-sec and E units are J/gmol.
Transport Equations for Urea, HNCO, and NCO
When the SNCR model with urea injection is employed, in addition to the usual transport
equations, ANSYS FLUENT solves the following three additional mass transport equations
for urea, HNCO and NCO species.
∂
(ρYCO(NH2 )2 ) + ∇ · (ρ~v YCO(NH2 )2 ) = ∇ · (ρDYCO(NH2 )2 ) + SCO(NH2 )2
∂t
(13.1-91)
∂
(ρYHNCO ) + ∇ · (ρ~v YHNCO ) = ∇ · (ρDYHNCO ) + SHNCO
∂t
(13.1-92)
Release 12.0 c ANSYS, Inc. January 29, 2009
13-33
Pollutant Formation
∂
(ρYNCO ) + ∇ · (ρ~v YNCO ) = ∇ · (ρDYNCO ) + SNCO
∂t
(13.1-93)
where YCO(NH2 )2 , YHNCO and YNCO are mass fractions of urea, HNCO and NCO in the
gas phase. Source terms SCO(NH2 )2 , SHNCO and SNCO are determined according to the
rate equations given in Tables 13.1.2 and 13.1.3 and the additional source terms due to
reagent injection. These additional source terms are determined next. The source terms
in the transport equations can be written as follows:
SCO(NH2 )2 = Spl,CO(NH2 )2 + SCO(NH2 )2 −reac
(13.1-94)
SHNCO = Spl,HNCO + SHNCO−reac
(13.1-95)
SNCO = SNCO−reac
(13.1-96)
Apart from the source terms for the above three species, additional source terms for N O,
N H3 and N 2 O are also determined as follows, which should be added to the previously
calculated sources due to fuel NOx :
SNO = SNO−reac
(13.1-97)
SNH3 = Spl,NH3 + SNH3 −reac
(13.1-98)
SN2 O = SN2 O−reac
(13.1-99)
Source terms Si−reac for ith species are determined from the rate equations given in Tables 13.1.2 and 13.1.3.
Urea Production due to Reagent Injection
The rate of urea production is equivalent to the rate of reagent release into the gas phase
through droplet evaporation:
Spl,CO(NH2 )2 =
Sreagent
V
(13.1-100)
where Sreagent is the rate of reagent release from the liquid droplets to the gas phase
(kg/s) and V is the cell volume (m3 ).
13-34
Release 12.0 c ANSYS, Inc. January 29, 2009
13.1 NOx Formation
N H3 Production due to Reagent Injection
If the urea decomposition model is set to the user-specified option, then the rate of N H3
production is proportional to the rate of reagent release into the gas phase through
droplet evaporation:
Spl,NH3 = M CFN H3
Sreagent
V
(13.1-101)
where Sreagent is the rate of reagent release from the liquid droplets to the gas phase
(kg/s), M CFN H3 is the mole fraction of N H3 in the N H3 /HN CO mixture created from
urea decomposition and V is the cell volume (m3 ).
HNCO Production due to Reagent Injection
If the urea decomposition model is set to the user-specified option, then the rate of HNCO
production is proportional to the rate of reagent release into the gas phase through droplet
evaporation:
Spl,HNCO = M CFHN CO
Sreagent
V
(13.1-102)
where Sreagent , the injection source term, is the rate of reagent release from the liquid droplets to the gas phase (kg/s), M CFHN CO is the mole fraction of HNCO in the
N H3 /HN CO mixture created from urea decomposition and V is the cell volume (m3 ).
i
The mole conversion fractions (MCF) for species N H3 and HNCO are
determined through the user species values such that if one mole of urea
decomposes into 1.1 moles of N H3 and 0.9 moles of HNCO, then M CFN H3
= 0.55 and M CFHN CO = 0.45. When the user-specified option is used for
urea decomposition, then Spl,CO(NH2 )2 = 0.
However, the default option for urea decomposition is through rate limiting reactions
given in Table 13.1.3 and the source terms are calculated accordingly. In this case, both
values of Spl,N H3 and Spl,HN CO are zero.
Release 12.0 c ANSYS, Inc. January 29, 2009
13-35
Pollutant Formation
13.1.9
NOx Formation in Turbulent Flows
The kinetic mechanisms of NOx formation and destruction described in the preceding
sections have all been obtained from laboratory experiments using either a laminar premixed flame or shock-tube studies where molecular diffusion conditions are well defined.
In any practical combustion system, however, the flow is highly turbulent. The turbulent
mixing process results in temporal fluctuations in temperature and species concentration
that will influence the characteristics of the flame.
The relationships among NOx formation rate, temperature, and species concentration are
highly nonlinear. Hence, if time-averaged composition and temperature are employed
in any model to predict the mean NOx formation rate, significant errors will result.
Temperature and composition fluctuations must be taken into account by considering
the probability density functions which describe the time variation.
The Turbulence-Chemistry Interaction Model
In turbulent combustion calculations, ANSYS FLUENT solves the density-weighted timeaveraged Navier-Stokes equations for temperature, velocity, and species concentrations
or mean mixture fraction and variance. To calculate NO concentration, a time-averaged
NO formation rate must be computed at each point in the domain using the averaged
flow-field information.
Methods of modeling the mean turbulent reaction rate can be based on either moment
methods [380] or probability density function (PDF) techniques [148]. ANSYS FLUENT
uses the PDF approach.
i
The PDF method described here applies to the NOx transport equations
only. The preceding combustion simulation can use either the generalized finite-rate chemistry model by Magnussen and Hjertager or the nonpremixed combustion model. For details on these models, refer to Chapters 7 and 8.
The PDF Approach
The PDF method has proven very useful in the theoretical description of turbulent
flow [149]. In the ANSYS FLUENT NOx model, a single- or joint-variable PDF in terms
of a normalized temperature, species mass fraction, or the combination of both is used to
predict the NOx emission. If the non-premixed or partially premixed combustion model
is used to model combustion, then a one- or two-variable PDF in terms of mixture fraction(s) is also available. The mean values of the independent variables needed for the
PDF construction are obtained from the solution of the transport equations.
13-36
Release 12.0 c ANSYS, Inc. January 29, 2009
13.1 NOx Formation
The General Expression for the Mean Reaction Rate
The mean turbulent reaction rate w can be described in terms of the instantaneous rate
w and a single or joint PDF of various variables. In general,
w=
Z
···
Z
w(V1 , V2 , . . .)P (V1 , V2 , . . .)dV1 dV2 . . .
(13.1-103)
where V1 , V2 ,... are temperature and/or the various species concentrations present. P is
the probability density function (PDF).
The Mean Reaction Rate Used in ANSYS FLUENT
The PDF is used for weighting against the instantaneous rates of production of NO (e.g.,
Equation 13.1-15) and subsequent integration over suitable ranges to obtain the mean
turbulent reaction rate. Hence we have
S NO =
Z
SNO (V1 )P1 (V1 )dV1
(13.1-104)
or, for two variables
S NO =
Z Z
SNO (V1 , V2 )P (V1 , V2 )dV1 dV2
(13.1-105)
where S NO is the mean turbulent rate of production of NO, SNO is the instantaneous rate
of production given by, for example, Equation 13.1-15, and P1 (V1 ) and P (V1 , V2 ) are the
PDFs of the variables V1 and, if relevant, V2 . The same treatment applies for the HCN
or NH3 source terms.
Equation 13.1-104 or 13.1-105 must be integrated at every node and at every iteration.
For a PDF in terms of temperature, the limits of integration are determined from the
minimum and maximum values of temperature in the combustion solution. For a PDF in
terms of mixture fraction, the limits of the integrations in Equation 13.1-104 or 13.1-105
are determined from the values stored in the look-up tables.
Statistical Independence
In the case of the two-variable PDF, it is further assumed that the variables V1 and V2
are statistically independent so that P (V1 , V2 ) can be expressed as
P (V1 , V2 ) = P1 (V1 )P2 (V2 )
Release 12.0 c ANSYS, Inc. January 29, 2009
(13.1-106)
13-37
Pollutant Formation
The Beta PDF Option
ANSYS FLUENT can assume P to be a two-moment beta function that is appropriate for
combustion calculations [123, 231]. The equation for the beta function is
P (V ) =
Γ(α + β) α−1
V α−1 (1 − V )β−1
V
(1 − V )β−1 = Z 1
Γ(α)Γ(β)
V α−1 (1 − V )β−1 dV
(13.1-107)
0
where Γ( ) is the Gamma function, α and β depend on m, the mean value of the quantity
in question, and its variance, σ 2 :
!
m(1 − m)
α=m
−1
σ2
(13.1-108)
!
m(1 − m)
β = (1 − m)
−1
σ2
(13.1-109)
The beta function requires that the independent variable V assume values between 0 and
1. Thus, field variables such as temperature must be normalized. See Section 21.1.1: Setting Turbulence Parameters in the separate User’s Guide for information on using the
beta PDF when using single-mixture fraction models and two-mixture fraction models.
The Gaussian PDF Option
ANSYS FLUENT can also assume P to exhibit a clipped Gaussian form with delta functions at the tails.
The cumulative density function for a Gaussian PDF (GCDF ) may be expressed in terms
of the error function as follows:
GCDF =
√
1
1 + erf (m − m) / 2σ 2
2
(13.1-110)
where erf ( ) is the error function, m is the quantity in question, and m and σ 2 are the
mean and variance values of m, respectively. The error function may be expressed in
terms of the incomplete gamma function (gammp( )):
for m < 0 : erf (m) = −gammp(0.5, m2 )
for m ≥ 0 : erf (m) = gammp(0.5, m2 )
13-38
(13.1-111)
Release 12.0 c ANSYS, Inc. January 29, 2009
13.2 SOx Formation
The Calculation Method for σ 2
The variance, σ 2 , can be computed by solving the following transport equation during
the combustion calculation or pollutant postprocessing stage:
∂ 2
µt
ρσ + ∇ · (ρ~v σ 2 ) = ∇
∇σ 2 + Cg µt (∇m)2 − Cd ρ σ 2
∂t
σt
k
(13.1-112)
where the constants σt , Cg and Cd take the values 0.85, 2.86, and 2.0, respectively.
Note that the previous equation may only be solved for temperature. This solution may
be computationally intensive, and therefore may not always be applicable for a postprocessing treatment of NOx prediction. When this is the case or when solving for species,
the calculation of σ 2 is instead based on an approximate form of the variance transport
equation (also referred to as the algebraic form). The approximate form assumes equal
production and dissipation of variance, and is as follows:
σ2 =
µt k Cg
µt k Cg ∂m
(∇m)2 =
ρ Cd
ρ Cd
∂x
!2
+
∂m
∂y
!2
+
!2
∂m
∂z
(13.1-113)
The term in the brackets is the dissipation rate of the independent variable.
For a PDF in terms of mixture fraction, the mixture fraction variance has already been
solved as part of the basic combustion calculation, so no additional calculation for σ 2 is
required.
13.2
SOx Formation
The following sections include information on the theory used in the SOx model. For
information about using the SOx models in ANSYS FLUENT, see Section 21.2.1: Using
the SOx Model in the separate User’s Guide.
• Section 13.2.1: Overview
• Section 13.2.2: Governing Equations for SOx Transport
• Section 13.2.3: Reaction Mechanisms for Sulfur Oxidation
• Section 13.2.4: SO2 and H 2 S Production in a Gaseous Fuel
• Section 13.2.5: SO2 and H 2 S Production in a Liquid Fuel
• Section 13.2.6: SO2 and H 2 S Production from Coal
• Section 13.2.7: SOx Formation in Turbulent Flows
Release 12.0 c ANSYS, Inc. January 29, 2009
13-39
Pollutant Formation
13.2.1
Overview
Sulfur exists in coal as organic sulfur, pyretic and sulfates [1], and exists in liquid fuels
mostly in organic form [235], with mass fractions ranging from 0.5% to 3%. All SOx
emissions are produced because of the oxidation of fuel-bound sulfur. During the combustion process, fuel sulfur is oxidized to SO2 and SO3 . A portion of the gaseous SOx
will condense on the particles, attaching an amount of water and thus forming sulfuric
acid, or may react further to form sulfates. While SOx emissions are the main cause of
acid rain, SO3 also contributes to particulate emissions, and is responsible for corrosion
of combustion equipment. Furthermore, there is a growing interest in the interaction
of sulfur species with the nitrogen oxide chemistry [235], as NO levels are affected by
the presence of sulfur species. The evidence to date indicates that thermal NO levels
(Section 13.1.3: Thermal NOx Formation) are reduced in the presence of SO2 . However,
the effect of sulfur compounds on the fuel NOx formation is yet to be clarified.
Sulfur emissions are regulated from stationary sources and from automotive fuels. Sulfur pollutants can be captured during the combustion process, or with after treatment
methods, such as wet or dry scrubbing. Coal fired boilers are by far the biggest single
SOx emissions source, accounting for over 50% of total SO2 emissions [55].
For higher sulfur concentrations in the fuel, the SOx concentration field should be resolved
together with the main combustion calculation using any of the ANSYS FLUENT reaction
models. For cases where the sulfur fraction in fuel is low, the post-processing option can
be used, which solves transport equations for H 2 S, SO2 , SO, SH, and SO3 .
The Formation of SOx
The SOx model incorporates the following stages:
1. Sulfur release from the fuel
For liquid fuels, one can conveniently assume that sulfur is released as H2 S [235].
However, the process is more complicated in the case of coal; here some of the
sulfur is decomposed into the gas phase during devolatilization as H 2 S, COS, SO2
and CS2 , while part of the sulfur is retained in the char to be oxidized at a later
stage. The percentage of sulfur retained in char is rank dependent [1].
2. Sulfur reaction in the gas phase
In oxygen rich flames the predominant sulfur species are SO, SO2 and SO3 . At lower
oxygen concentrations H 2 S, S2 and SH are also present in significant proportions,
while SO3 becomes negligible [235]. In PCGC-3 as well as in the works of Norman
et al. [251] the gas phase sulfur species are assumed to be in equilibrium.
3. Sulfur retention in sorbents
Sulfur pollutants can be absorbed by sorbent particles, injected either in situ, or in
the post flame region.
13-40
Release 12.0 c ANSYS, Inc. January 29, 2009
13.2 SOx Formation
For low sulfur fuels, we can assume that sulfur is mainly released as H 2 S. The rate
of release can be determined similarly to that of fuel-bound N. For the char S it can
be assumed that SO2 is produced directly at the same rate as that of char burnout.
Transport equations for H 2 S, SO2 , SO, SH, and SO3 species are incorporated and an
appropriate reaction set has been developed as described in the ensuing sections.
13.2.2 Governing Equations for SOx Transport
ANSYS FLUENT solves the mass transport equations for the SO2 species, taking into
account convection, diffusion, production and consumption of SO2 and related species.
This approach is completely general, being derived from the fundamental principle of
mass conservation. The effect of residence time in SOx mechanisms, a Lagrangian reference frame concept, is included through the convection terms in the governing equations
written in the Eulerian reference frame. If all fuel sulfur is assumed to convert directly
to SO2 and the other product and intermediate species are assumed negligible, then only
the SO2 species transport equation is needed:
∂
(ρYSO2 ) + ∇ · (ρ~v YSO2 ) = ∇ · (ρD∇YSO2 ) + SSO2
∂t
(13.2-1)
As discussed in Section 13.2.3: Reaction Mechanisms for Sulfur Oxidation, SOx formation mechanisms involve multiple reactions among multiple species, and tracking sulfurcontaining intermediate species is important. ANSYS FLUENT solves transport equations
for the H 2 S, SO3 , SO, and SH species in addition to the SO2 species:
∂
(ρYH2 S ) + ∇ · (ρ~v YH2 S ) = ∇ · (ρDYH2 S ) + SH2 S
∂t
(13.2-2)
∂
(ρYSO3 ) + ∇ · (ρ~v YSO3 ) = ∇ · (ρDYSO3 ) + SSO3
∂t
(13.2-3)
∂
(ρYSO ) + ∇ · (ρ~v YSO ) = ∇ · (ρDYSO ) + SSO
∂t
(13.2-4)
∂
(ρYSH ) + ∇ · (ρ~v YSH ) = ∇ · (ρDYSH ) + SSH
∂t
(13.2-5)
where YSO2 , YH2 S , YSO3 , YSO , and YSH are mass fractions of SO2 , H 2 S, SO3 , SO, and SH
in the gas phase. The source terms SSO2 , SH2 S , SSO3 , SSO , and SSH are to be determined
depending on the form of fuel sulfur release (SO2 and/or H 2 S) and inclusion of SO3 , SO
and SH in the SOx mechanism.
Release 12.0 c ANSYS, Inc. January 29, 2009
13-41
Pollutant Formation
13.2.3
Reaction Mechanisms for Sulfur Oxidation
A detailed reaction mechanism for sulfur oxidation has been proposed by Kramlich [172].
The mechanism consists of 20 reversible reactions and includes 12 species (S, S2 , SH, SO,
SO2 , H 2 S, H, H2 , OH, H 2 O, O and O2 ). The mechanism has been reduced to 8 steps and
10 species (with S and S2 removed), and validated in Perfectly Stirred Reactor (PSR)
and Plug Flow Reactor (PFR) simulations. Table 13.2.1 lists the reduced mechanism
with the modified rate constants. For reduction calculations O and OH concentrations
have been calculated through partial equilibrium assumptions based on O2 and H 2 O
concentrations, respectively. N2 was used as the dilutant. Since each reaction of the
eight-step reduced mechanism is reversible, for each adjacent pair of reactions given in
Table 13.2.1, the second reaction is in fact the reverse reaction of the first.
The reduced mechanism given in Table 13.2.1 closely follows the SO2 concentration
levels but slightly overpredicts the H 2 S concentrations at temperatures below 1500 K.
Above 1500 K, both mechanisms are in close agreement for SO2 and H 2 S concentration
predictions. However, SO and SH are not well correlated by the reduced mechanism
when compared against the predictions using the original detailed mechanism.
A major concern in these mechanisms is the presence of H radical and the method in
which to calculate its concentration in the flow field. At present, the concentration of
H radical is assumed to be proportional to the O radical concentration, which can be
evaluated from one of the existing methods in ANSYS FLUENT; viz. Partial Equilibrium (Section 13.1.3: Method 2: Partial Equilibrium Approach) or Equilibrium (Section 13.1.3: Method 1: Equilibrium Approach). The user is then given the option to
vary the proportionality constant. Although this assumption is open to debate, the lack
of simple relation to calculate the H radical concentration in a flame has prompted the
present choice.
Present implementation allows the user to either include or remove SO3 from the calculations. Also, depending on the form of fuel sulfur release (e.g., H 2 S or SO2 ) the species
H 2 S may or may not be present for the calculation. The user is also given the extended
option of partitioning the intermediate fuel sulfur species to H 2 S and SO2 . However,
there is no literature to guide the user on how to select a correct partition fraction.
A is in m3 /gmol-s, E is J/gmol (assumed 1 cal = 4.18585 J), A units for the thirteenth
reaction is m6 /gmol2 -s, and A units for the fifteenth reaction is m6 /gmol2 -s.
In addition, the following two reactions were included in ANSYS FLUENT to complete
the SOx mechanism, with the rate constants taken from Hunter’s work [135].
SO2 + O + M ⇐⇒ SO3 + M
(13.2-6)
M = argon, nitrogen, oxygen
kf 1 = 3.63 x 102 exp(+4185.85/RT) m6 /gmol2 /sec
13-42
Release 12.0 c ANSYS, Inc. January 29, 2009
13.2 SOx Formation
Table 13.2.1: Eight-Step Reduced Mechanism (Rate Constant k
AT b exp(−E/RT ))
Reaction
H 2 S + H → SH + H2
SH + H2 → H 2 S + H
OH + H 2 S → H 2 O + SH
H 2 O + SH → OH + H 2 S
SO + OH → H + SO2
H + SO2 → SO + OH
SH + O → SO + H
SO + H → SH + O
O + H 2 S → SH + OH
SH + OH → O + H 2 S
SO + O2 → SO2 + O
SO2 + O → SO + O2
H + SH + M → H 2 S + M
H 2 S + M → H + SH + M
SO + O + M → SO2 + M
SO2 + M → SO + O + M
Release 12.0 c ANSYS, Inc. January 29, 2009
A
1.819702E+07
9.375623E+06
1.380385E+02
3.104557E+07
1.621810E+08
7.691299E+09
3.548135E+08
2.985385E+09
4.365162E+03
9.885528E+08
4.466832E+05
1.663412E+06
1.096478E+03
8.669613E+14
8.709647E+09 k
1.905464E+14
b
0.0E+00
0.0E+00
0.0E+00
0.0E+00
0.0E+00
0.0E+00
0.0E+00
0.0E+00
0.0E+00
0.0E+00
0.0E+00
0.0E+00
0.0E+00
0.0E+00
-1.8E+00
0.0E+00
=
E
7.484300E+03
6.253660E+04
3.742150E+03
1.218543E+05
2.565926E+03
1.187023E+05
2.687316E+03
1.694600E+05
1.380493E+04
6.035996E+04
2.703222E+04
7.613643E+04
0.000000E+00
3.819463E+05
0.000000E+00
5.207365E+05
13-43
Pollutant Formation
where R = 8.313 J/gmol-K
kr1 = 7.41 x 1014 exp(-346123.75/RT) m3 /gmol/sec
SO3 + O ⇐⇒ SO2 + O2
(13.2-7)
kf 2 = 1.2 x 106 exp(-39765.575/RT) m3 /gmol/sec
The reverse rate of Equation 13.2-7 was determined through the equilibrium constant for
that equation.
13.2.4
SO2 and H 2 S Production in a Gaseous Fuel
The rate of SO2 or H 2 S production is equivalent to the rate of combustion of the fuel:
Spl,i =
where
Spl,i
Rcf
YS,fuel
=
=
=
Rcf YS,fuel Mw,i
Mw,S
(13.2-8)
source of i (kg/m3 -s), where i = SO2 or H 2 S
mean limiting reaction rate of fuel (kg/m3 -s)
mass fraction of sulfur in the fuel
The mean limiting reaction rate of fuel, Rcf , is calculated from the Magnussen combustion
model, so the gaseous fuel option for SOx formation is available only when the generalized
finite-rate model is used.
13.2.5
SO2 and H 2 S Production in a Liquid Fuel
The rate of SO2 or H 2 S production is equivalent to the rate of fuel release into the gas
phase through droplet evaporation:
Spl,i =
where
13.2.6
Spl,i
Sfuel
YS,fuel
V
=
=
=
=
Sfuel YS,fuel Mw,i
Mw,S V
(13.2-9)
source of i (kg/m3 -s), where i = SO2 or H 2 S
rate of fuel release from the liquid droplets to the gas (kg/s)
mass fraction of sulfur in the fuel
cell volume (m3 )
SO2 and H 2 S Production from Coal
For coal, it is assumed that sulfur is distributed between the volatiles and the char. Since
there is no reason to assume that S is equally distributed between the volatiles and the
char, the fraction of S in the volatiles and the char should be specified separately.
13-44
Release 12.0 c ANSYS, Inc. January 29, 2009
13.2 SOx Formation
SO2 and H 2 S from Char
The source of SO2 and H 2 S from the char is related to the rate of char combustion:
Schar,i =
where
Sc
Schar,i
YS,char
V
=
=
=
=
Sc YS,char Mw,i
Mw,S V
(13.2-10)
char burnout rate (kg/s)
source of i (kg/m3 -s) in char, where i = SO2 or H 2 S
mass fraction of sulfur in char
cell volume (m3 )
SO2 and H 2 S from Volatiles
The source of SO2 and H 2 S from the volatiles is related to the rate of volatile release:
Svol,i =
where
Svol,i
YS,vol
V
13.2.7
Svol YS,vol Mw,i
Mw,S V
(13.2-11)
= source of volatiles originating from
the coal particles into the gas phase (kg/s), where i = SO2 or H 2 S
= mass fraction of sulfur in the volatiles
= cell volume (m3 )
SOx Formation in Turbulent Flows
The kinetic mechanisms of SOx formation and destruction are obtained from laboratory experiments in a similar fashion to the NOx model. In any practical combustion
system, however, the flow is highly turbulent. The turbulent mixing process results in
temporal fluctuations in temperature and species concentration that will influence the
characteristics of the flame.
The relationships among SOx formation rate, temperature, and species concentration are
highly nonlinear. Hence, if time-averaged composition and temperature are employed
in any model to predict the mean SOx formation rate, significant errors will result.
Temperature and composition fluctuations must be taken into account by considering
the probability density functions which describe the time variation.
Release 12.0 c ANSYS, Inc. January 29, 2009
13-45
Pollutant Formation
The Turbulence-Chemistry Interaction Model
In turbulent combustion calculations, ANSYS FLUENT solves the density-weighted timeaveraged Navier-Stokes equations for temperature, velocity, and species concentrations
or mean mixture fraction and variance. To calculate SO2 concentration, a time-averaged
SO2 formation rate must be computed at each point in the domain using the averaged
flow-field information.
The PDF Approach
The PDF method has proven very useful in the theoretical description of turbulent
flow [149]. In the ANSYS FLUENT SOx model, a single- or joint-variable PDF in terms
of a normalized temperature, species mass fraction, or the combination of both is used
to predict the SOx emission. If the non-premixed combustion model is used to model
combustion, then a one- or two-variable PDF in terms of mixture fraction(s) is also available. The mean values of the independent variables needed for the PDF construction are
obtained from the solution of the transport equations.
The Mean Reaction Rate
The mean turbulent reaction rate described in Section 13.1.9: The General Expression for
the Mean Reaction Rate for the NOx model also applies to the SOx model. The PDF is
used for weighting against the instantaneous rates of production of SO2 and subsequent
integration over suitable ranges to obtain the mean turbulent reaction rate as described
in Equations 13.1-104 and 13.1-105 for NOx .
The PDF Options
As is the case with the NOx model, P can be calculated as either a two-moment beta function or as a clipped Gaussian function, as appropriate for combustion calculations [123,
231]. Equations 13.1-107 – 13.1-111 apply to the SOx model as well, with the variance
σ 2 computed by solving a transport equation during the combustion calculation stage,
using Equation 13.1-112 or Equation 13.1-113.
13-46
Release 12.0 c ANSYS, Inc. January 29, 2009
13.3 Soot Formation
13.3
Soot Formation
Information about the theory behind soot formation is presented in the following sections. For information about using soot formation models in ANSYS FLUENT, see Section 21.3.1: Using the Soot Models in the separate User’s Guide.
• Section 13.3.1: Overview and Limitations
• Section 13.3.2: Soot Model Theory
13.3.1
Overview and Limitations
ANSYS FLUENT provides four models for the prediction of soot formation in combustion
systems. In addition, the predicted soot concentration can be coupled with radiation.
That is, you can include the effect of soot on radiation absorption when you use the
P-1, discrete ordinates, or discrete transfer radiation model with a variable absorption
coefficient.
Predicting Soot Formation
ANSYS FLUENT predicts soot concentrations in a combustion system using one of four
available models:
• the one-step Khan and Greeves model [162], in which ANSYS FLUENT predicts the
rate of soot formation based on a simple empirical rate
• the two-step Tesner model [216, 349], in which ANSYS FLUENT predicts the formation of nuclei particles, with soot formation on the nuclei
• the Moss-Brookes model [39], in which ANSYS FLUENT predicts soot formation
for methane flames (and higher hydrocarbon species, if appropriately modified) by
solving transport equations for normalized radical nuclei concentration and the soot
mass fraction
• the Moss-Brookes-Hall model [120], which is an extension of the Moss-Brookes
model and is applicable for higher hydrocarbon fuels (e.g., kerosene)
The Khan and Greeves model is the default model used by ANSYS FLUENT when you
include soot formation.
Release 12.0 c ANSYS, Inc. January 29, 2009
13-47
Pollutant Formation
In the Khan and Greeves model and the Tesner model, combustion of the soot (and
particle nuclei) is assumed to be governed by the Magnussen combustion rate [216]. Note
that this limits the use of these soot formation models to turbulent flows. Both models
are empirically-based, approximate models of the soot formation process in combustion
systems. The detailed chemistry and physics of soot formation are quite complex and are
only approximated in these models. You should view the results of the Khan and Greeves
model and the Tesner model as qualitative indicators of your system performance unless
you can undertake experimental validation of the results.
The Moss-Brookes model has less impiricism and should theoretically provide superior
accuracy than the Khan and Greeves and Tesner models. The Hall extension provides
further options for modeling higher hydrocarbon fuels. Note that the Moss-Brookes-Hall
model is only available when the required species are present in the gas phase species
list.
Restrictions on Soot Modeling
The following restrictions apply to soot formation models:
• You must use the pressure-based solver. The soot models are not available with
either of the density-based solvers.
• The Khan and Greeves model and the Tesner model can model soot formation only
for turbulent flows (whereas the Moss-Brookes model and the Moss-Brookes-Hall
model can be used with both laminar and turbulent flows).
• The soot model cannot be used in conjunction with the premixed combustion model.
13.3.2
Soot Model Theory
The One-Step Soot Formation Model
In the one-step Khan and Greeves model [162], ANSYS FLUENT solves a single transport
equation for the soot mass fraction:
∂
µt
(ρYsoot ) + ∇ · (ρ~v Ysoot ) = ∇ ·
∇Ysoot + Rsoot
∂t
σsoot
(13.3-1)
where
Ysoot
σsoot
Rsoot
= soot mass fraction
= turbulent Prandtl number for soot transport
= net rate of soot generation (kg/m3 -s)
Rsoot , the net rate of soot generation, is the balance of soot formation, Rsoot,form , and
soot combustion, Rsoot,comb :
13-48
Release 12.0 c ANSYS, Inc. January 29, 2009
13.3 Soot Formation
Rsoot = Rsoot,form − Rsoot,comb
(13.3-2)
The rate of soot formation is given by a simple empirical rate expression:
Rsoot,form = Cs pfuel φr e−E/RT
(13.3-3)
where
Cs
pfuel
φ
r
E/R
=
=
=
=
=
soot formation constant (kg/N-m-s)
fuel partial pressure (Pa)
equivalence ratio
equivalence ratio exponent
activation temperature (K)
The rate of soot combustion is the minimum of two rate expressions [216]:
Rsoot,comb = min[R1 , R2 ]
(13.3-4)
The two rates are computed as
R1 = AρYsoot
k
(13.3-5)
and
R2 = Aρ
Yox
νsoot
Ysoot νsoot
Ysoot νsoot + Yfuel νfuel
k
(13.3-6)
where
A
Yox , Yfuel
νsoot , νfuel
= constant in the Magnussen model
= mass fractions of oxidizer and fuel
= mass stoichiometries for soot and fuel combustion
The default constants for the one-step model are valid for a wide range of hydrocarbon
fuels.
Release 12.0 c ANSYS, Inc. January 29, 2009
13-49
Pollutant Formation
The Two-Step Soot Formation Model
The two-step Tesner model [349] predicts the generation of radical nuclei and then computes the formation of soot on these nuclei. ANSYS FLUENT thus solves transport
equations for two scalar quantities: the soot mass fraction (Equation 13.3-1) and the
normalized radical nuclei concentration:
∂
µt
(ρb∗nuc ) + ∇ · (ρ~v b∗nuc ) = ∇ ·
∇b∗
+ R∗nuc
∂t
σnuc nuc
(13.3-7)
where
b∗nuc
σnuc
R∗nuc
= normalized radical nuclei concentration (particles ×10−15 /kg)
= turbulent Prandtl number for nuclei transport
= normalized net rate of nuclei generation (particles ×10−15 /m3 -s)
In these transport equations, the rates of nuclei and soot generation are the net rates,
involving a balance between formation and combustion.
Soot Generation Rate
The two-step model computes the net rate of soot generation, Rsoot , in the same way as
the one-step model, as a balance of soot formation and soot combustion:
Rsoot = Rsoot,form − Rsoot,comb
(13.3-8)
In the two-step model, however, the rate of soot formation, Rsoot,form , depends on the
concentration of radical nuclei, cnuc :
Rsoot,form = mp (α − βNsoot )cnuc
(13.3-9)
where
mp
Nsoot
cnuc
α
β
=
=
=
=
=
mean mass of soot particle (kg/particle)
concentration of soot particles (particles/m3 )
radical nuclei concentration = ρbnuc (particles/m3 )
empirical constant (s−1 )
empirical constant (m3 /particle-s)
The rate of soot combustion, Rsoot,comb , is computed in the same way as for the one-step
model, using Equations 13.3-4–13.3-6.
The default constants for the two-step model are for combustion of acetylene (C2 H2 ).
According to Ahmad et al. [2], these values should be modified for other fuels, since the
sooting characteristics of acetylene are known to be different from those of saturated
hydrocarbon fuels.
13-50
Release 12.0 c ANSYS, Inc. January 29, 2009
13.3 Soot Formation
Nuclei Generation Rate
The net rate of nuclei generation in the two-step model is given by the balance of the
nuclei formation rate and the nuclei combustion rate:
R∗nuc = R∗nuc,form − R∗nuc,comb
(13.3-10)
where
R∗nuc,form
R∗nuc,comb
= rate of nuclei formation (particles ×10−15 /m3 -s)
= rate of nuclei combustion (particles ×10−15 /m3 -s)
The rate of nuclei formation, R∗nuc,form , depends on a spontaneous formation and branching process, described by
R∗nuc,form = η0 + (f − g)c∗nuc − g0 c∗nuc Nsoot
(13.3-11)
η0 = a∗0 cfuel e−E/RT
(13.3-12)
where
c∗nuc
a∗0
a0
cfuel
f −g
g0
=
=
=
=
=
=
normalized nuclei concentration (= ρb∗nuc )
a0 /1015
pre-exponential rate constant (particles/kg-s)
fuel concentration (kg/m3 )
linear branching − termination coefficient (s−1 )
linear termination on soot particles (m3 /particle-s)
Note that the branching term, (f − g)c∗nuc , in Equation 13.3-11 is included only when
the kinetic rate, η0 , is greater than the limiting formation rate (105 particles/m3 -s, by
default).
The rate of nuclei combustion is assumed to be proportional to the rate of soot combustion:
R∗nuc,comb = Rsoot,comb
b∗nuc
Ysoot
(13.3-13)
where the soot combustion rate, Rsoot,comb , is given by Equation 13.3-4.
Release 12.0 c ANSYS, Inc. January 29, 2009
13-51
Pollutant Formation
The Moss-Brookes Model
The Moss-Brookes model solves transport equations for normalized radical nuclei concentration b∗nuc and soot mass fraction Ysoot :
∂
µt
dM
(ρYsoot ) + ∇ · (ρ~v Ysoot ) = ∇ ·
∇Ysoot +
∂t
σsoot
dt
(13.3-14)
∂
µt
1 dN
(ρb∗nuc ) + ∇ · (ρ~v b∗nuc ) = ∇ ·
∇b∗nuc +
∂t
σnuc
Nnorm dt
(13.3-15)
where
Ysoot
M
b∗nuc
N
Nnorm
=
=
=
=
=
soot mass fraction
soot mass concentration (kg/m3 )
normalized radical nuclei concentration (particles ×10−15 /kg) =
soot particle number density (particles/m3 )
1015 particles
N
ρNnorm
The instantaneous production rate of soot particles, subject to nucleation from the gas
phase and coagulation in the free molecular regime, is given by
dN
Xprec P l
Tα
= Cα NA
exp −
− Cβ
dt
RT
T
|
{z
} |
Nucleation
24RT
ρsoot NA
!1/2
{z
2
d1/2
p N
Coagulation
(13.3-16)
}
where Cα , Cβ and l are model constants. Here, NA (= 6.022045x1026 kmol−1 ) is the
Avogadro number and Xprec is the mole fraction of soot precursor (for methane, the
precursor is assumed to be acetylene, whereas for kerosene it is a combination of acetylene
and benzene). The mass density of soot, ρsoot , is assumed to be 1800 kg/m3 and dp is
the mean diameter of a soot particle. The nucleation rate for soot particles is taken
to be proportional to the local acetylene concentration for methane. The activation
temperature Tα for the nucleation reaction is that proposed by Lindstedt [199].
13-52
Release 12.0 c ANSYS, Inc. January 29, 2009
13.3 Soot Formation
The source term for soot mass concentration is modeled by the expression
dM
dt
= MP Cα
|
Xprec P l
Xsgs P
Tα
+ Cγ
exp −
RT {z
T }
RT
|
Nucleation
− Coxid Cω ηcoll
|
XOH P
RT
√
1/3
T (πN )
{z
Oxidation
6M
ρsoot
m
Tγ
6M
exp −
(πN )1/3
T
ρsoot
!2/3 n
{z
}
Surface Growth
!2/3
(13.3-17)
}
where Cγ , Coxid , Cω , m, and n are additional model constants. The constant MP (= 144
kg/kgmol) is the mass of an incipient soot particle, here taken to consist of 12 carbon
atoms. Even though the model is not found to be sensitive to this assumption, a nonzero
initial mass is needed to begin the process of surface growth. Here, Xsgs is the mole
fraction of the participating surface growth species. For paraffinic fuels, soot particles
have been found to grow primarily by the addition of gaseous species at their surfaces,
particularly acetylene that has been found in abundance in the sooting regions of laminar
methane diffusion flames.
The model assumes that the hydroxyl radical is the dominant oxidizing agent in methane/air
diffusion flames and that the surface-specific oxidation rate of soot by the OH radical may
be formulated according to the model proposed by Fenimore and Jones [93]. Assuming a
collision efficiency (ηcoll ) of 0.04, the oxidation rate may be written as (Equation 13.3-17.
The process of determination of the exponents l, m, and n are explained in detail by
Brookes and Moss [39]. The constants Cα and Cβ are determined through numerical
modeling of a laminar flame for which experimental data exists.
The set of constants proposed by Brookes and Moss for methane flames are given below:
Cα
Tα
Cβ
Cγ
Tγ
Cω
ηcoll
Coxid
=
=
=
=
=
=
=
=
54 s−1 (model constant for soot inception rate)
21000 K (activation temperature of soot inception)
1.0 (model constant for coagulation rate)
11700 kg.m.kmol−1 .s−1 (surface growth rate scaling factor)
12100 K (activation temperature of surface growth rate)
105.8125 kg.m.kmol−1 .K−1/2 .s−1 (oxidation model constant)
0.04 (collisional efficiency parameter)
0.015 (oxidation rate scaling parameter)
Note that the implementation of the Moss-Brookes model in ANSYS FLUENT uses the
values listed above, except for Coxid which is set to unity by default.
The closure for the mean soot source terms in the above equations was also described in
detail by Brookes and Moss [39]. The uncorrelated closure is the preferred option for a
tractable solution of the above transport equations.
Release 12.0 c ANSYS, Inc. January 29, 2009
13-53
Pollutant Formation
Moss et al. [239] have shown the above model applied to kerosene flames by modifying only
the soot precursor species (in the original model the precursor was acetylene, whereas
for kerosene flames the precursor was assumed to be a combination of both acetylene
and benzene) and by setting the value of oxidation scaling parameter Coxid to unity. A
good comparison against the experimental measurements for the lower pressure (7 bar)
conditions was observed. The predictions of soot formation within methane flames have
shown the Brooks and Moss [39] model to be superior compared with the standard Tesner
et al. [349] formulation.
The Coal-Derived Soot Extension (Beta Feature)
The present implementation provides an extension to the Moss-Brookes soot model that
accounts for coal-derived soot, based on the work of Brown [41]. This extension includes
an additional transport equation for the tar evolved during coal devolatilization. The
Moss-Brookes model assumes that the physical properties of tar is similar to those of
volatiles, such that the combined effect of volatile and tar on the gas phase flame simulation may be replaced by a single volatile stream (consisting of volatile and tar). In
reality, however, this may not be the case, and so the coal-derived soot extension allows
you to treat the tar contribution similar to that of volatiles.
The following set of paths was assumed for the coal-derived soot formation [214] (see
Figure 13.3.1).
Coal
Devolatilization
Char + Light Gases + Tar
Formation
Primary Soot
Gasification
Light Gases
Agglomeration
Soot Agglomerates
Tar
Figure 13.3.1: Presumed Path for Coal-Derived Soot
13-54
Release 12.0 c ANSYS, Inc. February 9, 2009
13.3 Soot Formation
Nucleation is assumed to be the first step in formation of soot in most light gas flames,
and acetylene is understood to be the major species involved. In heavier gas flames,
benzene and other polycyclic aromatic hydrocarbons (PAHs) may contribute to soot
formation as well. Soot formation in coal flames is thought to occur as tars or the higher
molecular weight hydrocarbons given off during devolatilization combine and condense to
form soot particles. This is a different mechanism to that of soot formation from gaseous
fuels. The related source term for each path is given as follows:
Ssoot = Formationsoot − Oxidationsoot
(13.3-18)
Star = Formationtar − Formationsoot − Gasificationtar − Oxidationtar
Snuclei =
1
Nnorm
NA
Formationsoot − Agglomerationnuclei
Mw,soot
(13.3-19)
!
(13.3-20)
where Nnorm is equal to 1015 particles, NA is Avogadro’s Number, and Mw,soot is the
molecular weight of the soot particle. The remaining terms in the previous overall source
expressions are defined as follows:
Formationtar = SPtar
(13.3-21)
Oxidationtar = ρ2 Ytar YO2 AOtar exp {−EOtar /RT }
(13.3-22)
Gasificationtar = ρ Ytar AGtar exp {−EGtar /RT }
(13.3-23)
Formationsoot = ρ Ytar AFsoot exp {−EFsoot /RT }
(13.3-24)
Agglomerationnuclei = 2Ca
Release 12.0 c ANSYS, Inc. January 29, 2009
6Mw,C
πρsoot
!1
6
6kB T
ρsoot
!1
2
ρYsoot
Mw,C
!1
6
11
(ρNnorm b∗nuc ) 6
(13.3-25)
13-55
Pollutant Formation
The soot oxidation term (Oxidationsoot ) is similar to that shown in Equation 13.3-17
in the Moss-Brookes soot model theory (Fenimore-Jones or Lee oxidation model). Soot
density (ρsoot ) is assumed to be 1950 kg/m3 and the collision constant Ca is set to 3.0.
Mw,C (= 12 kg/kgmol) is the molecular weight of carbon and kB (= 1.3806503e-23 J/K)
is the Boltzmann constant. An incipient soot particle is assumed to consist of 9e+04
carbon atoms, thus making Mw,soot = 108e+04 kg/kgmol. b∗nuc is the normalized radical
nuclei concentration (i.e., the number of particles ×10−15 /kg). Since the coal-derived
soot particles are large, the turbulent Schmidt number used in the transport equations
for soot mass fraction and the normalized number density must be modified to account
for the particle size. A value of 700 for the turbulent Schmidt number is suggested for
soot mass fraction and nuclei transport.
The term SPtar is the tar release rate from coal (kg/m3 -s) and comes from the coal
particle source computations of the discrete phase model. It is assumed that the mass
fraction of tar in coal volatiles is in the range 0.3–0.5, and therefore the SPtar term is
related to the volatile source term via the tar mass fraction in volatiles. One of the main
assumptions of this implementation is that tar may be decoupled from the flow field
computations, since tar is a fraction of volatiles and volatile transport is fully coupled
with the flow field.
The values used for the pre-exponential constant A and the activation energy E in Equations 13.3-22–13.3-24 are listed in Table 13.3.1.
Table 13.3.1: Rate Constants for Coal-Derived Soot
Term
Oxidationtar
Gasificationtar
Formationsoot
A
6.77e+05 (m3 /kg-s)
9.77e+10 (1/s)
5.02e+08 (1/s)
E (kJ/kgmol)
52,300
286,900
198,900
The Moss-Brookes-Hall Model
Since the Moss-Brookes model was mainly developed and validated for methane flames,
a further extension for higher hydrocarbon fuels called the Moss-Brookes-Hall model was
also included in the present ANSYS FLUENT implementation. Here, the extended version
is a model reported by Wen et al. [374] based on model extensions proposed by Hall et
al. [120] and an oxidation model proposed by Lee et al. [184]. The work of Hall [120] is
based on a soot inception rate due to two-ringed and three-ringed aromatics, as opposed
to the Moss-Brookes assumption of a soot inception due to acetylene or benzene (for
higher hydrocarbons).
13-56
Release 12.0 c ANSYS, Inc. January 29, 2009
13.3 Soot Formation
Hall et al. [120] proposed a soot inception rate based on the formation rates of two-ringed
and three-ringed aromatics (C10 H7 and C14 H10 ), from acetylene (C2 H2 ), benzene (C6 H6 ),
and the phenyl radical (C6 H5 ) based on the following mechanisms:
2 C 2 H2 + C 6 H 5 *
) C10 H7 + H2
(13.3-26)
C 2 H2 + C 6 H6 + C 6 H 5 *
) C14 H10 + H + H2
(13.3-27)
Based on their laminar methane flame data, the inception rate of soot particles was given
to be eight times the formation rate of species C10 H7 and C14 H10 , as shown by
!
dN
dt
inception
NA 2 YC2 H2
= 8Cα,1
ρ
MP
WC2 H2
!2
YC6 H5 WH2
Tα,1
exp −
WC6 H5 YH2
T
"
#
NA 2 YC2 H2 YC6 H6 YC6 H5 WH2
Tα,2
+8Cα,2
ρ
exp −
MP
WC2 H2 WC6 H6 WC6 H5 YH2
T
(13.3-28)
where Cα,1 = 127x108.88 s−1 , Cα,2 = 178x109.50 s−1 , Tα,1 = 4378 K, and Tα,2 = 6390 K
as determined by Hall et al. [120]. In their model, the mass of an incipient soot particle
was assumed to be 1200 kg/kgmol (corresponding to 100 carbon atoms, as opposed to
12 carbon atoms used by Brookes and Moss [39]). The mass density of soot was assumed
to be 2000 kg/m3 , which is also slightly different from the value used by Brookes and
Moss. [39]
Both the coagulation term and the surface growth term were formulated similar to those
used by Brookes and Moss [39] with a slight modification to the constant Cγ so that the
value is 9000.6 kg.m.kmol−1 .s−1 (based on the model developed by Lindstedt [200]).
For the soot oxidation term, oxidation due to O2 (based on measurements and model
based on Lee et al. [184]) was added, in addition to the soot oxidation due to the hydroxyl
radical. By assuming that the kinetics of surface reactions is the limiting mechanism and
that the particles are small enough to neglect the diffusion effect on the soot oxidation,
they derived the specific rate of soot oxidation by molecular oxygen. Therefore the full
soot oxidation term, including that due to hydroxyl radical, is of the form
dM
dt
!
= −Coxid Cω,1 ηcoll
oxidation
−Coxid Cω,2
Release 12.0 c ANSYS, Inc. January 29, 2009
XOH P
RT
XO2 P
RT
√
1/3
T (πN )
6M
ρsoot
!2/3
Tω,2 √
6M
exp −
T (πN )1/3
T
ρsoot
!2/3
(13.3-29)
13-57
Pollutant Formation
Here, the collision efficiency is assumed to be 0.13 (compared to 0.04 used by Brookes
and Moss) and the oxidation rate scaling parameter is assumed to be unity. The model
constants used are as follows:
where
Cω,1
Cω,2
Tω,2
= 105.81 kg.m.kmol−1 .K−1/2 .s−1 (same as that used by Brookes and
Moss)
= 8903.51 kg.m.kmol−1 .K−1/2 .s−1
= 19778 K
Soot Formation in Turbulent Flows
The kinetic mechanisms of soot formation and destruction for the Moss-Brookes model
and the Hall extension are obtained from laboratory experiments in a similar fashion
to the NOx model. In any practical combustion system, however, the flow is highly
turbulent. The turbulent mixing process results in temporal fluctuations in temperature
and species concentration that will influence the characteristics of the flame.
The relationships among soot formation rate, temperature, and species concentration are
highly nonlinear. Hence, if time-averaged composition and temperature are employed
in any model to predict the mean soot formation rate, significant errors will result.
Temperature and composition fluctuations must be taken into account by considering
the probability density functions which describe the time variation.
The Turbulence-Chemistry Interaction Model
In turbulent combustion calculations, ANSYS FLUENT solves the density-weighted timeaveraged Navier-Stokes equations for temperature, velocity, and species concentrations
or mean mixture fraction and variance. To calculate soot concentration for the MossBrookes model and the Hall extension, a time-averaged soot formation rate must be
computed at each point in the domain using the averaged flow-field information.
The PDF Approach
The PDF method has proven very useful in the theoretical description of turbulent
flow [149]. In the ANSYS FLUENT Moss-Brookes model and the Hall extension, a singleor joint-variable PDF in terms of a normalized temperature, species mass fraction, or the
combination of both is used to predict the soot formation. If the non-premixed combustion model is used to model combustion, then a one- or two-variable PDF in terms of
mixture fraction(s) is also available. The mean values of the independent variables needed
for the PDF construction are obtained from the solution of the transport equations.
13-58
Release 12.0 c ANSYS, Inc. January 29, 2009
13.3 Soot Formation
The Mean Reaction Rate
The mean turbulent reaction rate described in Section 13.1.9: The General Expression
for the Mean Reaction Rate for the NOx model also applies to the Moss-Brookes model
and the Hall extension. The PDF is used for weighting against the instantaneous rates
of production of soot and subsequent integration over suitable ranges to obtain the mean
turbulent reaction rate as described in Equations 13.1-104 and 13.1-105 for NOx .
The PDF Options
As is the case with the NOx model, P can be calculated as either a two-moment beta function or as a clipped Gaussian function, as appropriate for combustion calculations [123,
231]. Equations 13.1-107 – 13.1-111 apply to the Moss-Brookes model and Hall extension as well, with the variance σ 2 computed by solving a transport equation during the
combustion calculation stage, using Equation 13.1-112 or Equation 13.1-113.
The Effect of Soot on the Radiation Absorption Coefficient
A description of the modeling of soot-radiation interaction is provided in Section 5.3.8: The
Effect of Soot on the Absorption Coefficient.
Release 12.0 c ANSYS, Inc. January 29, 2009
13-59
Pollutant Formation
13-60
Release 12.0 c ANSYS, Inc. January 29, 2009
Chapter 14.
Aerodynamically Generated Noise
The discipline of acoustics is intimately related to fluid dynamics. Many sounds that are
technologically important in industrial applications are generated by and propagated in
fluid flows. The phenomena associated with sounds can therefore be understood and analyzed in the general framework of fluid dynamics. (The governing equations for acoustics
are indeed the same as the ones governing fluid flows.)
The main challenge in numerically predicting sound waves stems from the well-recognized
fact that sounds have much lower energy than fluid flows, typically by several orders of
magnitude. This poses a great challenge to the computation of sounds in terms of difficulty of numerically resolving sound waves, especially when one is interested in predicting
sound propagation to the far field. Another challenge comes from the difficulty of predicting the very flow phenomena (e.g., turbulence) in the near field that are responsible
for generating sounds.
This chapter provides an overview and theoretical background of ANSYS FLUENT’s approaches to computing aerodynamically generated sound. For more information about
using the acoustics model, see Chapter 22: Predicting Aerodynamically Generated Noise
in the separate User’s Guide.
• Section 14.1: Overview
• Section 14.2: Acoustics Model Theory
14.1
Overview
Considering the breadth of the discipline and the challenges encountered in aerodynamically generated noise, it is not surprising that a number of computational approaches
have been proposed over the years whose sophistication, applicability, and cost widely
vary.
ANSYS FLUENT offers three approaches to computing aerodynamically generated noise;
a direct method, an integral method based on acoustic analogy and a method that utilizes
broadband noise source models.
This section is divided into the following sections:
• Section 14.1.1: Direct Method
• Section 14.1.2: Integral Method Based on Acoustic Analogy
• Section 14.1.3: Broadband Noise Source Models
Release 12.0 c ANSYS, Inc. January 29, 2009
14-1
Aerodynamically Generated Noise
14.1.1
Direct Method
In this method, both generation and propagation of sound waves are directly computed
by solving the appropriate fluid dynamics equations. Prediction of sound waves always
requires time-accurate solutions to the governing equations. Furthermore, in most practical applications of the direct method, one has to employ governing equations that are
capable of modeling viscous and turbulence effects, such as unsteady Navier-Stokes equations (i.e., DNS), RANS equations, and filtered equations used in DES and LES.
The direct method is thus computationally difficult and expensive inasmuch as it requires
highly accurate numerics, very fine computational meshes all the way to receivers, and
acoustically nonreflecting boundary conditions. The computational cost becomes prohibitive when sound is to be predicted in the far field (e.g., hundreds of chord-lengths in
the case of an airfoil). The direct method becomes feasible when receivers are in the near
field (e.g., cabin noise). In many such situations involving near-field sound, sounds (or
pseudo-sounds for that matter) are predominantly due to local hydrodynamic pressure
which can be predicted with a reasonable cost and accuracy.
Since sound propagation is directly resolved in this method, one normally needs to solve
the compressible form of the governing equations (e.g., compressible RANS equations,
compressible form of filtered equations for LES). Only in situations where the flow is low
and subsonic, and the receivers in the near field consist primarily of local hydrodynamic
pressure fluctuations (i.e., pseudo sound), can incompressible flow formulations be used.
However, this incompressible treatment will not permit you to simulate resonance and
feedback phenomena.
14.1.2
Integral Method Based on Acoustic Analogy
For predictions of mid- to far-field noise, the methods based on Lighthill’s acoustic analogy [195] offer viable alternatives to the direct method. In this approach, the near-field
flow obtained from appropriate governing equations such as unsteady RANS equations,
DES, or LES are used to predict the sound with the aid of analytically derived integral
solutions to wave equations. The acoustic analogy essentially decouples the propagation
of sound from its generation, allowing one to separate the flow solution process from the
acoustics analysis.
ANSYS FLUENT offers a method based on the Ffowcs Williams and Hawkings (FW-H)
formulation [95]. The FW-H formulation adopts the most general form of Lighthill’s
acoustic analogy, and is capable of predicting sound generated by equivalent acoustic
sources such as monopoles, dipoles, and quadrupoles. ANSYS FLUENT adopts a timedomain integral formulation wherein time histories of sound pressure, or acoustic signals,
at prescribed receiver locations are directly computed by evaluating a few surface integrals.
14-2
Release 12.0 c ANSYS, Inc. January 29, 2009
14.1 Overview
Time-accurate solutions of the flow-field variables, such as pressure, velocity components,
and density on source (emission) surfaces, are required to evaluate the surface integrals.
Time-accurate solutions can be obtained from unsteady Reynolds-averaged Navier-Stokes
(URANS) equations, large eddy simulation (LES), or detached eddy simulation (DES) as
appropriate for the flow at hand and the features that you want to capture (e.g., vortex
shedding). The source surfaces can be placed not only on impermeable walls, but also on
interior (permeable) surfaces, which enables you to account for the contributions from
the quadrupoles enclosed by the source surfaces. Both broadband and tonal noise can be
predicted depending on the nature of the flow (noise source) being considered, turbulence
model employed, and the time scale of the flow resolved in the flow calculation.
The FW-H acoustics model in ANSYS FLUENT allows you to select multiple source
surfaces and receivers. It also permits you either to save the source data for a future use,
or to carry out an “on the fly” acoustic calculation simultaneously as the transient flow
calculation proceeds, or both. Sound pressure signals thus obtained can be processed
using the fast Fourier transform (FFT) and associated postprocessing capabilities to
compute and plot such acoustic quantities as the overall sound pressure level (SPL) and
power spectra.
One important limitation of ANSYS FLUENT’s FW-H model is that it is applicable only
to predicting the propagation of sound toward free space. Thus, while the model can be
legitimately used to predict far-field noise due to external aerodynamic flows, such as
the flows around ground vehicles and aircrafts, it cannot be used for predicting the noise
propagation inside ducts or wall-enclosed space.
14.1.3 Broadband Noise Source Models
In many practical applications involving turbulent flows, noise does not have any distinct
tones, and the sound energy is continuously distributed over a broad range of frequencies.
In those situations involving broadband noise, statistical turbulence quantities readily
computable from RANS equations can be utilized, in conjunction with semi-empirical
correlations and Lighthill’s acoustic analogy, to shed some light on the source of broadband noise.
Release 12.0 c ANSYS, Inc. January 29, 2009
14-3
Aerodynamically Generated Noise
ANSYS FLUENT offers several such source models that enable you to quantify the local
contribution (per unit surface area or volume) to the total acoustic power generated by
the flow. They include the following:
• Proudman’s formula
• jet noise source model
• boundary layer noise source model
• source terms in the linearized Euler equations
• source terms in Lilley’s equation
Considering that one would ultimately want to come up with some measures to mitigate
the noise generated by the flow in question, the source models can be employed to extract
useful diagnostics on the noise source to determine which portion of the flow is primarily
responsible for the noise generation. Note, however, that these source models do not
predict the sound at receivers.
Unlike the direct method and the FW-H integral method, the broadband noise source
models do not require transient solutions to any governing fluid dynamics equations.
All source models require what typical RANS models would provide, such as the mean
velocity field, turbulent kinetic energy (k) and the dissipation rate (ε). Therefore, the
use of broadband noise source models requires the least computational resources.
14.2
Acoustics Model Theory
This section describes the theoretical background for the Ffowcs Williams and Hawkings
model and the broadband noise source models.
This section is divided into the following sections:
• Section 14.2.1: The Ffowcs Williams and Hawkings Model
• Section 14.2.2: Broadband Noise Source Models
14-4
Release 12.0 c ANSYS, Inc. January 29, 2009
14.2 Acoustics Model Theory
14.2.1
The Ffowcs Williams and Hawkings Model
The Ffowcs Williams and Hawkings (FW-H) equation is essentially an inhomogeneous
wave equation that can be derived by manipulating the continuity equation and the
Navier-Stokes equations. The FW-H [38, 95] equation can be written as:
1 ∂ 2 p0
∂2
2 0
−
∇
p
=
{Tij H(f )}
a20 ∂t2
∂xi ∂xj
∂
−
{[Pij nj + ρui (un − vn )] δ(f )}
∂xi
∂
+
{[ρ0 vn + ρ (un − vn )] δ(f )}
∂t
(14.2-1)
where
ui
un
vi
vn
δ(f )
H(f )
=
=
=
=
=
=
fluid velocity component in the xi direction
fluid velocity component normal to the surface f = 0
surface velocity components in the xi direction
surface velocity component normal to the surface
Dirac delta function
Heaviside function
p0 is the sound pressure at the far field (p0 = p − p0 ). f = 0 denotes a mathematical
surface introduced to “embed” the exterior flow problem (f > 0) in an unbounded space,
which facilitates the use of generalized function theory and the free-space Green function
to obtain the solution. The surface (f = 0) corresponds to the source (emission) surface,
and can be made coincident with a body (impermeable) surface or a permeable surface
off the body surface. ni is the unit normal vector pointing toward the exterior region
(f > 0), a0 is the far-field sound speed, and Tij is the Lighthill stress tensor, defined as
Tij = ρui uj + Pij − a20 (ρ − ρ0 ) δij
(14.2-2)
Pij is the compressive stress tensor. For a Stokesian fluid, this is given by
"
∂ui ∂uj
2 ∂uk
Pij = pδij − µ
+
−
δij
∂xj
∂xi
3 ∂xk
#
(14.2-3)
The free-stream quantities are denoted by the subscript 0.
Release 12.0 c ANSYS, Inc. January 29, 2009
14-5
Aerodynamically Generated Noise
The solution to Equation 14.2-1 is obtained using the free-space Green function (δ(g)/4πr).
The complete solution consists of surface integrals and volume integrals. The surface integrals represent the contributions from monopole and dipole acoustic sources and partially
from quadrupole sources, whereas the volume integrals represent quadrupole (volume)
sources in the region outside the source surface. The contribution of the volume integrals
becomes small when the flow is low subsonic and the source surface encloses the source
region. In ANSYS FLUENT, the volume integrals are dropped. Thus, we have
p0 (~x, t) = p0T (~x, t) + p0L (~x, t)
(14.2-4)
where
4πp0T (~x, t) =
f =0
r (1 − Mr )2
Z
f =0
4πp0L (~x, t)
ρ0 U˙n + Uṅ
+
Z
dS
n
o
ρ0 Un rṀr + a0 (Mr − M 2 )
r2 (1 − Mr )3
dS
(14.2-5)
"
#
1 Z
L̇r
=
dS
a0 f =0 r (1 − Mr )2
+
"
Z
f =0
#
L r − LM
dS
2
r (1 − Mr )2
n
o
Lr rṀr + a0 (Mr − M 2 )
1 Z
dS
+
a0 f =0
r2 (1 − Mr )3
(14.2-6)
where
ρ
(ui − vi )
ρ0
= Pij n̂j + ρui (un − vn )
Ui = vi +
(14.2-7)
Li
(14.2-8)
When the integration surface coincides with an impenetrable wall, the two terms on the
right in Equation 14.2-4, p0T (~x, t) and p0L (~x, t), are often referred to as thickness and
loading terms, respectively, in light of their physical meanings. The square brackets in
Equations 14.2-5 and 14.2-6 denote that the kernels of the integrals are computed at the
corresponding retarded times, τ , defined as follows, given the observer time, t, and the
distance to the observer, r,
τ =t−
14-6
r
a0
(14.2-9)
Release 12.0 c ANSYS, Inc. January 29, 2009
14.2 Acoustics Model Theory
The various subscripted quantities appearing in Equations 14.2-5 and 14.2-6 are the
inner products of a vector and a unit vector implied by the subscript. For instance,
~ · ~ˆr = Li ri and Un = U
~ · ~n = Ui ni , where ~r and ~n denote the unit vectors in
Lr = L
the radiation and wall-normal directions, respectively. The dot over a variable denotes
source-time differentiation of that variable.
Please note the following remarks regarding the applicability of this integral solution:
• The FW-H formulation in ANSYS FLUENT can handle rotating surfaces as well as
stationary surfaces.
• It is not required that the surface f = 0 coincide with body surfaces or walls. The
formulation permits source surfaces to be permeable, and therefore can be placed
in the interior of the flow.
• When a permeable source surface (either interior or nonconformal sliding interface)
is placed at a certain distance off the body surface, the integral solutions given by
Equations 14.2-5 and 14.2-6 include the contributions from the quadrupole sources
within the region enclosed by the source surface. When using a permeable source
surface, the mesh resolution needs to be fine enough to resolve the transient flow
structures inside the volume enclosed by the permeable surface.
14.2.2
Broadband Noise Source Models
Proudman’s Formula
Proudman [280], using Lighthill’s acoustic analogy, derived a formula for acoustic power
generated by isotropic turbulence without mean flow. More recently, Lilley [196] rederived the formula by accounting for the retarded time difference which was neglected in
Proudman’s original derivation. Both derivations yield acoustic power due to the unit
volume of isotropic turbulence (in W/m3 ) as
PA = αρ0
u3
`
!
u5
a50
(14.2-10)
where u and ` are the turbulence velocity and length scales, respectively, and a0 is
the speed of sound. α in Equation 14.2-10 is a model constant. In terms of k and ε,
Equation 14.2-10 can be rewritten as
PA = αε ρ0 εMt5
where
√
Mt =
Release 12.0 c ANSYS, Inc. January 29, 2009
(14.2-11)
2k
a0
(14.2-12)
14-7
Aerodynamically Generated Noise
The rescaled constant, α , is set to 0.1 in ANSYS FLUENT based on the calibration of
Sarkar and Hussaini [301] using direct numerical simulation of isotropic turbulence.
ANSYS FLUENT can also report the acoustic power in dB, which is computed from
LP = 10 log
PA
Pref
(14.2-13)
where Pref is the reference acoustic power (Pref = 10−12 W/m3 by default).
The Proudman’s formula gives an approximate measure of the local contribution to total
acoustic power per unit volume in a given turbulence field. Proper caution, however,
should be taken when interpreting the results in view of the assumptions made in the
derivation, such as high Reynolds number, small Mach number, isotropy of turbulence,
and zero mean motion.
The Jet Noise Source Model
This source model for axisymmetric jets is based on the works of Goldstein [113] who
modified the model originally proposed by Ribner [293] to better account for anisotropy
of turbulence in axisymmetric turbulent jets.
In Goldstein’s model, the total acoustic power emitted by the unit volume of a turbulent
jet is computed from
PA (~y ) =
Z
2π
0
= 2πr
π
Z
2
Z0
I(r, θ; ~y )r2 sin θdθ dψ
π
I(r, θ; ~y ) sin θ dθ
(14.2-14)
0
where r and θ are the radial and angular coordinates of the receiver location, and I(r, θ; ~y )
is the directional acoustic intensity per unit volume of a jet defined by
2
12 ρ0 ωf4 L1 L22 u2t1 Dself
24 ρ0 ωf4 L1 L42 u2t1
I(r, θ; ~y ) =
+
5 π a50 r2
C5
π a50 r2
∂U
∂r
!2
Dshear
C5
(14.2-15)
C in Equation 14.2-15 is the modified convection factor defined by
C = 1 − Mc cos θ
(14.2-16)
and
Dself = 1 + 2(
1 M2
1.5 ∆2
+
+ M − 1.5N (3 − 3N + 2 −
) sin4 θ
3 7
∆
2
1 1
2
= cos2 θ cos2 θ +
−
2N
sin
θ
2 ∆2
"
Dshear
14-8
M
− N ) cos2 θ sin2 θ
9
#
(14.2-17)
(14.2-18)
Release 12.0 c ANSYS, Inc. January 29, 2009
14.2 Acoustics Model Theory
The remaining parameters are defined as
L2
L1
3
1 2
M =
∆−
2 ∆
u2t2
N = 1−
u2t1
∆ =
L1 =
L2 =
u2t2
(14.2-20)
(14.2-21)
3/2
(14.2-22)
ωf
u2t1
(14.2-19)
3/2
(14.2-23)
= 2π
k
(14.2-24)
where u2t1 and u2t2 are computed differently depending on the turbulence model chosen for
the computation. When the RSM is selected, they are computed from the corresponding
normal stresses. For all other two-equation turbulence models, they are obtained from
8
k
9
4
=
k
9
u2t1 =
(14.2-25)
u2t2
(14.2-26)
ANSYS FLUENT reports the acoustic power both in the dimensional units (W/m3 ) and
in dB computed from
PA
LP = 10 log
Pref
is the reference acoustic power (Pref = 10−12 W/m3 by default).
where Pref
(14.2-27)
The Boundary Layer Noise Source Model
Far-field sound generated by turbulent boundary layer flow over a solid body at low
Mach numbers is often of practical interest. The Curle’s integral [64] based on acoustic
analogy can be used to approximate the local contribution from the body surface to the
total acoustic power. To that end, one can start with the Curle’s integral
p0 (~x, t) =
Release 12.0 c ANSYS, Inc. January 29, 2009
1 Z (xi − yi ) ni ∂p
(~y , τ ) dS(~y )
4πa0 S
r2
∂t
(14.2-28)
14-9
Aerodynamically Generated Noise
where τ denotes the emission time (τ = t − r/a0 ), and S the integration surface.
Using this, the sound intensity in the far field can then be approximated by
p02
"
#2
1 Z cos2 θ ∂p
≈
(~y , τ ) Ac (~y ) dS(~y )
16π 2 a20 S r2
∂t
(14.2-29)
where Ac is the correlation area, r ≡ |~x − ~y |, and cos θ is the angle between |~x − ~y | and
the wall-normal direction ~n.
The total acoustic power emitted from the entire body surface can be computed from
PA
1 Z 2π Z π 02 2
=
p r sin θ dθdψ
ρ 0 a0 0 0
=
Z
I(~y ) dS(~y )
(14.2-30)
S
where
"
Ac (~y ) ∂p
I(~y ) ≡
12ρ0 πa30 ∂t
#2
(14.2-31)
which can be interpreted as the local contribution per unit surface area of the body surface
to the total acoustic power. The mean-square time derivative of the surface pressure
and the correlation area are further approximated in terms of turbulent quantities like
turbulent kinetic energy, dissipation rate, and wall shear.
ANSYS FLUENT reports the acoustic surface power defined by Equation 14.2-31 both in
physical (W/m2 ) and dB units.
Source Terms in the Linearized Euler Equations
The linearized Euler equations (LEE) can be derived from the Navier-Stokes equations
starting from decompositions of the flow variables into mean, turbulent, and acoustic
components, and by assuming that the acoustic components are much smaller than the
mean and turbulent components. The resulting linearized Euler equations for the acoustic
velocity components can be written as
∂uai
∂uai
∂Ui 1 ∂pa ρa ∂P
+ Uj
+ uaj
+
− 2
=
∂t
∂xj
∂xj ρ ∂xi
ρ ∂xi
−Uj
|
∂u0i
∂Ui
∂u0 1 ∂p0
∂u0
∂ 0 0
− u0j
− i+
uu
− u0j i −
∂xj
∂xj
∂xj ρ ∂xi
∂t
∂xj j i
{z
Lsh
}
(14.2-32)
| {z }
Lse
where the subscript “a” refers to the corresponding acoustic components, and the prime
superscript refers to the turbulent components.
14-10
Release 12.0 c ANSYS, Inc. January 29, 2009
14.2 Acoustics Model Theory
The right side of Equation 14.2-32 can be considered as effective source terms responsible
for sound generation. Among them, the first three terms involving turbulence are the
main contributors. The first two terms denoted by Lsh are often referred to as “shearnoise” source terms, since they involve the mean shear. The third term denoted by Lse
is often called the “self-noise” source term, as it involves turbulent velocity components
only.
The turbulent velocity field needed to compute the LEE source terms is obtained using
the method of stochastic noise generation and radiation (SNGR) [23]. In this method,
the turbulent velocity field and its derivatives are computed from a sum of N Fourier
modes.
~u (~x, t) = 2
N
X
ũn cos ~kn · ~x + ψn ~σn
(14.2-33)
n=1
where ũn , ψn , ~σn are the amplitude, phase, and directional (unit) vector of the nth Fourier
mode associated with the wave-number vector ~kn .
Note that the source terms in the LEE are vector quantities, having two or three components depending on the dimension of the problem at hand.
Source Terms in Lilley’s Equation
Lilley’s equation is a third-order wave equation that can be derived by combining the
conservation of mass and momentum of compressible fluids. When the viscous terms are
omitted, it can be written in the following form:
D D2 Π
∂
−
Dt Dt2
∂xj
"
∂Π
a
∂xj
2
!#
∂uk ∂
∂Π
+2
a2
∂xj ∂xk
∂xj
!
= −2
∂uk ∂uj ∂ui
∂xi ∂xk ∂xj
(14.2-34)
where Π = (1/γ) ln ppo .
Lilley’s equation can be linearized about the underlying steady flow as
ui (~x, t) = Ui (~x) + u0i (~x, t)
(14.2-35)
where u0 (~x, t) is the turbulent velocity component.
Substituting Equation 14.2-35 into the source term of Equation 14.2-34, we have
∂uk ∂uj ∂ui
∂xi ∂xk ∂xj
∂Uk ∂Uj ∂Ui
∂u0k ∂u0j ∂u0i
∂u0k ∂u0j ∂Ui
∂Uk ∂Uj ∂u0i
= −2
−2
−6
−6
∂xi ∂xk ∂xj
∂xi ∂xk ∂xj
∂xi ∂xk ∂xj
∂xi ∂xk ∂xj
S ≡ −2
|
{z
} |
Self-Noise Terms
Release 12.0 c ANSYS, Inc. January 29, 2009
{z
Shear-Noise Terms
(14.2-36)
}
14-11
Aerodynamically Generated Noise
The resulting source terms in Equation 14.2-36 are evaluated using the mean velocity field
and the turbulent (fluctuating) velocity components synthesized by the SNGR method.
As with the LEE source terms, the source terms in Equation 14.2-36 are grouped depending on whether the mean velocity gradients are involved (shear noise or self noise),
and reported separately in ANSYS FLUENT.
14-12
Release 12.0 c ANSYS, Inc. January 29, 2009
Chapter 15.
Discrete Phase
This chapter describes the theory behind the Lagrangian discrete phase capabilities available in ANSYS FLUENT. For information about how to use discrete phase models, see
Chapter 23: Modeling Discrete Phase in the separate User’s Guide. Information in this
chapter is organized into the following sections:
• Section 15.1: Introduction
• Section 15.2: Particle Motion Theory
• Section 15.3: Laws for Drag Coefficients
• Section 15.4: Laws for Heat and Mass Exchange
• Section 15.5: Vapor Liquid Equilibrium Theory
• Section 15.6: Wall-Jet Model Theory
• Section 15.7: Wall-Film Model Theory
• Section 15.8: Particle Erosion and Accretion Theory
• Section 15.9: Atomizer Model Theory
• Section 15.10: Secondary Breakup Model Theory
• Section 15.11: Droplet Collision and Coalescence Model Theory
• Section 15.12: One-Way and Two-Way Coupling
15.1
Introduction
Advances in computational fluid mechanics have provided the basis for further insight into
the dynamics of multiphase flows. Currently there are two approaches for the numerical
calculation of multiphase flows: the Euler-Lagrange approach (discussed below) and the
Euler-Euler approach (discussed in Section 16.2.1: Approaches to Multiphase Modeling).
Release 12.0 c ANSYS, Inc. January 29, 2009
15-1
Discrete Phase
The Euler-Lagrange Approach
The Lagrangian discrete phase model in ANSYS FLUENT (described in this chapter)
follows the Euler-Lagrange approach. The fluid phase is treated as a continuum by
solving the Navier-Stokes equations, while the dispersed phase is solved by tracking a
large number of particles, bubbles, or droplets through the calculated flow field. The
dispersed phase can exchange momentum, mass, and energy with the fluid phase.
A fundamental assumption made in this model is that the dispersed second phase occupies
a low volume fraction, even though high mass loading (ṁparticles ≥ ṁfluid ) is acceptable.
The particle or droplet trajectories are computed individually at specified intervals during
the fluid phase calculation. This makes the model appropriate for the modeling of spray
dryers, coal and liquid fuel combustion, and some particle-laden flows, but inappropriate
for the modeling of liquid-liquid mixtures, fluidized beds, or any application where the
volume fraction of the second phase cannot be neglected.
Limitations of the discrete phase model are listed in Section 23.1.2: Limitations in the
separate User’s Guide.
15.2
Particle Motion Theory
This section is composed of the following:
• Section 15.2.1: Equations of Motion for Particles
• Section 15.2.2: Turbulent Dispersion of Particles
• Section 15.2.3: Integration of Particle Equation of Motion
15.2.1
Equations of Motion for Particles
Particle Force Balance
ANSYS FLUENT predicts the trajectory of a discrete phase particle (or droplet or bubble)
by integrating the force balance on the particle, which is written in a Lagrangian reference
frame. This force balance equates the particle inertia with the forces acting on the
particle, and can be written (for the x direction in Cartesian coordinates) as
dup
gx (ρp − ρ)
= FD (u − up ) +
+ Fx
dt
ρp
(15.2-1)
where Fx is an additional acceleration (force/unit particle mass) term, FD (u − up ) is the
drag force per unit particle mass and
15-2
Release 12.0 c ANSYS, Inc. January 29, 2009
15.2 Particle Motion Theory
FD =
18µ CD Re
ρp d2p
24
(15.2-2)
Here, u is the fluid phase velocity, up is the particle velocity, µ is the molecular viscosity
of the fluid, ρ is the fluid density, ρp is the density of the particle, and dp is the particle
diameter. Re is the relative Reynolds number, which is defined as
Re ≡
ρdp |up − u|
µ
(15.2-3)
Inclusion of the Gravity Term
While Equation 15.2-1 includes a force of gravity on the particle, it is important to note
that in ANSYS FLUENT the default gravitational acceleration is zero. If you want to
include the gravitational force, you must remember to define the magnitude and direction
of the gravity vector in the Operating Conditions dialog box.
Other Forces
Equation 15.2-1 incorporates additional forces (Fx ) in the particle force balance that can
be important under special circumstances. The first of these is the “virtual mass” force,
the force required to accelerate the fluid surrounding the particle. This force can be
written as
Fx =
1ρ d
(u − up )
2 ρp dt
(15.2-4)
and is important when ρ > ρp . An additional force arises due to the pressure gradient in
the fluid:
!
∂u
ρ
up i
(15.2-5)
Fx =
ρp
∂xi
Forces in Rotating Reference Frames
The additional force term, Fx , in Equation 15.2-1 also includes forces on particles that
arise due to rotation of the reference frame. These forces arise when you are modeling
flows in rotating frames of reference (see Section 2.2: Flow in a Rotating Reference Frame).
For rotation defined about the z axis, for example, the forces on the particles in the
Cartesian x and y directions can be written as
!
ρ
ρ
1−
Ω2 x + 2Ω uy,p − uy
ρp
ρp
Release 12.0 c ANSYS, Inc. January 29, 2009
!
(15.2-6)
15-3
Discrete Phase
where uy,p and uy are the particle and fluid velocities in the Cartesian y direction, and
!
ρ
ρ
Ω2 y − 2Ω ux,p − ux
1−
ρp
ρp
!
(15.2-7)
where ux,p and ux are the particle and fluid velocities in the Cartesian x direction.
Thermophoretic Force
Small particles suspended in a gas that has a temperature gradient experience a force
in the direction opposite to that of the gradient. This phenomenon is known as thermophoresis. ANSYS FLUENT can optionally include a thermophoretic effect on particles
in the additional acceleration (force/unit mass) term, Fx , in Equation 15.2-1:
Fx = −DT,p
1 ∂T
mp T ∂x
(15.2-8)
where DT,p is the thermophoretic coefficient. You can define the coefficient to be constant,
polynomial, or a user-defined function, or you can use the form suggested by Talbot [345]:
Fx = −
where:
Kn
λ
K
k
=
=
=
=
kp
CS
Ct
Cm
mp
T
µ
=
=
=
=
=
=
=
6πdp µ2 Cs (K + Ct Kn)
1 ∂T
ρ(1 + 3Cm Kn)(1 + 2K + 2Ct Kn) mp T ∂x
(15.2-9)
Knudsen number = 2 λ/dp
mean free path of the fluid
k/kp
fluid thermal conductivity based on translational
energy only = (15/4) µR
particle thermal conductivity
1.17
2.18
1.14
particle mass
local fluid temperature
fluid viscosity
This expression assumes that the particle is a sphere and that the fluid is an ideal gas.
15-4
Release 12.0 c ANSYS, Inc. January 29, 2009
15.2 Particle Motion Theory
Brownian Force
For sub-micron particles, the effects of Brownian motion can be optionally included in the
additional force term. The components of the Brownian force are modeled as a Gaussian
white noise process with spectral intensity Sn,ij given by [191]
Sn,ij = S0 δij
(15.2-10)
where δij is the Kronecker delta function, and
S0 =
216νkB T
π 2 ρd5p
ρp 2
ρ
(15.2-11)
Cc
T is the absolute temperature of the fluid, ν is the kinematic viscosity, and kB is the
Boltzmann constant. Amplitudes of the Brownian force components are of the form
s
Fbi = ζi
πSo
∆t
(15.2-12)
where ζi are zero-mean, unit-variance-independent Gaussian random numbers. The amplitudes of the Brownian force components are evaluated at each time step. The energy
equation must be enabled in order for the Brownian force to take effect. Brownian force
is intended only for laminar simulations.
Saffman’s Lift Force
The Saffman’s lift force, or lift due to shear, can also be included in the additional force
term as an option. The lift force used is from Li and Ahmadi [191] and is a generalization
of the expression provided by Saffman [298]:
F~ =
2Kν 1/2 ρdij
(~v − ~vp )
ρp dp (dlk dkl )1/4
(15.2-13)
where K = 2.594 and dij is the deformation tensor. This form of the lift force is intended for small particle Reynolds numbers. Also, the particle Reynolds number based
on the particle-fluid velocity difference must be smaller than the square root of the particle Reynolds number based on the shear field. This option is recommended only for
submicron particles.
Release 12.0 c ANSYS, Inc. January 29, 2009
15-5
Discrete Phase
15.2.2
Turbulent Dispersion of Particles
The dispersion of particles due to turbulence in the fluid phase can be predicted using
the stochastic tracking model or the particle cloud model (see Section 15.2.2: Turbulent
Dispersion of Particles). The stochastic tracking (random walk) model includes the effect
of instantaneous turbulent velocity fluctuations on the particle trajectories through the
use of stochastic methods (see Section 15.2.2: Stochastic Tracking). The particle cloud
model tracks the statistical evolution of a cloud of particles about a mean trajectory
(see Section 15.2.2: Particle Cloud Tracking). The concentration of particles within the
cloud is represented by a Gaussian probability density function (PDF) about the mean
trajectory. For stochastic tracking a model is available to account for the generation or
dissipation of turbulence in the continuous phase (see Section 15.12.1: Coupling Between
the Discrete and Continuous Phases).
i
Turbulent dispersion of particles cannot be included if the Spalart-Allmaras
turbulence model is used.
Stochastic Tracking
When the flow is turbulent, ANSYS FLUENT will predict the trajectories of particles
using the mean fluid phase velocity, u, in the trajectory equations (Equation 15.2-1).
Optionally, you can include the instantaneous value of the fluctuating gas flow velocity,
u = u + u0
(15.2-14)
to predict the dispersion of the particles due to turbulence.
In the stochastic tracking approach, ANSYS FLUENT predicts the turbulent dispersion
of particles by integrating the trajectory equations for individual particles, using the
0
instantaneous fluid velocity, u + u (t), along the particle path during the integration.
By computing the trajectory in this manner for a sufficient number of representative
particles (termed the “number of tries”), the random effects of turbulence on the particle
dispersion can be included.
ANSYS FLUENT uses a stochastic method (random walk model) to determine the instantaneous gas velocity. In the discrete random walk (DRW) model, the fluctuating velocity
components are discrete piecewise constant functions of time. Their random value is kept
constant over an interval of time given by the characteristic lifetime of the eddies.
The DRW model may give nonphysical results in strongly nonhomogeneous diffusiondominated flows, where small particles should become uniformly distributed. Instead,
the DRW will show a tendency for such particles to concentrate in low-turbulence regions
of the flow.
15-6
Release 12.0 c ANSYS, Inc. January 29, 2009
15.2 Particle Motion Theory
The Integral Time
Prediction of particle dispersion makes use of the concept of the integral time scale, T ,
which describes the time spent in turbulent motion along the particle path, ds:
T =
Z
∞
0
up 0 (t)up 0 (t + s)
ds
up 0 2
(15.2-15)
The integral time is proportional to the particle dispersion rate, as larger values indicate
more turbulent motion in the flow. It can be shown that the particle diffusivity is given
by ui 0 uj 0 T .
For small “tracer” particles that move with the fluid (zero drift velocity), the integral time
becomes the fluid Lagrangian integral time, TL . This time scale can be approximated as
TL = CL
k
(15.2-16)
where CL is to be determined as it is not well known. By matching the diffusivity of
tracer particles, ui 0 uj 0 TL , to the scalar diffusion rate predicted by the turbulence model,
νt /σ, one can obtain
TL ≈ 0.15
k
(15.2-17)
k
(15.2-18)
for the k- model and its variants, and
TL ≈ 0.30
when the Reynolds stress model (RSM) is used [67]. For the k-ω models, substitute
ω = /k into Equation 15.2-16. The LES model uses the equivalent LES time scales.
The Discrete Random Walk Model
In the discrete random walk (DRW) model, or “eddy lifetime” model, the interaction of
a particle with a succession of discrete stylized fluid phase turbulent eddies is simulated.
Each eddy is characterized by
• a Gaussian distributed random velocity fluctuation, u0 , v 0 , and w0
• a time scale, τe
Release 12.0 c ANSYS, Inc. January 29, 2009
15-7
Discrete Phase
The values of u0 , v 0 , and w0 that prevail during the lifetime of the turbulent eddy are
sampled by assuming that they obey a Gaussian probability distribution, so that
q
0
u = ζ u0 2
(15.2-19)
where ζ is a normally distributed random number, and the remainder of the right-hand
side is the local RMS value of the velocity fluctuations. Since the kinetic energy of
turbulence is known at each point in the flow, these values of the RMS fluctuating
components can be defined (assuming isotropy) as
q
02
u =
q
02
q
v =
w0 2 =
q
2k/3
(15.2-20)
for the k- model, the k-ω model, and their variants. When the RSM is used, nonisotropy
of the stresses is included in the derivation of the velocity fluctuations:
u
0
q
= ζ u0 2
(15.2-21)
q
v0 = ζ v02
(15.2-22)
q
w0 = ζ w0 2
(15.2-23)
when viewed in a reference frame in which the second moment of the turbulence is diagonal [389]. For the LES model, the velocity fluctuations are equivalent in all directions.
See Section 4.11.4: Inlet Boundary Conditions for the LES Model for details.
The characteristic lifetime of the eddy is defined either as a constant:
τe = 2TL
(15.2-24)
where TL is given by Equation 15.2-16 in general (Equation 15.2-17 by default), or as a
random variation about TL :
τe = −TL ln(r)
(15.2-25)
where r is a uniform random number between 0 and 1 and TL is given by Equation 15.2-17.
The option of random calculation of τe yields a more realistic description of the correlation
function.
The particle eddy crossing time is defined as
"
tcross
15-8
Le
= −τ ln 1 −
τ |u − up |
!#
(15.2-26)
Release 12.0 c ANSYS, Inc. January 29, 2009
15.2 Particle Motion Theory
where τ is the particle relaxation time, Le is the eddy length scale, and |u − up | is the
magnitude of the relative velocity.
The particle is assumed to interact with the fluid phase eddy over the smaller of the
eddy lifetime and the eddy crossing time. When this time is reached, a new value of the
instantaneous velocity is obtained by applying a new value of ζ in Equation 15.2-19.
Using the DRW Model
The only inputs required for the DRW model are the value for the integral time-scale
constant, CL (see Equations 15.2-16 and 15.2-24) and the choice of the method used for
the prediction of the eddy lifetime. You can choose to use either a constant value or
a random value by selecting the appropriate option in the Set Injection Properties
dialog box for each injection, as described in Section 23.3.16: Stochastic Tracking in the
separate User’s Guide.
i
Turbulent dispersion of particles cannot be included if the Spalart-Allmaras
turbulence model is used.
Particle Cloud Tracking
Particle dispersion due to turbulent fluctuations can also be modeled with the particle
cloud model [21, 22, 144, 204]. The turbulent dispersion of particles about a mean
trajectory is calculated using statistical methods. The concentration of particles about
the mean trajectory is represented by a Gaussian probability density function (PDF)
whose variance is based on the degree of particle dispersion due to turbulent fluctuations.
The mean trajectory is obtained by solving the ensemble-averaged equations of motion
for all particles represented by the cloud (see Section 15.2.2: Particle Cloud Tracking).
The cloud enters the domain either as a point source or with an initial diameter. The
cloud expands due to turbulent dispersion as it is transported through the domain until
it exits. As mentioned before, the distribution of particles in the cloud is defined by a
probability density function (PDF) based on the position in the cloud relative to the cloud
center. The value of the PDF represents the probability of finding particles represented
by that cloud with residence time t at location xi in the flow field. The average particle
number density can be obtained by weighting the total flow rate of particles represented
by that cloud, ṁ, as
hn(xi )i = ṁP (xi , t)
(15.2-27)
The PDFs for particle position are assumed to be multivariate Gaussian. These are
completely described by their mean, µi , and variance, σi 2 , and are of the form
Release 12.0 c ANSYS, Inc. January 29, 2009
15-9
Discrete Phase
1
P (xi , t) =
(2π)3/2
3
Y
e−s/2
(15.2-28)
σi
i=1
where
s=
3
X
x i − µi 2
(15.2-29)
σi
i=1
The mean of the PDF, or the center of the cloud, at a given time represents the most
likely location of the particles in the cloud. The mean location is obtained by integrating
a particle velocity as defined by an equation of motion for the cloud of particles:
µi (t) ≡ hxi (t)i =
t
Z
0
hVi (t1 )idt1 + hxi (0)i
(15.2-30)
The equations of motion are constructed using an ensemble average.
The radius of the particle cloud is based on the variance of the PDF. The variance, σi2 (t),
of the PDF can be expressed in terms of two particle turbulence statistical quantities:
σi2 (t)
=2
t
Z
0
hu02
p,i (t2 )i
t2
Z
Rp,ii (t2 , t1 )dt1 dt2
0
(15.2-31)
0
2
where hup,i
i are the mean square velocity fluctuations, and Rp,ij (t2 , t1 ) is the particle
velocity correlation function:
Rp,ij (t2 , t1 ) = h
hu0p,i (t2 )u0p,j (t1 )i
i1/2
(15.2-32)
02
hu02
p,i (t2 )up,j (t2 )i
By using the substitution τ = |t2 − t1 |, and the fact that
Rp,ij (t2 , t1 ) = Rp,ij (t4 , t3 )
(15.2-33)
whenever |t2 − t1 | = |t4 − t3 |, we can write
σi2 (t)
=2
Z
0
t
hu02
p,i (t2 )i
Z
0
t2
Rp,ii (τ )dτ dt2
(15.2-34)
Note that cross correlations in the definition of the variance (Rp,ij , i 6= j) have been
neglected.
15-10
Release 12.0 c ANSYS, Inc. January 29, 2009
15.2 Particle Motion Theory
The form of the particle velocity correlation function used determines the particle dispersion in the cloud model. ANSYS FLUENT uses a correlation function first proposed
by Wang [365], and used by Jain [144]. When the gravity vector is aligned with the
z-coordinate direction, Rij takes the form:
u02 −(τ /τa )
St2 B 2 + 1
=
e
StT B − 0.5mT γ T
θ
θ
!
2
02
u −(τ B/T )
mT StT γB
τ
+
e
−1 +
+ 0.5mT γ
θ
θ
T
!
Rp,11
Rp,22 = Rp,11
u02 StT B −(τ /τa ) u02 −(τ B/T )
Rp,33 =
e
−
e
θ
θ
where B =
(15.2-35)
(15.2-36)
(15.2-37)
q
1 + m2T γ 2 and τa is the aerodynamic response time of the particle:
τa =
ρp d2p
18µ
(15.2-38)
and
T =
Tf E =
γ =
St =
StT =
θ =
m =
TmE =
mT =
mT TmE
m
3/4 3/2
Cµ k
( 23 k)1/2
τa g
u0
τa
TmE
τa
T
St2T (1 + m2T γ 2 ) − 1
ū
u0
ū
Tf E 0
"u
#
G(m)
m 1−
(1 + St)0.4(1+0.01St)
2 Z∞
G(m) = √
π 0
1+
Release 12.0 c ANSYS, Inc. January 29, 2009
(15.2-39)
(15.2-40)
(15.2-41)
(15.2-42)
(15.2-43)
(15.2-44)
(15.2-45)
(15.2-46)
(15.2-47)
2
e−y dy
m2
π
5/2
√
( π erf(y)y − 1 + e−y2 )
(15.2-48)
15-11
Discrete Phase
Using this correlation function, the variance is integrated over the life of the cloud. At
any given time, the cloud radius is set to three standard deviations in the coordinate
directions. The cloud radius is limited to three standard deviations since at least 99.2%
of the area under a Gaussian PDF is accounted for at this distance. Once the cells
within the cloud are established, the fluid properties are ensemble-averaged for the mean
trajectory, and the mean path is integrated in time. This is done with a weighting factor
defined as
Z
W (xi , t) ≡ Z
Vcell
P (xi , t)dV
Vcloud
(15.2-49)
P (xi , t)dV
If coupled calculations are performed, sources are distributed to the cells in the cloud
based on the same weighting factors.
Using the Cloud Model
The only inputs required for the cloud model are the values of the minimum and maximum
cloud diameters. The cloud model is enabled in the Set Injection Properties dialog
box for each injection, as described in Section 23.3.16: Cloud Tracking in the separate
User’s Guide.
i
15.2.3
The cloud model is not available for unsteady particle tracking, or in parallel, when using the message passing option for the particles.
Integration of Particle Equation of Motion
The trajectory equations, and any auxiliary equations describing heat or mass transfer
to/from the particle, are solved by stepwise integration over discrete time steps. Integration of time in Equation 15.2-1 yields the velocity of the particle at each point along the
trajectory, with the trajectory itself predicted by
dx
= up
dt
(15.2-50)
Note that Equation 15.2-1 and Equation 15.2-50 are a set of coupled ordinary differential
equations, and Equation 15.2-1 can be cast into the following general form
dup
1
= (u − up ) + a
dt
τp
(15.2-51)
where the term a includes accelerations due to all other forces except drag force.
15-12
Release 12.0 c ANSYS, Inc. January 29, 2009
15.2 Particle Motion Theory
This set can be solved for constant u, a and τp by analytical integration. For the particle
velocity at the new location un+1
we get
p
un+1
p
− ∆t
τ
n
=u +e
p
unp
−u
n
− ∆t
τ
− aτp e
p
−1
(15.2-52)
The new location xn+1
can be computed from a similar relationship.
p
− ∆t
τ
= xnp + ∆t(un + aτp ) + τp 1 − e
xn+1
p
p
unp − un − aτp
(15.2-53)
In these equations unp and un represent particle velocities and fluid velocities at the old
location. Equations 15.2-52 and 15.2-53 are applied when using the analytic discretization
scheme.
The set of Equation 15.2-1 and Equation 15.2-50 can also be solved using numerical discretization schemes. When applying the Euler implicit discretization to Equation 15.2-51
we get
un+1
=
p
unp + ∆t(a +
1+
un
)
τp
(15.2-54)
∆t
τp
When applying a trapezoidal discretization to Equation 15.2-51 the variables up and un
on the right hand side are taken as averages, while accelerations, a, due to other forces
are held constant. We get
un+1
− unp
1
p
= (u∗ − u∗p ) + an
∆t
τp
(15.2-55)
The averages u∗p and u∗ are computed from
1 n
(u + un+1
)
p
2 p
1 n
=
(u + un+1 )
2
= un + ∆tunp · ∇un
u∗p =
(15.2-56)
u∗
(15.2-57)
un+1
(15.2-58)
The particle velocity at the new location n + 1 is computed by
un+1
=
p
unp (1 −
1 ∆t
)
2 τp
Release 12.0 c ANSYS, Inc. January 29, 2009
+
∆t
τp
un + 12 ∆tunp · ∇un + ∆ta
1+
1 ∆t
2 τp
(15.2-59)
15-13
Discrete Phase
For the implicit and the trapezoidal schemes the new particle location is always computed
by a trapezoidal discretization of Equation 15.2-50.
1 n
n
n+1
xn+1
=
x
+
∆t
u
+
u
p
p
p
p
2
(15.2-60)
Equations 15.2-51 and 15.2-50 can also be computed using a Runge-Kutta scheme which
was published by Cash and Karp [48]. The ordinary differential equations can be considered as vectors, where the left hand side is the derivative ~y 0 and the right hand side is
an arbitrary function f~(t, ~y ).
~y 0 = f~(t, ~y )
(15.2-61)
~y n+1 = ~y n + c1~k1 + c2~k2 + c3~k3 + c4~k4 + c5~k5 + c6~k6
(15.2-62)
We get
with
~k1 = ∆tf~(t, ~y n )
~k2 = ∆tf~(t + a2 ∆t, ~y n + b21~k1 )
~k3 = ∆tf~(t + a3 ∆t, ~y n + b31~k1 + b32~k2 )
~k4 = ∆tf~(t + a4 ∆t, ~y n + b41~k1 + b42~k2 + b43~k3 )
~k5 = ∆tf~(t + a5 ∆t, ~y n + b51~k1 + b52~k2 + b53~k3 + b54~k4 )
~k6 = ∆tf~(t + a6 ∆t, ~y n + b61~k1 + b62~k2 + b63~k3 + b64~k4 + b65~k5 )
The coefficients a2 . . . a6 , b21 . . . b65 , and c1 . . . c6 are taken from Cash and Karp [48]
This scheme provides an embedded error control, which is switched off, when no Accuracy
Control is enabled.
For rotating reference frames, the integration is carried out in the rotating frame with
the extra terms described in Equation 15.2-6 and Equation 15.2-7, thus accounting for
system rotation. Using the mechanisms available for accuracy control, the trajectory
integration will be done accurately in time.
The analytic scheme is very efficient. It can become inaccurate for large steps and in situations where the particles are not in hydrodynamic equilibrium with the continuous flow.
The numerical schemes implicit and trapezoidal, in combination with Automated Tracking
Scheme Selection, consider most of the changes in the forces acting on the particles and
are chosen as default schemes. The runge-kutta scheme is recommended of nondrag force
changes along a particle integration step.
15-14
Release 12.0 c ANSYS, Inc. January 29, 2009
15.3 Laws for Drag Coefficients
The integration step size of the higher-order schemes, trapezoidal and runge-kutta, is
limited to a stable range. Therefore it is recommended to use them in combination with
Automated Tracking Scheme Selection.
For the massless particle type, the particle velocity is equal to the velocity of the continuous phase, hence the solution of only the trajectory Equation 15.2-50 is required where
the particle velocity up = u. The new particle location along the trajectory is always
computed by Equations 15.2-58 and 15.2-60, with up = u.
15.3
Laws for Drag Coefficients
Several laws for drag coefficients, CD , are available for the Euler-Lagrange Model.
Instructions for selecting the drag law are provided in Section 23.2.4: Drag Laws in the
separate User’s Guide.
15.3.1
Spherical Drag Law
The drag coefficient, CD , for smooth particles can be taken from
CD = a1 +
a2
a3
+ 2
Re Re
(15.3-1)
where a1 , a2 , and a3 are constants that apply over several ranges of Re given by Morsi
and Alexander [238].
15.3.2
Non-spherical Drag Law
For non-spherical particles Haider and Levenspiel [119] developed the correlation
CD =
24
b3 Resph
1 + b1 Resph b2 +
Resph
b4 + Resph
(15.3-2)
where
b1
b2
b3
b4
=
=
=
=
exp(2.3288 − 6.4581φ + 2.4486φ2 )
0.0964 + 0.5565φ
exp(4.905 − 13.8944φ + 18.4222φ2 − 10.2599φ3 )
exp(1.4681 + 12.2584φ − 20.7322φ2 + 15.8855φ3 )
The shape factor, φ, is defined as
φ=
Release 12.0 c ANSYS, Inc. January 29, 2009
s
S
(15.3-3)
(15.3-4)
15-15
Discrete Phase
where s is the surface area of a sphere having the same volume as the particle, and S
is the actual surface area of the particle. The Reynolds number Resph is computed with
the diameter of a sphere having the same volume.
i
15.3.3
The shape factor cannot exceed a value of 1.
Stokes-Cunningham Drag Law
For sub-micron particles, a form of Stokes’ drag law is available [261]. In this case, FD
is defined as
FD =
18µ
dp 2 ρp Cc
(15.3-5)
The factor Cc is the Cunningham correction to Stokes’ drag law, which you can compute
from
Cc = 1 +
2λ
(1.257 + 0.4e−(1.1dp /2λ) )
dp
(15.3-6)
where λ is the molecular mean free path.
15.3.4
High-Mach-Number Drag Law
A high-Mach-number drag law is also available. This drag law is similar to the spherical
law (Equation 15.3-1) with corrections [57] to account for a particle Mach number greater
than 0.4 at a particle Reynolds number greater than 20.
15.3.5
Dynamic Drag Model Theory
Accurate determination of droplet drag coefficients is crucial for accurate spray modeling. ANSYS FLUENT provides a method that determines the droplet drag coefficient
dynamically, accounting for variations in the droplet shape.
The dynamic drag model is applicable in almost any circumstance. It is compatible with
both the TAB and wave models for droplet breakup. When the collision model is turned
on, collisions reset the distortion and distortion velocities of the colliding droplets.
Many droplet drag models assume the droplet remains spherical throughout the domain.
With this assumption, the drag of a spherical object is determined by the following [205]:
Cd,sphere =
15-16
0.424
Re > 1000
(15.3-7)
24
Re
1+
1
Re2/3
6
Re ≤ 1000
Release 12.0 c ANSYS, Inc. January 29, 2009
15.3 Laws for Drag Coefficients
However, as an initially spherical droplet moves through a gas, its shape is distorted
significantly when the Weber number is large. In the extreme case, the droplet shape
will approach that of a disk. The drag of a disk, however, is significantly higher than that
of a sphere. Since the droplet drag coefficient is highly dependent upon the droplet shape,
a drag model that assumes the droplet is spherical is unsatisfactory. The dynamic drag
model accounts for the effects of droplet distortion, linearly varying the drag between
that of a sphere (Equation 15.3-7) and a value of 1.54 corresponding to a disk [205]. The
drag coefficient is given by
Cd = Cd,sphere (1 + 2.632y)
(15.3-8)
where y is the droplet distortion, as determined by the solution of
d2 y
CF ρg u2 Ck σ
Cd µl dy
=
−
y−
2
2
3
dt
Cb ρl r
ρl r
ρl r2 dt
(15.3-9)
In the limit of no distortion (y = 0), the drag coefficient of a sphere will be obtained,
while at maximum distortion (y = 1) the drag coefficient corresponding to a disk will be
obtained.
Note that Equation 15.3-9 is obtained from the TAB model for spray breakup, described
in Section 15.10.1: Taylor Analogy Breakup (TAB) Model, but the dynamic drag model
can be used with either of the breakup models.
15.3.6
Dense Discrete Phase Model Drag Laws
The drag laws that are suitable for dense gas-solid flow are the Wen and Yu, the Gidaspow, and the Syamlal-O’Brien drag model. A detailed theoretical background to the
correlations, along with a recommendation of when to use each model, can be found in
Section 16.5.4: Fluid-Solid Exchange Coefficient (see also Section 24.5.2: Specifying the
Drag Function in the separate User’s Guide). All three correlations incorporate group
effects and therefore are dependent on the particle phase volume fraction. Thus, the
new drag models are only available when the DPM volume fraction is computed, i.e. in
conjunction with the Dense Discrete Phase Model.
Release 12.0 c ANSYS, Inc. January 29, 2009
15-17
Discrete Phase
15.4
Laws for Heat and Mass Exchange
Using ANSYS FLUENT’s discrete phase modeling capability, reacting particles or droplets
can be modeled and their impact on the continuous phase can be examined. Several heat
and mass transfer relationships, termed “laws”, are available in ANSYS FLUENT and the
physical models employed in these laws are described in this section.
The laws that you activate depend upon the particle type that you select. In the Set
Injection Properties dialog box you will specify the Particle Type, and ANSYS FLUENT
will use a given set of heat and mass transfer laws for the chosen type. All particle types
have predefined sequences of physical laws as shown in the table below:
Particle Type
Massless
Inert
Droplet
Combusting
Multicomponent
Description
–
inert/heating or cooling
heating/evaporation/boiling
heating;
evolution of volatiles/swelling;
heterogeneous surface reaction
multicomponent droplets/particles
Laws Activated
–
1, 6
1, 2, 3, 6
1, 4, 5, 6
7
In addition to the above laws, you can define your own laws using a user-defined function.
More information about user-defined functions can be found in the separate UDF Manual.
You can also extend combusting particles to include an evaporating/boiling material by
selecting Wet Combustion in the Set Injection Properties dialog box.
ANSYS FLUENT’s physical laws (Laws 1 through 6), which describe the heat and mass
transfer conditions listed in this table, are explained in detail in the sections that follow.
15-18
Release 12.0 c ANSYS, Inc. January 29, 2009
15.4 Laws for Heat and Mass Exchange
15.4.1
Inert Heating or Cooling (Law 1/Law 6)
The inert heating or cooling laws (Laws 1 and 6) are applied when the particle temperature is less than the vaporization temperature that you define, Tvap , and after the volatile
fraction, fv,0 , of a particle has been consumed. These conditions may be written as
Law 1:
Tp < Tvap
(15.4-1)
mp ≤ (1 − fv,0 )mp,0
(15.4-2)
Law 6:
where Tp is the particle temperature, mp,0 is the initial mass of the particle, and mp is
its current mass.
Law 1 is applied until the temperature of the particle/droplet reaches the vaporization temperature. At this point a noninert particle/droplet may proceed to obey one
of the mass-transfer laws (2, 3, 4, and/or 5), returning to Law 6 when the volatile
portion of the particle/droplet has been consumed. (Note that the vaporization temperature, Tvap , is an arbitrary modeling constant used to define the onset of the vaporization/boiling/volatilization laws.)
When using Law 1 or Law 6, ANSYS FLUENT uses a simple heat balance to relate the
particle temperature, Tp (t), to the convective heat transfer and the absorption/emission
of radiation at the particle surface:
mp cp
dTp
4
= hAp (T∞ − Tp ) + p Ap σ(θR
− Tp4 )
dt
(15.4-3)
where
mp
cp
Ap
T∞
h
p
σ
θR
=
=
=
=
=
=
=
=
mass of the particle (kg)
heat capacity of the particle (J/kg-K)
surface area of the particle (m2 )
local temperature of the continuous phase (K)
convective heat transfer coefficient (W/m2 -K)
particle emissivity (dimensionless)
Stefan-Boltzmann constant (5.67 x 10−8 W/m2 -K4 )
G 1/4
radiation temperature, ( 4σ
)
Equation 15.4-3 assumes that there is negligible internal resistance to heat transfer, i.e.,
the particle is at uniform temperature throughout.
G is the incident radiation in W/m2 :
G=
Z
IdΩ
(15.4-4)
Ω=4π
Release 12.0 c ANSYS, Inc. January 29, 2009
15-19
Discrete Phase
where I is the radiation intensity and Ω is the solid angle.
Radiation heat transfer to the particle is included only if you have enabled the P-1 or
discrete ordinates radiation model and you have activated radiation heat transfer to
particles using the Particle Radiation Interaction option in the Discrete Phase Model
dialog box.
Equation 15.4-3 is integrated in time using an approximate, linearized form that assumes
that the particle temperature changes slowly from one time value to the next:
mp cp
n h
i
h
io
dTp
4
= Ap − h + p σTp3 Tp + hT∞ + p σθR
dt
(15.4-5)
As the particle trajectory is computed, ANSYS FLUENT integrates Equation 15.4-5 to
obtain the particle temperature at the next time value, yielding
Tp (t + ∆t) = αp + [Tp (t) − αp ]e−βp ∆t
(15.4-6)
where ∆t is the integration time step and
4
hT∞ + p σθR
h + p σTp3 (t)
(15.4-7)
Ap (h + p σTp3 (t))
m p cp
(15.4-8)
αp =
and
βp =
ANSYS FLUENT can also solve Equation 15.4-5 in conjunction with the equivalent mass
transfer equation using a stiff coupled solver. See Section 23.2.8: Including Coupled
Heat-Mass Solution Effects on the Particles in the separate User’s Guide for details.
The heat transfer coefficient, h, is evaluated using the correlation of Ranz and Marshall [284, 285]:
Nu =
hdp
1/2
= 2.0 + 0.6Red Pr1/3
k∞
(15.4-9)
where
dp
k∞
Red
Pr
15-20
= particle diameter (m)
= thermal conductivity of the continuous phase (W/m-K)
= Reynolds number based on the particle diameter and
the relative velocity (Equation 15.2-3)
= Prandtl number of the continuous phase (cp µ/k∞ )
Release 12.0 c ANSYS, Inc. January 29, 2009
15.4 Laws for Heat and Mass Exchange
Finally, the heat lost or gained by the particle as it traverses each computational cell
appears as a source or sink of heat in subsequent calculations of the continuous phase
energy equation. During Laws 1 and 6, particles/droplets do not exchange mass with the
continuous phase and do not participate in any chemical reaction.
15.4.2 Droplet Vaporization (Law 2)
Law 2 is applied to predict the vaporization from a discrete phase droplet. Law 2 is
initiated when the temperature of the droplet reaches the vaporization temperature,
Tvap , and continues until the droplet reaches the boiling point, Tbp , or until the droplet’s
volatile fraction is completely consumed:
Tvap ≤ Tp < Tbp
(15.4-10)
mp > (1 − fv,0 )mp,0
(15.4-11)
The onset of the vaporization law is determined by the setting of Tvap , a modeling parameter that has no physical significance. Note that once vaporization is initiated (by
the droplet reaching this threshold temperature), it will continue to vaporize even if the
droplet temperature falls below Tvap . Vaporization will be halted only if the droplet
temperature falls below the dew point. In such cases, the droplet will remain in Law
2 but no evaporation will be predicted. When the boiling point is reached, the droplet
vaporization is predicted by a boiling rate, Law 3, as described in a section that follows.
Mass Transfer During Law 2
During Law 2, the rate of vaporization is governed by gradient diffusion, with the flux of
droplet vapor into the gas phase related to the difference in vapor concentration at the
droplet surface and the bulk gas:
Ni = kc (Ci,s − Ci,∞ )
(15.4-12)
where
Ni
kc
Ci,s
Ci,∞
= molar flux of vapor (kgmol/m2 -s)
= mass transfer coefficient (m/s)
= vapor concentration at the droplet surface (kgmol/m3 )
= vapor concentration in the bulk gas (kgmol/m3 )
Note that ANSYS FLUENT’s vaporization law assumes that Ni is positive (evaporation).
If conditions exist in which Ni is negative (i.e., the droplet temperature falls below the
dew point and condensation conditions exist), ANSYS FLUENT treats the droplet as inert
(Ni = 0.0).
Release 12.0 c ANSYS, Inc. January 29, 2009
15-21
Discrete Phase
The concentration of vapor at the droplet surface is evaluated by assuming that the
partial pressure of vapor at the interface is equal to the saturated vapor pressure, psat ,
at the particle droplet temperature, Tp :
Ci,s =
psat (Tp )
RTp
(15.4-13)
where R is the universal gas constant.
The concentration of vapor in the bulk gas is known from solution of the transport
equation for species i for nonpremixed or partially premixed combustion calculations:
Ci,∞ = Xi
p
RT∞
(15.4-14)
where Xi is the local bulk mole fraction of species i, p is the local absolute pressure,
and T∞ is the local bulk temperature in the gas. The mass transfer coefficient in Equation 15.4-12 is calculated from the Sherwood number correlation [284, 285]:
ShAB =
where
Di,m
Sc
dp
kc dp
1/2
= 2.0 + 0.6Red Sc1/3
Di,m
(15.4-15)
= diffusion coefficient of vapor in the bulk (m2 /s)
= the Schmidt number, ρDµi,m
= particle (droplet) diameter (m)
The vapor flux given by Equation 15.4-12 becomes a source of species i in the gas phase
species transport equation, (see Section 23.5: Setting Material Properties for the Discrete
Phase in the separate User’s Guide) or in the mixture fraction equation for nonpremixed
combustion calculations.
The mass of the droplet is reduced according to
mp (t + ∆t) = mp (t) − Ni Ap Mw,i ∆t
where
Mw,i
mp
Ap
(15.4-16)
= molecular weight of species i (kg/kgmol)
= mass of the droplet (kg)
= surface area of the droplet (m2 )
ANSYS FLUENT can also solve Equation 15.4-16 in conjunction with the equivalent heat
transfer equation using a stiff coupled solver. See Section 23.2.8: Including Coupled
Heat-Mass Solution Effects on the Particles in the separate User’s Guide for details.
15-22
Release 12.0 c ANSYS, Inc. January 29, 2009
15.4 Laws for Heat and Mass Exchange
Defining the Vapor Pressure and Diffusion Coefficient
You must define the vapor pressure as a polynomial or piecewise linear function of temperature (psat (T )) during the problem definition. Note that the vapor pressure definition
is critical, as psat is used to obtain the driving force for the evaporation process (Equations 15.4-12 and 15.4-13). You should provide accurate vapor pressure values for temperatures over the entire range of possible droplet temperatures in your problem. Vapor
pressure data can be obtained from a physics or engineering handbook (e.g., [266]).
You must also input the diffusion coefficient, Di,m , during the setup of the discrete phase
material properties. Note that the diffusion coefficient inputs that you supply for the
continuous phase are not used in the discrete phase model.
Heat Transfer to the Droplet
Finally, the droplet temperature is updated according to a heat balance that relates the
sensible heat change in the droplet to the convective and latent heat transfer between
the droplet and the continuous phase:
mp cp
where
cp
Tp
h
T∞
dmp
dt
hfg
p
σ
θR
dTp
dmp
= hAp (T∞ − Tp ) +
hfg + Ap p σ(θR 4 − Tp 4 )
dt
dt
=
=
=
=
=
=
=
=
=
(15.4-17)
droplet heat capacity (J/kg-K)
droplet temperature (K)
convective heat transfer coefficient (W/m2 -K)
temperature of continuous phase (K)
rate of evaporation (kg/s)
latent heat (J/kg)
particle emissivity (dimensionless)
Stefan-Boltzmann constant (5.67 x 10−8 W/m2 -K4 )
I 1/4
) , where I is the radiation intensity
radiation temperature, ( 4σ
Radiation heat transfer to the particle is included only if you have enabled the P-1 or
discrete ordinates radiation model and you have activated radiation heat transfer to
particles using the Particle Radiation Interaction option in the Discrete Phase Model
dialog box.
The heat transferred to or from the gas phase becomes a source/sink of energy during
subsequent calculations of the continuous phase energy equation.
Release 12.0 c ANSYS, Inc. January 29, 2009
15-23
Discrete Phase
15.4.3
Droplet Boiling (Law 3)
Law 3 is applied to predict the convective boiling of a discrete phase droplet when the
temperature of the droplet has reached the boiling temperature, Tbp , and while the mass
of the droplet exceeds the nonvolatile fraction, (1 − fv,0 ):
Tp ≥ Tbp
(15.4-18)
mp > (1 − fv,0 )mp,0
(15.4-19)
and
When the droplet temperature reaches the boiling point, a boiling rate equation is applied [173]:
"
q
d(dp )
4k∞
cp,∞ (T∞ − Tp )
=
(1 + 0.23 Red ) ln 1 +
dt
ρp cp,∞ dp
hfg
where
cp,∞
ρp
k∞
#
(15.4-20)
= heat capacity of the gas (J/kg-K)
= droplet density (kg/m3 )
= thermal conductivity of the gas (W/m-K)
Equation 15.4-20 was derived assuming steady flow at constant pressure. Note that the
model requires T∞ > Tbp in order for boiling to occur and that the droplet remains at
fixed temperature (Tbp ) throughout the boiling law.
When radiation heat transfer is active, ANSYS FLUENT uses a slight modification of
Equation 15.4-20, derived by starting from Equation 15.4-17 and assuming that the
droplet temperature is constant. This yields
−
dmp
hfg = hAp (T∞ − Tp ) + Ap p σ(θR 4 − Tp 4 )
dt
(15.4-21)
or
"
#
d(dp )
2
k∞ Nu
4
−
=
(T∞ − Tp ) + p σ(θR
− Tp4 )
dt
ρp hfg
dp
(15.4-22)
Using Equation 15.4-9 for the Nusselt number correlation and replacing the Prandtl
number term with an empirical constant, Equation 15.4-22 becomes
#
"
√
d(dp )
2
2k∞ [1 + 0.23 Red ]
4
(T∞ − Tp ) + p σ(θR
− Tp4 )
−
=
dp
dt
ρp hfg
15-24
(15.4-23)
Release 12.0 c ANSYS, Inc. January 29, 2009
15.4 Laws for Heat and Mass Exchange
In the absence of radiation, this result matches that of Equation 15.4-20 in the limit that
the argument of the logarithm is close to unity. ANSYS FLUENT uses Equation 15.4-23
when radiation is active in your model and Equation 15.4-20 when radiation is not active.
Radiation heat transfer to the particle is included only if you have enabled the P-1 or
discrete ordinates radiation model and you have activated radiation heat transfer to
particles using the Particle Radiation Interaction option in the Discrete Phase Model
dialog box.
The droplet is assumed to stay at constant temperature while the boiling rate is applied.
Once the boiling law is entered it is applied for the duration of the particle trajectory.
The energy required for vaporization appears as a (negative) source term in the energy
equation for the gas phase. The evaporated liquid enters the gas phase as species i,
as defined by your input for the destination species (see Section 23.5: Setting Material
Properties for the Discrete Phase in the separate User’s Guide).
15.4.4
Devolatilization (Law 4)
The devolatilization law is applied to a combusting particle when the temperature of the
particle reaches the vaporization temperature, Tvap , and remains in effect while the mass
of the particle, mp , exceeds the mass of the nonvolatiles in the particle:
Tp ≥ Tvap and Tp ≥ Tbp
(15.4-24)
mp > (1 − fv,0 )(1 − fw,0 )mp,0
(15.4-25)
and
where fw,0 is the mass fraction of the evaporating/boiling material if Wet Combustion is
selected (otherwise, fw,0 = 0). As implied by Equation 15.4-24, the boiling point, Tbp ,
and the vaporization temperature, Tvap , should be set equal to each other when Law 4
is to be used. When wet combustion is active, Tbp and Tvap refer to the boiling and
evaporation temperatures for the combusting material only.
ANSYS FLUENT provides a choice of four devolatilization models:
• the constant rate model (the default model)
• the single kinetic rate model
• the two competing rates model (the Kobayashi model)
• the chemical percolation devolatilization (CPD) model
Each of these models is described, in turn, below.
Release 12.0 c ANSYS, Inc. January 29, 2009
15-25
Discrete Phase
Choosing the Devolatilization Model
You will choose the devolatilization model when you are setting physical properties for the
combusting-particle material in the Create/Edit Materials dialog box, as described in
Section 23.5.2: Description of the Properties in the separate User’s Guide. By default,
the constant rate model (Equation 15.4-26) will be used.
The Constant Rate Devolatilization Model
The constant rate devolatilization law dictates that volatiles are released at a constant
rate [20]:
−
where
mp
fv,0
mp,0
A0
=
=
=
=
1
dmp
= A0
fv,0 (1 − fw,0 )mp,0 dt
(15.4-26)
particle mass (kg)
fraction of volatiles initially present in the particle
initial particle mass (kg)
rate constant (s−1 )
The rate constant A0 is defined as part of your modeling inputs, with a default value of 12
s−1 derived from the work of Pillai [271] on coal combustion. Proper use of the constant
devolatilization rate requires that the vaporization temperature, which controls the onset
of devolatilization, be set appropriately. Values in the literature show this temperature
to be about 600 K [20].
The volatile fraction of the particle enters the gas phase as the devolatilizing species i,
defined by you (see Section 23.5: Setting Material Properties for the Discrete Phase in
the separate User’s Guide). Once in the gas phase, the volatiles may react according to
the inputs governing the gas phase chemistry.
The Single Kinetic Rate Model
The single kinetic rate devolatilization model assumes that the rate of devolatilization is
first-order dependent on the amount of volatiles remaining in the particle [10]:
−
where
mp
fv,0
fw,0
mp,0
k
15-26
dmp
= k[mp − (1 − fv,0 )(1 − fw,0 )mp,0 ]
dt
(15.4-27)
=
=
=
particle mass (kg)
mass fraction of volatiles initially present in the particle
mass fraction of evaporating/boiling material (if wet combustion
is modeled)
= initial particle mass (kg)
= kinetic rate (s−1 )
Release 12.0 c ANSYS, Inc. January 29, 2009
15.4 Laws for Heat and Mass Exchange
Note that fv,0 , the fraction of volatiles in the particle, should be defined using a value
slightly in excess of that determined by proximate analysis. The kinetic rate, k, is defined
by input of an Arrhenius type pre-exponential factor and an activation energy:
k = A1 e−(E/RT )
(15.4-28)
ANSYS FLUENT uses default rate constants, A1 and E [10].
Equation 15.4-27 has the approximate analytical solution:
mp (t + ∆t) = (1 − fv,0 )(1 − fw,0 )mp,0 + [mp (t) − (1 − fv,0 )(1 − fw,0 )mp,0 ]e−k∆t (15.4-29)
which is obtained by assuming that the particle temperature varies only slightly between
discrete time integration steps.
ANSYS FLUENT can also solve Equation 15.4-29 in conjunction with the equivalent heat
transfer equation using a stiff coupled solver. See Section 23.2.8: Including Coupled
Heat-Mass Solution Effects on the Particles in the separate User’s Guide for details.
The Two Competing Rates (Kobayashi) Model
ANSYS FLUENT also provides the kinetic devolatilization rate expressions of the form
proposed by Kobayashi [169]:
R1 = A1 e−(E1 /RTp )
(15.4-30)
R2 = A2 e−(E2 /RTp )
(15.4-31)
where R1 and R2 are competing rates that may control the devolatilization over different
temperature ranges. The two kinetic rates are weighted to yield an expression for the
devolatilization as
Z t
Z t
mv (t)
=
(α1 R1 + α2 R2 ) exp − (R1 + R2 ) dt dt
(1 − fw,0 )mp,0 − ma
0
0
where
mv (t)
mp,0
α1 , α2
ma
=
=
=
=
(15.4-32)
volatile yield up to time t
initial particle mass at injection
yield factors
ash content in the particle
Release 12.0 c ANSYS, Inc. January 29, 2009
15-27
Discrete Phase
The Kobayashi model requires input of the kinetic rate parameters, A1 , E1 , A2 , and E2 ,
and the yields of the two competing reactions, α1 and α2 . ANSYS FLUENT uses default
values for the yield factors of 0.3 for the first (slow) reaction and 1.0 for the second
(fast) reaction. It is recommended in the literature [169] that α1 be set to the fraction
of volatiles determined by proximate analysis, since this rate represents devolatilization
at low temperature. The second yield parameter, α2 , should be set close to unity, which
is the yield of volatiles at very high temperature.
By default, Equation 15.4-32 is integrated in time analytically, assuming the particle
temperature to be constant over the discrete time integration step. ANSYS FLUENT can
also solve Equation 15.4-32 in conjunction with the equivalent heat transfer equation
using a stiff coupled solver. See Section 23.2.8: Including Coupled Heat-Mass Solution
Effects on the Particles in the separate User’s Guide for details.
The CPD Model
In contrast to the coal devolatilization models presented above, which are based on empirical rate relationships, the chemical percolation devolatilization (CPD) model characterizes the devolatilization behavior of rapidly heated coal based on the physical and
chemical transformations of the coal structure [100, 101, 116].
General Description
During coal pyrolysis, the labile bonds between the aromatic clusters in the coal structure
lattice are cleaved, resulting in two general classes of fragments. One set of fragments
has a low molecular weight (and correspondingly high vapor pressure) and escapes from
the coal particle as a light gas. The other set of fragments consists of tar gas precursors
that have a relatively high molecular weight (and correspondingly low vapor pressure)
and tend to remain in the coal for a long period of time during typical devolatilization
conditions. During this time, reattachment with the coal lattice (which is referred to as
crosslinking) can occur. The high molecular weight compounds plus the residual lattice
are referred to as metaplast. The softening behavior of a coal particle is determined
by the quantity and nature of the metaplast generated during devolatilization. The
portion of the lattice structure that remains after devolatilization is comprised of char
and mineral-compound-based ash.
The CPD model characterizes the chemical and physical processes by considering the
coal structure as a simplified lattice or network of chemical bridges that link the aromatic
clusters. Modeling the cleavage of the bridges and the generation of light gas, char, and
tar precursors is then considered to be analogous to the chemical reaction scheme shown
in Figure 15.4.1.
15-28
Release 12.0 c ANSYS, Inc. January 29, 2009
15.4 Laws for Heat and Mass Exchange
Figure 15.4.1: Coal Bridge
Release 12.0 c ANSYS, Inc. January 29, 2009
15-29
Discrete Phase
The variable £ represents the original population of labile bridges in the coal lattice.
Upon heating, these bridges become the set of reactive bridges, £∗ . For the reactive
bridges, two competing paths are available. In one path, the bridges react to form side
chains, δ. The side chains may detach from the aromatic clusters to form light gas, g1 .
As bridges between neighboring aromatic clusters are cleaved, a certain fraction of the
coal becomes detached from the coal lattice. These detached aromatic clusters are the
heavy-molecular-weight tar precursors that form the metaplast. The metaplast vaporizes
to form coal tar. While waiting for vaporization, the metaplast can also reattach to the
coal lattice matrix (crosslinking). In the other path, the bridges react and become a char
bridge, c, with the release of an associated light gas product, g2 . The total population of
bridges in the coal lattice matrix can be represented by the variable p, where p = £ + c.
Reaction Rates
Given this set of variables that characterizes the coal lattice structure during devolatilization, the following set of reaction rate expressions can be defined for each, starting with
the assumption that the reactive bridges are destroyed at the same rate at which they
∗
are created ( ∂£
= 0):
∂t
d£
dt
dc
dt
dδ
dt
dg1
dt
dg2
dt
15-30
= −kb £
= kb
"
=
(15.4-33)
£
ρ+1
(15.4-34)
#
£
2ρkb
− kg δ
ρ+1
(15.4-35)
= kg δ
(15.4-36)
dc
dt
(15.4-37)
= 2
Release 12.0 c ANSYS, Inc. January 29, 2009
15.4 Laws for Heat and Mass Exchange
where the rate constants for bridge breaking and gas release steps, kb and kg , are expressed
in Arrhenius form with a distributed activation energy:
k = Ae−(E±Eσ )/RT
(15.4-38)
where A, E, and Eσ are, respectively, the pre-exponential factor, the activation energy,
and the distributed variation in the activation energy, R is the universal gas constant,
and T is the temperature. The ratio of rate constants, ρ = kδ /kc , is set to 0.9 in this
model based on experimental data.
Mass Conservation
The following mass conservation relationships are imposed:
g = g1 + g2
g1 = 2f − σ
g2 = 2(c − c0 )
(15.4-39)
(15.4-40)
(15.4-41)
where f is the fraction of broken bridges (f = 1 − p). The initial conditions for this
system are given by the following:
c(0)
£(0)
δ(0)
g(0)
=
=
=
=
c0
£0 = p 0 − c 0
2f0 = 2(1 − c0 − £0 )
g1 (0) = g2 (0) = 0
(15.4-42)
(15.4-43)
(15.4-44)
(15.4-45)
where c0 is the initial fraction of char bridges, p0 is the initial fraction of bridges in the
coal lattice, and £0 is the initial fraction of labile bridges in the coal lattice.
Release 12.0 c ANSYS, Inc. January 29, 2009
15-31
Discrete Phase
Fractional Change in the Coal Mass
Given the set of reaction equations for the coal structure parameters, it is necessary to
relate these quantities to changes in coal mass and the related release of volatile products.
To accomplish this, the fractional change in the coal mass as a function of time is divided
into three parts: light gas (fgas ), tar precursor fragments (ffrag ), and char (fchar ). This is
accomplished by using the following relationships, which are obtained using percolation
lattice statistics:
r(g1 + g2 )(σ + 1)
4 + 2r(1 − c0 )(σ + 1)
2
ffrag (t) =
[ΦF (p) + rΩK(p)]
2 + r(1 − c0 )(σ + 1)
fchar (t) = 1 − fgas (t) − ffrag (t)
fgas (t) =
(15.4-46)
(15.4-47)
(15.4-48)
The variables Φ, Ω, F (p), and K(p) are the statistical relationships related to the cleaving
of bridges based on the percolation lattice statistics, and are given by the following
equations:
"
£ (σ − 1)δ
Φ = 1+r
+
p
4(1 − p)
δ
£
Ω =
−
2(1 − p)
p
p0
p
F (p) =
K(p) =
(15.4-49)
(15.4-50)
! σ+1
σ−1
(15.4-51)
σ+1 0
1−
p
2
#
p0
p
! σ+1
σ−1
(15.4-52)
r is the ratio of bridge mass to site mass, mb /ma , where
mb = 2Mw,δ
ma = Mw,1 − (σ + 1)Mw,δ
15-32
(15.4-53)
(15.4-54)
Release 12.0 c ANSYS, Inc. January 29, 2009
15.4 Laws for Heat and Mass Exchange
where Mw,δ and Mw,1 are the side chain and cluster molecular weights respectively. σ + 1
is the lattice coordination number, which is determined from solid-state nuclear magnetic
Resonance (NMR) measurements related to coal structure parameters, and p0 is the root
of the following equation in p (the total number of bridges in the coal lattice matrix):
p0 (1 − p0 )σ−1 = p(1 − p)σ−1
(15.4-55)
In accounting for mass in the metaplast (tar precursor fragments), the part that vaporizes
is treated in a manner similar to flash vaporization, where it is assumed that the finite
fragments undergo vapor/liquid phase equilibration on a time scale that is rapid with
respect to the bridge reactions. As an estimate of the vapor/liquid that is present at
any time, a vapor pressure correlation based on a simple form of Raoult’s Law is used.
The vapor pressure treatment is largely responsible for predicting pressure-dependent
devolatilization yields. For the part of the metaplast that reattaches to the coal lattice,
a cross-linking rate expression given by the following equation is used:
dmcross
= mfrag Across e−(Ecross /RT )
dt
(15.4-56)
where mcross is the amount of mass reattaching to the matrix, mfrag is the amount of
mass in the tar precursor fragments (metaplast), and Across and Ecross are rate expression
constants.
CPD Inputs
Given the set of equations and corresponding rate constants introduced for the CPD
model, the number of constants that must be defined to use the model is a primary
concern. For the relationships defined previously, it can be shown that the following
parameters are coal independent [100]:
• Ab , Eb , Eσb , Ag , Eg , and Eσg for the rate constants kb and kg
• Across , Ecross , and ρ
These constants are included in the submodel formulation and are not input or modified
during problem setup.
Release 12.0 c ANSYS, Inc. January 29, 2009
15-33
Discrete Phase
There are an additional five parameters that are coal-specific and must be specified during
the problem setup:
• initial fraction of bridges in the coal lattice, p0
• initial fraction of char bridges, c0
• lattice coordination number, σ + 1
• cluster molecular weight, Mw,1
• side chain molecular weight, Mw,δ
The first four of these are coal structure quantities that are obtained from NMR experimental data. The last quantity, representing the char bridges that either exist in the
parent coal or are formed very early in the devolatilization process, is estimated based
on the coal rank. These quantities are entered in the Create/Edit Materials dialog box, as
described in Section 23.5.2: Description of the Properties in the separate User’s Guide.
Values for the coal-dependent parameters for a variety of coals are listed in Table 15.4.1.
Table 15.4.1: Chemical Structure Parameters for
Coal Type
Zap (AR)
Wyodak (AR)
Utah (AR)
Ill6 (AR)
Pitt8 (AR)
Stockton (AR)
Freeport (AR)
Pocahontas (AR)
Blue (Sandia)
Rose (AFR)
1443 (lignite, ACERC)
1488 (subbituminous, ACERC)
1468 (anthracite, ACERC)
σ+1
3.9
5.6
5.1
5.0
4.5
4.8
5.3
4.4
5.0
5.8
4.8
4.7
4.7
p0
.63
.55
.49
.63
.62
.69
.67
.74
.42
.57
.59
.54
.89
13
C NMR for 13 Coals
Mw,1
277
410
359
316
294
275
302
299
410
459
297
310
656
Mw,δ
40
42
36
27
24
20
17
14
47
48
36
37
12
c0
.20
.14
0
0
0
0
0
.20
.15
.10
.20
.15
.25
AR refers to eight types of coal from the Argonne premium sample bank [329, 363]. Sandia refers to
the coal examined at Sandia National Laboratories [99]. AFR refers to coal examined at Advanced Fuel
Research. ACERC refers to three types of coal examined at the Advanced Combustion Engineering
Research Center.
15-34
Release 12.0 c ANSYS, Inc. January 29, 2009
15.4 Laws for Heat and Mass Exchange
Particle Swelling During Devolatilization
The particle diameter changes during devolatilization according to the swelling coefficient,
Csw , which is defined by you and applied in the following relationship:
dp
(1 − fw,0 )mp,0 − mp
= 1 + (Csw − 1)
dp,0
fv,0 (1 − fw,0 )mp,0
where
dp,0
dp
(15.4-57)
= particle diameter at the start of devolatilization
= current particle diameter
w,0 )mp,0 −mp
The term (1−f
is the ratio of the mass that has been devolatilized to the total
fv,0 (1−fw,0 )mp,0
volatile mass of the particle. This quantity approaches a value of 1.0 as the devolatilization law is applied. When the swelling coefficient is equal to 1.0, the particle diameter
stays constant. When the swelling coefficient is equal to 2.0, the final particle diameter doubles when all of the volatile component has vaporized, and when the swelling
coefficient is equal to 0.5 the final particle diameter is half of its initial diameter.
Heat Transfer to the Particle During Devolatilization
Heat transfer to the particle during the devolatilization process includes contributions
from convection, radiation (if active), and the heat consumed during devolatilization:
mp cp
dTp
dmp
= hAp (T∞ − Tp ) +
hfg + Ap p σ(θR 4 − Tp 4 )
dt
dt
(15.4-58)
Radiation heat transfer to the particle is included only if you have enabled the P-1 or
discrete ordinates radiation model and you have activated radiation heat transfer to
particles using the Particle Radiation Interaction option in the Discrete Phase Model
dialog box.
By default, Equation 15.4-58 is solved analytically, by assuming that the temperature
and mass of the particle do not change significantly between time steps:
Tp (t + ∆t) = αp + [Tp (t) − αp ]e−βp ∆t
(15.4-59)
where
αp =
p
hfg + Ap p σθR 4
hAp T∞ + dm
dt
hAp + p Ap σTp 3
(15.4-60)
and
Release 12.0 c ANSYS, Inc. January 29, 2009
15-35
Discrete Phase
βp =
Ap (h + p σTp 3 )
m p cp
(15.4-61)
ANSYS FLUENT can also solve Equation 15.4-58 in conjunction with the equivalent mass
transfer equation using a stiff coupled solver. See Section 23.2.8: Including Coupled
Heat-Mass Solution Effects on the Particles in the separate User’s Guide for details.
15.4.5
Surface Combustion (Law 5)
After the volatile component of the particle is completely evolved, a surface reaction
begins which consumes the combustible fraction, fcomb , of the particle. Law 5 is thus
active (for a combusting particle) after the volatiles are evolved:
mp < (1 − fv,0 )(1 − fw,0 )mp,0
(15.4-62)
and until the combustible fraction is consumed:
mp > (1 − fv,0 − fcomb )(1 − fw,0 )mp,0
(15.4-63)
When the combustible fraction, fcomb , has been consumed in Law 5, the combusting
particle may contain residual “ash” that reverts to the inert heating law, Law 6 (described
previously).
With the exception of the multiple surface reactions model, the surface combustion law
consumes the reactive content of the particle as governed by the stoichiometric requirement, Sb , of the surface “burnout” reaction:
char(s) + Sb ox(g) −→ products(g)
(15.4-64)
where Sb is defined in terms of mass of oxidant per mass of char, and the oxidant and
product species are defined in the Set Injection Properties dialog box.
ANSYS FLUENT provides a choice of four heterogeneous surface reaction rate models for
combusting particles:
• the diffusion-limited rate model (the default model)
• the kinetics/diffusion-limited rate model
• the intrinsic model
• the multiple surface reactions model
15-36
Release 12.0 c ANSYS, Inc. January 29, 2009
15.4 Laws for Heat and Mass Exchange
Each of these models is described in detail below. You will choose the surface combustion
model when you are setting physical properties for the combusting-particle material, as
described in Section 23.5.2: Description of the Properties in the separate User’s Guide.
By default, the diffusion-limited rate model will be used.
The Diffusion-Limited Surface Reaction Rate Model
The diffusion-limited surface reaction rate model which is the default model in ANSYS
FLUENT, assumes that the surface reaction proceeds at a rate determined by the diffusion
of the gaseous oxidant to the surface of the particle:
dmp
Yox T∞ ρ
= −4πdp Di,m
dt
Sb (Tp + T∞ )
where
Di,m
Yox
ρ
Sb
=
=
=
=
(15.4-65)
diffusion coefficient for oxidant in the bulk (m2 /s)
local mass fraction of oxidant in the gas
gas density (kg/m3 )
stoichiometry of Equation 15.4-64
Equation 15.4-65 is derived from the model of Baum and Street [20] with the kinetic contribution to the surface reaction rate ignored. The diffusion-limited rate model assumes
that the diameter of the particles does not change. Since the mass of the particles is
decreasing, the effective density decreases, and the char particles become more porous.
The Kinetic/Diffusion Surface Reaction Rate Model
The kinetic/diffusion-limited rate model assumes that the surface reaction rate is determined either by kinetics or by a diffusion rate. ANSYS FLUENT uses the model of Baum
and Street [20] and Field [96], in which a diffusion rate coefficient
[(Tp + T∞ )/2]0.75
D0 = C1
dp
(15.4-66)
R = C2 e−(E/RTp )
(15.4-67)
and a kinetic rate
are weighted to yield a char combustion rate of
dmp
D0 R
= −Ap pox
dt
D0 + R
Release 12.0 c ANSYS, Inc. January 29, 2009
(15.4-68)
15-37
Discrete Phase
where Ap is the surface area of the droplet (πd2p ), pox is the partial pressure of oxidant
species in the gas surrounding the combusting particle, and the kinetic rate, R, incorporates the effects of chemical reaction on the internal surface of the char particle (intrinsic
reaction) and pore diffusion. In ANSYS FLUENT, Equation 15.4-68 is recast in terms of
the oxidant mass fraction, Yox , as
dmp
ρRT∞ Yox D0 R
= −Ap
dt
Mw,ox
D0 + R
(15.4-69)
The particle size is assumed to remain constant in this model while the density is allowed
to decrease.
When this model is enabled, the rate constants used in Equations 15.4-66 and 15.4-67 are
entered in the Create/Edit Materials dialog box, as described in Section 23.5: Setting
Material Properties for the Discrete Phase in the separate User’s Guide.
The Intrinsic Model
The intrinsic model in ANSYS FLUENT is based on Smith’s model [324], assuming the
order of reaction is equal to unity. Like the kinetic/diffusion model, the intrinsic model
assumes that the surface reaction rate includes the effects of both bulk diffusion and
chemical reaction (see Equation 15.4-69). The intrinsic model uses Equation 15.4-66 to
compute the diffusion rate coefficient, D0 , but the chemical rate, R, is explicitly expressed
in terms of the intrinsic chemical and pore diffusion rates:
R=η
dp
ρ p Ag k i
6
(15.4-70)
η is the effectiveness factor, or the ratio of the actual combustion rate to the rate attainable if no pore diffusion resistance existed [182]:
η=
3
(φ coth φ − 1)
φ2
(15.4-71)
where φ is the Thiele modulus:
"
dp Sb ρp Ag ki pox
φ=
2
De ρox
15-38
#1/2
(15.4-72)
Release 12.0 c ANSYS, Inc. January 29, 2009
15.4 Laws for Heat and Mass Exchange
ρox is the density of oxidant in the bulk gas (kg/m3 ) and De is the effective diffusion
coefficient in the particle pores. Assuming that the pore size distribution is unimodal
and the bulk and Knudsen diffusion proceed in parallel, De is given by
θ
1
1
De = 2
+
τ DKn D0
−1
(15.4-73)
where D0 is the bulk molecular diffusion coefficient and θ is the porosity of the char
particle:
θ =1−
ρp
ρt
(15.4-74)
ρp and ρt are, respectively, the apparent and true densities of the pyrolysis char.
τ (in Equation
√ 15.4-73) is the tortuosity of the pores. The default value for τ in ANSYS
FLUENT is 2, which corresponds to an average intersecting angle between the pores
and the external surface of 45◦ [182].
DKn is the Knudsen diffusion coefficient:
s
DKn = 97.0rp
Tp
Mw,ox
(15.4-75)
where Tp is the particle temperature and rp is the mean pore radius of the char particle, which can be measured by mercury porosimetry. Note that macropores (rp > 150
Å) dominate in low-rank chars while micropores (rp < 10 Å) dominate in high-rank
chars [182].
Ag (in Equations 15.4-70 and 15.4-72) is the specific internal surface area of the char
particle, which is assumed in this model to remain constant during char combustion.
Internal surface area data for various pyrolysis chars can be found in [323]. The mean
value of the internal surface area during char combustion is higher than that of the
pyrolysis char [182]. For example, an estimated mean value for bituminous chars is 300
m2 /g [50].
ki (in Equations 15.4-70 and 15.4-72) is the intrinsic reactivity, which is of Arrhenius
form:
ki = Ai e−(Ei /RTp )
(15.4-76)
where the pre-exponential factor Ai and the activation energy Ei can be measured for
each char. In the absence of such measurements, the default values provided by ANSYS
FLUENT (which are taken from a least squares fit of data of a wide range of porous
carbons, including chars [323]) can be used.
Release 12.0 c ANSYS, Inc. January 29, 2009
15-39
Discrete Phase
To allow a more adequate description of the char particle size (and hence density) variation during combustion, you can specify the burning mode α, relating the char particle
diameter to the fractional degree of burnout U (where U = 1 − mp /mp,0 ) by [322]
dp
= (1 − U )α
dp,0
(15.4-77)
where mp is the char particle mass and the subscript zero refers to initial conditions (i.e.,
at the start of char combustion). Note that 0 ≤ α ≤ 1/3 where the limiting values 0 and
1/3 correspond, respectively, to a constant size with decreasing density (zone 1) and a
decreasing size with constant density (zone 3) during burnout. In zone 2, an intermediate
value of α = 0.25, corresponding to a decrease of both size and density, has been found
to work well for a variety of chars [322].
When this model is enabled, the rate constants used in Equations 15.4-66, 15.4-70,
15.4-72, 15.4-73, 15.4-75, 15.4-76, and 15.4-77 are entered in the Create/Edit Materials dialog box, as described in Section 23.5: Setting Material Properties for the Discrete
Phase in the separate User’s Guide.
The Multiple Surface Reactions Model
Modeling multiple particle surface reactions follows a pattern similar to the wall surface
reaction models, where the surface species is now a “particle surface species”. For the
mixture material defined in the Species Model dialog box, the particle surface species can
be depleted or produced by the stoichiometry of the particle surface reaction (defined in
the Reactions dialog box). The particle surface species constitutes the reactive char mass
of the particle, hence, if a particle surface species is depleted, the reactive “char” content
of the particle is consumed, and in turn, when a surface species is produced, it is added
to the particle “char” mass. Any number of particle surface species and any number of
particle surface reactions can be defined for any given combusting particle.
Multiple injections can be accommodated, and combusting particles reacting according
to the multiple surface reactions model can coexist in the calculation, with combusting
particles following other char combustion laws. The model is based on oxidation studies
of char particles, but it is also applicable to gas-solid reactions in general, not only to
char oxidation reactions.
See Section 7.3: Particle Surface Reactions for information about particle surface reactions.
15-40
Release 12.0 c ANSYS, Inc. January 29, 2009
15.4 Laws for Heat and Mass Exchange
Limitations
Note the following limitations of the multiple surface reactions model:
• The model is not available together with the unsteady tracking option.
• The model is available only with the species transport model for volumetric reactions, and not with the nonpremixed, premixed, or partially premixed combustion
models.
Heat and Mass Transfer During Char Combustion
The surface reaction consumes the oxidant species in the gas phase; i.e., it supplies a
(negative) source term during the computation of the transport equation for this species.
Similarly, the surface reaction is a source of species in the gas phase: the product of
the heterogeneous surface reaction appears in the gas phase as a user-selected chemical
species. The surface reaction also consumes or produces energy, in an amount determined
by the heat of reaction defined by you.
The particle heat balance during surface reaction is
m p cp
dTp
dmp
= hAp (T∞ − Tp ) − fh
Hreac + Ap p σ(θR 4 − Tp 4 )
dt
dt
(15.4-78)
where Hreac is the heat released by the surface reaction. Note that only a portion (1 − fh )
of the energy produced by the surface reaction appears as a heat source in the gasphase energy equation: the particle absorbs a fraction fh of this heat directly. For coal
combustion, it is recommended that fh be set to 1.0 if the char burnout product is CO
and 0.3 if the char burnout product is CO2 [33].
Radiation heat transfer to the particle is included only if you have enabled the P-1 or
discrete ordinates radiation model and you have activated radiation heat transfer to
particles using the Particle Radiation Interaction option in the Discrete Phase Model
dialog box.
By default, Equation 15.4-78 is solved analytically, by assuming that the temperature
and mass of the particle do not change significantly between time steps. ANSYS FLUENT
can also solve Equation 15.4-78 in conjunction with the equivalent mass transfer equation
using a stiff coupled solver. See Section 23.2.8: Including Coupled Heat-Mass Solution
Effects on the Particles in the separate User’s Guide for details.
Release 12.0 c ANSYS, Inc. January 29, 2009
15-41
Discrete Phase
15.4.6
Multicomponent Particle Definition (Law 7)
Multicomponent particles are described in ANSYS FLUENT as a mixture of species within
droplets/particles. The particle mass m is the sum of the masses of the components
m=
X
mi
(15.4-79)
i
The density of the particle ρp can be either constant, or volume-averaged:
ρp =
X mi
i
!−1
(15.4-80)
mρi
For particles containing more than one component it is difficult to assign the whole
particle to one process like boiling or heating. Therefore it can be only modeled by a law
integrating all processes of relevance in one equation. The source terms for temperature
and component mass are the sum of the sources from the partial processes:
mp cp
dTp
dt
!
4
= Ap p σ(θR
− Tp4 ) + hAp (T∞ − Tp ) +
X dmi
i
dmi
dt
dt
(hi,p − hi,g )
(15.4-81)
!
= Ap Mw,i kc,i (Ci,s − Ci,∞ )
(15.4-82)
The equation for the particle temperature T consists of terms for radiation, convective
heating (Equation 15.4-3) and vaporization. Radiation heat transfer to the particle is
included only if you have enabled P-1 or Discrete-Ordinates (DO) radiation and you have
activated radiation heat transfer to the particles using the Particle Radiation Interaction
option in the Discrete Phase Model dialog box.
The mass of the particle components mi is only influenced by the vaporization (Equation 15.4-12), where Mw,i is the molecular weight of species i. The mass transfer coefficient
kc,i of component i is calculated from the Sherwood correlation (Equation 15.4-15). The
concentration of vapor at the particle surface Ci,s depends on the saturation pressure of
the component.
Raoult’s Law
The correlation between the vapor concentration of a species Ci,s over the surface and
its mole fraction in the condensed phase XiL is described by Raoult’s law:
Ci,s =
15-42
pi
X Lp
= i
RT
RT
(15.4-83)
Release 12.0 c ANSYS, Inc. January 29, 2009
15.5 Vapor Liquid Equilibrium Theory
Peng-Robinson Real Gas Model
For the calculation of the vapor concentration of a species Ci,S over the surface depends
on whether the compressability of the vapor phase Z V is taken into account:
Ci,S = xi V
p
Z V RT
(15.4-84)
The data for the vapor pressure are no longer available, when a droplet material is chosen
as the component of a mixture, because it is not necessary for the calculation.
Besides using Raoult’s Law and the Peng-Robinson equation of state, you can define your
own user-defined function for delivering the vapor concentration at the particle surface .
For more information, see Section 2.5.15: DEFINE DPM VP EQUILIB in the separate UDF
Manual.
15.5 Vapor Liquid Equilibrium Theory
A number of industrially important processes, such as distillation, absorption and extraction, bring into contact two phases which are not at equilibrium. The rate at which
a species is transferred from one phase to the other depends on the departure of the
system from equilibrium. The quantitative treatment of these rate processes requires
knowledge of the equilibrium states of the system. Apart from these cases, vapor-liquid
equilibrium (VLE) relationships in multicomponent systems are needed for the solution
of many other classes of engineering problems, such as the computation of evaporation
rates in spray combustion applications.
In ANSYS FLUENT the rate of vaporization of a single component droplet is computed
from Equation 15.4-12, where Ci,s is the equilibrium concentration of the droplet species
in the gas phase, and is computed in Equation 15.4-13 as:
Ci,s = psat /RTp
(15.5-1)
where Tp is the droplet temperature, and psat is the saturation pressure of the droplet
species at Tp .
For the general case where N components are evaporating from a droplet (distillation),
the evaporation rate of each species is again given by Equation 15.4-12; however, psat in
Equation 15.5-1 must be replaced by pi , the partial pressure of species i, to calculate the
concentration of i at the droplet surface.
The partial pressure of species i can be obtained from the general expression for two phase
equilibrium, equating the fugacity of the liquid and vapor mixture components [275]:
fi V = xi V φi V p = xi L φi L p = fi L
Release 12.0 c ANSYS, Inc. January 29, 2009
(15.5-2)
15-43
Discrete Phase
where xi is the mole fraction, φi is the fugacity coefficient for the species i in the mixture,
and p is the absolute pressure. The superscripts V and L are the vapor and the liquid
phase variables, respectively. The fugacity coefficients account for the nonideality in the
gas and liquid mixture. The fugacity of the liquid phase can be calculated from the pure
component’s saturation pressure psat,i [325]:
"
L
L
L
fi = xi φi p =
γi xLi φsat,i L psat,i exp
Vi L (p − psat,i )
RT
#
(15.5-3)
Here, φsat,i L is the fugacity coefficient for pure i at the saturation pressure; γi is the activity coefficient for species i in the mixture, and accounts for the nonideality in the liquid
phase; T is the particle surface temperature. We assume perfect thermal conductivity
inside the particle, so the particle temperature is used instead; R is the universal gas
constant; Vi L is the molar volume of the liquid. The exponential term is the Poynting
correction factor and accounts for the compressibility effects within the liquid. Except at
high pressures, the Poynting factor is usually negligible. Under low pressure conditions
where the gas phase may be assumed to be ideal, φi V ≈ 1 and φsat,i ≈ 1 . Furthermore,
if the liquid is also assumed to be ideal, γ ≈ 1, then Equation 15.5-2 reduces to Raoult’s
law,
xi V p = xi L psat,i
(15.5-4)
Raoult’s law is the default vapor-liquid equilibrium expression used in the ANSYS FLUENT multicomponent droplet model. However, there is a UDF hook available for userdefined vapor-liquid equilibrium models.
While Raoult’s law represents the simplest form of the VLE equation, keep in mind that
it is of limited use, as the assumptions made for its derivation are usually unrealistic.
The most critical assumption is that the liquid phase is an ideal solution. This is not
likely to be valid, unless the system is made up of species of similar molecular sizes and
chemical nature, such as in the case of benzene and toluene, or n-heptane and n-hexane.
When Raoult’s law is applicable, the vaporization rate of each species from a multicomponent droplet can be computed from Equation 15.4-12, with the equilibrium concentration
of species i in the gas phase Ci,s computed as:
Ci,s = xi psat,i /RTp
(15.5-5)
where Tp is the droplet temperature, xi is the mole fraction of species i in the droplet,
and psat,i is the saturation pressure of species i at Tp .
For higher pressures, especially near or above the critical point of the components, real
gas effects must be considered. Most models describing the fugacity coefficients use a
cubic equation of state with the general form:
15-44
Release 12.0 c ANSYS, Inc. January 29, 2009
15.5 Vapor Liquid Equilibrium Theory
RT
a(V − η)
−
V − b (V − b)(V 2 + δV − )
p=
(15.5-6)
where V is the molar volume. For in-cylinder applications, the Peng-Robinson equation
of state is often used [265], where δ = 2b, = −b2 , and η = b:
p=
RT
a
− 2
V − b V + 2bV − b2
(15.5-7)
This equation defines the compressibility
Z=
pV
RT
aV /RT
=
− 2
RT
V − b V + 2bV − b2
(15.5-8)
The implementation of the Peng-Robinson equation of state in ANSYS FLUENT uses this
expression for both phases, the particle liquid and the vapor phase. The parameters a
and b are determined by the composition using a simple mixing law:
a =
N X
N
X
√
x i x j ai aj
i=1 j=1
b =
N
X
x i bi
(15.5-9)
i=1
where N is the number of components in the mixture. The pure component parameters
can be obtained using the relationship with the Peng-Robinson constants:
!
ai =
2
R2 Tc,i
T
1 + (0.480 + 1.574ωi − 0.176ωi 2 ) 1 −
4.57235
pc,i
Tc,i
bi = 0.077796
RTc,i
Pc,i
!1/2 2
(15.5-10)
where Tc,i is the critical temperature, pc,i is the critical pressure and ωi is the accentric
factor of the component i.
The fugacities of the components depend on the compressibility of the liquid and vapor
phase:
lnφi =
Release 12.0 c ANSYS, Inc. January 29, 2009
∂(Aγ /RT )
∂Ni
!
− lnZ
(15.5-11)
T,V,Nj6=i
15-45
Discrete Phase
where Aγ is the residual Helmholtz energy, which is a function of the compressibility:
Z ∞
Aγ
dV
[1 − Z]
=
+ lnZ
RT
V
V
(15.5-12)
In summary, the vapor mole fraction xi V , the pressure p, and the compressibilities of the
vapor (Z V ) and the liquid (Z L ) phase at the surface of the particle are determined from
the liquid particle mole fraction of the components xi L and the particle temperature Tp .
The surface vapor concentrations are calculated using the following equation:
Ci,S = xi V
15.6
p
(15.5-13)
Z V RT
Wall-Jet Model Theory
The direction and velocity of the droplet particles are given by the resulting momentum flux, which is a function of the impingement angle, φ, and Weber number. See
Figure 15.6.1.
z
y
φ
H(Ψ)
Ψ
x
x
side view
top view
Figure 15.6.1: “Wall Jet” Boundary Condition for the Discrete Phase
The wall-jet type boundary condition assumes an analogy with an inviscid jet impacting
a solid wall. Equation 15.6-1 shows the analytical solution for an axisymmetric impingement assuming an empirical function for the sheet height (H) as a function of the angle
that the drop leaves the impingement (Ψ).
Ψ
H(Ψ) = Hπ eβ(1− π )
(15.6-1)
where Hπ is the sheet height at Ψ = π and β is a constant determined from conservation
of mass and momentum. The probability that a drop leaves the impingement point at
an angle between Ψ and Ψ + δΨ is given by integrating the expression for H(Ψ)
15-46
Release 12.0 c ANSYS, Inc. January 29, 2009
15.7 Wall-Film Model Theory
π
Ψ = − ln[1 − P (1 − e−β )]
β
(15.6-2)
where P is a random number between 0 and 1. The expression for β is given in Naber
and Reitz [244] as
sin(φ) =
15.7
eβ + 1
(eβ − 1)(1 + ( βπ )2 )
(15.6-3)
Wall-Film Model Theory
This section is composed of the following:
• Section 15.7.1: Introduction
• Section 15.7.2: Interaction During Impact with a Boundary
• Section 15.7.3: Splashing
• Section 15.7.4: Separation Criteria
• Section 15.7.5: Conservation Equations for Wall-Film Particles
15.7.1
Introduction
ANSYS FLUENT has a specific boundary condition for simulation of internal combustion
engines, called the wall-film model.
Spray-wall interaction is an important part of the mixture formation process in port fuel
injected (PFI) engines. A fuel spray impinges on a surface, usually at the intake port near
the intake valve, as well as at the intake valve itself, where it splashes and subsequently
evaporates. The evaporated mixture is entrained into the cylinder of the engine, where
it is mixed with the fresh charge and any residual gas in the cylinder. The mixture that
is compressed and burned, finally exits through the exhaust port. The process repeats
itself between 200 and 8000 times per minute, depending on the engine.
Several cycles worth of fuel remain in the intake tract due to film formation on the
walls. This in turn makes the film important in hydrocarbon emissions for PFI engines.
Additionally, film can form inside combustion chambers of direct injection (DI) types
of engines. In a direct injection engine, fuel is injected directly into the combustion
chamber, where the spray can impinge upon the piston if the injection event is early or
late in the cycle. The modeling of the wall-film inside a DI engine, especially in diesel
engines, is compounded by the presence of carbon deposits on the surfaces of the engine.
This carbon deposit absorbs the liquid film as it impinges upon it. It is believed that
Release 12.0 c ANSYS, Inc. January 29, 2009
15-47
Discrete Phase
the carbon deposits adsorb the fuel later in the cycle, however this phenomena is very
complex and is not well understood.
DPM particles are used to model the wall-film. The wall-film model in ANSYS FLUENT
allows a single component liquid drop to impinge upon a boundary surface and form a
thin film. The model can be broken down into four major subtopics: interaction during
the initial impact with a wall boundary, subsequent tracking on surfaces, calculation of
film variables, and coupling to the gas phase. Figure 15.7.1 schematically shows the basic
mechanisms considered for the wall-film model.
Major Physical Phenomena
Convective
heat transfer
Impinging
Fuel Drops
Splashing
Evaporation
Shear Forces
Film separation
and sheet breakup
Conduction
Figure 15.7.1: Mechanisms of Splashing, Momentum, Heat and Mass Transfer for the Wall-Film
The main assumptions and restrictions for the wall-film model are as follows:
• The layer is thin, less than 500 microns in thickness. This limitation is due to the
assumption of a linear velocity profile in the film.
• The temperature in the film particles change relatively slowly so that an analytical
integration scheme can be utilized.
• Film particles are assumed to be in direct contact with the wall surface and the
heat transfer from the wall to the film takes place by conduction.
• The film temperature never exceeds the boiling temperature for the liquid.
• The simulation is transient.
• The wall-film model is not available with the Workpile Algorithm shared memory
option in parallel processing.
15-48
Release 12.0 c ANSYS, Inc. January 29, 2009
15.7 Wall-Film Model Theory
If you wish to model a spray impacting a very hot wall, the wall-jet model may be
more appropriate as the assumption in the wall-jet impingement model is that there is
a vapor layer underneath the drops which keeps them from making direct contact with
the boundary surface. This may be a more accurate assumption for in-cylinder diesel
computations at typical operating conditions.
15.7.2 Interaction During Impact with a Boundary
The wall interaction is based on the work of Stanton [336] and O’Rourke [258], where
the regimes are calculated for a drop-wall interaction based on local information. The
four regimes, stick, rebound, spread, and splash are based on the impact energy and wall
temperature. The following chart is helpful in showing the cutoffs.
E 6
Splash
Spread
Rebound
Stick
-
Tb
Tw
Figure 15.7.2: Simplified Decision Chart for Wall Interaction Criterion.
Below the boiling temperature of the liquid, the impinging droplet can either stick, spread
or splash, while above the boiling temperature, the particle can either rebound or splash.
The criteria by which the regimes are partitioned are based on the impact energy and
the boiling temperature of the liquid. The impact energy is defined by
ρV 2 D
E = r
σ
2
1
min (h0 /D, 1) + δbl /D
!
(15.7-1)
where ρ is the liquid density, Vr is the relative velocity of the particle in the frame of the
wall (i.e. Vr2 = (Vp − Vw )2 ), D is the diameter of the droplet, and σ is the surface tension
of the liquid. Here, δbl is a boundary layer thickness, defined by
D
δbl = √
Re
(15.7-2)
where the Reynolds number is defined as Re = ρVr D/µ. By defining the energy as in
Equation 15.7-1, the presence of the film on the wall suppresses the splash, but does not
give unphysical results when the film height approaches zero.
Release 12.0 c ANSYS, Inc. January 29, 2009
15-49
Discrete Phase
The sticking regime is applied when the dimensionless energy E is less than 16, and the
particle velocity is set equal to the wall velocity. In the spreading regime, the initial direction and velocity of the particle are set using the wall-jet model, where the probability
of the drop having a particular direction along the surface is given by an analogy of an
inviscid liquid jet with an empirically defined radial dependence for the momentum flux.
If the wall temperature is above the boiling temperature of the liquid, impingement events
below a critical impact energy (Ecr ) results in the particles rebounding from the wall. For
the rebound regime, the particle rebounds with the following coefficient of restitution:
e = 0.993 − 1.76ΘI + 1.56Θ2I − 0.49Θ3I
(15.7-3)
where ΘI is the impingement angle as measured from the wall surface.
Splashing occurs when the impingement energy is above a critical energy threshold,
defined as Ecr = 57.7. The number of splashed droplet parcels is set in the Wall boundary
condition dialog box with a default number of 4, however, you can select numbers between
zero and ten. The splashing algorithm follows that described by Stanton [336] and is
detailed in Section 15.7.3: Splashing.
15.7.3
Splashing
If the particle impinging on the surface has a sufficiently high energy, the particle splashes
and several new particles are created. You can explicitly set the number of particles created by each impact in the DPM tab of the Wall boundary condition dialog box. The
number of splashed parcels may be set to an integer value between zero and ten. The
properties (diameter, magnitude, and direction) of the splashed parcels are randomly
sampled from the experimentally obtained distribution functions described in the following sections. Setting the number of splashed parcels to zero turns off the splashing
calculation. Bear in mind that each splashed parcel can be considered a discrete sample
of the distribution curves and that selecting the number of splashed drops in the Wall
boundary condition dialog box does not limit the number of splashed drops, only the
number of parcels representing those drops.
Therefore, for each splashed parcel, a different diameter is obtained by sampling a cumulative probability distribution function (CPDF), which is obtained from a Weibull
distribution function and fitted to the data from Mundo, et al. [241]. The equation is
pdf
d
D
!
d
d
= 2 2 exp −
D
D
!2
(15.7-4)
and it represents the probability of finding drops of diameter di in a sample of splashed
drops. This distribution is similar to the Nakamura-Tanasawa distribution function used
√
by O’Rourke [258], but with the peak of the distribution function being D = dmax / 2.
To ensure that the distribution functions produce physical results with an increasing
15-50
Release 12.0 c ANSYS, Inc. January 29, 2009
15.7 Wall-Film Model Theory
Weber number, the following expression for dmax from O’Rourke [258] is used. The peak
of the splashed diameter distribution is
2
Ecrit
6.4
,
, 0.06
dmax /d0 = MAX
2
E We
!
(15.7-5)
where the expression for energy is given by Equation 15.7-1. Low Weber number impacts
are described by the second term in Equation 15.7-5 and the peak of the minimum
splashed diameter distribution is never less than 0.06 for very high energy impacts in any
of the experiments analyzed by O’Rourke [258]. The Weber number in Equation 15.7-5
is defined using the relative velocity and drop diameter:
We =
ρVr2 D
σ
(15.7-6)
The cumulative probability distribution function (CPDF) is needed so that a diameter
can be sampled from the experimental data. The CPDF is obtained from integrating
Equation 15.7-4 to obtain
cpdf
d
D
!
= 1 − exp −
!2
d
D
(15.7-7)
which is bounded by zero and one. An expression for the diameter (which is a function
of D, the impingement Weber number W e, and the impingement energy) is obtained by
inverting Equation 15.7-7 and sampling the CPDF between zero and one. The expression
for the diameter of the ith splashed parcel is therefore given by,
q
di = D − ln (1 − ci )
where ci is the ith random sample. Once the diameter of the splashed drop has been
determined, the probability of finding that drop in a given sample is determined by
evaluating Equation 15.7-4 at the given diameter. The number of drops per parcel can
be expressed as a function of the total number of splashed drops:
Ni = Ntot pdfi
(15.7-8)
where the pdfi is for the ith sample. The values of pdfi are then normalized so that their
sum is one. Both the number per parcel (Ni ) and the total number of splashed drops
(Ntot ) is unknown, but an expression for Ntot can be obtained from the conservation of
mass if the total splashed mass is known.
The amount of mass splashed from the surface is a quadratic function of the splashing
energy, obtained from the experimental data from Mundo [241]. The splashed mass
fraction ys is given by
(
ys =
2
2
1.8x10−4 (E 2 − Ecrit
) , Ecrit
< E 2 < 7500
2
0.70
, E > 7500
Release 12.0 c ANSYS, Inc. January 29, 2009
15-51
Discrete Phase
The authors (O’Rourke et al. [258]) noted that nearly all of the impacts for typical diesel
sprays are well above the upper bound and so the splashing event nearly always ejects
70% of the mass of the impinging drop. To obtain an expression for the total number of
drops, we note that overall conservation of mass requires that the sum of the total mass
of the splashed parcel(s) must equal the splashed mass fraction, or
Nparcels
X
ρπ
Ntot
pdfn d3n = ys m0
6
n=1
(15.7-9)
where m0 is the total mass of the impinging parcel. The expression for the total number
of splashed drops is
ys m0
Ntot = ρπ PNparcels
(pdfn d3n )
n=1
6
The number of splashed drops per parcel is then determined by Equation 15.7-8 with the
values of pdfi given by Equation 15.7-4.
To calculate the velocity with which the splashed drops leave the surface, additional
correlations are sampled for the normal component of the velocity. A Weibull function,
fit to the data from Mundo [241], is used as the PDF for the normal component. The
probability density is given by
Vni
pdf
Vnd
bv
=
Θv
Vni /Vnd
Θv
!bv −1
exp −
Vni /Vnd
Θv
!bv
(15.7-10)
where
(
bv =
2.1,
ΘI ≤ 50◦
1.10 + 0.02ΘI , ΘI > 50◦
(15.7-11)
and
Θv = 0.158e0.017ΘI
(15.7-12)
where ΘI is the angle at which the parcel impacts the surface, or the impingement angle.
The tangential component of the velocity is obtained from the expression for the reflection
angle Θs :
Θs = 65.4 + 0.226Θl
(15.7-13)
combined with
Vti =
Vni
tan(Θs )
(15.7-14)
Finally, an energy balance is performed for the new parcels so that the sum of the kinetic
and surface energies of the new drops does not exceed that of the old drops. The energy
balance is given by
N
Nparcel
X
X
1 parcel
1
mi Vi2 + πσ
Ni d2i = md Vd2 mi Vi2 + πσ md d2i − Ecrit
2 i=1
2
i=1
15-52
Release 12.0 c ANSYS, Inc. January 29, 2009
15.7 Wall-Film Model Theory
where Ecrit is the threshold energy for splashing to occur. To ensure conservation of
energy, the following correction factor is computed:
K=
1
m V2
2 d d
(mi Vi2 ) + πσ (md d2i ) − Ecrit − πσ
1
2
PNparcel
i=1
(mi Vi2 )
PNparcel
i=1
(Ni d2i )
.
(15.7-15)
This correction factor is needed due to the relatively small number of sampled points for
the velocity of the splashed drops (see Stanton [337] for more detail). The components
of the splashed parcel are multiplied by the square root of K in Equation 15.7-15 so that
energy will be conserved. The normal and tangential velocity components of the splashed
parcels are therefore given by
√
√
Vni0 = KVni
and
Vti0 = KVti
ANSYS FLUENT will limit the velocity of the splashed parcels so that they do not exceed
the impact velocity of the original parcel. It is important to note that splashing events are
inherently transient, so the splashing submodel is only available with unsteady tracking
in ANSYS FLUENT. Splashing can also cause large increases in source terms in the cells
in which it occurs, which can cause difficulty in convergence between time steps. Thus,
it may be necessary to use a smaller time step during the simulation when splashing is
enabled.
15.7.4
Separation Criteria
The film can separate from the wall when the stress at an edge of the film exceeds
the adhesion forces holding the film to the wall. These forces are complex and highly
dependent on local surface conditions. An order of magnitude analysis of a film rounding
a sharp corner shows that the stresses at the edge of a film are proportional to the angle
which the film negotiates. In ANSYS FLUENT, you can specify the maximum angle that
the film can negotiate using a special text command. For more information, contact your
ANSYS FLUENT support engineer.
Release 12.0 c ANSYS, Inc. January 29, 2009
15-53
Discrete Phase
15.7.5
Conservation Equations for Wall-Film Particles
Conservation equations for momentum, mass, and energy for individual parcels in the
wall-film are described below. The particle-based approach for thin films was first formulated by O’Rourke [257] and most of the following derivation is based closely on that
work.
Momentum
The equation for the momentum of a parcel on the film is
ρh
d~up
˙
˙
+ h(∇s pf )α = τg~tg + τw~tw + P~ imp,α − Ṁimp,α~up + F~ n,α + ρh(~g − ~aw )
dt
(15.7-16)
where α denotes the current face on which the particle resides, h denotes the current film
height at the particle location, ∇s is the gradient operator restricted to the surface, and
pf is the pressure on the surface of the film. On the right-hand side of Equation 15.7-16,
τg denotes the magnitude of the shear stress of the gas flow on the surface of the film, t~g
is the unit vector in the direction of the relative motion of the gas and the film surface,
µl is the liquid viscosity, and τw is the magnitude of the stress that the wall exerts on
the film. Similarly to the expression for t~g , t~w is the unit vector in the direction of the
relative motion of the film and the wall. The remaining expressions on the right-hand
˙
side of Equation 15.7-16 are P~ imp,α which denotes the impingement pressure on the film
~˙ imp,α is the impingement momentum source, and F~˙ n,α is the force necessary
surface, M
to keep the film on the surface, as determined by
~up · n̂α = 0.
(15.7-17)
Here, ρh(~g − ~aw ) is the body force term. Note that the body force term can be very
significant, despite the small values of film thickness due to the very high acceleration
rates seen in simulations with moving boundaries. The requirement represented by Equation 15.7-17 is explicitly enforced at each time step in ANSYS FLUENT for all particles
representing the wall-film.
The term h(∇s pf )α is the surface gradient of the pressure on the face, pf . This pressure,
pf , is the sum of the fluid pressure and the impingement pressure from the drops on the
face, given by
˙
pf = Pcell − P~ imp,α · n̂ + Ṁimp,α~up · n̂
where the impingement mass Ṁimp,α is given by
Ṁimp,α =
ZZZ
ρl Vp~v · n̂f (~xs , ~v , r, Td , t)drd~v dTd
(15.7-18)
and the impingement pressure is given by
˙
P~ imp,α =
15-54
ZZZ
ρl Vp~v~v · n̂f (~xs , ~v , r, Td , t)drd~v dTd
(15.7-19)
Release 12.0 c ANSYS, Inc. January 29, 2009
15.7 Wall-Film Model Theory
where Vp is the volume of the drop. An approximation of the impingement mass in
Equation 15.7-18 is given by
Ṁimp,α =
Ns
X
!,
ρVp
Aα ∆t,
(15.7-20)
n=0
and the corresponding expression of the impingement pressure in Equation 15.7-19 is
given by
,
Ni
X
˙
P~ imp,α =
ρVp (~un+1
− ~unp ) Aα ∆t.
(15.7-21)
p
n=0
The summation in Equation 15.7-20 is over all the drops which actually stick to the face
α during the time step (Ns ). The summation in Equation 15.7-21 is over all the particles
which impinge upon the face during the same interval (Ni ).
The expression for the stress that the gas exerts on the surface of the wall-film, τg , in
Equation 15.7-16 is given by
2
τg = Cf (~ug − 2~up )2 = Cf Vrel
g
where Cf is the skin friction coefficient and ~ug is the gas velocity evaluated at the film
height above the wall. The assumption made in evaluating the skin friction coefficient
is that the wall shear stress from the gas is constant over the thickness of the film and
the boundary layer above the film (in the normal direction from the face). The stress is
tangent to the wall in the direction of the difference between the wall-film velocity and
the gas velocity, so the unit vector in the direction of the velocity difference along the
surface is
V~relg − (V~relg · n̂)n̂
t̂g =
|V~relg − (V~relg · n̂)n̂|
where n̂ is the normal face . The expression for the stress that the wall exerts on the
film, τw , in Equation 15.7-16 is given by
τw = −
µl
µl
|2~up − ~uw | = − |V~relw |
h
h
where µl is the liquid viscosity and ~uw is the velocity of the wall. Here, τw acts in the
direction of the velocity difference between the wall and the film, as given by
t̂w =
V~relw − (V~relw · n̂)n̂
.
|V~relw − (V~relw · n̂)n̂|
Note that the tangential unit vectors, t̂g and t̂w , are independent and can point in completely different directions.
Since ANSYS FLUENT solves a particle position equation of the form
d~up
= α − β~up ,
dt
Release 12.0 c ANSYS, Inc. January 29, 2009
15-55
Discrete Phase
Equation 15.7-16 must be rearranged. The film particle acceleration is then given by
2Cf |Vrelg | 2µl
d~up Cf |Vrelg |
(∇s pf )α µl |u~w |
P~imp
Ṁimp
−
=
t̂g −
+
t̂
+
+
~
g
+
+
~up .
w
dt
ρh
ρ
ρh2
ρh
ρh
ρh2
ρh
(15.7-22)
The terms for Mimp and P~imp are used from the previous time step and the differential
equations for the particle motion are solved with the existing integration routines.
!
Mass Transfer from the Film
The film vaporization law is applied when the film particle is above the vaporization
temperature Tvap . A wall particle has the temperature limited by the boiling temperature
Tbp and does not have a specific boiling law associated with the physics of film boiling.
The vaporization rate of the film is governed by gradient diffusion from the surface
exposed to the gas phase. The gradient of vapor concentration between the film surface
and the gas phase is
Ṅi = Bf (Ci,s − Ci,∞ )
(15.7-23)
where Ṅi is the molar flux of vapor (with units of kgmol/m2 -s), Bf is the mass transfer
coefficient (in m/s), and Ci,s and Ci,∞ are the vapor concentrations on the film surface
and in the bulk gas, respectively. The units of vapor concentration are kgmol/m3 .
The vapor concentration at the surface is evaluated using the saturated vapor pressure
at the film surface temperature and the bulk gas concentration is obtained from the flow
field solution. The vaporization rate is sensitive to the saturated vapor pressure, similar
to droplet vaporization.
The mass transfer coefficient is obtained using a Nusselt correlation for the heat transfer
coefficient and replacing the Prandtl number with the Schmidt number. The equation is
Bf x
N ux =
=
kf
(
0.332Rex1/2 Sc1/3 Rex < 2500, 0.6 < Sc < 50
1/3
0.0296Re4/5
Rex > 2500, 0.6 < Sc < 60
x Sc
(15.7-24)
where the Reynolds number is based on a representative length derived from the face
area. The temperature for the film surface is equal to the gas temperature, but is limited
by the boiling temperature of the liquid. The particle properties are evaluated at the
surface temperature when used in correlation 15.7-24.
For multicomponent vaporization, the Schmidt number based on the diffusivity of each
species is used to calculate the correlation in equation 15.7-24 for each component.
The mass of the particle is decreased by
mp (t + ∆t) = mp (t) − Ni Ap Mw,i ∆t
(15.7-25)
where Mw,i is the molecular weight of the gas phase species to which the vapor from the
liquid is added. The diameter of the film particle is decreased to account for the mass
15-56
Release 12.0 c ANSYS, Inc. January 29, 2009
15.7 Wall-Film Model Theory
loss in the individual parcel. This keeps the number of drops in the parcel constant and
acts only as a place holder. When the parcel detaches from the boundary, the diameter
is set to the height of the film and the number in the parcel is adjusted so that the overall
mass of the parcel is conserved.
Energy Transfer from the Film
To obtain an equation for the temperature in the film, energy flux from the gas side as
well as energy flux from the wall side must be considered. The assumed temperature
profile in the liquid is bilinear, with the surface temperature Ts being the maximum
temperature of the gas at the film height. Furthermore, the boiling point of the liquid
and the wall temperature will be the maximum of the wall face temperature Tw , and
will be the same boiling temperature as the liquid. An energy balance on a film particle
yields
d
{mp Cp Tp } = Qcond + Qconv
(15.7-26)
dt
where Qcond is the conduction from the wall, given by
Qcond =
κAp
(Tw − Tp )
h
where κ is the thermal conductivity of the liquid and h is the film height at the location
of the particle, as seen in Figure 15.7.3. The convection from the top surface, Qconv is
given by
Qconv = hf Ap (Tg − Tp )
where hf is the film heat transfer coefficient given by Equation 15.7-24 and Ap is the
area represented by a film particle, taken to be a mass weighted percentage of the face
area, Af . Contributions from the impingement terms are neglected in this formulation,
as well as contributions from the gradients of the mean temperature on the edges of the
film.
Ts
2h
Tp
Tw
Figure 15.7.3: Assumption of a Bilinear Temperature Profile in the Film
Release 12.0 c ANSYS, Inc. January 29, 2009
15-57
Discrete Phase
Assuming that the temperature changes slowly for each particle in the film, the equation
for the change in temperature of a non vaporizing particle can be written as
κ
dTp
κ
mp Cp
= Ap − hf +
Tp + hTg + Tw
dt
h
h
(15.7-27)
As the particle trajectory is computed, ANSYS FLUENT integrates Equation 15.7-27 to
obtain the particle temperature at the next time value, yielding
Tp (t + ∆t) = αp + [Tp (t) − αp ]e−βp ∆t
(15.7-28)
where ∆t is the integration time step and αp and βp are given by
αp =
hf Tg + κh Tw
hf + κh
(15.7-29)
βp =
Ap (hf + κh )
mp Cp
(15.7-30)
and
When the particle changes its mass during vaporization, an additional term is added to
Equation 15.7-27 to account for the enthalpy of vaporization, which is given by
dTp
κ
κ
mp Cp
= Ap − hf +
Tp + hTg + Tw + ṁp hf g
dt
h
h
(15.7-31)
where hf g is the latent heat of vaporization (with units of J/kg) and the expression ṁp
is the rate of evaporation in kg/s. This alters the expression for αp in Equation 15.7-29
so that
hf Tg + κh Tw + ṁp hf g /Ap
αp =
(15.7-32)
hf + κh
When the wall-film model is active, the heat flux from the wall to the liquid film is
subtracted from the heat flux from the wall to the gas phase. Additionally, enthalpy
from vaporization of the liquid from the wall is subtracted from the cell to which the
vapor mass goes. Since film boiling is modeled by limiting the liquid phase temperature
to the boiling point of the material, energy in excess of that absorbed by the liquid will
be put into the gas phase. When the thermal boundary conditions on the wall are set
to a constant heat flux, the local temperature of the wall face is used as the thermal
boundary condition for the wall-film particles.
i
15-58
The wall-film model has been specifically implemented for in-cylinder flows
and should be used with caution for other applications.
Release 12.0 c ANSYS, Inc. January 29, 2009
15.8 Particle Erosion and Accretion Theory
15.8
Particle Erosion and Accretion Theory
Particle erosion and accretion rates can be monitored at wall boundaries. The erosion
rate is defined as
Nparticles
Rerosion =
X
p=1
ṁp C(dp )f (α)v b(v)
Aface
(15.8-1)
where C(dp ) is a function of particle diameter, α is the impact angle of the particle path
with the wall face, f (α) is a function of impact angle, v is the relative particle velocity,
b(v) is a function of relative particle velocity, and Aface is the area of the cell face at the
wall. Default values are C = 1.8 × 10−9 , f = 1, and b = 0.
Since C, f , and b are defined as boundary conditions at a wall, rather than properties
of a material, the default values are not updated to reflect the material being used. You
will need to specify appropriate values at all walls. Values of these functions for sand
eroding both carbon steel and aluminum are given by Edwards et al. [86].
The erosion rate as calculated above is displayed in units of removed material/(areatime), i.e., mass flux, and can therefore be changed accordingly to the defined units in
ANSYS FLUENT. The functions C and f have to be specified in consistent units to build
a dimensionless group with the relative particle velocity and its exponent. To compute
an erosion rate in terms of length/time (mm/year, for example) you can either define a
custom field function to divide the erosion rate by the density of the wall material or
include this division in the units for C and/or f . Note that the units given by ANSYS
FLUENT when displaying the erosion rate are no longer valid in the latter case.
A variety of erosion models [97, 221, 85, 249, 126, 299] containing model constants [126,
85] and angle functions can be easily implemented into ANSYS FLUENT. The equations
describing some of the erosion models can be modified to appear in the form of the
general equation describing the erosion rate, Equation 15.8-1. For example, the Tulsa
Angle Dependent Model [85] described by Equation 15.8-2
ER = 1559B −0.59 Fs v 1.73 f (α)
(15.8-2)
can be rewritten in the form of Equation 15.8-1 with the following substitutions:
v 1.73
1559B −0.59 Fs
= v b(v)
= C(dp )
where ER is the erosion rate, B is the Brinell hardness, and Fs is a particle shape
coefficient.
Release 12.0 c ANSYS, Inc. January 29, 2009
15-59
Discrete Phase
User-defined functions can be used to describe erosion models of any form. For more
complex models, such as those models with varying function angles, f (α), the default
Erosion Model in the Wall boundary condition dialog box cannot be used. Hence, a userdefined function should be used instead. For information on how to apply user-defined
functions for DPM erosion models, see Section 2.5.4: DEFINE DPM EROSION in the separate
UDF Manual, or contact your support engineer for further assistance.
Note that the particle erosion and accretion rates can be displayed only when coupled
calculations are enabled.
The accretion rate is defined as
Nparticles
Raccretion =
X
p=1
15.9
ṁp
Aface
(15.8-3)
Atomizer Model Theory
In addition to the simple injection types described in Section 23.3.1: Injection Types in
the separate User’s Guide, ANSYS FLUENT also provides more complex injection types
for sprays describing primary breakup phenomena. For most types of injections, you will
need to provide the initial diameter, position, and velocity of the particles. For sprays,
however, there are models available to predict the droplet size and velocity distributions.
All of the atomization models use physical atomizer parameters, such as orifice diameter
and mass flow rate, to calculate initial droplet size, velocity, and position.
For realistic atomizer simulations, the droplets must be randomly distributed, both spatially through a dispersion angle and in their time of release. For other types of injections
in ANSYS FLUENT (nonatomizer), all of the droplets are released along fixed trajectories
at the beginning of the time step. The atomizer models use stochastic trajectory selection and staggering to attain a random distribution. Further information on staggering
can be found in section Section 23.2.8: Staggering of Particles in Space and Time in the
separate User’s Guide.
Stochastic trajectory selection is the random dispersion of initial droplet directions. All
of the atomizer models provide an initial dispersion angle, and the stochastic trajectory
selection picks an initial direction within this angle. This approach improves the accuracy
of the results for spray-dominated flows. The droplets will be more evenly spread among
the computational cells near the atomizer, which improves the coupling to the gas phase
by spreading drag more smoothly over the cells near the injection. Source terms in
the energy and species conservation equations are also more evenly distributed among
neighboring cells, improving solution convergence.
15-60
Release 12.0 c ANSYS, Inc. January 29, 2009
15.9 Atomizer Model Theory
Five atomizer models are available in ANSYS FLUENT to predict the spray characteristics
from knowledge of global parameters such as nozzle type and liquid flow rate. You can
choose them as injection types and define the associated parameters in the Set Injection
Properties dialog box, as described in Section 23.3.1: Injection Types in the separate
User’s Guide. Details about the atomizer models are provided below.
Information is organized into the following subsections:
• Section 15.9.1: The Plain-Orifice Atomizer Model
• Section 15.9.2: The Pressure-Swirl Atomizer Model
• Section 15.9.3: The Air-Blast/Air-Assist Atomizer Model
• Section 15.9.4: The Flat-Fan Atomizer Model
• Section 15.9.5: The Effervescent Atomizer Model
15.9.1
The Plain-Orifice Atomizer Model
The plain-orifice is the most common type of atomizer and the most simply made. However there is nothing simple about the physics of the internal nozzle flow and the external
atomization. In the plain-orifice atomizer model in ANSYS FLUENT, the liquid is accelerated through a nozzle, forms a liquid jet and then breaks up to form droplets. This
apparently simple process is dauntingly complex. The plain orifice may operate in three
different regimes: single-phase, cavitating and flipped [330]. The transition between
regimes is abrupt, producing dramatically different sprays. The internal regime determines the velocity at the orifice exit, as well as the initial droplet size and the angle of
droplet dispersion. Diagrams of each case are shown in Figures 15.9.1, 15.9.2, and 15.9.3.
Release 12.0 c ANSYS, Inc. January 29, 2009
15-61
Discrete Phase
r
p
p
d
1
liquid jet
orifice walls
2
downstream
gas
L
Figure 15.9.1: Single-Phase Nozzle Flow (Liquid Completely Fills the Orifice)
vapor
liquid jet
vapor
orifice walls
downstream
gas
Figure 15.9.2: Cavitating Nozzle Flow (Vapor Pockets Form Just After the
Inlet Corners)
liquid jet
orifice walls
downstream
gas
Figure 15.9.3: Flipped Nozzle Flow (Downstream Gas Surrounds the Liquid
Jet Inside the Nozzle)
15-62
Release 12.0 c ANSYS, Inc. January 29, 2009
15.9 Atomizer Model Theory
Internal Nozzle State
To accurately predict the spray characteristics, the plain-orifice model in ANSYS FLUENT
must identify the correct state of the internal nozzle flow because the nozzle state has
a tremendous effect on the external spray. Unfortunately, there is no established theory
for determining the nozzle state. One must rely on empirical models obtained from
experimental data. ANSYS FLUENT uses several dimensionless parameters to determine
the internal flow regime for the plain-orifice atomizer model. These parameters and the
decision-making process are summarized below.
A list of the parameters that control internal nozzle flow is given in Table 15.9.1. These
parameters may be combined to form nondimensional characteristic lengths such as r/d
and L/d, as well as nondimensional groups like the Reynolds number based on hydraulic
“head” (Reh ) and the cavitation parameter (K).
Table 15.9.1: List of Governing Parameters for Internal Nozzle Flow
nozzle diameter
nozzle length
radius of curvature of the inlet corner
upstream pressure
downstream pressure
viscosity
liquid density
vapor pressure
dρl
Reh =
µ
K=
s
2(p1 − p2 )
ρl
p1 − pv
p1 − p2
d
L
r
p1
p2
µ
ρl
pv
(15.9-1)
(15.9-2)
The liquid flow often contracts in the nozzle, as can be seen in Figures 15.9.2 and 15.9.3.
Nurick [252] found it helpful to use a coefficient of contraction (Cc ) to represent the
reduction in the cross-sectional area of the liquid jet. The coefficient of contraction is
defined as the area of the stream of contracting liquid over the total cross-sectional area
of the nozzle. ANSYS FLUENT uses Nurick’s fit for the coefficient of contraction:
Cc = q
Release 12.0 c ANSYS, Inc. January 29, 2009
1
2
Cct
1
−
11.4r
d
(15.9-3)
15-63
Discrete Phase
Here, Cct is a theoretical constant equal to 0.611, which comes from potential flow analysis
of flipped nozzles.
Coefficient of Discharge
Another important parameter for describing the performance of nozzles is the coefficient
of discharge (Cd ). The coefficient of discharge is the ratio of the mass flow rate through
the nozzle to the theoretical maximum mass flow rate:
Cd =
ṁeff
(15.9-4)
q
A 2ρl (p1 − p2 )
where ṁeff is the effective mass flow rate of the nozzle, defined by
ṁeff =
2π ṁ
∆φ
(15.9-5)
Here, ṁ is the mass flow rate specified in the user interface, and ∆φ is the difference
between the azimuthal stop angle and the azimuthal start angle
∆φ = φstop − φstart
(15.9-6)
as input by you (see Section 23.3.7: Point Properties for Plain-Orifice Atomizer Injections
in the separate User’s Guide). Note that the mass flow rate that you input should be
for the appropriate start and stop angles, in other words the correct mass flow rate for
the sector being modeled. Note also that for ∆φ of 2π, the effective mass flow rate is
identical to the mass flow rate in the interface.
The cavitation number (K in Equation 15.9-2) is an essential parameter for predicting
the inception of cavitation. The inception of cavitation is known to occur at a value
of Kincep ≈ 1.9 for short, sharp-edged nozzles. However, to include the effects of inlet
rounding and viscosity, an empirical relationship is used:
r
= 1.9 1 −
d
Kincep
2
−
1000
Reh
(15.9-7)
Similarly, a critical value of K where flip occurs is given by
Kcrit = 1 +
1
1+
L
4d
1+
2000
Reh
e70r/d
(15.9-8)
If r/d is greater than 0.05, then flip is deemed impossible and Kcrit is set to 1.0.
15-64
Release 12.0 c ANSYS, Inc. January 29, 2009
15.9 Atomizer Model Theory
The cavitation number, K, is compared to the values of Kincep and Kcrit to identify the
nozzle state. The decision tree is shown in Figure 15.9.4. Depending on the state of the
nozzle, a unique closure is chosen for the above equations.
For a single-phase nozzle (K > Kincep , K ≥ Kcrit ) [193], the coefficient of discharge is
given by
Cd =
1
1
Cdu
(15.9-9)
+ 20 (1+2.25L/d)
Reh
where Cdu is the ultimate discharge coefficient, and is defined as
Cdu = 0.827 − 0.0085
L
d
(15.9-10)
For a cavitating nozzle (Kcrit ≤ K ≤ Kincep ) [252] the coefficient of discharge is determined from
√
Cd = Cc K
(15.9-11)
For a flipped nozzle (K < Kcrit ) [252],
Cd = Cct = 0.611
K ≤ Kincep
K < Kcrit
flipped
(15.9-12)
K > K incep
K ≥ K crit
K < Kcrit
K ≥ Kcrit
cavitating
flipped
single phase
Figure 15.9.4: Decision Tree for the State of the Cavitating Nozzle
All of the nozzle flow equations are solved iteratively, along with the appropriate relationship for coefficient of discharge as given by the nozzle state. The nozzle state may change
as the upstream or downstream pressures change. Once the nozzle state is determined,
the exit velocity is calculated, and appropriate correlations for spray angle and initial
droplet size distribution are determined.
Release 12.0 c ANSYS, Inc. January 29, 2009
15-65
Discrete Phase
Exit Velocity
For a single-phase nozzle, the estimate of exit velocity (u) comes from the conservation
of mass and the assumption of a uniform exit velocity:
u=
ṁeff
ρl A
(15.9-13)
For the cavitating nozzle, Schmidt and Corradini [306] have shown that the uniform exit
velocity is not accurate. Instead, they derived an expression for a higher velocity over a
reduced area:
u=
2Cc p1 − p2 + (1 − 2Cc )pv
(15.9-14)
q
Cc 2ρl (p1 − pv )
This analytical relation is used for cavitating nozzles in ANSYS FLUENT. For the case of
flipped nozzles, the exit velocity is found from the conservation of mass and the value of
the reduced flow area:
u=
ṁeff
ρl Cct A
(15.9-15)
Spray Angle
The correlation for the spray angle (θ) comes from the work of Ranz [283]:
h q
ρg
−1 4π
tan
CA
ρl
θ
=
2
0.01
√
3
6
i
single phase, cavitating
(15.9-16)
flipped
The spray angle for both single-phase and cavitating nozzles depends on the ratio of the
gas and liquid densities and also the parameter CA . For flipped nozzles, the spray angle
has a constant value.
The parameter CA , which you must specify, is thought to be a constant for a given nozzle
geometry. The larger the value, the narrower the spray. Reitz [288] suggests the following
correlation for CA :
CA = 3 +
15-66
L
3.6d
(15.9-17)
Release 12.0 c ANSYS, Inc. January 29, 2009
15.9 Atomizer Model Theory
The spray angle is sensitive to the internal flow regime of the nozzle. Hence, you may
wish to choose smaller values of CA for cavitating nozzles than for single-phase nozzles.
Typical values range from 4.0 to 6.0. The spray angle for flipped nozzles is a small,
arbitrary value that represents the lack of any turbulence or initial disturbance from the
nozzle.
Droplet Diameter Distribution
One of the basic characteristics of an injection is the distribution of drop size. For an
atomizer, the droplet diameter distribution is closely related to the nozzle state. ANSYS
FLUENT’s spray models use a two-parameter Rosin-Rammler distribution, characterized
by the most probable droplet size and a spread parameter. The most probable droplet
size, d0 is obtained in ANSYS FLUENT from the Sauter mean diameter, d32 [186]. For
more information about the Rosin-Rammler size distribution, see Section 23.3.13: Using
the Rosin-Rammler Diameter Distribution Method in the separate User’s Guide.
For single-phase nozzle flows, the correlation of Wu et al. [383] is used to calculate d32
and relate the initial drop size to the estimated turbulence quantities of the liquid jet:
d32 = 133.0λWe−0.74 ,
(15.9-18)
where λ = d/8, λ is the radial integral length scale at the jet exit based upon fullydeveloped turbulent pipe flow, and We is the Weber number, defined as
We ≡
ρl u 2 λ
.
σ
(15.9-19)
Here, σ is the droplet surface tension. For a more detailed discussion of droplet surface
tension and the Weber number, see Section 15.10: Secondary Breakup Model Theory. For
more information about mean particle diameters, see Section 23.7.8: Summary Reporting
of Current Particles in the separate User’s Guide.
For cavitating nozzles, ANSYS FLUENT uses a slight modification of Equation 15.9-18.
The initial jet diameter used in Wu’s correlation, d, is calculated from the effective area of
the cavitating orifice exit, and thus represents the effective diameter of the exiting liquid
jet, deff . For an explanation of effective area of cavitating nozzles, please see Schmidt
and Corradini [306].
The length scale for a cavitating nozzle is λ = deff /8, where
s
deff =
Release 12.0 c ANSYS, Inc. January 29, 2009
4ṁeff
.
πρl u
(15.9-20)
15-67
Discrete Phase
For the case of the flipped nozzle, the initial droplet diameter is set to the diameter of
the liquid jet:
q
d0 = d Cct
(15.9-21)
where d0 is defined as the most probable diameter.
The second parameter required to specify the droplet size distribution is the spread
parameter, s. The values for the spread parameter are chosen from past modeling experience and from a review of experimental observations. Table 15.9.2 lists the values of s
for the three nozzle states. The larger the value of the spread parameter, the narrower
the droplet size distribution.
Table 15.9.2: Values of Spread Parameter for Different Nozzle States
State
single phase
cavitating
flipped
Spread Parameter
3.5
1.5
∞
Since the correlations of Wu et al. provide the Sauter mean diameter, d32 , these are
converted to the most probable diameter, d0 . Lefebvre [186] gives the most general
relationship between the Sauter mean diameter and most probable diameter for a RosinRammler distribution. The simplified version for s=3.5 is as follows:
d0 = 1.2726d32
1
1−
s
1/s
(15.9-22)
At this point, the droplet size, velocity, and spray angle have been determined and the
initialization of the injections is complete.
15-68
Release 12.0 c ANSYS, Inc. January 29, 2009
15.9 Atomizer Model Theory
15.9.2
The Pressure-Swirl Atomizer Model
Another important type of atomizer is the pressure-swirl atomizer, sometimes referred to
by the gas-turbine community as a simplex atomizer. This type of atomizer accelerates
the liquid through nozzles known as swirl ports into a central swirl chamber. The swirling
liquid pushes against the walls of the swirl chamber and develops a hollow air core. It
then emerges from the orifice as a thinning sheet, which is unstable, breaking up into
ligaments and droplets. The pressure-swirl atomizer is very widely used for liquid-fuel
combustion in gas turbines, oil furnaces, and direct-injection spark-ignited automobile
engines. The transition from internal injector flow to fully-developed spray can be divided
into three steps: film formation, sheet breakup, and atomization. A sketch of how this
process is thought to occur is shown in Figure 15.9.5.
half angle
dispersion
angle
Figure 15.9.5: Theoretical Progression from the Internal Atomizer Flow to
the External Spray
The interaction between the air and the sheet is not well understood. It is generally accepted that an aerodynamic instability causes the sheet to break up. The mathematical
analysis below assumes that Kelvin-Helmholtz waves grow on the sheet and eventually
break the liquid into ligaments. It is then assumed that the ligaments break up into
droplets due to varicose instability. Once the liquid droplets are formed, the spray evolution is determined by drag, collision, coalescence, and secondary breakup.
Release 12.0 c ANSYS, Inc. January 29, 2009
15-69
Discrete Phase
The pressure-swirl atomizer model used in ANSYS FLUENT is called the Linearized Instability Sheet Atomization (LISA) model of Schmidt et al. [308]. The LISA model is
divided into two stages:
1. film formation
2. sheet breakup and atomization
Both parts of the model are described below.
Film Formation
The centrifugal motion of the liquid within the injector creates an air core surrounded
by a liquid film. The thickness of this film, t, is related to the mass flow rate by
ṁeff = πρut(dinj − t)
(15.9-23)
where dinj is the injector exit diameter, and ṁeff is the effective mass flow rate, which
is defined by Equation 15.9-5 . The other unknown in Equation 15.9-23 is u, the axial
component of velocity at the injector exit. This quantity depends on internal details
of the injector and is difficult to calculate from first principles. Instead, the approach
of Han et al. [122] is used. The total velocity is assumed to be related to the injector
pressure by
s
U = kv
2∆p
ρl
(15.9-24)
where kv is the velocity coefficient. Lefebvre [186] has noted that kv is a function of the
injector design and injection pressure. If the swirl ports are treated as nozzles and if it is
assumed that the dominant portion of the pressure drop occurs at those ports, kv is the
expression for the discharge coefficient (Cd ). For single-phase nozzles with sharp inlet
corners and L/d ratios of 4, a typical Cd value is 0.78 or less [193]. If the nozzles are
cavitating, the value of Cd may be as low as 0.61. Hence, 0.78 should be a practical upper
bound for kv . Reducing kv by 10% to 0.7 approximates the effect of other momentum
losses on the discharge coefficient.
Physical limits on kv require that it be less than unity from conservation of energy, yet
be large enough to permit sufficient mass flow. To guarantee that the size of the air core
is non-negative, the following expression is used for kv :
"
4ṁeff
kv = max 0.7, 2
d0 ρl cos θ
15-70
s
ρl
2∆p
#
(15.9-25)
Release 12.0 c ANSYS, Inc. January 29, 2009
15.9 Atomizer Model Theory
Assuming that ∆p is known, Equation 15.9-24 can be used to find U . Once U is determined, u is found from
u = U cos θ
(15.9-26)
where θ is the spray angle, which is assumed to be known. At this point, the thickness
and axial component of the liquid film are known at the injector exit. The tangential
component of velocity (w = U sin θ) is assumed to be equal to the radial velocity component of the liquid sheet downstream of the nozzle exit. The axial component of velocity
is assumed to remain constant.
Sheet Breakup and Atomization
The pressure-swirl atomizer model includes the effects of the surrounding gas, liquid
viscosity, and surface tension on the breakup of the liquid sheet. Details of the theoretical
development of the model are given in Senecal et al. [310] and are only briefly presented
here. For a more robust implementation, the gas-phase velocity is neglected in calculating
the relative liquid-gas velocity and is instead set by you. This avoids having the injector
parameters depend too heavily on the usually under-resolved gas-phase velocity field very
near the injection location.
The model assumes that a two-dimensional, viscous, incompressible liquid sheet of thickness 2h moves with velocity U through a quiescent, inviscid, incompressible gas medium.
The liquid and gas have densities of ρl and ρg , respectively, and the viscosity of the
liquid is µl . A coordinate system is used that moves with the sheet, and a spectrum of
infinitesimal wavy disturbances of the form
η = η0 eikx+ωt
(15.9-27)
is imposed on the initially steady motion. The spectrum of disturbances results in fluctuating velocities and pressures for both the liquid and the gas. In Equation 15.9-27, η0
is the initial wave amplitude, k = 2π/λ is the wave number, and ω = ωr + iωi is the
complex growth rate. The most unstable disturbance has the largest value of ωr , denoted
here by Ω, and is assumed to be responsible for sheet breakup. Thus, it is desired to
obtain a dispersion relation ω = ω(k) from which the most unstable disturbance can be
calculated as a function of wave number.
Squire [335], Li and Tankin [192], and Hagerty and Shea [118] have shown that two
solutions, or modes, exist that satisfy the governing equations subject to the boundary
conditions at the upper and lower interfaces. The first solution, called the sinuous mode,
has waves at the upper and lower interfaces in phase. The second solution is called the
varicose mode which has the waves at the upper and lower interfaces π radians out of
phase. It has been shown by numerous authors (e.g., Senecal et. al. [310]) that the
Release 12.0 c ANSYS, Inc. January 29, 2009
15-71
Discrete Phase
sinuous mode dominates the growth of varicose waves for low velocities and low gas-toliquid density ratios. In addition, it can be shown that the sinuous and varicose modes
become indistinguishable for high-velocity flows. As a result, the atomization model in
ANSYS FLUENT is based upon the growth of sinuous waves on the liquid sheet.
As derived in Senecal et al. [310], the dispersion relation for the sinuous mode is given
by
ω 2 [tanh(kh) + Q] + [4νl k 2 tanh(kh) + 2iQkU ] +
4νl k 4 tanh(kh) − 4νl2 k 3 ` tanh(`h) − QU 2 k 2 +
σk 3
=0
ρl
(15.9-28)
where Q = ρg /ρl and `2 = k 2 + ω/νl .
Above a critical Weber number of Weg = 27/16 (based on the liquid velocity, gas density,
and sheet half-thickness), the fastest-growing waves are short. For Weg < 27/16, the
wavelengths are long compared to the sheet thickness. The speed of modern high pressure
fuel injection systems is high enough to ensure that the film Weber number is well above
this critical limit.
An order-of-magnitude analysis using typical values shows that the terms of second order
in viscosity can be neglected in comparison to the other terms in Equation 15.9-28. Using
this assumption, Equation 15.9-28 reduces to
ωr =
1
−2νl k 2 tanh(kh) +
tanh(kh) + Q
v
"
#
u
3
u
t4ν 2 k 4 tanh2 (kh) − Q2 U 2 k 2 − [tanh(kh) + Q] −QU 2 k 2 + σk
l
ρl
(15.9-29)
For waves that are long compared with the sheet thickness, a mechanism of sheet disintegration proposed by Dombrowski and Johns [74] is adopted. For long waves, ligaments
are assumed to form from the sheet breakup process once the unstable waves reach a
critical amplitude. If the surface disturbance has reached a value of ηb at breakup, a
breakup time, τ , can be evaluated:
ηb = η0 eΩτ
1
ηb
⇒ ln
Ω
η0
!
(15.9-30)
where Ω, the maximum growth rate, is found by numerically maximizing Equation 15.9-29
as a function of k. The maximum is found using a binary search that checks the sign of
the derivative. The sheet breaks up and ligaments will be formed at a length given by
15-72
Release 12.0 c ANSYS, Inc. January 29, 2009
15.9 Atomizer Model Theory
ηb
U
Lb = U τ = ln
Ω
η0
!
(15.9-31)
where the quantity ln( ηη0b ) is an empirical sheet constant that you must specify. The
default value of 12 was obtained theoretically by Weber [369] for liquid jets. Dombrowski
and Hooper [73] showed that a value of 12 for the sheet constant agreed favorably with
experimental sheet breakup lengths over a range of Weber numbers from 2 to 200.
The diameter of the ligaments formed at the point of breakup can be obtained from a
mass balance. If it is assumed that the ligaments are formed from tears in the sheet twice
per wavelength, the resulting diameter is given by
s
dL =
8h
Ks
(15.9-32)
where Ks is the wave number corresponding to the maximum growth rate, Ω. The
ligament diameter depends on the sheet thickness, which is a function of the breakup
length. The film thickness is calculated from the breakup length and the radial distance
from the center line to the mid-line of the sheet at the atomizer exit, r0 :
hend =
r0 h0
r0 + Lb sin
θ
2
(15.9-33)
This mechanism is not used for waves that are short compared to the sheet thickness.
For short waves, the ligament diameter is assumed to be linearly proportional to the
wavelength that breaks up the sheet,
dL =
2πCL
Ks
(15.9-34)
where CL , or the ligament constant, is equal to 0.5 by default.
In either the long-wave or the short-wave case, the breakup from ligaments to droplets
is assumed to behave according to Weber’s [369] analysis for capillary instability.
d0 = 1.88dL (1 + 3Oh)1/6
(15.9-35)
Here, Oh is the Ohnesorge number which is a combination of the Reynolds number
and the Weber number (see Section 15.10.2: Jet Stability Analysis for more details about
Oh). Once d0 has been determined from Equation 15.9-35, it is assumed that this droplet
diameter is the most probable droplet size of a Rosin-Rammler distribution with a spread
parameter of 3.5 and a default dispersion angle of 6◦ (which can be modified in the
GUI). The choice of spread parameter and dispersion angle is based on past modeling
Release 12.0 c ANSYS, Inc. January 29, 2009
15-73
Discrete Phase
experience [307]. It is important to note that the spray cone angle must be specified by
you when using this model.
15.9.3
The Air-Blast/Air-Assist Atomizer Model
In order to accelerate the breakup of liquid sheets from an atomizer, an additional air
stream is often directed through the atomizer. The liquid is formed into a sheet by a nozzle, and air is then directed against the sheet to promote atomization. This technique is
called air-assisted atomization or air-blast atomization, depending on the quantity of air
and its velocity. The addition of the external air stream past the sheet produces smaller
droplets than without the air. Though the exact mechanism for this enhanced performance is not completely understood, it is thought that the assisting air may accelerate
the sheet instability. The air may also help disperse the droplets, preventing collisions
between them. Air-assisted atomization is used in many of the same applications as
pressure-swirl atomization, where especially fine atomization is required.
ANSYS FLUENT’s air-blast atomization model is a variation of the pressure-swirl model.
One important difference between them is that the sheet thickness is set directly in
the air-blast atomizer model. This input is necessary because of the variety of sheet
formation mechanisms used in air-blast atomizers. Hence the air-blast atomizer model
does not contain the sheet formation equations that were included in the pressure-swirl
atomizer model (Equations 15.9-23–15.9-26). You will also specify the maximum relative
velocity that is produced by the sheet and air. Though this quantity could be calculated,
specifying a value relieves you from the necessity of finely resolving the atomizer internal
flow. This feature is convenient for simulations in large domains, where the atomizer is
very small by comparison.
An additional difference is that the air-blast atomizer model assumes that the sheet
breakup is always due to short waves. This assumption is a consequence of the greater
sheet thickness commonly found in air-blast atomizers. Hence the ligament diameter is
assumed to be linearly proportional to the wavelength of the fastest-growing wave on the
sheet, and is calculated from Equation 15.9-34.
Other inputs are similar to the pressure-swirl model – you must provide the mass flow rate
and spray angle. The angle in the case of the air-blast atomizer is the initial trajectory of
the film as it leaves the end of the orifice. The value of the angle is negative if the initial
film trajectory is inward, towards the centerline. Specification of the inner and outer
diameters of the film at the atomizer exit are also required, in addition to the dispersion
angle whose default value is 6◦ (which can be modified in the GUI).
Since the air-blast atomizer model does not include internal gas flows, you must create the
air streams surrounding the injector as boundary conditions within the ANSYS FLUENT
simulation. These streams are ordinary continuous-phase flows and require no special
treatment.
15-74
Release 12.0 c ANSYS, Inc. January 29, 2009
15.9 Atomizer Model Theory
15.9.4
The Flat-Fan Atomizer Model
The flat-fan atomizer is very similar to the pressure-swirl atomizer, but it makes a flat
sheet and does not use swirl. The liquid emerges from a wide, thin orifice as a flat liquid
sheet that breaks up into droplets. The primary atomization process is thought to be
similar to the pressure-swirl atomizer. Some researchers believe that flat-fan atomization,
because of jet impingement, is very similar to the atomization of a flat sheet. The flat-fan
model could serve doubly for this application.
The flat-fan atomizer is available only for 3D models. An image of the three-dimensional
flat fan is shown in Figure 15.9.6. The model assumes that the fan originates from a
virtual origin. You need to provide the location of this origin, which is the intersection of
the lines that mark the sides of the fan as well as the location of the center point of the
arc from which the fan originates. ANSYS FLUENT will find the vector that points from
the origin to the center point in order to determine the direction of the injection. You
also need to provide the half-angle of the fan arc, the width of the orifice (in the normal
direction) and the mass flow rate of the liquid to use the flat-fan atomizer model.
dispersion
angle
half
angle
dispersion
angle
Figure 15.9.6: Flat Fan Viewed from Above and from the Side
Release 12.0 c ANSYS, Inc. January 29, 2009
15-75
Discrete Phase
The breakup of the flat fan is calculated very much like the breakup of the sheet in the
pressure-swirl atomizer. The sheet breaks up into ligaments which then form individual
droplets. The only difference is that for short waves, the flat fan sheet is assumed to form
ligaments at half-wavelength intervals. Hence the ligament diameter for short waves is
given by
s
dL =
16h
Ks
(15.9-36)
In this case, dL in Equation 15.9-36 is taken to be the most probable diameter, with a
Rosin-Rammler spread parameter of 3.5 and a default dispersion angle of 6◦ . This angle
can be set in the Set Injection Properties dialog box. In all other respects, the flat-fan
atomizer model is like the sheet breakup portion of the pressure-swirl atomizer.
15.9.5
The Effervescent Atomizer Model
Effervescent atomization is the injection of liquid infused with a super-heated (with
respect to downstream conditions) liquid or propellant. As the volatile liquid exits the
nozzle, it rapidly changes phase. This phase change quickly breaks up the stream into
small droplets with a wide dispersion angle. The model also applies to cases where a
very hot liquid is discharged.
Since the physics of effervescence is not well understood, the model must rely on rough
empirical fits. The photographs of Reitz and Bracco [288] provide some insights. These
photographs show a dense liquid core to the spray, surrounded by a wide shroud of smaller
droplets.
The initial velocity of the droplets is computed from conservation of mass, assuming the
exiting jet has a cross-sectional area that is Cct times the nozzle area, where Cct is a fixed
constant, equal to 0.611 as specified in Equations 15.9-3 and 15.9-12.
u=
ṁeff
ρl Cct A
(15.9-37)
The maximum droplet diameter is set to the effective diameter of the exiting jet:
q
dmax = d Cct
15-76
(15.9-38)
Release 12.0 c ANSYS, Inc. January 29, 2009
15.10 Secondary Breakup Model Theory
The droplet size is then sampled from a Rosin-Rammler distribution with a spread parameter of 4.0. (See Section 23.3.13: Using the Rosin-Rammler Diameter Distribution
Method in the separate User’s Guide for details on the Rosin-Rammler distribution.)
The most probable droplet size depends on the angle, θ, between the droplet’s stochastic
trajectory and the injection direction:
d0 = dmax e−(θ/Θs )
2
(15.9-39)
The dispersion angle multiplier, Θs , is computed from the quality, x, and the specified
value for the dispersion constant, Ceff :
ṁvapor
(ṁvapor + ṁliquid )
x
=
Ceff
x =
Θs
(15.9-40)
(15.9-41)
This technique creates a spray with large droplets in the central core and a shroud of
smaller surrounding droplets. The droplet temperature is initialized to 0.99 times the
saturation temperature, such that the temperature of the droplet is close to boiling. To
complete the model, the flashing vapor must also be included in the calculation. This
vapor is part of the continuous phase and not part of the discrete phase model. You
must create an inlet at the point of injection when you specify boundary conditions for
the continuous phase. When the effervescent atomizer model is selected, you will need to
specify the nozzle diameter, mass flow rate, mixture quality, saturation temperature of
the volatile substance, spray half-angle and dispersion constant in addition to specifying
the position and direction of the injector.
15.10
Secondary Breakup Model Theory
ANSYS FLUENT offers two droplet breakup models: the Taylor analogy breakup (TAB)
model and the wave model. The TAB model is recommended for low-Weber-number
injections and is well suited for low-speed sprays into a standard atmosphere. For Weber
numbers greater than 100, the wave model is more applicable. The wave model is popular
for use in high-speed fuel-injection applications. Details for each model are provided
below.
Release 12.0 c ANSYS, Inc. January 29, 2009
15-77
Discrete Phase
15.10.1
Taylor Analogy Breakup (TAB) Model
Introduction
The Taylor analogy breakup (TAB) model is a classic method for calculating droplet
breakup, which is applicable to many engineering sprays. This method is based upon
Taylor’s analogy [347] between an oscillating and distorting droplet and a spring mass
system. Table 15.10.1 illustrates the analogous components.
Table 15.10.1: Comparison of a Spring-Mass System to a Distorting Droplet
Spring-Mass System
restoring force of spring
external force
damping force
Distorting and Oscillating Droplet
surface tension forces
droplet drag force
droplet viscosity forces
The resulting TAB model equation set, which governs the oscillating and distorting
droplet, can be solved to determine the droplet oscillation and distortion at any given
time. As described in detail below, when the droplet oscillations grow to a critical value
the “parent” droplet will break up into a number of smaller “child” droplets. As a
droplet is distorted from a spherical shape, the drag coefficient changes. A drag model
that incorporates the distorting droplet effects is available in ANSYS FLUENT. See Section 15.3.5: Dynamic Drag Model Theory for details.
Use and Limitations
The TAB model is best for low-Weber-number sprays. Extremely high-Weber-number
sprays result in shattering of droplets, which is not described well by the spring-mass
analogy.
Droplet Distortion
The equation governing a damped, forced oscillator is [256]
F − kx − d
dx
d2 x
=m 2
dt
dt
(15.10-1)
where x is the displacement of the droplet equator from its spherical (undisturbed) position. The coefficients of this equation are taken from Taylor’s analogy:
F
ρg u 2
= CF
m
ρl r
15-78
(15.10-2)
Release 12.0 c ANSYS, Inc. January 29, 2009
15.10 Secondary Breakup Model Theory
k
σ
= Ck 3
m
ρl r
d
µl
= Cd 2
m
ρl r
(15.10-3)
(15.10-4)
where ρl and ρg are the discrete phase and continuous phase densities, u is the relative
velocity of the droplet, r is the undisturbed droplet radius, σ is the droplet surface
tension, and µl is the droplet viscosity. The dimensionless constants CF , Ck , and Cd will
be defined later.
The droplet is assumed to break up if the distortion grows to a critical ratio of the droplet
radius. This breakup requirement is given as
x > Cb r
(15.10-5)
Where Cb is a constant equal to 0.5, if breakup is assumed to occur when the distortion is
equal to half the droplet radius, i.e., oscillations at the north and south pole with this amplitude will meet at the droplet center. This implicitly assumes that the droplet is undergoing only one (fundamental) oscillation mode. Equation 15.10-1 is nondimensionalized
by setting y = x/(Cb r) and substituting the relationships in Equations 15.10-2–15.10-4:
d2 y
CF ρg u2 Ck σ
Cd µl dy
=
−
y−
2
2
3
dt
Cb ρl r
ρl r
ρl r2 dt
(15.10-6)
where breakup now occurs for y > 1. For under-damped droplets, the equation governing
y can easily be determined from Equation 15.10-6 if the relative velocity is assumed to
be constant:
"
−(t/td )
y(t) = Wec + e
1
(y0 − Wec ) cos(ωt) +
ω
!
#
dy0 y0 − Wec
+
sin(ωt)
dt
td
(15.10-7)
where
We =
Wec =
y0 =
dy0
=
dt
1
=
td
Release 12.0 c ANSYS, Inc. January 29, 2009
ρg u 2 r
σ
CF
We
Ck Cb
y(0)
dy
(0)
dt
Cd µl
2 ρl r 2
(15.10-8)
(15.10-9)
(15.10-10)
(15.10-11)
(15.10-12)
15-79
Discrete Phase
ω 2 = Ck
1
σ
− 2
3
ρl r
td
(15.10-13)
In Equation 15.10-7, u is the relative velocity between the droplet and the gas phase
and We is the droplet Weber number, a dimensionless parameter defined as the ratio
of aerodynamic forces to surface tension forces. The droplet oscillation frequency is
represented by ω. The default value of y0 is 0, based upon the work of Liu et al. [205].
The constants have been chosen to match experiments and theory [174]:
Ck = 8
Cd = 5
1
CF =
3
If Equation 15.10-7 is solved for all droplets, those with y > 1 are assumed to break up.
The size and velocity of the new child droplets must be determined.
Size of Child Droplets
The size of the child droplets is determined by equating the energy of the parent droplet
to the combined energy of the child droplets. The energy of the parent droplet is [256]
Eparent
π
dy
= 4πr2 σ + K ρl r5
5
dt
!2
+ ω2y2
(15.10-14)
where K is the ratio of the total energy in distortion and oscillation to the energy in the
fundamental mode, of the order ( 10
). The child droplets are assumed to be nondistorted
3
and nonoscillating. Thus, the energy of the child droplets can be shown to be
Echild
r
π
dy
= 4πr σ
+ ρl r 5
r32 6
dt
!2
2
(15.10-15)
where r32 is the Sauter mean radius of the droplet size distribution. r32 can be found
by equating the energy of the parent and child droplets (i.e., Equations 15.10-14 and
15.10-15), setting y = 1, and ω 2 = 8σ/ρl r3 :
r32 =
r
1+
8Ky 2
20
+
ρl r 3 (dy/dt)2
σ
6K−5
120
(15.10-16)
Once the size of the child droplets is determined, the number of child droplets can easily
be determined by mass conservation.
15-80
Release 12.0 c ANSYS, Inc. January 29, 2009
15.10 Secondary Breakup Model Theory
Velocity of Child Droplets
The TAB model allows for a velocity component normal to the parent droplet velocity
to be imposed upon the child droplets. When breakup occurs, the equator of the parent
droplet is traveling at a velocity of dx/dt = Cb r(dy/dt). Therefore, the child droplets
will have a velocity normal to the parent droplet velocity given by
vnormal = Cv Cb r
dy
dt
(15.10-17)
where Cv is a constant of order (1).
Droplet Breakup
To model droplet breakup, the TAB model first determines the amplitude for an undamped oscillation (td ≈ ∞) for each droplet at time step n using the following:
A=
v
u
u
t
(dy/dt)n
(y n − Wec )2 +
ω
!2
(15.10-18)
According to Equation 15.10-18, breakup is possible only if the following condition is
satisfied:
Wec + A > 1
(15.10-19)
This is the limiting case, as damping will only reduce the chance of breakup. If a
droplet fails the above criterion, breakup does not occur. The only additional calculations
required then, are to update y using a discretized form of Equation 15.10-7 and its
derivative, which are both based on work done by O’Rourke and Amsden [256]:
(
y
dy
dt
n+1
−(∆t/td )
= Wec + e
!n+1
=
"
dy
dt
!n
y n − Wec
+
sin(ωt)
td
(15.10-20)
#
)
Wec − y n+1
+
td
(
−(∆t/td )
ωe
1
(y − Wec ) cos(ωt) +
ω
n
1
ω
"
dy
dt
!n
y n − Wec
+
cos(ω∆t) − (y n − Wec ) sin(ω∆t)
td
Release 12.0 c ANSYS, Inc. January 29, 2009
#
)
(15.10-21)
15-81
Discrete Phase
All of the constants in these expressions are assumed to be constant throughout the time
step.
If the criterion of Equation 15.10-19 is met, then breakup is possible. The breakup
time, tbu , must be determined to see if breakup occurs within the time step ∆t. The
value of tbu is set to the time required for oscillations to grow sufficiently large that the
magnitude of the droplet distortion, y, is equal to unity. The breakup time is determined
under the assumption that the droplet oscillation is undamped for its first period. The
breakup time is therefore the smallest root greater than tn of an undamped version of
Equation 15.10-7:
Wec + A cos[ω(t − tn ) + φ] = 1
(15.10-22)
where
cos φ =
y n − Wec
A
(15.10-23)
(dy/dt)n
Aω
(15.10-24)
and
sin φ = −
If tbu > tn+1 , then breakup will not occur during the current time step, and y and
(dy/dt) are updated by Equations 15.10-20 and 15.10-21. The breakup calculation then
continues with the next droplet. Conversely, if tn < tbu < tn+1 , then breakup will occur
and the child droplet radii are determined by Equation 15.10-16. The number of child
droplets, N , is determined by mass conservation:
N n+1 = N n
rn
rn+1
3
(15.10-25)
It is assumed that the child droplets are neither distorted nor oscillating; i.e., y =
(dy/dt) = 0. The child droplets are represented by a number of child parcels which
are created from the original parcel. These child parcels are distributed equally along
the equator of the parent droplet in a plane normal to the parent relative velocity vector.
The diameter of each of the child parcels is sampled from a Rosin Rammler distribution
based on the Sauter mean radius (Equation 15.10-16) and a spread parameter of 3.5.
15-82
Release 12.0 c ANSYS, Inc. January 29, 2009
15.10 Secondary Breakup Model Theory
A velocity component normal to the relative velocity vector, with magnitude computed
by Equation 15.10-17, is imposed upon the child droplets. It is decomposed at the equator
into components pointing radially outward.
i
A large number of child parcels ensures a smooth distribution of particle
diameters and source terms which is needed when simulating, for example,
evaporating sprays.
15.10.2
Wave Breakup Model
Introduction
An alternative to the TAB model that is appropriate for high-Weber-number flows is the
wave breakup model of Reitz [287], which considers the breakup of the droplets to be
induced by the relative velocity between the gas and liquid phases. The model assumes
that the time of breakup and the resulting droplet size are related to the fastest-growing
Kelvin-Helmholtz instability, derived from the jet stability analysis described below. The
wavelength and growth rate of this instability are used to predict details of the newlyformed droplets.
Use and Limitations
The wave model is appropriate for high-speed injections, where the Kelvin-Helmholtz
instability is believed to dominate droplet breakup (We > 100). Because this breakup
model can increase the number of computational parcels, you may wish to inject a modest
number of droplets initially.
Jet Stability Analysis
The jet stability analysis described in detail by Reitz and Bracco [289] is presented briefly
here. The analysis considers the stability of a cylindrical, viscous, liquid jet of radius
a issuing from a circular orifice at a velocity v into a stagnant, incompressible, inviscid
gas of density ρ2 . The liquid has a density, ρ1 , and viscosity, µ1 , and a cylindrical
polar coordinate system is used which moves with the jet. An arbitrary infinitesimal
axisymmetric surface displacement of the form
η = η0 eikz+ωt
(15.10-26)
is imposed on the initially steady motion and it is thus desired to find the dispersion
relation ω = ω(k) which relates the real part of the growth rate, ω, to its wave number,
k = 2π/λ.
Release 12.0 c ANSYS, Inc. January 29, 2009
15-83
Discrete Phase
In order to determine the dispersion relation, the linearized equations for the hydrodynamics of the liquid are solved assuming wave solutions of the form
φ1 = C1 I0 (kr)eikz+ωt
ψ1 = C2 I1 (Lr)eikz+ωt
(15.10-27)
(15.10-28)
where φ1 and ψ1 are the velocity potential and stream function, respectively, C1 and
C2 are integration constants, I0 and I1 are modified Bessel functions of the first kind,
L2 = k 2 + ω/ν1 , and ν1 is the liquid kinematic viscosity [287]. The liquid pressure is
obtained from the inviscid part of the liquid equations. In addition, the inviscid gas
equations can be solved to obtain the fluctuating gas pressure at r = a:
− p21 = −ρ2 (U − iωk)2 kη
K0 (ka)
K1 (ka)
(15.10-29)
where K0 and K1 are modified Bessel functions of the second kind and u is the relative
velocity between the liquid and the gas. The linearized boundary conditions are
∂η
∂t
∂v1
= −
∂z
(15.10-30)
v1 =
∂u1
∂r
(15.10-31)
and
σ
∂2η
− p1 + 2µ1 − 2 η + a2 2
a
∂z
!
+ p2 = 0
(15.10-32)
which are mathematical statements of the liquid kinematic free surface condition, continuity of shear stress, and continuity of normal stress, respectively. Note that u1 is the
axial perturbation liquid velocity, v1 is the radial perturbation liquid velocity, and σ is
the surface tension. Also note that Equation 15.10-31 was obtained under the assumption
that v2 = 0.
15-84
Release 12.0 c ANSYS, Inc. January 29, 2009
15.10 Secondary Breakup Model Theory
As described by Reitz [287], Equations 15.10-30 and 15.10-31 can be used to eliminate
the integration constants C1 and C2 in Equations 15.10-27 and 15.10-28. Thus, when
the pressure and velocity solutions are substituted into Equation 15.10-32, the desired
dispersion relation is obtained:
I10 (ka)
2kL I1 (ka) I10 (La)
ω + 2ν1 k ω
−
=
I0 (ka) k 2 + L2 I0 (ka) I1 (La)
"
2
σk
L2 − a2
2 2
(1
−
k
a
)
ρ 1 a2
L 2 + a2
#
2
!
I1 (ka) ρ2
ω
+
U −i
I0 (ka) ρ1
k
2
L 2 − a2
L 2 + a2
!
I1 (ka) K0 (ka)
(15.10-33)
I0 (ka) K1 (ka)
As shown by Reitz [287], Equation 15.10-33 predicts that a maximum growth rate (or
most unstable wave) exists for a given set of flow conditions. Curve fits of numerical
solutions to Equation 15.10-33 were generated for the maximum growth rate, Ω, and the
corresponding wavelength, Λ, and are given by Reitz [287]:
Λ
(1 + 0.45Oh0.5 )(1 + 0.4Ta0.7 )
= 9.02
a
(1 + 0.87We21.67 )0.6
!
ρ1 a3
(0.34 + 0.38We1.5
2 )
Ω
=
σ
(1 + Oh)(1 + 1.4Ta0.6 )
(15.10-34)
(15.10-35)
√
√
where Oh = We1 /Re1 is the Ohnesorge number and Ta = Oh We2 is the Taylor
number. Furthermore, We1 = ρ1 U 2 a/σ and We2 = ρ2 U 2 a/σ are the liquid and gas
Weber numbers, respectively, and Re1 = U a/ν1 is the Reynolds number.
Droplet Breakup
In the wave model, breakup of droplet parcels is calculated by assuming that the radius
of the newly-formed droplets is proportional to the wavelength of the fastest-growing
unstable surface wave on the parent droplet. In other words,
r = B0 Λ
(15.10-36)
where B0 is a model constant set equal to 0.61 based on the work of Reitz [287]. Furthermore, the rate of change of droplet radius in the parent parcel is given by
da
(a − r)
=−
, r≤a
dt
τ
Release 12.0 c ANSYS, Inc. January 29, 2009
(15.10-37)
15-85
Discrete Phase
where the breakup time, τ , is given by
τ=
3.726B1 a
ΛΩ
(15.10-38)
and Λ and Ω are obtained from Equations 15.10-34 and 15.10-35, respectively. The
breakup time constant, B1 , is set to a value of 1.73 as recommended by Liu et al. [205].
Values of B1 can range between 1 and 60, depending on the injector characterization.
In the wave model, mass is accumulated from the parent drop at a rate given by Equation 15.10-38 until the shed mass is equal to 5% of the initial parcel mass. At this time, a
new parcel is created with a radius given by Equation 15.10-36. The new parcel is given
the same properties as the parent parcel (i.e., temperature, material, position, etc.) with
the exception of radius and velocity. The new parcel is given a component of velocity
randomly selected in the plane orthogonal to the direction vector of the parent parcel,
and the momentum of the parent parcel is adjusted so that momentum is conserved. The
velocity magnitude of the new parcel is the same as the parent parcel.
You must also specify the model constants which determine how the gas phase interacts
with the liquid droplets. For example, the breakup time constant B1 is the constant
multiplying the time scale which determines how quickly the parcel will loose mass.
Therefore, a larger number means that it takes longer for the particle to loose a given
amount. A larger number for B1 in the context of interaction with the gas phase would
mean that the interaction with the subgrid is less intense. B0 is the constant for the drop
size and is generally taken to be 0.61.
15.11
Droplet Collision and Coalescence Model Theory
15.11.1
Introduction
When your simulation includes tracking of droplets, ANSYS FLUENT provides an option
for estimating the number of droplet collisions and their outcomes in a computationally
efficient manner. The difficulty in any collision calculation is that for N droplets, each
droplet has N − 1 possible collision partners. Thus, the number of possible collision pairs
is approximately 12 N 2 . (The factor of 12 appears because droplet A colliding with droplet
B is identical to droplet B colliding with droplet A. This symmetry reduces the number
of possible collision events by half.)
An important consideration is that the collision algorithm must calculate 12 N 2 possible
collision events at every time step. Since a spray can consist of several million droplets,
the computational cost of a collision calculation from first principles is prohibitive. This
motivates the concept of parcels. Parcels are statistical representations of a number of
individual droplets. For example, if ANSYS FLUENT tracks a set of parcels, each of which
represents 1000 droplets, the cost of the collision calculation is reduced by a factor of
106 . Because the cost of the collision calculation still scales with the square of N , the
15-86
Release 12.0 c ANSYS, Inc. January 29, 2009
15.11 Droplet Collision and Coalescence Model Theory
reduction of cost is significant; however, the effort to calculate the possible intersection
of so many parcel trajectories would still be prohibitively expensive.
The algorithm of O’Rourke [255] efficiently reduces the computational cost of the spray
calculation. Rather than using geometry to see if parcel paths intersect, O’Rourke’s
method is a stochastic estimate of collisions. O’Rourke also makes the assumption that
two parcels may collide only if they are located in the same continuous-phase cell. These
two assumptions are valid only when the continuous-phase cell size is small compared
to the size of the spray. For these conditions, the method of O’Rourke is second-order
accurate at estimating the chance of collisions. The concept of parcels together with
the algorithm of O’Rourke makes the calculation of collision possible for practical spray
problems.
Once it is decided that two parcels of droplets collide, the algorithm further determines
the type of collision. Only coalescence and bouncing outcomes are considered. The
probability of each outcome is calculated from the collisional Weber number (W ec ) and
a fit to experimental observations. Here,
W ec =
2
D
ρUrel
σ
(15.11-1)
where Urel is the relative velocity between two parcels and D is the arithmetic mean
diameter of the two parcels. The state of the two colliding parcels is modified based on
the outcome of the collision.
15.11.2
Use and Limitations
The collision model assumes that the frequency of collisions is much less than the particle time step. If the particle time step is too large, then the results may be timestep-dependent. You should adjust the particle length scale accordingly. Additionally,
the model is most applicable for low-Weber-number collisions where collisions result in
bouncing and coalescence. Above a Weber number of about 100, the outcome of collision
could be shattering.
Sometimes the collision model can cause mesh-dependent artifacts to appear in the spray.
This is a result of the assumption that droplets can collide only within the same cell.
These tend to be visible when the source of injection is at a mesh vertex. The coalescence
of droplets tends to cause the spray to pull away from cell boundaries. In two dimensions,
a finer mesh and more computational droplets can be used to reduce these effects. In
three dimensions, best results are achieved when the spray is modeled using a polar mesh
with the spray at the center.
If the collision model is used in a transient simulation, multiple DPM iterations per time
step cannot be specified in the Number of Continuous Phase Iterations per DPM Iteration
field in the Discrete Phase Model dialog box. In such cases, only one DPM iteration
per time step will be calculated.
Release 12.0 c ANSYS, Inc. January 29, 2009
15-87
Discrete Phase
15.11.3
Theory
As noted above, O’Rourke’s algorithm assumes that two droplets may collide only if they
are in the same continuous-phase cell. This assumption can prevent droplets that are
quite close to each other, but not in the same cell, from colliding, although the effect of
this error is lessened by allowing some droplets that are farther apart to collide. The
overall accuracy of the scheme is second-order in space.
Probability of Collision
The probability of collision of two droplets is derived from the point of view of the larger
droplet, called the collector droplet and identified below with the number 1. The smaller
droplet is identified in the following derivation with the number 2. The calculation is in
the frame of reference of the larger droplet so that the velocity of the collector droplet is
zero. Only the relative distance between the collector and the smaller droplet is important
in this derivation. If the smaller droplet is on a collision course with the collector, the
centers will pass within a distance of r1 + r2 . More precisely, if the smaller droplet center
passes within a flat circle centered around the collector of area π(r1 + r2 )2 perpendicular
to the trajectory of the smaller droplet, a collision will take place. This disk can be used
to define the collision volume, which is the area of the aforementioned disk multiplied by
the distance traveled by the smaller droplet in one time step, namely π(r1 + r2 )2 vrel ∆t.
The algorithm of O’Rourke uses the concept of a collision volume to calculate the probability of collision. Rather than calculating whether or not the position of the smaller
droplet center is within the collision volume, the algorithm calculates the probability
of the smaller droplet being within the collision volume. It is known that the smaller
droplet is somewhere within the continuous-phase cell of volume V . If there is a uniform
probability of the droplet being anywhere within the cell, then the chance of the droplet
being within the collision volume is the ratio of the two volumes. Thus, the probability
of the collector colliding with the smaller droplet is
P1 =
π(r1 + r2 )2 vrel ∆t
V
(15.11-2)
Equation 15.11-2 can be generalized for parcels, where there are n1 and n2 droplets in
the collector and smaller droplet parcels, respectively. The collector undergoes a mean
expected number of collisions given by
n̄ =
15-88
n2 π(r1 + r2 )2 vrel ∆t
V
(15.11-3)
Release 12.0 c ANSYS, Inc. January 29, 2009
15.11 Droplet Collision and Coalescence Model Theory
The actual number of collisions that the collector experiences is not generally the mean
expected number of collisions. The probability distribution of the number of collisions
follows a Poisson distribution, according to O’Rourke, which is given by
P (n) = e−n̄
n̄n
n!
(15.11-4)
where n is the number of collisions between a collector and other droplets.
Collision Outcomes
Once it is determined that two parcels collide, the outcome of the collision must be
determined. In general, the outcome tends to be coalescence if the droplets collide headon, and bouncing if the collision is more oblique. In the reference frame being used here,
the probability of coalescence can be related to the offset of the collector droplet center
and the trajectory of the smaller droplet. The critical offset is a function of the collisional
Weber number and the relative radii of the collector and the smaller droplet.
The critical offset is calculated by O’Rourke using the expression
bcrit
v
!
u
u
2.4f
t
= (r1 + r2 ) min 1.0,
(15.11-5)
We
where f is a function of r1 /r2 , defined as
r1
f
r2
r1
=
r2
3
r1
− 2.4
r2
2
r1
+ 2.7
(15.11-6)
r2
√
The value of the actual collision parameter, b, is (r1 + r2 ) Y , where Y is a random
number between 0 and 1. The calculated value of b is compared to bcrit , and if b < bcrit ,
the result of the collision is coalescence. Equation 15.11-4 gives the number of smaller
droplets that coalesce with the collector. The properties of the coalesced droplets are
found from the basic conservation laws.
In the case of a grazing collision, the new velocities are calculated based on conservation
of momentum and kinetic energy. It is assumed that some fraction of the kinetic energy
of the droplets is lost to viscous dissipation and angular momentum generation. This
fraction is related to b, the collision offset parameter. Using assumed forms for the energy
loss, O’Rourke derived the following expression for the new velocity:
v10
m1 v1 + m2 v2 + m2 (v1 − v2 )
=
m1 + m2
Release 12.0 c ANSYS, Inc. January 29, 2009
b − bcrit
r1 + r2 − bcrit
!
(15.11-7)
15-89
Discrete Phase
This relation is used for each of the components of velocity. No other droplet properties
are altered in grazing collisions.
15.12
One-Way and Two-Way Coupling
You can use ANSYS FLUENT to predict the discrete phase patterns based on a fixed
continuous phase flow field (an uncoupled approach or “one-way coupling”), or you can
include the effect of the discrete phase on the continuum (a coupled approach or “two-way
coupling”). In the coupled approach, the continuous phase flow pattern is impacted by
the discrete phase (and vice versa), and you can alternate calculations of the continuous
phase and discrete phase equations until a converged coupled solution is achieved.
15.12.1
Coupling Between the Discrete and Continuous Phases
As the trajectory of a particle is computed, ANSYS FLUENT keeps track of the heat, mass,
and momentum gained or lost by the particle stream that follows that trajectory and these
quantities can be incorporated in the subsequent continuous phase calculations. Thus,
while the continuous phase always impacts the discrete phase, you can also incorporate
the effect of the discrete phase trajectories on the continuum. This two-way coupling
is accomplished by alternately solving the discrete and continuous phase equations until
the solutions in both phases have stopped changing. This interphase exchange of heat,
mass, and momentum from the particle to the continuous phase is depicted qualitatively
in Figure 15.12.1. Note that no interchange terms are computed for particles defined as
massless, where the discrete phase trajectories have no impact on the continuum.
typical
particle
trajectory
mass-exchange
heat-exchange
momentum-exchange
typical continuous
phase control volume
Figure 15.12.1: Heat, Mass, and Momentum Transfer Between the Discrete
and Continuous Phases
15-90
Release 12.0 c ANSYS, Inc. January 29, 2009
15.12 One-Way and Two-Way Coupling
15.12.2
Momentum Exchange
The momentum transfer from the continuous phase to the discrete phase is computed in
ANSYS FLUENT by examining the change in momentum of a particle as it passes through
each control volume in the ANSYS FLUENT model. This momentum change is computed
as
!
F =
X
18µCD Re
(up − u) + Fother ṁp ∆t
ρp d2p 24
(15.12-1)
where
µ
ρp
dp
Re
up
u
CD
ṁp
∆t
Fother
=
=
=
=
=
=
=
=
=
=
viscosity of the fluid
density of the particle
diameter of the particle
relative Reynolds number
velocity of the particle
velocity of the fluid
drag coefficient
mass flow rate of the particles
time step
other interaction forces
This momentum exchange appears as a momentum source in the continuous phase momentum balance in any subsequent calculations of the continuous phase flow field and
can be reported by ANSYS FLUENT as described in Section 23.7: Postprocessing for the
Discrete Phase in the separate User’s Guide.
15.12.3
Heat Exchange
The heat transfer from the continuous phase to the discrete phase is computed in ANSYS
FLUENT by examining the change in thermal energy of a particle as it passes through
each control volume in the ANSYS FLUENT model. In the absence of a chemical reaction
(i.e., for all particle laws except Law 5) the heat exchange is computed as
"
#
Z Tp
Z Tp
out
in
ṁp,0
Q=
(mp in − mp out )[−Hlatref + Hpyrol ] − mp out
cp p dT + mp in
cp p dT
mp,0
Tref
Tref
(15.12-2)
Release 12.0 c ANSYS, Inc. January 29, 2009
15-91
Discrete Phase
where
ṁp,0
mp,0
mp in
mp out
cp p
Hpyrol
Tp in
Tp out
Tref
Hlatref
=
=
=
=
=
=
=
=
=
=
initial mass flow rate of the particle injection (kg/s)
initial mass of the particle (kg)
mass of the particle on cell entry (kg)
mass of the particle on cell exit (kg)
heat capacity of the particle (J/kg-K)
heat of pyrolysis as volatiles are evolved (J/kg)
temperature of the particle on cell entry (K)
temperature of the particle on cell exit (K)
reference temperature for enthalpy (K)
latent heat at reference conditions (J/kg)
The latent heat at the reference conditions Hlatref for droplet particles is computed as
the difference of the liquid and gas standard formation enthalpies, and can be related to
the latent heat at the boiling point as follows:
Hlatref = Hlat −
Z
Tbp
Tref
cp g dT +
Z
Tbp
Tref
cp p dT
(15.12-3)
where
cp g
Tbp
Hlat
= heat capacity of gas product species (J/kg-K)
= boiling point temperature (K)
= latent heat at the boiling point temperature (J/kg)
For the volatile part of the combusting particles, some constraints are applied to ensure
that the enthalpy source terms do not depend on the particle history. The formulation
should be consistent with the mixing of two gas streams, one consisting of the fluid and
the other consisting of the volatiles. Hence Hlatref is derived by applying a correction to
Hlat , which accounts for different heat capacities in the particle and gaseous phase:
Hlatref = Hlat −
Z
Tp,init
Tref
cp g dT +
Z
Tp,init
Tref
cp p dT
(15.12-4)
where
Tp,init
15.12.4
= particle initial temperature (K)
Mass Exchange
The mass transfer from the discrete phase to the continuous phase is computed in ANSYS
FLUENT by examining the change in mass of a particle as it passes through each control
volume in the ANSYS FLUENT model. The mass change is computed simply as
M=
15-92
∆mp
ṁp,0
mp,0
(15.12-5)
Release 12.0 c ANSYS, Inc. January 29, 2009
15.12 One-Way and Two-Way Coupling
This mass exchange appears as a source of mass in the continuous phase continuity
equation and as a source of a chemical species defined by you. The mass sources are
included in any subsequent calculations of the continuous phase flow field and are reported
by ANSYS FLUENT as described in Section 23.7: Postprocessing for the Discrete Phase
in the separate User’s Guide.
15.12.5
Under-Relaxation of the Interphase Exchange Terms
Note that the interphase exchange of momentum, heat, and mass is under-relaxed during
the calculation, so that
Fnew = Fold + α(Fcalculated − Fold )
(15.12-6)
Qnew = Qold + α(Qcalculated − Qold )
(15.12-7)
Mnew = Mold + α(Mcalculated − Mold )
(15.12-8)
where α is the under-relaxation factor for particles/droplets. The default value for α is
0.5. This value may be reduced to improve the stability of coupled calculations. Note
that the value of α does not influence the predictions obtained in the final converged
solution.
Two options exist when updating the new particle source terms Fnew , Qnew and Mnew . The
first option is to compute the new source terms and the particle source terms, Fcalculated ,
Qcalculated and Mcalculated , at the same time. The second option is to update the new
source terms, Fnew , Qnew and Mnew , every flow iteration, while the particle source terms,
Fcalculated , Qcalculated and Mcalculated , are calculated every Discrete Phase Model iteration.
The latter option is recommended for transient flows, where the particles are updated
once per flow time step.
Figure 15.12.2 shows how the source term, S, when applied to the flow equations, changes
with the number of updates for varying under-relaxation factors. In Figure 15.12.2, S∞
is the final source term for which a value is reached after a certain number of updates and
S0 is the initial source term at the start of the computation. The value of S0 is typically
zero at the beginning of the calculation.
Figure 15.12.2 can be applied to this option as well. Keep in mind that the DPM source
terms are updated every continuous flow iteration.
Release 12.0 c ANSYS, Inc. January 29, 2009
15-93
Discrete Phase
Figure 15.12.2: Effect of Number of Source Term Updates on Source Term
Applied to Flow Equations
15-94
Release 12.0 c ANSYS, Inc. January 29, 2009
15.12 One-Way and Two-Way Coupling
15.12.6
Interphase Exchange During Stochastic Tracking
When stochastic tracking is performed, the interphase exchange terms, computed via
Equations 15.12-1 to 15.12-8, are computed for each stochastic trajectory with the particle
mass flow rate, ṁp0 , divided by the number of stochastic tracks computed. This implies
that an equal mass flow of particles follows each stochastic trajectory.
15.12.7
Interphase Exchange During Cloud Tracking
When the particle cloud model is used, the interphase exchange terms are computed via
Equations 15.12-1 to 15.12-8 based on ensemble-averaged flow properties in the particle
cloud. The exchange terms are then distributed to all the cells in the cloud based on the
weighting factor defined in Equation 15.2-49.
Release 12.0 c ANSYS, Inc. January 29, 2009
15-95
Discrete Phase
15-96
Release 12.0 c ANSYS, Inc. January 29, 2009
Chapter 16.
Multiphase Flows
This chapter discusses the general multiphase models that are available in ANSYS FLUENT. Section 16.1: Introduction provides a brief introduction to multiphase modeling,
Chapter 15: Discrete Phase discusses the Lagrangian dispersed phase model, and Chapter 17: Solidification and Melting describes ANSYS FLUENT’s model for solidification and
melting. For information about using the general multiphase models in ANSYS FLUENT,
see Chapter 24: Modeling Multiphase Flows in the separate User’s Guide. Information
about the various theories behind the multiphase models is presented in the following
sections:
• Section 16.1: Introduction
• Section 16.2: Choosing a General Multiphase Model
• Section 16.3: Volume of Fluid (VOF) Model Theory
• Section 16.4: Mixture Model Theory
• Section 16.5: Eulerian Model Theory
• Section 16.6: Wet Steam Model Theory
• Section 16.7: Modeling Mass Transfer in Multiphase Flows
• Section 16.8: Modeling Species Transport in Multiphase Flows
Release 12.0 c ANSYS, Inc. January 29, 2009
16-1
Multiphase Flows
16.1
Introduction
A large number of flows encountered in nature and technology are a mixture of phases.
Physical phases of matter are gas, liquid, and solid, but the concept of phase in a multiphase flow system is applied in a broader sense. In multiphase flow, a phase can be
defined as an identifiable class of material that has a particular inertial response to and
interaction with the flow and the potential field in which it is immersed. For example,
different-sized solid particles of the same material can be treated as different phases because each collection of particles with the same size will have a similar dynamical response
to the flow field.
Information is organized into the following subsections:
• Section 16.1.1: Multiphase Flow Regimes
• Section 16.1.2: Examples of Multiphase Systems
16.1.1
Multiphase Flow Regimes
Multiphase flow regimes can be grouped into four categories: gas-liquid or liquid-liquid
flows; gas-solid flows; liquid-solid flows; and three-phase flows.
Gas-Liquid or Liquid-Liquid Flows
The following regimes are gas-liquid or liquid-liquid flows:
• Bubbly flow: This is the flow of discrete gaseous or fluid bubbles in a continuous
fluid.
• Droplet flow: This is the flow of discrete fluid droplets in a continuous gas.
• Slug flow: This is the flow of large bubbles in a continuous fluid.
• Stratified/free-surface flow: This is the flow of immiscible fluids separated by a
clearly-defined interface.
See Figure 16.1.1 for illustrations of these regimes.
16-2
Release 12.0 c ANSYS, Inc. January 29, 2009
16.1 Introduction
Gas-Solid Flows
The following regimes are gas-solid flows:
• Particle-laden flow: This is flow of discrete particles in a continuous gas.
• Pneumatic transport: This is a flow pattern that depends on factors such as solid
loading, Reynolds numbers, and particle properties. Typical patterns are dune
flow, slug flow, and homogeneous flow.
• Fluidized bed: This consists of a vertical cylinder containing particles, into which
a gas is introduced through a distributor. The gas rising through the bed suspends
the particles. Depending on the gas flow rate, bubbles appear and rise through the
bed, intensifying the mixing within the bed.
See Figure 16.1.1 for illustrations of these regimes.
Liquid-Solid Flows
The following regimes are liquid-solid flows:
• Slurry flow: This flow is the transport of particles in liquids. The fundamental
behavior of liquid-solid flows varies with the properties of the solid particles relative
to those of the liquid. In slurry flows, the Stokes number (see Equation 16.2-4) is
normally less than 1. When the Stokes number is larger than 1, the characteristic
of the flow is liquid-solid fluidization.
• Hydrotransport: This describes densely-distributed solid particles in a continuous
liquid
• Sedimentation: This describes a tall column initially containing a uniform dispersed
mixture of particles. At the bottom, the particles will slow down and form a sludge
layer. At the top, a clear interface will appear, and in the middle a constant settling
zone will exist.
See Figure 16.1.1 for illustrations of these regimes.
Three-Phase Flows
Three-phase flows are combinations of the other flow regimes listed in the previous sections.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-3
Multiphase Flows
slug flow
stratified/free-surface flow
sedimentation
bubbly, droplet, or
particle-laden flow
pneumatic transport,
hydrotransport, or slurry flow
fluidized bed
Figure 16.1.1: Multiphase Flow Regimes
16-4
Release 12.0 c ANSYS, Inc. January 29, 2009
16.2 Choosing a General Multiphase Model
16.1.2
Examples of Multiphase Systems
Specific examples of each regime described in Section 16.1.1: Multiphase Flow Regimes
are listed below:
• Bubbly flow examples include absorbers, aeration, air lift pumps, cavitation, evaporators, flotation, and scrubbers.
• Droplet flow examples include absorbers, atomizers, combustors, cryogenic pumping, dryers, evaporation, gas cooling, and scrubbers.
• Slug flow examples include large bubble motion in pipes or tanks.
• Stratified/free-surface flow examples include sloshing in offshore separator devices
and boiling and condensation in nuclear reactors.
• Particle-laden flow examples include cyclone separators, air classifiers, dust collectors, and dust-laden environmental flows.
• Pneumatic transport examples include transport of cement, grains, and metal powders.
• Fluidized bed examples include fluidized bed reactors and circulating fluidized beds.
• Slurry flow examples include slurry transport and mineral processing
• Hydrotransport examples include mineral processing and biomedical and physiochemical fluid systems
• Sedimentation examples include mineral processing.
16.2
Choosing a General Multiphase Model
The first step in solving any multiphase problem is to determine which of the regimes
provides some broad guidelines for determining appropriate models for each regime, and
how to determine the degree of interphase coupling for flows involving bubbles, droplets,
or particles, and the appropriate model for different amounts of coupling.
Information is organized into the following subsections:
• Section 16.2.1: Approaches to Multiphase Modeling
• Section 16.2.2: Model Comparisons
• Section 16.2.3: Time Schemes in Multiphase Flow
• Section 16.2.4: Stability and Convergence
Release 12.0 c ANSYS, Inc. January 29, 2009
16-5
Multiphase Flows
16.2.1
Approaches to Multiphase Modeling
Advances in computational fluid mechanics have provided the basis for further insight
into the dynamics of multiphase flows. Currently there are two approaches for the numerical calculation of multiphase flows: the Euler-Lagrange approach (discussed in Section 15.1: Introduction) and the Euler-Euler approach (discussed in the following section).
The Euler-Euler Approach
In the Euler-Euler approach, the different phases are treated mathematically as interpenetrating continua. Since the volume of a phase cannot be occupied by the other
phases, the concept of phasic volume fraction is introduced. These volume fractions are
assumed to be continuous functions of space and time and their sum is equal to one.
Conservation equations for each phase are derived to obtain a set of equations, which
have similar structure for all phases. These equations are closed by providing constitutive
relations that are obtained from empirical information, or, in the case of granular flows,
by application of kinetic theory.
In ANSYS FLUENT, three different Euler-Euler multiphase models are available: the
volume of fluid (VOF) model, the mixture model, and the Eulerian model.
The VOF Model
The VOF model (described in Section 16.3: Volume of Fluid (VOF) Model Theory) is
a surface-tracking technique applied to a fixed Eulerian mesh. It is designed for two or
more immiscible fluids where the position of the interface between the fluids is of interest.
In the VOF model, a single set of momentum equations is shared by the fluids, and the
volume fraction of each of the fluids in each computational cell is tracked throughout the
domain. Applications of the VOF model include stratified flows, free-surface flows, filling,
sloshing, the motion of large bubbles in a liquid, the motion of liquid after a dam break,
the prediction of jet breakup (surface tension), and the steady or transient tracking of
any liquid-gas interface.
The Mixture Model
The mixture model (described in Section 16.4: Mixture Model Theory) is designed for two
or more phases (fluid or particulate). As in the Eulerian model, the phases are treated as
interpenetrating continua. The mixture model solves for the mixture momentum equation
and prescribes relative velocities to describe the dispersed phases. Applications of the
mixture model include particle-laden flows with low loading, bubbly flows, sedimentation,
and cyclone separators. The mixture model can also be used without relative velocities
for the dispersed phases to model homogeneous multiphase flow.
16-6
Release 12.0 c ANSYS, Inc. January 29, 2009
16.2 Choosing a General Multiphase Model
The Eulerian Model
The Eulerian model (described in Section 16.5: Eulerian Model Theory) is the most
complex of the multiphase models in ANSYS FLUENT. It solves a set of n momentum
and continuity equations for each phase. Coupling is achieved through the pressure and
interphase exchange coefficients. The manner in which this coupling is handled depends
upon the type of phases involved; granular (fluid-solid) flows are handled differently
than nongranular (fluid-fluid) flows. For granular flows, the properties are obtained from
application of kinetic theory. Momentum exchange between the phases is also dependent
upon the type of mixture being modeled. ANSYS FLUENT’s user-defined functions allow
you to customize the calculation of the momentum exchange. Applications of the Eulerian
multiphase model include bubble columns, risers, particle suspension, and fluidized beds.
16.2.2
Model Comparisons
In general, once you have determined the flow regime that best represents your multiphase
system, you can select the appropriate model based on the following guidelines:
• For bubbly, droplet, and particle-laden flows in which the phases mix and/or
dispersed-phase volume fractions exceed 10%, use either the mixture model (described in Section 16.4: Mixture Model Theory) or the Eulerian model (described
in Section 16.5: Eulerian Model Theory).
• For slug flows, use the VOF model. See Section 16.3: Volume of Fluid (VOF) Model
Theory for more information about the VOF model.
• For stratified/free-surface flows, use the VOF model. See Section 16.3: Volume of
Fluid (VOF) Model Theory for more information about the VOF model.
• For pneumatic transport, use the mixture model for homogeneous flow (described
in Section 16.4: Mixture Model Theory) or the Eulerian model for granular flow
(described in Section 16.5: Eulerian Model Theory).
• For fluidized beds, use the Eulerian model for granular flow. See Section 16.5: Eulerian Model Theory for more information about the Eulerian model.
• For slurry flows and hydrotransport, use the mixture or Eulerian model (described,
respectively, in Sections 16.4 and 16.5).
• For sedimentation, use the Eulerian model. See Section 16.5: Eulerian Model
Theory for more information about the Eulerian model.
• For general, complex multiphase flows that involve multiple flow regimes, select
the aspect of the flow that is of most interest, and choose the model that is most
appropriate for that aspect of the flow. Note that the accuracy of results will not
be as good as for flows that involve just one flow regime, since the model you use
will be valid for only part of the flow you are modeling.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-7
Multiphase Flows
As discussed in this section, the VOF model is appropriate for stratified or free-surface
flows, and the mixture and Eulerian models are appropriate for flows in which the phases
mix or separate and/or dispersed-phase volume fractions exceed 10%. (Flows in which
the dispersed-phase volume fractions are less than or equal to 10% can be modeled using
the discrete phase model described in Chapter 15: Discrete Phase.)
To choose between the mixture model and the Eulerian model, you should consider the
following guidelines:
• If there is a wide distribution of the dispersed phases (i.e., if the particles vary
in size and the largest particles do not separate from the primary flow field), the
mixture model may be preferable (i.e., less computationally expensive). If the
dispersed phases are concentrated just in portions of the domain, you should use
the Eulerian model instead.
• If interphase drag laws that are applicable to your system are available (either
within ANSYS FLUENT or through a user-defined function), the Eulerian model
can usually provide more accurate results than the mixture model. Even though
you can apply the same drag laws to the mixture model, as you can for a nongranular
Eulerian simulation, if the interphase drag laws are unknown or their applicability
to your system is questionable, the mixture model may be a better choice. For
most cases with spherical particles, then the Schiller-Naumann law is more than
adequate. For cases with nonspherical particles, then a user-defined function can
be used.
• If you want to solve a simpler problem, which requires less computational effort, the
mixture model may be a better option, since it solves a smaller number of equations
than the Eulerian model. If accuracy is more important than computational effort,
the Eulerian model is a better choice. Keep in mind, however, that the complexity
of the Eulerian model can make it less computationally stable than the mixture
model.
ANSYS FLUENT’s multiphase models are compatible with ANSYS FLUENT’s dynamic
mesh modeling feature. For more information on the dynamic mesh feature, see Section 3: Flows Using Sliding and Deforming Meshes. For more information about how
other ANSYS FLUENT models are compatible with ANSYS FLUENT’s multiphase models, see Appendix A: ANSYS FLUENT Model Compatibility in the separate User’s Guide.
16-8
Release 12.0 c ANSYS, Inc. January 29, 2009
16.2 Choosing a General Multiphase Model
Detailed Guidelines
For stratified and slug flows, the choice of the VOF model, as indicated in Section 16.2.2: Model
Comparisons, is straightforward. Choosing a model for the other types of flows is less
straightforward. As a general guide, there are some parameters that help to identify the
appropriate multiphase model for these other flows: the particulate loading, β, and the
Stokes number, St. (Note that the word “particle” is used in this discussion to refer to
a particle, droplet, or bubble.)
The Effect of Particulate Loading
Particulate loading has a major impact on phase interactions. The particulate loading is
defined as the mass density ratio of the dispersed phase (d) to that of the carrier phase
(c):
β=
αd ρd
αc ρc
(16.2-1)
ρd
ρc
(16.2-2)
The material density ratio
γ=
is greater than 1000 for gas-solid flows, about 1 for liquid-solid flows, and less than 0.001
for gas-liquid flows.
Using these parameters it is possible to estimate the average distance between the individual particles of the particulate phase. An estimate of this distance has been given by
Crowe et al. [62]:
L
π1+κ
=
dd
6 κ
1/3
(16.2-3)
where κ = βγ . Information about these parameters is important for determining how the
dispersed phase should be treated. For example, for a gas-particle flow with a particulate
loading of 1, the interparticle space dLd is about 8; the particle can therefore be treated
as isolated (i.e., very low particulate loading).
Release 12.0 c ANSYS, Inc. January 29, 2009
16-9
Multiphase Flows
Depending on the particulate loading, the degree of interaction between the phases can
be divided into the following three categories:
• For very low loading, the coupling between the phases is one-way (i.e., the fluid
carrier influences the particles via drag and turbulence, but the particles have no
influence on the fluid carrier). The discrete phase (Chapter 15: Discrete Phase),
mixture, and Eulerian models can all handle this type of problem correctly. Since
the Eulerian model is the most expensive, the discrete phase or mixture model is
recommended.
• For intermediate loading, the coupling is two-way (i.e., the fluid carrier influences
the particulate phase via drag and turbulence, but the particles in turn influence
the carrier fluid via reduction in mean momentum and turbulence). The discrete
phase(Chapter 15: Discrete Phase) , mixture, and Eulerian models are all applicable
in this case, but you need to take into account other factors in order to decide
which model is more appropriate. See below for information about using the Stokes
number as a guide.
• For high loading, there is two-way coupling plus particle pressure and viscous
stresses due to particles (four-way coupling). Only the Eulerian model will handle
this type of problem correctly.
The Significance of the Stokes Number
For systems with intermediate particulate loading, estimating the value of the Stokes
number can help you select the most appropriate model. The Stokes number can be
defined as the relation between the particle response time and the system response time:
St =
τd
ts
(16.2-4)
ρ d2
d d
where τd = 18µ
and ts is based on the characteristic length (Ls ) and the characteristic
c
velocity (Vs ) of the system under investigation: ts = LVss .
For St 1.0, the particle will follow the flow closely and any of the three models (discrete
phase(Chapter 15: Discrete Phase) , mixture, or Eulerian) is applicable; you can therefore
choose the least expensive (the mixture model, in most cases), or the most appropriate
considering other factors. For St > 1.0, the particles will move independently of the flow
and either the discrete phase model (Chapter 15: Discrete Phase) or the Eulerian model
is applicable. For St ≈ 1.0, again any of the three models is applicable; you can choose
the least expensive or the most appropriate considering other factors.
16-10
Release 12.0 c ANSYS, Inc. January 29, 2009
16.2 Choosing a General Multiphase Model
Examples
For a coal classifier with a characteristic length of 1 m and a characteristic velocity of
10 m/s, the Stokes number is 0.04 for particles with a diameter of 30 microns, but 4.0
for particles with a diameter of 300 microns. Clearly the mixture model will not be
applicable to the latter case.
For the case of mineral processing, in a system with a characteristic length of 0.2 m and a
characteristic velocity of 2 m/s, the Stokes number is 0.005 for particles with a diameter
of 300 microns. In this case, you can choose between the mixture and Eulerian models.
(The volume fractions are too high for the discrete phase model (Chapter 15: Discrete
Phase), as noted below.)
Other Considerations
Keep in mind that the use of the discrete phase model (Chapter 15: Discrete Phase) is
limited to low volume fractions. Also, the discrete phase model is the only multiphase
model that allows you to specify the particle distribution or include combustion modeling
in your simulation.
16.2.3
Time Schemes in Multiphase Flow
In many multiphase applications, the process can vary spatially as well as temporally. In
order to accurately model multiphase flow, both higher-order spatial and time discretization schemes are necessary. In addition to the first-order time scheme in ANSYS FLUENT,
the second-order time scheme is available in the Mixture and Eulerian multiphase models,
and with the VOF Implicit Scheme.
i
The second-order time scheme cannot be used with the VOF Explicit
Schemes.
The second-order time scheme has been adapted to all the transport equations, including mixture phase momentum equations, energy equations, species transport equations,
turbulence models, phase volume fraction equations, the pressure correction equation,
and the granular flow model. In multiphase flow, a general transport equation (similar
to that of Equation 18.3-15) may be written as
∂(αρφ)
+ ∇ · (αρV~ φ) = ∇ · τ + Sφ
∂t
(16.2-5)
Where φ is either a mixture (for the mixture model) or a phase variable, α is the phase
volume fraction (unity for the mixture equation), ρ is the mixture phase density, V~ is
the mixture or phase velocity (depending on the equations), τ is the diffusion term, and
Sφ is the source term.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-11
Multiphase Flows
As a fully implicit scheme, this second-order time-accurate scheme achieves its accuracy
by using an Euler backward approximation in time (see Equation 18.3-17). The general
transport equation, Equation 16.2-5 is discretized as
3(αp ρp φp V ol)n+1 − 4(αp ρp φp V ol)n + (αp ρp φp )n−1
=
2∆t
X
(16.2-6)
[Anb (φnb − φp )]n+1 + S U n+1 − S p n+1 φp n+1
Equation 16.2-6 can be written in simpler form:
Ap φp =
X
An bφn b + Sφ
(16.2-7)
where
Ap =
P
Anb n+1 + S p n+1 +
Sφ = S U n+1 +
1.5(αp ρp V ol)n+1
∆t
2(αp ρp φp V ol)n −0.5(αp ρp φp V ol)n−1
∆t
This scheme is easily implemented based on ANSYS FLUENT’s existing first-order Euler
scheme. It is unconditionally stable, however, the negative coefficient at the time level
tn−1 , of the three-time level method, may produce oscillatory solutions if the time steps
are large.
This problem can be eliminated if a bounded second-order scheme is introduced. However, oscillating solutions are most likely seen in compressible liquid flows. Therefore, in
this version of ANSYS FLUENT, a bounded second-order time scheme has been implemented for compressible liquid flows only. For single phase and multiphase compressible
liquid flows, the second-order time scheme is, by default, the bounded scheme.
16.2.4
Stability and Convergence
The process of solving a multiphase system is inherently difficult and you may encounter
some stability or convergence problems.
When solving a time-dependent problem, a proper initial field is required to avoid instabilities, which usually arise from poor initial fields. If the CPU time is a concern for
transient problems, then the best option is to use PC SIMPLE. When body forces are
significant, or if the solution requires higher order numerical schemes, it is recommended
that you start with a small time step, which can be increased after performing a few time
steps to get a better approximation of the pressure field.
For a steady solution, it is recommended that you use the Multiphase Coupled solver, described in detail in Section 24.7.1: Coupled Solution for Multiphase Flows in the separate
User’s Guide. The iterative nature of this solver requires a good starting patched field.
16-12
Release 12.0 c ANSYS, Inc. January 29, 2009
16.3 Volume of Fluid (VOF) Model Theory
If difficulties are encountered due to higher order schemes, or due to the complexities of
the problem, you may need to reduce the Courant number. The default Courant number
is 200 but it can be reduced to as low as 4. This can later be increased if the iteration
process runs smoothly. In addition, there are explicit under-relaxation factors for velocities and pressure. All other under-relaxation factors are implicit. Lower under-relaxation
factors for the volume of fraction equation may delay the solution dramatically with the
Coupled solver (any value 0.5 or above is adequate); on the contrary, PC SIMPLE would
normally need a low under-relaxation for the volume fraction equation.
In addition, ANSYS FLUENT offers a Full Multiphase Coupled solver where all velocities, pressure correction and volume fraction correction are solved simultaneously, which
currently is not as robust as the others.
Furthermore, ANSYS FLUENT has an option to solve stratified immiscible fluids within
the Eulerian multiphase formulation. This feature is similar to the single fluid VOF
solution, but in the context of multiple velocities.
16.3
Volume of Fluid (VOF) Model Theory
Information is organized into the following subsections:
• Section 16.3.1: Overview and Limitations of the VOF Model
• Section 16.3.2: Volume Fraction Equation
• Section 16.3.3: Material Properties
• Section 16.3.4: Momentum Equation
• Section 16.3.5: Energy Equation
• Section 16.3.6: Additional Scalar Equations
• Section 16.3.7: Time Dependence
• Section 16.3.8: Surface Tension and Wall Adhesion
• Section 16.3.9: Open Channel Flow
• Section 16.3.10: Open Channel Wave Boundary Conditions
Release 12.0 c ANSYS, Inc. January 29, 2009
16-13
Multiphase Flows
16.3.1
Overview and Limitations of the VOF Model
Overview
The VOF model can model two or more immiscible fluids by solving a single set of
momentum equations and tracking the volume fraction of each of the fluids throughout
the domain. Typical applications include the prediction of jet breakup, the motion of
large bubbles in a liquid, the motion of liquid after a dam break, and the steady or
transient tracking of any liquid-gas interface.
Limitations
The following restrictions apply to the VOF model in ANSYS FLUENT:
• You must use the pressure-based solver. The VOF model is not available with the
density-based solver.
• All control volumes must be filled with either a single fluid phase or a combination
of phases. The VOF model does not allow for void regions where no fluid of any
type is present.
• Only one of the phases can be defined as a compressible ideal gas. There is no
limitation on using compressible liquids using user-defined functions.
• Streamwise periodic flow (either specified mass flow rate or specified pressure drop)
cannot be modeled when the VOF model is used.
• The second-order implicit time-stepping formulation cannot be used with the VOF
explicit scheme.
• When tracking particles in parallel, the DPM model cannot be used with the VOF
model if the shared memory option is enabled (Section 23.8: Parallel Processing
for the Discrete Phase Model in the separate User’s Guide). (Note that using the
message passing option, when running in parallel, enables the compatibility of all
multiphase flow models with the DPM model.)
16-14
Release 12.0 c ANSYS, Inc. January 29, 2009
16.3 Volume of Fluid (VOF) Model Theory
Steady-State and Transient VOF Calculations
The VOF formulation in ANSYS FLUENT is generally used to compute a time-dependent
solution, but for problems in which you are concerned only with a steady-state solution,
it is possible to perform a steady-state calculation. A steady-state VOF calculation is
sensible only when your solution is independent of the initial conditions and there are
distinct inflow boundaries for the individual phases. For example, since the shape of the
free surface inside a rotating cup depends on the initial level of the fluid, such a problem
must be solved using the time-dependent formulation. On the other hand, the flow of
water in a channel with a region of air on top and a separate air inlet can be solved with
the steady-state formulation.
The VOF formulation relies on the fact that two or more fluids (or phases) are not
interpenetrating. For each additional phase that you add to your model, a variable is
introduced: the volume fraction of the phase in the computational cell. In each control
volume, the volume fractions of all phases sum to unity. The fields for all variables and
properties are shared by the phases and represent volume-averaged values, as long as
the volume fraction of each of the phases is known at each location. Thus the variables
and properties in any given cell are either purely representative of one of the phases, or
representative of a mixture of the phases, depending upon the volume fraction values.
In other words, if the q th fluid’s volume fraction in the cell is denoted as αq , then the
following three conditions are possible:
• αq = 0: The cell is empty (of the q th fluid).
• αq = 1: The cell is full (of the q th fluid).
• 0 < αq < 1: The cell contains the interface between the q th fluid and one or more
other fluids.
Based on the local value of αq , the appropriate properties and variables will be assigned
to each control volume within the domain.
16.3.2
Volume Fraction Equation
The tracking of the interface(s) between the phases is accomplished by the solution of a
continuity equation for the volume fraction of one (or more) of the phases. For the q th
phase, this equation has the following form:
n
X
1 ∂
(αq ρq ) + ∇ · (αq ρq~vq ) = Sαq + (ṁpq − ṁqp )
ρq ∂t
p=1
(16.3-1)
where ṁqp is the mass transfer from phase q to phase p and ṁpq is the mass transfer from
phase p to phase q. By default, the source term on the right-hand side of Equation 16.3-1,
Release 12.0 c ANSYS, Inc. January 29, 2009
16-15
Multiphase Flows
Sαq , is zero, but you can specify a constant or user-defined mass source for each phase.
See Section 16.7: Modeling Mass Transfer in Multiphase Flows for more information on
the modeling of mass transfer in ANSYS FLUENT’s general multiphase models.
The volume fraction equation will not be solved for the primary phase; the primary-phase
volume fraction will be computed based on the following constraint:
n
X
αq = 1
(16.3-2)
q=1
The volume fraction equation may be solved either through implicit or explicit time
discretization.
The Implicit Scheme
When the implicit scheme is used for time discretization, ANSYS FLUENT’s standard
finite-difference interpolation schemes, QUICK, Second Order Upwind and First Order Upwind, and the Modified HRIC schemes, are used to obtain the face fluxes for all cells,
including those near the interface.
n
X
X
αqn+1 ρn+1
− αqn ρnq
q
n+1 n+1
Sα +
V + (ρn+1
U
α
)
=
(ṁpq − ṁqp ) V
q
q
f
q,f
∆t
p=1
f
(16.3-3)
Since this equation requires the volume fraction values at the current time step (rather
than at the previous step, as for the explicit scheme), a standard scalar transport equation
is solved iteratively for each of the secondary-phase volume fractions at each time step.
The implicit scheme can be used for both time-dependent and steady-state calculations.
See Section 24.2.2: Choosing a Volume Fraction Formulation in the separate User’s Guide
for details.
The Explicit Scheme
In the explicit approach, ANSYS FLUENT’s standard finite-difference interpolation schemes
are applied to the volume fraction values that were computed at the previous time step.
n
X
X
αqn+1 ρn+1
− αqn ρnq
q
n
V + (ρq Ufn αq,f
) = (ṁpq − ṁqp ) + Sαq V
∆t
p=1
f
16-16
(16.3-4)
Release 12.0 c ANSYS, Inc. January 29, 2009
16.3 Volume of Fluid (VOF) Model Theory
where
n + 1 = index for new (current) time step
n
= index for previous time step
αq,f
= face value of the q th volume fraction, computed from the firstor second-order upwind, QUICK, modified HRIC, or CICSAM scheme
V
= volume of cell
Uf
= volume flux through the face, based on normal velocity
This formulation does not require iterative solution of the transport equation during each
time step, as is needed for the implicit scheme.
i
When the explicit scheme is used, a time-dependent solution must be computed.
When the explicit scheme is used for time discretization, the face fluxes can be interpolated either using interface reconstruction or using a finite volume discretization scheme
(Section 16.3.2: Interpolation near the Interface). The reconstruction based schemes
available in ANSYS FLUENT are Geo-Reconstruct and Donor-Acceptor. The discretization
schemes available with explicit scheme for VOF are First Order Upwind, Second Order
Upwind, CICSAM, Modified HRIC, and QUICK.
Interpolation near the Interface
ANSYS FLUENT’s control-volume formulation requires that convection and diffusion
fluxes through the control volume faces be computed and balanced with source terms
within the control volume itself.
In the geometric reconstruction and donor-acceptor schemes, ANSYS FLUENT applies a
special interpolation treatment to the cells that lie near the interface between two phases.
Figure 16.3.1 shows an actual interface shape along with the interfaces assumed during
computation by these two methods.
The explicit scheme and the implicit scheme treat these cells with the same interpolation as the cells that are completely filled with one phase or the other (i.e., using
the standard upwind (Section 18.3.1: First-Order Upwind Scheme), second-order (Section 18.3.1: Second-Order Upwind Scheme), QUICK (Section 18.3.1: QUICK Scheme,
modified HRIC (Section 18.3.1: Modified HRIC Scheme), or CICSAM scheme), rather
than applying a special treatment.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-17
Multiphase Flows
actual interface shape
interface shape represented by
the geometric reconstruction
(piecewise-linear) scheme
interface shape represented by
the donor-acceptor scheme
Figure 16.3.1: Interface Calculations
16-18
Release 12.0 c ANSYS, Inc. January 29, 2009
16.3 Volume of Fluid (VOF) Model Theory
The Geometric Reconstruction Scheme
In the geometric reconstruction approach, the standard interpolation schemes that are
used in ANSYS FLUENT are used to obtain the face fluxes whenever a cell is completely
filled with one phase or another. When the cell is near the interface between two phases,
the geometric reconstruction scheme is used.
The geometric reconstruction scheme represents the interface between fluids using a
piecewise-linear approach. In ANSYS FLUENT this scheme is the most accurate and
is applicable for general unstructured meshes. The geometric reconstruction scheme is
generalized for unstructured meshes from the work of Youngs [388]. It assumes that the
interface between two fluids has a linear slope within each cell, and uses this linear shape
for calculation of the advection of fluid through the cell faces. (See Figure 16.3.1.)
The first step in this reconstruction scheme is calculating the position of the linear interface relative to the center of each partially-filled cell, based on information about
the volume fraction and its derivatives in the cell. The second step is calculating the
advecting amount of fluid through each face using the computed linear interface representation and information about the normal and tangential velocity distribution on the
face. The third step is calculating the volume fraction in each cell using the balance of
fluxes calculated during the previous step.
i
When the geometric reconstruction scheme is used, a time-dependent solution must be computed. Also, if you are using a conformal mesh (i.e., if the
mesh node locations are identical at the boundaries where two subdomains
meet), you must ensure that there are no two-sided (zero-thickness) walls
within the domain. If there are, you will need to slit them, as described in
Section 6.8.6: Slitting Face Zones in the separate User’s Guide.
The Donor-Acceptor Scheme
In the donor-acceptor approach, the standard interpolation schemes that are used in
ANSYS FLUENT are used to obtain the face fluxes whenever a cell is completely filled
with one phase or another. When the cell is near the interface between two phases, a
“donor-acceptor” scheme is used to determine the amount of fluid advected through the
face [131]. This scheme identifies one cell as a donor of an amount of fluid from one phase
and another (neighbor) cell as the acceptor of that same amount of fluid, and is used to
prevent numerical diffusion at the interface. The amount of fluid from one phase that
can be convected across a cell boundary is limited by the minimum of two values: the
filled volume in the donor cell or the free volume in the acceptor cell.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-19
Multiphase Flows
The orientation of the interface is also used in determining the face fluxes. The interface
orientation is either horizontal or vertical, depending on the direction of the volume
fraction gradient of the q th phase within the cell, and that of the neighbor cell that shares
the face in question. Depending on the interface’s orientation as well as its motion, flux
values are obtained by pure upwinding, pure downwinding, or some combination of the
two.
i
When the donor-acceptor scheme is used, a time-dependent solution must
be computed. Also, the donor-acceptor scheme can be used only with
quadrilateral or hexahedral meshes. In addition, if you are using a conformal mesh (i.e., if the mesh node locations are identical at the boundaries
where two subdomains meet), you must ensure that there are no two-sided
(zero-thickness) walls within the domain. If there are, you will need to
slit them, as described in Section 6.8.6: Slitting Face Zones in the separate
User’s Guide.
The Compressive Interface Capturing Scheme for Arbitrary Meshes (CICSAM)
The compressive interface capturing scheme for arbitrary meshes (CICSAM), based on
Ubbink’s work [351], is a high resolution differencing scheme. The CICSAM scheme is
particularly suitable for flows with high ratios of viscosities between the phases. CICSAM
is implemented in ANSYS FLUENT as an explicit scheme and offers the advantage of
producing an interface that is almost as sharp as the geometric reconstruction scheme.
16.3.3
Material Properties
The properties appearing in the transport equations are determined by the presence of
the component phases in each control volume. In a two-phase system, for example, if
the phases are represented by the subscripts 1 and 2, and if the volume fraction of the
second of these is being tracked, the density in each cell is given by
ρ = α2 ρ2 + (1 − α2 )ρ1
(16.3-5)
In general, for an n-phase system, the volume-fraction-averaged density takes on the
following form:
ρ=
X
αq ρq
(16.3-6)
All other properties (e.g., viscosity) are computed in this manner.
16-20
Release 12.0 c ANSYS, Inc. January 29, 2009
16.3 Volume of Fluid (VOF) Model Theory
16.3.4
Momentum Equation
A single momentum equation is solved throughout the domain, and the resulting velocity
field is shared among the phases. The momentum equation, shown below, is dependent
on the volume fractions of all phases through the properties ρ and µ.
h
i
∂
(ρ~v ) + ∇ · (ρ~v~v ) = −∇p + ∇ · µ ∇~v + ∇~v T + ρ~g + F~
∂t
(16.3-7)
One limitation of the shared-fields approximation is that in cases where large velocity
differences exist between the phases, the accuracy of the velocities computed near the
interface can be adversely affected.
Note that if the viscosity ratio is more than 1x103 , this may lead to convergence difficulties. The compressive interface capturing scheme for arbitrary meshes (CICSAM)
(Section 16.3.2: The Compressive Interface Capturing Scheme for Arbitrary Meshes
(CICSAM)) is suitable for flows with high ratios of viscosities between the phases, thus
solving the problem of poor convergence.
16.3.5
Energy Equation
The energy equation, also shared among the phases, is shown below.
∂
(ρE) + ∇ · (~v (ρE + p)) = ∇ · (keff ∇T ) + Sh
∂t
(16.3-8)
The VOF model treats energy, E, and temperature, T , as mass-averaged variables:
n
X
E=
αq ρq Eq
q=1
n
X
(16.3-9)
αq ρq
q=1
where Eq for each phase is based on the specific heat of that phase and the shared
temperature.
The properties ρ and keff (effective thermal conductivity) are shared by the phases. The
source term, Sh , contains contributions from radiation, as well as any other volumetric
heat sources.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-21
Multiphase Flows
As with the velocity field, the accuracy of the temperature near the interface is limited in
cases where large temperature differences exist between the phases. Such problems also
arise in cases where the properties vary by several orders of magnitude. For example, if a
model includes liquid metal in combination with air, the conductivities of the materials
can differ by as much as four orders of magnitude. Such large discrepancies in properties
lead to equation sets with anisotropic coefficients, which in turn can lead to convergence
and precision limitations.
16.3.6 Additional Scalar Equations
Depending upon your problem definition, additional scalar equations may be involved in
your solution. In the case of turbulence quantities, a single set of transport equations is
solved, and the turbulence variables (e.g., k and or the Reynolds stresses) are shared
by the phases throughout the field.
16.3.7 Time Dependence
For time-dependent VOF calculations, Equation 16.3-1 is solved using an explicit timemarching scheme. ANSYS FLUENT automatically refines the time step for the integration
of the volume fraction equation, but you can influence this time step calculation by
modifying the Courant number. You can choose to update the volume fraction once
for each time step, or once for each iteration within each time step. These options are
discussed in more detail in Section 24.3.5: Setting Time-Dependent Parameters for the
VOF Model in the separate User’s Guide.
16.3.8
Surface Tension and Wall Adhesion
The VOF model can also include the effects of surface tension along the interface between
each pair of phases. The model can be augmented by the additional specification of the
contact angles between the phases and the walls. You can specify a surface tension
coefficient as a constant, as a function of temperature, or through a UDF. The solver
will include the additional tangential stress terms (causing what is termed as Marangoni
convection) that arise due to the variation in surface tension coefficient. Variable surface
tension coefficient effects are usually important only in zero/near-zero gravity conditions.
16-22
Release 12.0 c ANSYS, Inc. January 29, 2009
16.3 Volume of Fluid (VOF) Model Theory
Surface Tension
Surface tension arises as a result of attractive forces between molecules in a fluid. Consider an air bubble in water, for example. Within the bubble, the net force on a molecule
due to its neighbors is zero. At the surface, however, the net force is radially inward, and
the combined effect of the radial components of force across the entire spherical surface
is to make the surface contract, thereby increasing the pressure on the concave side of
the surface. The surface tension is a force, acting only at the surface, that is required
to maintain equilibrium in such instances. It acts to balance the radially inward intermolecular attractive force with the radially outward pressure gradient force across the
surface. In regions where two fluids are separated, but one of them is not in the form
of spherical bubbles, the surface tension acts to minimize free energy by decreasing the
area of the interface.
The surface tension model in ANSYS FLUENT is the continuum surface force (CSF) model
proposed by Brackbill et al. [34]. With this model, the addition of surface tension to the
VOF calculation results in a source term in the momentum equation. To understand the
origin of the source term, consider the special case where the surface tension is constant
along the surface, and where only the forces normal to the interface are considered. It
can be shown that the pressure drop across the surface depends upon the surface tension
coefficient, σ, and the surface curvature as measured by two radii in orthogonal directions,
R1 and R2 :
1
1
p2 − p1 = σ
+
R1 R2
(16.3-10)
where p1 and p2 are the pressures in the two fluids on either side of the interface.
In ANSYS FLUENT, a formulation of the CSF model is used, where the surface curvature
is computed from local gradients in the surface normal at the interface. Let n be the
surface normal, defined as the gradient of αq , the volume fraction of the q th phase.
n = ∇αq
(16.3-11)
The curvature, κ, is defined in terms of the divergence of the unit normal, n̂ [34]:
κ = ∇ · n̂
(16.3-12)
where
n̂ =
Release 12.0 c ANSYS, Inc. January 29, 2009
n
|n|
(16.3-13)
16-23
Multiphase Flows
The surface tension can be written in terms of the pressure jump across the surface. The
force at the surface can be expressed as a volume force using the divergence theorem. It
is this volume force that is the source term which is added to the momentum equation.
It has the following form:
Fvol =
X
σij
pairs ij, i 0), the flow is known to be
subcritical where disturbances can travel upstream as well as downstream. In this
case, downstream conditions might affect the flow upstream.
• When F r = 1 (thus Vw = 0), the flow is known to be critical, where upstream
propagating waves remain stationary. In this case, the character of the flow changes.
√
• When F r > 1, i.e., V > gy (thus Vw > 0), the flow is known to be supercritical
where disturbances cannot travel upstream. In this case, downstream conditions
do not affect the flow upstream.
Upstream Boundary Conditions
There are two options available for the upstream boundary condition for open channel
flows:
• pressure inlet
• mass flow rate
Pressure Inlet
The total pressure p0 at the inlet can be given as
1
→ →
−
→
p0 = (ρ − ρ0 )V 2 + (ρ − ρ0 )|−
g |(ĝ · ( b − −
a ))
2
(16.3-21)
→
−
→
where b and −
a are the position vectors of the face centroid and any point on the free
surface, respectively, Here, free surface is assumed to be horizontal and normal to the
→
→
direction of gravity. −
g is the gravity vector, |−
g | is the gravity magnitude, ĝ is the unit
vector of gravity, V is the velocity magnitude, ρ is the density of the mixture in the cell,
and ρ0 is the reference density.
From this, the dynamic pressure q is
q=
ρ − ρ0 2
V
2
(16.3-22)
and the static pressure ps is
→ →
−
→
ps = (ρ − ρ0 )|−
g |(ĝ · ( b − −
a ))
16-26
(16.3-23)
Release 12.0 c ANSYS, Inc. January 29, 2009
16.3 Volume of Fluid (VOF) Model Theory
which can be further expanded to
→
−
→
ps = (ρ − ρ0 )|−
g |((ĝ · b ) + ylocal )
(16.3-24)
where the distance from the free surface to the reference position, ylocal , is
→
ylocal = −(−
a · ĝ)
(16.3-25)
Mass Flow Rate
The mass flow rate for each phase associated with the open channel flow is defined by
ṁphase = ρphase (Areaphase )(V elocity)
(16.3-26)
Volume Fraction Specification
In open channel flows, ANSYS FLUENT internally calculates the volume fraction based
on the input parameters specified in the boundary conditions dialog box, therefore this
option has been disabled.
For subcritical inlet flows (Fr < 1), ANSYS FLUENT reconstructs the volume fraction
values on the boundary by using the values from the neighboring cells. This can be
accomplished using the following procedure:
• Calculate the node values of volume fraction at the boundary using the cell values.
• Calculate the volume fraction at the each face of boundary using the interpolated
node values.
For supercritical inlet flows (Fr > 1), the volume fraction value on the boundary can be
calculated using the fixed height of the free surface from the bottom.
Downstream Boundary Conditions
Pressure Outlet
Determining the static pressure is dependent on the Pressure Specification Method. Using
the Free Surface Level, the static pressure is dictated by Equation 16.3-23 and Equation 16.3-25, otherwise you must specify the static pressure as the Gauge Pressure.
For subcritical outlet flows (Fr < 1), if there are only two phases, then the pressure is
taken from the pressure profile specified over the boundary, otherwise the pressure is
taken from the neighboring cell. For supercritical flows (Fr >1), the pressure is always
taken from the neighboring cell.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-27
Multiphase Flows
Outflow Boundary
Outflow boundary conditions can be used at the outlet of open channel flows to model
flow exits where the details of the flow velocity and pressure are not known prior to
solving the flow problem. If the conditions are unknown at the outflow boundaries, then
ANSYS FLUENT will extrapolate the required information from the interior.
It is important, however, to understand the limitations of this boundary type:
• You can only use single outflow boundaries at the outlet, which is achieved by setting the flow rate weighting to 1. In other words, outflow splitting is not permitted
in open channel flows with outflow boundaries.
• There should be an initial flow field in the simulation to avoid convergence issues
due to flow reversal at the outflow, which will result in an unreliable solution.
• An outflow boundary condition can only be used with mass flow inlets. It is not
compatible with pressure inlets and pressure outlets. For example, if you choose
the inlet as pressure-inlet, then you can only use pressure-outlet at the outlet. If you
choose the inlet as mass-flow-inlet, then you can use either outflow or pressure-outlet
boundary conditions at the outlet. Note that this only holds true for open channel
flow.
• Note that the outflow boundary condition assumes that flow is fully developed
in the direction perpendicular to the outflow boundary surface. Therefore, such
surfaces should be placed accordingly.
Backflow Volume Fraction Specification
ANSYS FLUENT internally calculates the volume fraction values on the outlet boundary
by using the neighboring cell values, therefore, this option is disabled.
16.3.10
Open Channel Wave Boundary Conditions
The open channel wave boundary condition allows you to simulate the propagation of
waves, which is useful in the marine industry. This is an upstream boundary condition
and is applied to the velocity inlet of the VOF model. The wave profile for an incident
wave can be described as follows:
ζ = A cos(kx x + ky y − ωe t + )
(16.3-27)
where z is the wave height, A is the wave amplitude, is the phase difference, t is the
time, and kx and ky are the wave numbers in the x and y directions, respectively, such
that kx = k cos θ and ky = k sin θ.
16-28
Release 12.0 c ANSYS, Inc. January 29, 2009
16.3 Volume of Fluid (VOF) Model Theory
The wave number k is defined as
k=
2π
λ
(16.3-28)
where λ is the wave length and the effective wave frequency ωe is
ωe = ω + kU
(16.3-29)
U is the uniform incident wave velocity and ω, the wave frequency, is defined as
ω=
q
gk tanh(kh)
(16.3-30)
where h is the liquid height and g is the gravity magnitude.
The velocity components for the incident wave boundary condition can be described in
terms of shallow waves and short gravity waves.
Shallow waves are defined as
u
v
!
gkA cosh[k(z + h)]
=
ω
cosh(kh)
w=
cos θ
sin θ
!
cos(kx x + ky y − ωe t + )
gkA sinh[k(z + h)]
sin(kx x + ky y − ωe t + )
ω
cosh(kh)
(16.3-31)
(16.3-32)
Short gravity waves are defined as
u
v
!
gkA kz
=
e
ω
w=
cos θ
sin θ
!
cos(kx x + ky y − ωe t + )
gkA kz
e sin(kx x + ky y − ωe t + )
ω
(16.3-33)
(16.3-34)
where u, v, and w are the velocity components. Note that direction specifications for
the velocity components are such that u is based on the flow direction specified in the
wave velocity specification method, w is based on the gravity direction, and v is in the
cross direction of the flow and gravity direction. For more information on how to use
and set up this model, refer to Section 24.3.2: Modeling Open Channel Wave Boundary
Conditions in the separate User’s Guide.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-29
Multiphase Flows
16.4
Mixture Model Theory
Information is organized into the following subsections:
• Section 16.4.1: Overview and Limitations of the Mixture Model
• Section 16.4.2: Continuity Equation
• Section 16.4.3: Momentum Equation
• Section 16.4.4: Energy Equation
• Section 16.4.5: Relative (Slip) Velocity and the Drift Velocity
• Section 16.4.6: Volume Fraction Equation for the Secondary Phases
• Section 16.4.7: Granular Properties
• Section 16.4.8: Granular Temperature
• Section 16.4.9: Interfacial Area Concentration
• Section 16.4.10: Solids Pressure
16.4.1
Overview and Limitations of the Mixture Model
Overview
The mixture model is a simplified multiphase model that can be used in different ways.
It can be used to model multiphase flows where the phases move at different velocities,
but assume local equilibrium over short spatial length scales. It can be used to model
homogeneous multiphase flows with very strong coupling and phases moving at the same
velocity and lastly, the mixture models are used to calculate non-Newtonian viscosity.
The mixture model can model n phases (fluid or particulate) by solving the momentum,
continuity, and energy equations for the mixture, the volume fraction equations for the
secondary phases, and algebraic expressions for the relative velocities. Typical applications include sedimentation, cyclone separators, particle-laden flows with low loading,
and bubbly flows where the gas volume fraction remains low.
The mixture model is a good substitute for the full Eulerian multiphase model in several
cases. A full multiphase model may not be feasible when there is a wide distribution of
the particulate phase or when the interphase laws are unknown or their reliability can
be questioned. A simpler model like the mixture model can perform as well as a full
multiphase model while solving a smaller number of variables than the full multiphase
model.
The mixture model allows you to select granular phases and calculates all properties of
the granular phases. This is applicable for liquid-solid flows.
16-30
Release 12.0 c ANSYS, Inc. January 29, 2009
16.4 Mixture Model Theory
Limitations
The following limitations apply to the mixture model in ANSYS FLUENT:
• You must use the pressure-based solver. The mixture model is not available with
the density-based solver.
• Only one of the phases can be defined as a compressible ideal gas. There is no
limitation on using compressible liquids using user-defined functions.
• When the mixture model is used, do not model streamwise periodic flow with
specified mass flow rate.
• Do not model solidification and melting in conjunction with the mixture model.
• The Singhal et al. cavitation model (available with the mixture model) is not
compatible with the LES turbulence model.
• Do not use the relative formulation in combination with the MRF and mixture
model (see Section 10.3.1: Limitations in the separate User’s Guide).
• The mixture model does not allow for inviscid flows.
• The shell conduction model for walls is not allowed with the mixture model.
• When tracking particles in parallel, do not use the DPM model with the mixture
model if the shared memory option is enabled (Section 23.8: Parallel Processing
for the Discrete Phase Model in the separate User’s Guide). (Note that using the
message passing option, when running in parallel, enables the compatibility of all
multiphase flow models with the DPM model.)
The mixture model, like the VOF model, uses a single-fluid approach. It differs from the
VOF model in two respects:
• The mixture model allows the phases to be interpenetrating. The volume fractions
αq and αp for a control volume can therefore be equal to any value between 0 and
1, depending on the space occupied by phase q and phase p.
• The mixture model allows the phases to move at different velocities, using the
concept of slip velocities. (Note that the phases can also be assumed to move
at the same velocity, and the mixture model is then reduced to a homogeneous
multiphase model.)
The mixture model solves the continuity equation for the mixture, the momentum equation for the mixture, the energy equation for the mixture, and the volume fraction equation for the secondary phases, as well as algebraic expressions for the relative velocities
(if the phases are moving at different velocities).
Release 12.0 c ANSYS, Inc. January 29, 2009
16-31
Multiphase Flows
16.4.2
Continuity Equation
The continuity equation for the mixture is
∂
(ρm ) + ∇ · (ρm~vm ) = 0
∂t
(16.4-1)
where ~vm is the mass-averaged velocity:
Pn
~vm =
αk ρk~vk
ρm
k=1
(16.4-2)
and ρm is the mixture density:
ρm =
n
X
αk ρk
(16.4-3)
k=1
αk is the volume fraction of phase k.
16.4.3
Momentum Equation
The momentum equation for the mixture can be obtained by summing the individual
momentum equations for all phases. It can be expressed as
h
i
∂
T
(ρm~vm ) + ∇ · (ρm~vm~vm ) = −∇p + ∇ · µm ∇~vm + ∇~vm
+
∂t
ρm~g + F~ + ∇ ·
n
X
!
αk ρk~vdr,k~vdr,k
(16.4-4)
k=1
where n is the number of phases, F~ is a body force, and µm is the viscosity of the mixture:
µm =
n
X
αk µk
(16.4-5)
k=1
~vdr,k is the drift velocity for secondary phase k:
~vdr,k = ~vk − ~vm
16-32
(16.4-6)
Release 12.0 c ANSYS, Inc. January 29, 2009
16.4 Mixture Model Theory
16.4.4
Energy Equation
The energy equation for the mixture takes the following form:
n
n
X
∂ X
(αk ρk Ek ) + ∇ ·
(αk~vk (ρk Ek + p)) = ∇ · (keff ∇T ) + SE
∂t k=1
k=1
(16.4-7)
P
where keff is the effective conductivity ( αk (kk + kt )), where kt is the turbulent thermal
conductivity, defined according to the turbulence model being used). The first term on
the right-hand side of Equation 16.4-7 represents energy transfer due to conduction. SE
includes any other volumetric heat sources.
In Equation 16.4-7,
Ek = hk −
p
v2
+ k
ρk
2
(16.4-8)
for a compressible phase, and Ek = hk for an incompressible phase, where hk is the
sensible enthalpy for phase k.
16.4.5
Relative (Slip) Velocity and the Drift Velocity
The relative velocity (also referred to as the slip velocity) is defined as the velocity of a
secondary phase (p) relative to the velocity of the primary phase (q):
~vpq = ~vp − ~vq
(16.4-9)
The mass fraction for any phase (k) is defined as
ck =
αk ρk
ρm
(16.4-10)
The drift velocity and the relative velocity (~vqp ) are connected by the following expression:
~vdr,p = ~vpq −
n
X
ck~vqk
(16.4-11)
k=1
ANSYS FLUENT’s mixture model makes use of an algebraic slip formulation. The basic
assumption of the algebraic slip mixture model is that to prescribe an algebraic relation
for the relative velocity, a local equilibrium between the phases should be reached over
a short spatial length scale. Following Manninen et al. [217], the form of the relative
velocity is given by:
Release 12.0 c ANSYS, Inc. January 29, 2009
16-33
Multiphase Flows
~vpq =
τp (ρp − ρm )
~a
fdrag
ρp
(16.4-12)
ρp d2p
18µq
(16.4-13)
where τp is the particle relaxation time
τp =
d is the diameter of the particles (or droplets or bubbles) of secondary phase p, ~a is the
secondary-phase particle’s acceleration. The default drag function fdrag is taken from
Schiller and Naumann [305]:
(
fdrag =
1 + 0.15 Re0.687 Re ≤ 1000
0.0183 Re
Re > 1000
(16.4-14)
and the acceleration ~a is of the form
~a = ~g − (~vm · ∇)~vm −
∂~vm
∂t
(16.4-15)
The simplest algebraic slip formulation is the so-called drift flux model, in which the acceleration of the particle is given by gravity and/or a centrifugal force and the particulate
relaxation time is modified to take into account the presence of other particles.
In turbulent flows the relative velocity should contain a diffusion term due to the dispersion appearing in the momentum equation for the dispersed phase. ANSYS FLUENT
adds this dispersion to the relative velocity:
~vpq
(ρp − ρm )d2p
ηt
~a −
=
18µq fdrag
σt
∇αp ∇αq
−
αp
αq
!
(16.4-16)
where σt is a Prandtl/Schmidt number set to 0.75 and ηt is the turbulent diffusivity. This
diffusivity is calculated from the continuous-dispersed fluctuating velocity correlation,
such that
k2
ηt = Cµ
#
γγ
(1 + Cβ ζγ2 )−1/2
1 + γγ
|~vpq |
ζγ = q
2/3k
16-34
(16.4-17)
(16.4-18)
Release 12.0 c ANSYS, Inc. January 29, 2009
16.4 Mixture Model Theory
where
Cβ = 1.8 − 1.35 cos2 θ
and
cos θ =
~vpq · ~vp
|~vpq ||~vp |
γγ is the time ratio between the time scale of the energetic turbulent eddies affected by
the crossing-trajectories effect and the particle relaxation time.
When you are solving a mixture multiphase calculation with slip velocity, you can directly
prescribe formulations for the drag function. The following choices are available:
• Schiller-Naumann (the default formulation)
• Morsi-Alexander
• symmetric
• constant
• user-defined
See Section 16.5.4: Interphase Exchange Coefficients for more information on these drag
functions and their formulations, and Section 24.4.1: Defining the Phases for the Mixture
Model in the separate User’s Guide for instructions on how to enable them.
Note that, if the slip velocity is not solved, the mixture model is reduced to a homogeneous
multiphase model. In addition, the mixture model can be customized (using user-defined
functions) to use a formulation other than the algebraic slip method for the slip velocity.
See the separate UDF Manual for details.
16.4.6
Volume Fraction Equation for the Secondary Phases
From the continuity equation for secondary phase p, the volume fraction equation for
secondary phase p can be obtained:
n
X
∂
(αp ρp ) + ∇ · (αp ρp~vm ) = −∇ · (αp ρp~vdr,p ) + (ṁqp − ṁpq )
∂t
q=1
Release 12.0 c ANSYS, Inc. January 29, 2009
(16.4-19)
16-35
Multiphase Flows
16.4.7
Granular Properties
Since the concentration of particles is an important factor in the calculation of the effective viscosity for the mixture, we may use the granular viscosity to get a value for the
viscosity of the suspension. The volume weighted averaged for the viscosity would now
contain shear viscosity arising from particle momentum exchange due to translation and
collision.
The collisional and kinetic parts, and the optional frictional part, are added to give the
solids shear viscosity:
µs = µs,col + µs,kin + µs,fr
(16.4-20)
Collisional Viscosity
The collisional part of the shear viscosity is modeled as [110, 343]
4
Θs
= αs ρs ds g0,ss (1 + ess )
5
π
µs,col
1/2
αs
(16.4-21)
Kinetic Viscosity
ANSYS FLUENT provides two expressions for the kinetic viscosity.
The default expression is from Syamlal et al. [343]:
µs,kin
√
αs ds ρs Θs π
2
=
1 + (1 + ess ) (3ess − 1) αs g0,ss
6 (3 − ess )
5
(16.4-22)
The following optional expression from Gidaspow et al. [110] is also available:
µs,kin
16-36
√
2
10ρs ds Θs π
4
=
1 + g0,ss αs (1 + ess ) αs
96αs (1 + ess ) g0,ss
5
(16.4-23)
Release 12.0 c ANSYS, Inc. January 29, 2009
16.4 Mixture Model Theory
16.4.8
Granular Temperature
The viscosities need the specification of the granular temperature for the sth solids phase.
Here we use an algebraic equation from the granular temperature transport equation. This
is only applicable for dense fluidized beds where the convection and the diffusion term
can be neglected under the premise that production and dissipation of granular energy
are in equilibrium.
0 = (−ps I + τ s ) : ∇~vs − γΘs + φls
(16.4-24)
where
(−ps I + τ s ) : ∇~vs
γΘs
φls
= the generation of energy by the solid stress tensor
= the collisional dissipation of energy
= the energy exchange between the lth
fluid or solid phase and the sth solid phase
The collisional dissipation of energy, γΘs , represents the rate of energy dissipation within
the sth solids phase due to collisions between particles. This term is represented by the
expression derived by Lun et al. [208]
γΘm =
12(1 − e2ss )g0,ss
√
ρs αs2 Θ3/2
s
ds π
(16.4-25)
The transfer of the kinetic energy of random fluctuations in particle velocity from the sth
solids phase to the lth fluid or solid phase is represented by φls [110]:
φls = −3Kls Θs
(16.4-26)
ANSYS FLUENT allows you to solve for the granular temperature with the following
options:
• algebraic formulation (the default)
This is obtained by neglecting convection and diffusion in the transport equation
(Equation 16.4-24) [343].
• constant granular temperature
This is useful in very dense situations where the random fluctuations are small.
• UDF for granular temperature
Release 12.0 c ANSYS, Inc. January 29, 2009
16-37
Multiphase Flows
16.4.9
Interfacial Area Concentration
Interfacial area concentration is defined as the interfacial area between two phases per
unit mixture volume. This is an important parameter for predicting mass, momentum
and energy transfers through the interface between the phases. In two-fluid flow systems,
one discrete (particles) and one continuous, the size and its distribution of the discrete
phase or particles can change rapidly due to growth (mass transfer between phases), expansion due to pressure changes, coalescence, breakage and/or nucleation mechanisms.
The Population Balance model (see the separate Population Balance Module Manual)
ideally captures this phenomenon, but is computationally expensive since several transport equations need to be solved using moment methods, or more if the discrete method
is used. The interfacial area concentration model uses a single transport equation per
secondary phase and is specific to bubbly flows in liquid at this stage.
The transport equation for the interfacial area concentration can be written as
1 Dρg
2 ṁg
∂(ρg χp )
+ ∇ · (ρg ~ug χp ) =
χp +
χp + ρg (SRC + SW E + ST I )
∂t
3 Dt
3 αg
(16.4-27)
where χp is the interfacial area concentration (m2 /m3 ), and αg is the gas volume fraction.
The first two terms on the right hand side of Equation 16.4-27 are of gas bubble expansion
due to compressibility and mass transfer (phase change). ṁg is the mass transfer rate into
the gas phase per unit mixture volume (kg/m3 /s). SRC and SW E are the coalescence sink
terms due to random collision and wake entrainment, respectively. ST I is the breakage
source term due to turbulent impact.
Two sets of models, the Hibiki-Ishii model [129] and the Ishii-Kim model [281, 139], exist
for those source and sink terms for the interfacial area concentration, which are based
on the works of Ishii et al. [129, 281]. According to their study, the mechanisms of
interactions can be summarized in five categories:
• Coalescence due to random collision driven by turbulence.
• Breakage due to the impact of turbulent eddies.
• Coalescence due to wake entrainment.
• Shearing-off of small bubbles from large cap bubbles.
• Breakage of large cap bubbles due to flow instability on the bubble surface.
In ANSYS FLUENT, only the first three effects will be considered.
16-38
Release 12.0 c ANSYS, Inc. January 29, 2009
16.4 Mixture Model Theory
Hibiki-Ishii Model
SRC = −
1 αg 2
( ) fc nb λc
3φ χp
= −(
= −
(16.4-28)
αg 2
Γc αg 2 1/3
db 5/6 ρf 1/2 1/3
) 11/3
exp(−Kc
)
χp db (αgmax − αg )
σ 1/2
1/2 1/3
Γc
1/3
αg 5/6
1/3
5/3
5/6 ρf
α
χ
exp[−K
ψ
(
) ]
g
p
c
ψ 11/3 (αgmax − αg )
σ 1/2
χp
where fc , λc and nb are the frequency of particle/bubble collision, the efficiency of coalescence from the collision, and the number of particles per unit mixture volume, respectively. The averaged size of the particle/bubble db is assumed to be calculated as
db = ψ
αg
χp
(16.4-29)
and
λc = exp(−Kc
ST I =
=(
db 5/6 ρf 1/2 1/3
)
σ 1/2
1 αg 2
( ) fB ne λB
3φ χp
(16.4-30)
(16.4-31)
αg 2 ΓB αg (1 − αg )1/3
σ
) 11/3
exp(−KB
)
5/3
χp db (αgmax − αg )
ρf db 2/3
ΓB (1 − αg )1/3 χp 5/3
KB σ
χp
= 11/3 2/3
exp[− 5/3
( )5/3 ]
2/3
ψ
αg (αgmax − αg )
ψ ρf
αg
where fB , λB and ne are the frequency of collision between particles/bubbles and turbulent eddies of the primary phase, the efficiency of breakage from the impact, and the
number of turbulent eddies per unit mixture volume, respectively. In Equation 16.4-31
λB = exp(−KB
σ
ρf db
5/3 2/3
)
(16.4-32)
The experimental adjustable coefficients are given as follows:
ΓC = 0.188; KC = 0.129; ΓB = 0.264; KB = 1.37 .
1
The shape factor ψ is given as 6 and φ as 36π
for spherical particles/bubbles. There is
no model for SW E in the Hibiki-Ishii formulation.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-39
Multiphase Flows
Ishii-Kim Model
nb 2 ut db 2
1 αg 2
( ) CRC [
]
(16.4-33)
3φ χp
αgmax 1/3 (αgmax 1/3 − αg 1/3 )
αgmax 1/3 αg 1/3
[1 − exp(−C
)]
αgmax 1/3 − αg 1/3
1
1
αgmax 1/3 αg 1/3
= − CRC ut χp 2 [
][1
−
exp(−C
)]
3π
αgmax 1/3 (αgmax 1/3 − αg 1/3 )
αgmax 1/3 − αg 1/3
SRC = −
SW E = −
1 αg 2 2 2
1
( ) nb db ur CD 1/3 = − CW E ur χp 2 CD 1/3
3φ χp
3π
1 αg 2
n b ut
W ecr 1/2
W ecr
( ) CT I (
)(1 −
) exp(−
)
3φ χp
db
We
We
1
χp 2
W ecr 1/2
W ecr
=
CT I ut
(1 −
) exp(−
)
18
αg
We
We
ST I =
(16.4-34)
(16.4-35)
where the mean bubble fluctuating velocity, ut , is given by 1/3 db 1/3 . The bubble terminal
velocity, ur , is a function of the bubble diameter and local time-averaged void fraction.
ur = (
CD = 24
db g∆ρ 1/2
)
3CD ρf
(16.4-36)
(1 + 0.1ReD 0.75 )
ρf ur db
and ReD ≡
(1 − αg )
ReD
µf
We =
ρf ut 2 db
σ
(16.4-37)
(16.4-38)
where µf is the molecular viscosity of the fluid phase, g is the gravitational acceleration
and σ is the interfacial tension. In this model, when the Weber number, W e, is less
than the critical Weber number, W ecr , the breakage rate equals zero, i.e. ST I = 0. The
coefficients used are given as follows [139]:
CRC
CW E
CT I
C
W ecr
αgm ax
16-40
= 0.004
= 0.002
= 0.085
= 3.0
= 6.0
= 0.75
Release 12.0 c ANSYS, Inc. January 29, 2009
16.5 Eulerian Model Theory
i
Currently, this model is only suitable for two-phase flow regimes, one phase
being gas and another liquid, i.e. bubbly column applications. However,
you can always use UDFs to include your own interfacial area concentration
models, which can apply to other flow regimes.
See the separate UDF Manual for details.
16.4.10
Solids Pressure
The total solid pressure is calculated and included in the mixture momentum equations:
Ps,total =
N
X
pq
(16.4-39)
q=1
where pq is presented in the section for granular flows by equation Equation 16.5-67
16.5
Eulerian Model Theory
Details about the Eulerian multiphase model are presented in the following subsections:
• Section 16.5.1: Overview and Limitations of the Eulerian Model
• Section 16.5.2: Volume Fraction Equation
• Section 16.5.3: Conservation Equations
• Section 16.5.4: Interphase Exchange Coefficients
• Section 16.5.5: Solids Pressure
• Section 16.5.6: Maximum Packing Limit in Binary Mixtures
• Section 16.5.7: Solids Shear Stresses
• Section 16.5.8: Granular Temperature
• Section 16.5.9: Interfacial Area Concentration
• Section 16.5.10: Description of Heat Transfer
• Section 16.5.11: Turbulence Models
• Section 16.5.12: Solution Method in ANSYS FLUENT
• Section 16.5.13: Dense Discrete Phase Model
• Section 16.5.14: Immiscible Fluid Model
Release 12.0 c ANSYS, Inc. January 29, 2009
16-41
Multiphase Flows
16.5.1
Overview and Limitations of the Eulerian Model
Overview
The Eulerian multiphase model in ANSYS FLUENT allows for the modeling of multiple
separate, yet interacting phases. The phases can be liquids, gases, or solids in nearly any
combination. An Eulerian treatment is used for each phase, in contrast to the EulerianLagrangian treatment that is used for the discrete phase model.
With the Eulerian multiphase model, the number of secondary phases is limited only
by memory requirements and convergence behavior. Any number of secondary phases
can be modeled, provided that sufficient memory is available. For complex multiphase
flows, however, you may find that your solution is limited by convergence behavior. See
Section 24.7.5: Eulerian Model in the separate User’s Guide for multiphase modeling
strategies.
ANSYS FLUENT’s Eulerian multiphase model does not distinguish between fluid-fluid
and fluid-solid (granular) multiphase flows. A granular flow is simply one that involves
at least one phase that has been designated as a granular phase.
The ANSYS FLUENT solution is based on the following:
• A single pressure is shared by all phases.
• Momentum and continuity equations are solved for each phase.
• The following parameters are available for granular phases:
– Granular temperature (solids fluctuating energy) can be calculated for each
solid phase. You can select either an algebraic formulation, a constant, a
user-defined function, or a partial differential equation.
– Solid-phase shear and bulk viscosities are obtained by applying kinetic theory to granular flows. Frictional viscosity for modeling granular flow is also
available. You can select appropriate models and user-defined functions for
all properties.
• Several interphase drag coefficient functions are available, which are appropriate
for various types of multiphase regimes. (You can also modify the interphase drag
coefficient through user-defined functions, as described in the separate UDF Manual.)
• All of the k- turbulence models are available, and may apply to all phases or to
the mixture.
16-42
Release 12.0 c ANSYS, Inc. January 29, 2009
16.5 Eulerian Model Theory
Limitations
All other features available in ANSYS FLUENT can be used in conjunction with the
Eulerian multiphase model, except for the following limitations:
• The Reynolds Stress turbulence model is not available on a per phase basis.
• Particle tracking (using the Lagrangian dispersed phase model) interacts only with
the primary phase.
• Streamwise periodic flow with specified mass flow rate cannot be modeled when
the Eulerian model is used (the user is allowed to specify a pressure drop).
• Inviscid flow is not allowed.
• Melting and solidification are not allowed.
• When tracking particles in parallel, the DPM model cannot be used with the Eulerian multiphase model if the shared memory option is enabled (Section 23.8: Parallel
Processing for the Discrete Phase Model in the separate User’s Guide). (Note that
using the message passing option, when running in parallel, enables the compatibility of all multiphase flow models with the DPM model.)
To change from a single-phase model, where a single set of conservation equations for
momentum, continuity and (optionally) energy is solved, to a multiphase model, additional sets of conservation equations must be introduced. In the process of introducing additional sets of conservation equations, the original set must also be modified.
The modifications involve, among other things, the introduction of the volume fractions
α1 , α2 , . . . αn for the multiple phases, as well as mechanisms for the exchange of momentum, heat, and mass between the phases.
16.5.2
Volume Fraction Equation
The description of multiphase flow as interpenetrating continua incorporates the concept
of phasic volume fractions, denoted here by αq . Volume fractions represent the space
occupied by each phase, and the laws of conservation of mass and momentum are satisfied
by each phase individually. The derivation of the conservation equations can be done by
ensemble averaging the local instantaneous balance for each of the phases [5] or by using
the mixture theory approach [31].
Release 12.0 c ANSYS, Inc. January 29, 2009
16-43
Multiphase Flows
The volume of phase q, Vq , is defined by
Vq =
Z
V
αq dV
(16.5-1)
where
n
X
αq = 1
(16.5-2)
ρ̂q = αq ρq
(16.5-3)
q=1
The effective density of phase q is
where ρq is the physical density of phase q.
The volume fraction equation may be solved either through implicit or explicit time discretization. For detailed information about both VOF schemes, refer to Section 16.3.2: The
Implicit Scheme and Section 16.3.2: The Explicit Scheme.
16.5.3
Conservation Equations
The general conservation equations from which the equations solved by ANSYS FLUENT
are derived are presented in this section, followed by the solved equations themselves.
Equations in General Form
Conservation of Mass
The continuity equation for phase q is
n
X
∂
(αq ρq ) + ∇ · (αq ρq~vq ) =
(ṁpq − ṁqp ) + Sq
∂t
p=1
(16.5-4)
where ~vq is the velocity of phase q and ṁpq characterizes the mass transfer from the pth
to q th phase, and ṁqp characterizes the mass transfer from phase q to phase p, and you
are able to specify these mechanisms separately.
By default, the source term Sq on the right-hand side of Equation 16.5-4 is zero, but
you can specify a constant or user-defined mass source for each phase. A similar term
appears in the momentum and enthalpy equations. See Section 16.7: Modeling Mass
Transfer in Multiphase Flows for more information on the modeling of mass transfer in
ANSYS FLUENT’s general multiphase models.
16-44
Release 12.0 c ANSYS, Inc. January 29, 2009
16.5 Eulerian Model Theory
Conservation of Momentum
The momentum balance for phase q yields
∂
(αq ρq~vq ) + ∇ · (αq ρq~vq~vq ) = −αq ∇p + ∇ · τ q + αq ρq~g +
∂t
n
X
~ pq + ṁpq~vpq − ṁqp~vqp ) + (F~q + F~lift,q + F~vm,q )
(R
(16.5-5)
p=1
where τ q is the q th phase stress-strain tensor
2
τ q = αq µq (∇~vq + ∇~vqT ) + αq (λq − µq )∇ · ~vq I
3
(16.5-6)
Here µq and λq are the shear and bulk viscosity of phase q, F~q is an external body force,
~ pq is an interaction force between
F~lift,q is a lift force, F~vm,q is a virtual mass force, R
phases, and p is the pressure shared by all phases.
~vpq is the interphase velocity, defined as follows. If ṁpq > 0 (i.e., phase p mass is being
transferred to phase q), ~vpq = ~vp ; if ṁpq < 0 (i.e., phase q mass is being transferred to
phase p), ~vpq = ~vq . Likewise, if ṁqp > 0 then vqp = vq , if ṁqp < 0 then vqp = vp .
~ pq .
Equation 16.5-5 must be closed with appropriate expressions for the interphase force R
This force depends on the friction, pressure, cohesion, and other effects, and is subject
~ pq = −R
~ qp and R
~ qq = 0.
to the conditions that R
ANSYS FLUENT uses a simple interaction term of the following form:
n
X
p=1
~ pq =
R
n
X
Kpq (~vp − ~vq )
(16.5-7)
p=1
where Kpq (= Kqp ) is the interphase momentum exchange coefficient (described in Section 16.5.4: Interphase Exchange Coefficients).
Lift Forces
For multiphase flows, ANSYS FLUENT can include the effect of lift forces on the secondary
phase particles (or droplets or bubbles). These lift forces act on a particle mainly due to
velocity gradients in the primary-phase flow field. The lift force will be more significant
for larger particles, but the ANSYS FLUENT model assumes that the particle diameter
is much smaller than the interparticle spacing. Thus, the inclusion of lift forces is not
appropriate for closely packed particles or for very small particles.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-45
Multiphase Flows
The lift force acting on a secondary phase p in a primary phase q is computed from [80]
F~lift = −0.5ρq αp (~vq − ~vp ) × (∇ × ~vq )
(16.5-8)
The lift force F~lift will be added to the right-hand side of the momentum equation for
both phases (F~lift,q = −F~lift,p ).
In most cases, the lift force is insignificant compared to the drag force, so there is no
reason to include this extra term. If the lift force is significant (e.g., if the phases separate
quickly), it may be appropriate to include this term. By default, F~lift is not included.
The lift force and lift coefficient can be specified for each pair of phases, if desired.
i
It is important that if you include the lift force in your calculation, you
need not include it everywhere in the computational domain since it is
computationally expensive to converge. For example, in the wall boundary
layer for turbulent bubbly flows in channels, the lift force is significant
when the slip velocity is large in the vicinity of high strain rates for the
primary phase.
Virtual Mass Force
For multiphase flows, ANSYS FLUENT includes the “virtual mass effect” that occurs
when a secondary phase p accelerates relative to the primary phase q. The inertia of the
primary-phase mass encountered by the accelerating particles (or droplets or bubbles)
exerts a “virtual mass force” on the particles [80]:
F~vm = 0.5αp ρq
The term
dq
dt
dq~vq dp~vp
−
dt
dt
!
(16.5-9)
denotes the phase material time derivative of the form
dq (φ)
∂(φ)
=
+ (~vq · ∇)φ
dt
∂t
(16.5-10)
The virtual mass force F~vm will be added to the right-hand side of the momentum equation
for both phases (F~vm,q = −F~vm,p ).
The virtual mass effect is significant when the secondary phase density is much smaller
than the primary phase density (e.g., for a transient bubble column). By default, F~vm is
not included.
16-46
Release 12.0 c ANSYS, Inc. January 29, 2009
16.5 Eulerian Model Theory
Conservation of Energy
To describe the conservation of energy in Eulerian multiphase applications, a separate
enthalpy equation can be written for each phase:
n
X
∂
∂pq
(αq ρq hq ) + ∇ · (αq ρq ~uq hq ) = αq
+ τ q : ∇~uq − ∇ · ~qq + Sq + (Qpq + ṁpq hpq − ṁqp hqp )
∂t
∂t
p=1
(16.5-11)
where hq is the specific enthalpy of the q th phase, ~qq is the heat flux, Sq is a source term
that includes sources of enthalpy (e.g., due to chemical reaction or radiation), Qpq is
the intensity of heat exchange between the pth and q th phases, and hpq is the interphase
enthalpy (e.g., the enthalpy of the vapor at the temperature of the droplets, in the case
of evaporation). The heat exchange between phases must comply with the local balance
conditions Qpq = −Qqp and Qqq = 0.
Equations Solved by ANSYS FLUENT
The equations for fluid-fluid and granular multiphase flows, as solved by ANSYS FLUENT,
are presented here for the general case of an n-phase flow.
Continuity Equation
The volume fraction of each phase is calculated from a continuity equation:
n
X
1 ∂
(αq ρq ) + ∇ · (αq ρq~vq ) =
(ṁpq − ṁqp )
ρrq ∂t
p=1
(16.5-12)
where ρrq is the phase reference density, or the volume averaged density of the q th phase
in the solution domain.
The solution of this equation for each secondary phase, along with the condition that the
volume fractions sum to one (given by Equation 16.5-2), allows for the calculation of the
primary-phase volume fraction. This treatment is common to fluid-fluid and granular
flows.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-47
Multiphase Flows
Fluid-Fluid Momentum Equations
The conservation of momentum for a fluid phase q is
∂
(αq ρq~vq ) + ∇ · (αq ρq~vq~vq ) = −αq ∇p + ∇ · τ q + αq ρq~g +
∂t
n
X
(Kpq (~vp − ~vq ) + ṁpq~vpq − ṁqp~vqp ) +
p=1
(F~q + F~lift,q + F~vm,q )
(16.5-13)
Here ~g is the acceleration due to gravity and τ q , F~q , F~lift,q , and F~vm,q are as defined for
Equation 16.5-5.
Fluid-Solid Momentum Equations
Following the work of [3, 49, 71, 110, 183, 208, 254, 343], ANSYS FLUENT uses a multifluid granular model to describe the flow behavior of a fluid-solid mixture. The solid-phase
stresses are derived by making an analogy between the random particle motion arising
from particle-particle collisions and the thermal motion of molecules in a gas, taking into
account the inelasticity of the granular phase. As is the case for a gas, the intensity of the
particle velocity fluctuations determines the stresses, viscosity, and pressure of the solid
phase. The kinetic energy associated with the particle velocity fluctuations is represented
by a “pseudothermal” or granular temperature which is proportional to the mean square
of the random motion of particles.
The conservation of momentum for the fluid phases is similar to Equation 16.5-13, and
that for the sth solid phase is
∂
(αs ρs~vs ) + ∇ · (αs ρs~vs~vs ) = −αs ∇p − ∇ps + ∇ · τ s + αs ρs~g +
∂t
N
X
(Kls (~vl − ~vs ) + ṁls~vls − ṁsl~vsl ) +
l=1
(F~s + F~lift,s + F~vm,s )
(16.5-14)
where ps is the sth solids pressure, Kls = Ksl is the momentum exchange coefficient
between fluid or solid phase l and solid phase s, N is the total number of phases, and
F~q , F~lift,q , and F~vm,q are as defined for Equation 16.5-5.
16-48
Release 12.0 c ANSYS, Inc. January 29, 2009
16.5 Eulerian Model Theory
Conservation of Energy
The equation solved by ANSYS FLUENT for the conservation of energy is Equation 16.5-11.
16.5.4
Interphase Exchange Coefficients
It can be seen in Equations 16.5-13 and 16.5-14 that momentum exchange between the
phases is based on the value of the fluid-fluid exchange coefficient Kpq and, for granular
flows, the fluid-solid and solid-solid exchange coefficients Kls .
Fluid-Fluid Exchange Coefficient
For fluid-fluid flows, each secondary phase is assumed to form droplets or bubbles. This
has an impact on how each of the fluids is assigned to a particular phase. For example,
in flows where there are unequal amounts of two fluids, the predominant fluid should be
modeled as the primary fluid, since the sparser fluid is more likely to form droplets or
bubbles. The exchange coefficient for these types of bubbly, liquid-liquid or gas-liquid
mixtures can be written in the following general form:
Kpq =
αq αp ρp f
τp
(16.5-15)
where f , the drag function, is defined differently for the different exchange-coefficient
models (as described below) and τp , the “particulate relaxation time”, is defined as
ρp d2p
τp =
18µq
(16.5-16)
where dp is the diameter of the bubbles or droplets of phase p.
Nearly all definitions of f include a drag coefficient (CD ) that is based on the relative
Reynolds number (Re). It is this drag function that differs among the exchange-coefficient
models. For all these situations, Kpq should tend to zero whenever the primary phase is
not present within the domain. To enforce this, the drag function f is always multiplied
by the volume fraction of the primary phase q, as is reflected in Equation 16.5-15.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-49
Multiphase Flows
• For the model of Schiller and Naumann [305]
f=
CD Re
24
(16.5-17)
where
(
CD =
24(1 + 0.15 Re0.687 )/Re Re ≤ 1000
0.44
Re > 1000
(16.5-18)
and Re is the relative Reynolds number. The relative Reynolds number for the
primary phase q and secondary phase p is obtained from
Re =
ρq |~vp − ~vq |dp
µq
(16.5-19)
The relative Reynolds number for secondary phases p and r is obtained from
Re =
ρrp |~vr − ~vp |drp
µrp
(16.5-20)
where µrp = αp µp + αr µr is the mixture viscosity of the phases p and r.
The Schiller and Naumann model is the default method, and it is acceptable for
general use for all fluid-fluid pairs of phases.
• For the Morsi and Alexander model [238]
f=
CD Re
24
(16.5-21)
where
CD = a1 +
16-50
a2
a3
+ 2
Re Re
(16.5-22)
Release 12.0 c ANSYS, Inc. January 29, 2009
16.5 Eulerian Model Theory
and Re is defined by Equation 16.5-19 or 16.5-20. The a’s are defined as follows:
a1 , a2 , a3 =
0, 24, 0
3.690, 22.73, 0.0903
1.222, 29.1667, −3.8889
0 < Re < 0.1
0.1 < Re < 1
1 < Re < 10
0.6167, 46.50, −116.67
10 < Re < 100
0.3644, 98.33, −2778
100 < Re < 1000
0.357, 148.62, −47500
1000 < Re < 5000
0.46, −490.546, 578700
5000 < Re < 10000
0.5191, −1662.5, 5416700 Re ≥ 10000
(16.5-23)
The Morsi and Alexander model is the most complete, adjusting the function definition frequently over a large range of Reynolds numbers, but calculations with
this model may be less stable than with the other models.
• For the symmetric model
Kpq =
αp (αp ρp + αq ρq )f
τpq
(16.5-24)
where
τpq
q 2
)
(αp ρp + αq ρq )( dp +d
2
=
18(αp µp + αq µq )
(16.5-25)
and
f=
CD Re
24
(16.5-26)
where
(
CD =
24(1 + 0.15 Re0.687 )/Re Re ≤ 1000
0.44
Re > 1000
(16.5-27)
and Re is defined by Equation 16.5-19 or 16.5-20. Note that if there is only one
dispersed phase, then dp = dq in Equation 16.5-25.
The symmetric model is recommended for flows in which the secondary (dispersed)
phase in one region of the domain becomes the primary (continuous) phase in
q)
another. Thus for a single dispersed phase, dp = dq and (dp +d
= dp . For example,
2
if air is injected into the bottom of a container filled halfway with water, the air
is the dispersed phase in the bottom half of the container; in the top half of the
container, the air is the continuous phase. This model can also be used for the
interaction between secondary phases.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-51
Multiphase Flows
You can specify different exchange coefficients for each pair of phases. It is also possible
to use user-defined functions to define exchange coefficients for each pair of phases. If the
exchange coefficient is equal to zero (i.e., if no exchange coefficient is specified), the flow
fields for the fluids will be computed independently, with the only “interaction” being
their complementary volume fractions within each computational cell.
Fluid-Solid Exchange Coefficient
The fluid-solid exchange coefficient Ksl can be written in the following general form:
Ksl =
αs ρs f
τs
(16.5-28)
where f is defined differently for the different exchange-coefficient models (as described
below), and τs , the “particulate relaxation time”, is defined as
τs =
ρs d2s
18µl
(16.5-29)
where ds is the diameter of particles of phase s.
All definitions of f include a drag function (CD ) that is based on the relative Reynolds
number (Res ). It is this drag function that differs among the exchange-coefficient models.
• For the Syamlal-O’Brien model [342]
f=
CD Res αl
2
24vr,s
(16.5-30)
where the drag function has a form derived by Dalla Valle [66]
CD = 0.63 + q
4.8
Res /vr,s
2
(16.5-31)
This model is based on measurements of the terminal velocities of particles in
fluidized or settling beds, with correlations that are a function of the volume fraction
and relative Reynolds number [294]:
Res =
ρl ds |~vs − ~vl |
µl
(16.5-32)
where the subscript l is for the lth fluid phase, s is for the sth solid phase, and ds is
the diameter of the sth solid phase particles.
16-52
Release 12.0 c ANSYS, Inc. January 29, 2009
16.5 Eulerian Model Theory
The fluid-solid exchange coefficient has the form
!
3αs αl ρl
Res
Ksl =
CD
|~vs − ~vl |
2
4vr,s ds
vr,s
(16.5-33)
where vr,s is the terminal velocity correlation for the solid phase [105]:
vr,s = 0.5 A − 0.06 Res +
q
2
(0.06 Res ) + 0.12 Res (2B − A) +
A2
(16.5-34)
with
A = αl4.14
(16.5-35)
B = 0.8αl1.28
(16.5-36)
B = αl2.65
(16.5-37)
and
for αl ≤ 0.85, and
for αl > 0.85.
This model is appropriate when the solids shear stresses are defined according to
Syamlal et al. [343] (Equation 16.5-83).
• For the model of Wen and Yu [373], the fluid-solid exchange coefficient is of the
following form:
3
αs αl ρl |~vs − ~vl | −2.65
Ksl = CD
αl
4
ds
(16.5-38)
where
CD =
i
24 h
1 + 0.15(αl Res )0.687
αl Res
(16.5-39)
and Res is defined by Equation 16.5-32.
This model is appropriate for dilute systems.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-53
Multiphase Flows
• The Gidaspow model [110] is a combination of the Wen and Yu model [373] and
the Ergun equation [88].
When αl > 0.8, the fluid-solid exchange coefficient Ksl is of the following form:
3
αs αl ρl |~vs − ~vl | −2.65
Ksl = CD
αl
4
ds
(16.5-40)
where
CD =
i
24 h
1 + 0.15(αl Res )0.687
αl Res
(16.5-41)
αs (1 − αl )µl
ρl αs |~vs − ~vl |
+ 1.75
2
αl ds
ds
(16.5-42)
When αl ≤ 0.8,
Ksl = 150
This model is recommended for dense fluidized beds.
Solid-Solid Exchange Coefficient
The solid-solid exchange coefficient Kls has the following form [341]:
Kls =
3 (1 + els )
π
2
2
+ Cfr,ls π8 αs ρs αl ρl (dl + ds )2 g0,ls
2π (ρl d3l + ρs d3s )
|~vl − ~vs |
(16.5-43)
where
els
Cfr,ls
dl
g0,ls
=
=
the coefficient of restitution
the coefficient of friction between the lth and sth
solid-phase particles (Cfr,ls = 0)
= the diameter of the particles of solid l
= the radial distribution coefficient
Note that the coefficient of restitution is described in Section 16.5.5: Solids Pressure
and the radial distribution coefficient is described in Section 16.5.5: Radial Distribution
Function.
16-54
Release 12.0 c ANSYS, Inc. January 29, 2009
16.5 Eulerian Model Theory
Universal Drag Laws for Bubble-Liquid and Droplet-Gas Flows
The universal drag laws [170] are suitable for the calculation of the drag coefficients
in bubble-liquid or droplet-gas flow regimes. The drag laws can apply to non-spherical
particles with the constraint of a pool flow regime, i.e. the hydraulic diameter of the flow
domain which is far larger than the averaged size of the particles.
The exchange coefficient for bubbly and droplet flows can be written in the general form
Kpq =
αq αp ρp f
τp
(16.5-44)
Where q represents the primary phase and p the particulate phase. The particulate
relaxation time τp is defined as
τp =
ρp dp 2
18µe
(16.5-45)
f=
CD Re
24
(16.5-46)
The drag function f is defined as
The relative Reynolds number for the primary phase q and the secondary phase p is
obtained based on the relative velocity of the two phases.
Re =
ρq |v~q − v~p |dp
µe
(16.5-47)
Where µe is the effective viscosity of the primary phase accounting for the effects of
family of particles in the continuum.
The Rayleigh-Taylor instability wavelength is
λRT =
σ
g∆ρpq
!0.5
(16.5-48)
Where σ is the surface tension, g the gravity, and ∆ρpq the absolute value of the density
difference between phases p and q.
The drag coefficient is defined differently for bubbly and droplet flows.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-55
Multiphase Flows
Bubble-Liquid Flow
CDvis =
24
(1 + 0.1Re0.75 )
Re
dp
1 + 17.67f ∗ 6/7
= 2/3(
)
λRT
18.67f ∗
(
CDdis
(16.5-49)
)2
; f ∗ = (1 − αp )1.5
8
CDcap = (1 − αp )2
3
(16.5-50)
(16.5-51)
• In the viscous regime, the following condition is satisfied:
CDdis < CDvis
(16.5-52)
The drag coefficient, CD , is computed as
CD = CDvis
(16.5-53)
• In the distorted bubble regime, the following condition is satisfied:
CDvis < CDdis < CDcap
(16.5-54)
The drag coefficient is calculated as
CD = CDdis
(16.5-55)
• In the regime of strongly deformed, capped bubbles, the following condition is
satisfied:
CDdis > CDcap
(16.5-56)
The drag coefficient can be written as
CD = CDcap
(16.5-57)
The effective viscosity for the bubble-liquid mixture is
µe =
16-56
µq
1 − αp
(16.5-58)
Release 12.0 c ANSYS, Inc. January 29, 2009
16.5 Eulerian Model Theory
Droplet-Gas Flow
• When Re < 1, the drag coefficient for the stokes regime is
CD =
24
Re
(16.5-59)
• When 1 ≤ Re ≤ 1000, the drag coefficient for the viscous regime is
CD =
24
(1 + 0.1Re0.75 )
Re
(16.5-60)
• For the Newton’s regime (Re ≥ 1000), the drag coefficient is
dp
1 + 17.67f ∗ 6/7
)
CD = 2/3(
λRT
18.67f ∗
(
)2
; f ∗ = (1 − αp )3
(16.5-61)
The effective viscosity for a bubble-liquid mixture is
µe =
i
16.5.5
µq
(1 − αp )2.5
(16.5-62)
The drag model is currently suitable for bubble-liquid and/or droplet-gas
flow when the characteristic length of the flow domain is much larger than
the averaged size of the particles.
Solids Pressure
For granular flows in the compressible regime (i.e., where the solids volume fraction is less
than its maximum allowed value), a solids pressure is calculated independently and used
for the pressure gradient term, ∇ps , in the granular-phase momentum equation. Because
a Maxwellian velocity distribution is used for the particles, a granular temperature is
introduced into the model, and appears in the expression for the solids pressure and
viscosities. The solids pressure is composed of a kinetic term and a second term due to
particle collisions:
ps = αs ρs Θs + 2ρs (1 + ess )αs2 g0,ss Θs
(16.5-63)
where ess is the coefficient of restitution for particle collisions, g0,ss is the radial distribution function, and Θs is the granular temperature. ANSYS FLUENT uses a default
value of 0.9 for ess , but the value can be adjusted to suit the particle type. The granular
temperature Θs is proportional to the kinetic energy of the fluctuating particle motion,
and will be described later in this section. The function g0,ss (described below in more
detail) is a distribution function that governs the transition from the “compressible”
Release 12.0 c ANSYS, Inc. January 29, 2009
16-57
Multiphase Flows
condition with α < αs,max , where the spacing between the solid particles can continue to
decrease, to the “incompressible” condition with α = αs,max , where no further decrease
in the spacing can occur. A value of 0.63 is the default for αs,max , but you can modify it
during the problem setup.
Other formulations that are also available in ANSYS FLUENT are [343]
ps = 2ρs (1 + ess )αs2 g0,ss Θs
(16.5-64)
and [213]
1
ps = αs ρs Θs [(1 + 4αs g0,ss ) + [(1 + ess )(1 − ess + 2µf ric )]]
(16.5-65)
2
When more than one solids phase are calculated, the above expression does not take into
account the effect of other phases. A derivation of the expressions from the Boltzman
equations for a granular mixture are beyond the scope of this manual, however there is
a need to provide a better formulation so that some properties may feel the presence of
other phases. A known problem is that N solid phases with identical properties should be
consistent when the same phases are described by a single solids phase. Equations derived
empirically may not satisfy this property and need to be changed accordingly without
deviating significantly from the original form. From [109], a general solids pressure
formulation in the presence of other phases could be of the form
pq = αq ρq Θq +
N
X
π
p=1
3
g0,pq d3qp nq np (1 + eqp )f (mp , mq , Θp , Θq )
(16.5-66)
q
where dpq = dp +d
is the average diameter, np , nq are the number of particles, mp and mq
2
are the masses of the particles in phases p and q, and f is a function of the masses of the
particles and their granular temperatures. For now, we have to simplify this expression
so that it depends only on the granular temperature of phase q
pq = αq ρq Θq +
N
X
d3pq
2
p=1
d3q
(1 + epq )g0,pq αq αp ρq Θq
(16.5-67)
Since all models need to be cast in the general form, it follows that
pq = αq ρq Θq + (
N
X
d3pq
p=1
d3q
pc,qp )ρq Θq
(16.5-68)
where pc,qp is the collisional part of the pressure between phases q and p.
The above expression reverts to the one solids phase expression when N = 1 and q = p
but also has the property of feeling the presence of other phases.
16-58
Release 12.0 c ANSYS, Inc. January 29, 2009
16.5 Eulerian Model Theory
Radial Distribution Function
The radial distribution function, g0 , is a correction factor that modifies the probability
of collisions between grains when the solid granular phase becomes dense. This function
may also be interpreted as the nondimensional distance between spheres:
g0 =
s + dp
s
(16.5-69)
where s is the distance between grains. From Equation 16.5-69 it can be observed that
for a dilute solid phase s → ∞, and therefore g0 → 1. In the limit when the solid phase
compacts, s → 0 and g0 → ∞. The radial distribution function is closely connected
to the factor χ of Chapman and Cowling’s [49] theory of nonuniform gases. χ is equal
to 1 for a rare gas, and increases and tends to infinity when the molecules are so close
together that motion is not possible.
In the literature there is no unique formulation for the radial distribution function. ANSYS FLUENT has a number of options:
• For one solids phase, use [254]:
g0 = 1 −
αs
αs,max
! 1 −1
3
(16.5-70)
This is an empirical function and does not extend easily to n phases. For two
identical phases with the property that αq = α1 + α2 , the above function is not
consistent for the calculation of the partial pressures p1 and p2 , pq = p1 +p2 . In order
to correct this problem, ANSYS FLUENT uses the following consistent formulation:
g0,ll = 1 −
αs
αs,max
! 1 −1
N
3
1 X
αk
+ dl
2
k=1
dk
(16.5-71)
where
αs =
N
X
αk
(16.5-72)
k=1
and k are solid phases only.
• The following expression is also available [137]:
g0,ll =
Release 12.0 c ANSYS, Inc. January 29, 2009
N
αk
3 X
d
+
l
αs
(1 − αs,max ) 2 k=1 dk
1
(16.5-73)
16-59
Multiphase Flows
• Also available [213], slightly modified for n solids phases, is the following:
g0,ll =
1 + 2.5αs + 4.59αs2 + 4.52αs3
1−
αs
3 0.678
N
1 X
αk
+ dl
2 k=1 dk
(16.5-74)
αs,max
• The following equation [343] is available:
αk
3( N
1
k=1 dk )
dk dl
=
+
(1 − αs ) (1 − αs )2 (dj + dk )
P
g0,kl
(16.5-75)
When the number of solid phases is greater than 1, Equation 16.5-71, Equation 16.5-73
and Equation 16.5-74 are extended to
g0,lm =
dm g0,ll + dl g0,mm
dm + dl
(16.5-76)
It is interesting to note that Equation 16.5-73 and Equation 16.5-74 compare well with [3]
experimental data, while Equation 16.5-75 reverts to the [46] derivation.
16.5.6
Maximum Packing Limit in Binary Mixtures
The packing limit is not a fixed quantity and may change according to the number of
particles present within a given volume and the diameter of the particles. Small particles
accumulate in between larger particles increasing the packing limit. For a binary mixture
ANSYS FLUENT uses the correlations proposed by [90].
For a binary mixture with diameters d1 > d2 , the mixture composition is defined as
1
X1 = α1α+α
2
where
X1 <=
α1,max
(α1,max + (1 − α1,max )α2,max )
(16.5-77)
as this is a condition for application of the maximum packing limit for binary mixtures.
The maximum packing limit for the mixture is given by
s
d2
](1 − α1,max )α2,max )
d1
X1
∗(α1,max + (1 − α1,max )α2,max )
α1,max
+α2,max
αs,max = (α1,max − α2,max + [1 −
16-60
(16.5-78)
(16.5-79)
Release 12.0 c ANSYS, Inc. January 29, 2009
16.5 Eulerian Model Theory
otherwise, the maximum packing limit for the binary mixture is
s
[1 −
d2
](α1,max + (1 − α1,max )α2,max )(1 − X1 ) + α1,max
d1
(16.5-80)
The packing limit is used for the calculation of the radial distribution function.
16.5.7 Solids Shear Stresses
The solids stress tensor contains shear and bulk viscosities arising from particle momentum exchange due to translation and collision. A frictional component of viscosity can
also be included to account for the viscous-plastic transition that occurs when particles
of a solid phase reach the maximum solid volume fraction.
The collisional and kinetic parts, and the optional frictional part, are added to give the
solids shear viscosity:
µs = µs,col + µs,kin + µs,fr
(16.5-81)
Collisional Viscosity
The collisional part of the shear viscosity is modeled as [110, 343]
4
Θs
µs,col = αs ρs ds g0,ss (1 + ess )
5
π
1/2
αs
(16.5-82)
Kinetic Viscosity
ANSYS FLUENT provides two expressions for the kinetic part.
The default expression is from Syamlal et al. [343]:
µs,kin
√
αs ds ρs Θs π
2
=
1 + (1 + ess ) (3ess − 1) αs g0,ss
6 (3 − ess )
5
(16.5-83)
The following optional expression from Gidaspow et al. [110] is also available:
µs,kin
√
2
4
10ρs ds Θs π
1 + g0,ss αs (1 + ess ) αs
=
96αs (1 + ess ) g0,ss
5
Release 12.0 c ANSYS, Inc. January 29, 2009
(16.5-84)
16-61
Multiphase Flows
Bulk Viscosity
The solids bulk viscosity accounts for the resistance of the granular particles to compression and expansion. It has the following form from Lun et al. [208]:
4
Θs
λs = αs ρs ds g0,ss (1 + ess )
3
π
1/2
(16.5-85)
Note that the bulk viscosity is set to a constant value of zero, by default. It is also
possible to select the Lun et al. expression or use a user-defined function.
Frictional Viscosity
In dense flow at low shear, where the secondary volume fraction for a solid phase nears
the packing limit, the generation of stress is mainly due to friction between particles.
The solids shear viscosity computed by ANSYS FLUENT does not, by default, account
for the friction between particles.
If the frictional viscosity is included in the calculation, ANSYS FLUENT uses Schaeffer’s [303] expression:
ps sin φ
µs,fr = √
2 I2D
(16.5-86)
where ps is the solids pressure, φ is the angle of internal friction, and I2D is the second
invariant of the deviatoric stress tensor. It is also possible to specify a constant or userdefined frictional viscosity.
In granular flows with high solids volume fraction, instantaneous collisions are less important. The application of kinetic theory to granular flows is no longer relevant since
particles are in contact and the resulting frictional stresses need to be taken into account.
ANSYS FLUENT extends the formulation of the frictional viscosity and employs other
models, as well as providing new hooks for UDFs. See the separate UDF Manual for
details.
The frictional stresses are usually written in Newtonian form:
~
τf riction = −Pf riction I~ + µf riction (∇~us + (∇~us )T )
(16.5-87)
The frictional stress is added to the stress predicted by the kinetic theory when the solids
volume fraction exceeds a critical value. This value is normally set to 0.5 when the flow
is three-dimensional and the maximum packing limit is about 0.63. Then
PS = Pkinetic + Pf riction
16-62
(16.5-88)
Release 12.0 c ANSYS, Inc. January 29, 2009
16.5 Eulerian Model Theory
µS = µkinetic + µf riction
(16.5-89)
The derivation of the frictional pressure is mainly semi-empirical, while the frictional viscosity can be derived from the first principles. The application of the modified Coulomb
law leads to an expression of the form
µf riction =
Pf riction sin φ
√
2 I2D
(16.5-90)
Where φ is the angle of internal friction and I2D is the second invariant of the deviatoric
stress tensor.
Two additional models are available in ANSYS FLUENT: the Johnson and Jackson [151]
model for frictional pressure and Syamlal et al [343].
The Johnson and Jackson [151] model for frictional pressure is defined as
Pf riction = F r
(αs − αs,min )n
(αs,max − αs )p
(16.5-91)
With coefficient Fr = 0.05, n=2 and p = 5 [253]. The critical value for the solids volume
fraction is 0.5. The coefficient Fr was modified to make it a function of the volume
fraction:
F r = 0.1αs
(16.5-92)
The frictional viscosity for this model is of the form
µf riction = Pf riction sin φ
(16.5-93)
The second model that is employed is Syamlal et al. [343], described in Equation 16.5-83.
Comparing the two models results in the frictional normal stress differing by orders of
magnitude.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-63
Multiphase Flows
The radial distribution function is an important parameter in the description of the solids
pressure resulting from granular kinetic theory. If we use the models of Lun et al. [208] or
Gidaspow [109] the radial function tends to infinity as the volume fraction tends to the
packing limit. It would then be possible to use this pressure directly in the calculation
of the frictional viscosity, as it has the desired effect. This approach is also available in
ANSYS FLUENT by default.
i
The introduction of the frictional viscosity helps in the description of frictional flows, however a complete description would require the introduction
of more physics to capture the elastic regime with the calculation of the
yield stress and the use of the flow-rule. These effects can be added by the
user via UDFs to model static regime. Small time steps are required to get
good convergence behavior.
16.5.8
Granular Temperature
The granular temperature for the sth solids phase is proportional to the kinetic energy of
the random motion of the particles. The transport equation derived from kinetic theory
takes the form [71]
"
#
3 ∂
(ρs αs Θs ) + ∇ · (ρs αs~vs Θs ) = (−ps I+τ s ) : ∇~vs +∇·(kΘs ∇Θs )−γΘs +φls (16.5-94)
2 ∂t
where
(−ps I + τ s ) : ∇~vs
kΘs ∇Θs
γΘs
φls
= the generation of energy by the solid stress tensor
= the diffusion of energy (kΘs is the diffusion coefficient)
= the collisional dissipation of energy
= the energy exchange between the lth
fluid or solid phase and the sth solid phase
Equation 16.5-94 contains the term kΘs ∇Θs describing the diffusive flux of granular
energy. When the default Syamlal et al. model [343] is used, the diffusion coefficient for
granular energy, kΘs is given by
kΘ s
√
15ds ρs αs Θs π
12 2
16
=
1 + η (4η − 3)αs g0,ss +
(41 − 33η)ηαs g0,ss )
4(41 − 33η)
5
15π
(16.5-95)
where
1
η = (1 + ess )
2
16-64
Release 12.0 c ANSYS, Inc. January 29, 2009
16.5 Eulerian Model Theory
ANSYS FLUENT uses the following expression if the optional model of Gidaspow et
al. [110] is enabled:
q
kΘ s
s
2
150ρs ds (Θπ)
6
Θs
=
1 + αs g0,ss (1 + es ) + 2ρs αs 2 ds (1 + ess )g0,ss
384(1 + ess )g0,ss
5
π
(16.5-96)
The collisional dissipation of energy, γΘs , represents the rate of energy dissipation within
the sth solids phase due to collisions between particles. This term is represented by the
expression derived by Lun et al. [208]
γΘm =
12(1 − e2ss )g0,ss
√
ρs αs2 Θ3/2
s
ds π
(16.5-97)
The transfer of the kinetic energy of random fluctuations in particle velocity from the sth
solids phase to the lth fluid or solid phase is represented by φls [110]:
φls = −3Kls Θs
(16.5-98)
ANSYS FLUENT allows the user to solve for the granular temperature with the following
options:
• algebraic formulation (the default)
It is obtained by neglecting convection and diffusion in the transport equation,
Equation 16.5-94 [343].
• partial differential equation
This is given by Equation 16.5-94 and it is allowed to choose different options for
it properties.
• constant granular temperature
This is useful in very dense situations where the random fluctuations are small.
• UDF for granular temperature
For a granular phase s, we may write the shear force at the wall in the following form:
q
π√
αs
3φ
ρs g0 Θs U~s,||
(16.5-99)
τ~s = −
6
αs,max
Here U~s,|| is the particle slip velocity parallel to the wall, φ is the specularity coefficient
between the particle and the wall, αs,max is the volume fraction for the particles at
maximum packing, and g0 is the radial distribution function that is model dependent.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-65
Multiphase Flows
The general boundary condition for granular temperature at the wall takes the form
[151]
qs =
16.5.9
q
3
π√
αs
π √ αs
3φ
ρs g0 Θs )U~s,|| · U~s,|| −
3
(1 − e2sw )ρs g0 Θs2
6
αs,max
4
αs,max
(16.5-100)
Interfacial Area Concentration
Interfacial area concentration is defined as the interfacial area between two phases per
unit mixture volume. This is an important parameter for predicting mass, momentum and energy transfers through the interface between the phases. The models that
are inplemented in ANSYS FLUENT are discussed in Section 16.4.9: Interfacial Area
Concentration.
16.5.10
Description of Heat Transfer
The internal energy balance for phase q is written in terms of the phase enthalpy, Equation 16.5-11, defined by
Hq =
Z
cp,q dTq
(16.5-101)
where cp,q is the specific heat at constant pressure of phase q. The thermal boundary
conditions used with multiphase flows are the same as those for a single-phase flow. See
Chapter 7: Cell Zone and Boundary Conditions in the separate User’s Guide for details.
The Heat Exchange Coefficient
The rate of energy transfer between phases is assumed to be a function of the temperature
difference
Qpq = hpq (Tp − Tq )
(16.5-102)
where hpq (= hqp ) is the heat transfer coefficient between the pth phase and the q th phase.
The heat transfer coefficient is related to the pth phase Nusselt number, Nup , by
hpq =
6κq αp αq Nup
dp 2
(16.5-103)
Here κq is the thermal conductivity of the q th phase. The Nusselt number is typically
determined from one of the many correlations reported in the literature. In the case of
fluid-fluid multiphase, ANSYS FLUENT uses the correlation of Ranz and Marshall [284,
285]:
16-66
Release 12.0 c ANSYS, Inc. January 29, 2009
16.5 Eulerian Model Theory
1/3
Nup = 2.0 + 0.6Re1/2
p Pr
(16.5-104)
where Rep is the relative Reynolds number based on the diameter of the pth phase and
the relative velocity |u~p − u~q |, and Pr is the Prandtl number of the q th phase:
Pr =
c p q µq
κq
(16.5-105)
In the case of granular flows (where p = s), ANSYS FLUENT uses a Nusselt number
correlation by Gunn [117], applicable to a porosity range of 0.35–1.0 and a Reynolds
number of up to 105 :
1/3
1/3
Nus = (7 − 10αf + 5αf2 )(1 + 0.7Re0.2
) + (1.33 − 2.4αf + 1.2αf2 )Re0.7
(16.5-106)
s Pr
s Pr
The Prandtl number is defined as above with q = f . For all these situations, hpq should
tend to zero whenever one of the phases is not present within the domain. To enforce
this, hpq is always multiplied by the volume fraction of the primary phase q, as reflected
in Equation 16.5-103.
16.5.11
Turbulence Models
To describe the effects of turbulent fluctuations of velocities and scalar quantities in
a single phase, ANSYS FLUENT uses various types of closure models, as described in
Chapter 4: Turbulence. In comparison to single-phase flows, the number of terms to be
modeled in the momentum equations in multiphase flows is large, and this makes the
modeling of turbulence in multiphase simulations extremely complex.
ANSYS FLUENT provides three methods for modeling turbulence in multiphase flows
within the context of the k- models. In addition, ANSYS FLUENT provides two turbulence options within the context of the Reynolds stress models (RSM).
The k- turbulence model options are:
• mixture turbulence model (the default)
• dispersed turbulence model
• turbulence model for each phase
i
Note that the descriptions of each method below are presented based on
the standard k- model. The multiphase modifications to the RNG and
realizable k- models are similar, and are therefore not presented explicitly.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-67
Multiphase Flows
The RSM turbulence model options are:
• mixture turbulence model (the default)
• dispersed turbulence model
For either category, the choice of model depends on the importance of the secondaryphase turbulence in your application.
k- Turbulence Models
ANSYS FLUENT provides three turbulence model options in the context of the k- models:
the mixture turbulence model (the default), the dispersed turbulence model, or a perphase turbulence model.
k- Mixture Turbulence Model
The mixture turbulence model is the default multiphase turbulence model. It represents
the first extension of the single-phase k- model, and it is applicable when phases separate,
for stratified (or nearly stratified) multiphase flows, and when the density ratio between
phases is close to 1. In these cases, using mixture properties and mixture velocities is
sufficient to capture important features of the turbulent flow.
The k and equations describing this model are as follows:
∂
µt,m
(ρm k) + ∇ · (ρm~vm k) = ∇ ·
∇k + Gk,m − ρm
∂t
σk
(16.5-107)
∂
µt,m
(ρm ) + ∇ · (ρm~vm ) = ∇ ·
∇ + (C1 Gk,m − C2 ρm )
∂t
σ
k
(16.5-108)
and
where the mixture density and velocity, ρm and ~vm , are computed from
ρm =
N
X
αi ρi
(16.5-109)
i=1
and
N
X
~vm =
αi ρi~vi
i=1
N
X
(16.5-110)
αi ρi
i=1
16-68
Release 12.0 c ANSYS, Inc. January 29, 2009
16.5 Eulerian Model Theory
the turbulent viscosity, µt,m , is computed from
µt,m = ρm Cµ
k2
(16.5-111)
and the production of turbulence kinetic energy, Gk,m , is computed from
Gk,m = µt,m (∇~vm + (∇~vm )T ) : ∇~vm
(16.5-112)
The constants in these equations are the same as those described in Section 4.4.1: Standard k- Model for the single-phase k- model.
k- Dispersed Turbulence Model
The dispersed turbulence model is the appropriate model when the concentrations of the
secondary phases are dilute. In this case, interparticle collisions are negligible and the
dominant process in the random motion of the secondary phases is the influence of the
primary-phase turbulence. Fluctuating quantities of the secondary phases can therefore
be given in terms of the mean characteristics of the primary phase and the ratio of the
particle relaxation time and eddy-particle interaction time.
The model is applicable when there is clearly one primary continuous phase and the rest
are dispersed dilute secondary phases.
Assumptions
The dispersed method for modeling turbulence in ANSYS FLUENT assumes the following:
• a modified k- model for the continuous phase
Turbulent predictions for the continuous phase are obtained using the standard
k- model supplemented with extra terms that include the interphase turbulent
momentum transfer.
• Tchen-theory correlations for the dispersed phases
Predictions for turbulence quantities for the dispersed phases are obtained using the
Tchen theory of dispersion of discrete particles by homogeneous turbulence [130].
Release 12.0 c ANSYS, Inc. January 29, 2009
16-69
Multiphase Flows
• interphase turbulent momentum transfer
In turbulent multiphase flows, the momentum exchange terms contain the correlation between the instantaneous distribution of the dispersed phases and the
turbulent fluid motion. It is possible to take into account the dispersion of the
dispersed phases transported by the turbulent fluid motion.
• a phase-weighted averaging process
The choice of averaging process has an impact on the modeling of dispersion in turbulent multiphase flows. A two-step averaging process leads to the appearance of
fluctuations in the phase volume fractions. When the two-step averaging process is
used with a phase-weighted average for the turbulence, however, turbulent fluctuations in the volume fractions do not appear. ANSYS FLUENT uses phase-weighted
averaging, so no volume fraction fluctuations are introduced into the continuity
equations.
Turbulence in the Continuous Phase
The eddy viscosity model is used to calculate averaged fluctuating quantities. The
Reynolds stress tensor for continuous phase q takes the following form:
2
~ q )I + ρq νt,q (∇U
~ q + ∇U
~qT )
τ 00q = − (ρq kq + ρq νt,q ∇ · U
3
(16.5-113)
~ q is the phase-weighted velocity.
where U
The turbulent viscosity µt,q is written in terms of the turbulent kinetic energy of phase
q:
µt,q = ρq Cµ
kq2
q
(16.5-114)
and a characteristic time of the energetic turbulent eddies is defined as
3 kq
τt,q = Cµ
2 q
(16.5-115)
where q is the dissipation rate and Cµ = 0.09.
The length scale of the turbulent eddies is
s
Lt,q =
3 kq3/2
Cµ
2
q
(16.5-116)
Turbulent predictions are obtained from the modified k- model:
16-70
Release 12.0 c ANSYS, Inc. January 29, 2009
16.5 Eulerian Model Theory
∂
~ q kq ) = ∇ · (αq µt,q ∇kq ) + αq Gk,q − αq ρq q + αq ρq Πkq (16.5-117)
(αq ρq kq ) + ∇ · (αq ρq U
∂t
σk
and
∂
~ q q ) = ∇ · (αq µt,q ∇q ) + αq q (C1 Gk,q − C2 ρq q ) + αq ρq Πq
(αq ρq q ) + ∇ · (αq ρq U
∂t
σ
kq
(16.5-118)
Here Πkq and Πq represent the influence of the dispersed phases on the continuous phase
q, and Gk,q is the production of turbulent kinetic energy, as defined in Section 4.4.4: Modeling Turbulent Production in the k- Models. All other terms have the same meaning
as in the single-phase k- model.
The term Πkq can be derived from the instantaneous equation of the continuous phase
and takes the following form, where M represents the number of secondary phases:
Πk q =
M
X
Kpq
p=1 αq ρq
~p − U
~ q ) · ~vdr )
(< ~vq00 · ~vp00 > +(U
(16.5-119)
which can be simplified to
Πk q =
M
X
Kpq
p=1
αq ρq
(kpq − 2kq + ~vpq · ~vdr )
(16.5-120)
where klq is the covariance of the velocities of the continuous phase q and the dispersed
phase l (calculated from Equation 16.5-128 below), ~vpq is the relative velocity, and ~vdr is
the drift velocity (defined by Equation 16.5-133 below).
Πq is modeled according to Elgobashi et al. [87]:
Πq = C3
q
Πk
kq q
(16.5-121)
where C3 = 1.2.
Turbulence in the Dispersed Phase
Time and length scales that characterize the motion are used to evaluate dispersion
coefficients, correlation functions, and the turbulent kinetic energy of each dispersed
phase.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-71
Multiphase Flows
The characteristic particle relaxation time connected with inertial effects acting on a
dispersed phase p is defined as
τF,pq =
−1
αp ρq Kpq
ρp
+ CV
ρq
!
(16.5-122)
The Lagrangian integral time scale calculated along particle trajectories, mainly affected
by the crossing-trajectory effect [63], is defined as
τt,q
τt,pq = q
(16.5-123)
(1 + Cβ ξ 2 )
where
ξ=
|~vpq |τt,q
Lt,q
(16.5-124)
and
Cβ = 1.8 − 1.35 cos2 θ
(16.5-125)
where θ is the angle between the mean particle velocity and the mean relative velocity.
The ratio between these two characteristic times is written as
ηpq =
τt,pq
τF,pq
(16.5-126)
Following Simonin [317], ANSYS FLUENT writes the turbulence quantities for dispersed
phase p as follows:
b2 + ηpq
kq
1 + ηpq
!
b + ηpq
2kq
1 + ηpq
1
kpq τt,pq
3
2
1
Dt,pq +
kp − b kpq τF,pq
3
3
!−1
ρp
(1 + CV )
+ CV
ρq
!
kp =
kpq =
Dt,pq =
Dp =
b =
(16.5-127)
(16.5-128)
(16.5-129)
(16.5-130)
(16.5-131)
and CV = 0.5 is the added-mass coefficient.
16-72
Release 12.0 c ANSYS, Inc. January 29, 2009
16.5 Eulerian Model Theory
Interphase Turbulent Momentum Transfer
The turbulent drag term for multiphase flows (Kpq (~vp −~vq ) in Equation 16.5-7) is modeled
as follows, for dispersed phase p and continuous phase q:
~p − U
~ q ) − Kpq~vdr
Kpq (~vp − ~vq ) = Kpq (U
(16.5-132)
The second term on the right-hand side of Equation 16.5-132 contains the drift velocity:
Dp
Dq
~vdr = −
∇αp −
∇αq
σpq αp
σpq αq
!
(16.5-133)
Here Dp and Dq are diffusivities, and σpq is a dispersion Prandtl number. When using
Tchen theory in multiphase flows, ANSYS FLUENT assumes Dp = Dq = Dt,pq and the
default value for σpq is 0.75.
The drift velocity results from turbulent fluctuations in the volume fraction. When
multiplied by the exchange coefficient Kpq , it serves as a correction to the momentum
exchange term for turbulent flows. This correction is not included, by default, but you can
enable it during the problem setup, as discussed in Section 24.5.4: Modeling Turbulence
in the separate User’s Guide.
k- Turbulence Model for Each Phase
The most general multiphase turbulence model solves a set of k and transport equations
for each phase. This turbulence model is the appropriate choice when the turbulence
transfer among the phases plays a dominant role.
Note that, since ANSYS FLUENT is solving two additional transport equations for each
secondary phase, the per-phase turbulence model is more computationally intensive than
the dispersed turbulence model.
Transport Equations
The Reynolds stress tensor and turbulent viscosity are computed using Equations 16.5-113
and 16.5-114. Turbulence predictions are obtained from
∂
~ q kq ) = ∇ · (αq (µq + µt,q )∇kq ) + (αq Gk,q − αq ρq q ) +
(αq ρq kq ) + ∇ · (αq ρq U
∂t
σk
N
X
N
X
N
X
µt,l
~l −U
~ q )· µt,q ∇αq (16.5-134)
~
~
∇αl + Klq (U
Klq (Clq kl −Cql kq )− Klq (Ul − Uq )·
αl σl
αq σq
l=1
l=1
l=1
Release 12.0 c ANSYS, Inc. January 29, 2009
16-73
Multiphase Flows
and
∂
~ q q ) = ∇ · (αq µt,q ∇q ) + q
(αq ρq q ) + ∇ · (αq ρq U
∂t
σ
kq
C3
N
X
"
C1 αq Gk,q − C2 αq ρq q +
N
X
N
X
~l − U
~ q ) · µt,l ∇αl +
~l − U
~ q ) · µt,q ∇αq
Klq (Clq kl − Cql kq ) −
Klq (U
Klq (U
αl σl
αq σq
l=1
l=1
l=1
(16.5-135)
!#
The terms Clq and Cql can be approximated as
ηlq
Clq = 2, Cql = 2
1 + ηlq
!
(16.5-136)
where ηlq is defined by Equation 16.5-126.
Interphase Turbulent Momentum Transfer
The turbulent drag term (Kpq (~vp − ~vq ) in Equation 16.5-7) is modeled as follows, where
l is the dispersed phase (replacing p in Equation 16.5-7) and q is the continuous phase:
N
X
l=1
Klq (~vl − ~vq ) =
N
X
l=1
~l − U
~q) −
Klq (U
N
X
Klq~vdr,lq
(16.5-137)
l=1
~ l and U
~ q are phase-weighted velocities, and ~vdr,lq is the drift velocity for phase l
Here U
(computed using Equation 16.5-133, substituting l for p). Note that ANSYS FLUENT
will compute the diffusivities Dl and Dq directly from the transport equations, rather
than using Tchen theory (as it does for the dispersed turbulence model).
As noted above, the drift velocity results from turbulent fluctuations in the volume
fraction. When multiplied by the exchange coefficient Klq , it serves as a correction to
the momentum exchange term for turbulent flows. This correction is not included, by
default, but you can enable it during the problem setup.
The turbulence model for each phase in ANSYS FLUENT accounts for the effect of the
turbulence field of one phase on the other(s). If you want to modify or enhance the
interaction of the multiple turbulence fields and interphase turbulent momentum transfer,
you can supply these terms using user-defined functions.
16-74
Release 12.0 c ANSYS, Inc. January 29, 2009
16.5 Eulerian Model Theory
RSM Turbulence Models
Multiphase turbulence modeling typically involves two equation models that are based
on single-phase models and often cannot accurately capture the underlying flow physics.
Additional turbulence modeling for multiphase flows is diminished even more when the
basic underlying single-phase model cannot capture the complex physics of the flow. In
such situations, the logical next step is to combine the Reynolds stress model with the
multiphase algorithm in order to handle challenging situations in which both factors,
RSM for turbulence and the Eulerian multiphase formulation, are a precondition for
accurate predictions [59].
The phase-averaged continuity and momentum equations for a continuous phase are:
∂
(αc ρc ) + ∇ · (αc ρc Ũc ) = 0
∂t
(16.5-138)
O
∂
(αc ρrmc Ũc ) + ∇ · (αc ρrmc Ũc
Ũc ) = −αc ∇p̃ + ∇ · τ̃ct + FDc
∂t
(16.5-139)
For simplicity, the laminar stress-strain tensor and other body forces such as gravity
have been omitted from Equations 16.5-138-16.5-139. The tilde denotes phase-averaged
variables while an overbar (e.g., αc ) reflects time-averaged values. In general, any variable
Φ can have a phase-average value defined as
Φ̃c =
αc Φc
αc
(16.5-140)
Considering only two phases for simplicity, the drag force between the continuous and
the dispersed phases can be defined as:
"
FDc = Kdc
αd u0d αc u0c
(Ũd − Ũc ) −
−
αd
αc
!#
(16.5-141)
where Kdc is the drag coefficient. Several terms in the Equation 16.5-141 need to be
modeled in order to close the phase-averaged momentum equations. Full descriptions of
all modeling assumptions can be found in [58]. This section only describes the different
modeling definition of the turbulent stresses τ˜t that appears in Equation 16.5-139.
The turbulent stress that appears in the momentum equations need to be defined on a
per-phase basis and can be calculated as:
τ˜t k = −αk ρk R̃k,ij
Release 12.0 c ANSYS, Inc. January 29, 2009
(16.5-142)
16-75
Multiphase Flows
where the subscript k is replaced by c for the primary (i.e., continuous) phase or by
d for any secondary (i.e., dispersed) phases. As is the case for single-phase flows, the
current multiphase Reynolds stress model (RSM) also solves the transport equations for
Reynolds stresses Rij . ANSYS FLUENT includes two methods for modeling turbulence in
multiphase flows within the context of the RSM model: the dispersed turbulence model,
and the mixture turbulence model.
RSM Dispersed Turbulence Model
The dispersed turbulence model is used when the concentrations of the secondary phase
are dilute and the primary phase turbulence is regarded as the dominant process. Consequently, the transport equations for turbulence quantities are only solved for the primary
(continuous) phase, while the predictions of turbulence quantities for dispersed phases
are obtained using the Tchen theory. The transport equation for the primary phase
Reynolds stresses in the case of the dispersed model are:
∂
∂
∂ Ũj
∂ Ũi
(αρR̃ij ) +
(αρŨk R̃ij ) = −αρ R̃ik
+ R̃jk
∂t
∂xk
∂xk
∂xk
!
"
#
∂
∂
+
(R̃ij )
αµ
∂xk
∂xk
∂
∂u0 ∂u0
[αρu0i u0j u0k ] + αp( i + j )
∂xk
∂xj ∂xi
− αρ˜ij + ΠR,ij
−
(16.5-143)
The variables in Equation 16.5-143 are per continuous phase c and the subscript is omitted
for clarity. The last term of Equation 16.5-143, ΠR,ij , takes into account the interaction
between the continuous and the dispersed phase turbulence. A general model for this
term can be of the form:
ΠR,ij = Kdc C1,dc (Rdc,ij − Rc,ij ) + Kdc C2,dc adc,i bdc,j
(16.5-144)
where C1 and C2 are unknown coefficients, adc,i is the relative velocity, bdc,j represents
the drift or the relative velocity, and Rdc,ij is the unknown particulate-fluid velocity
correlation. To simplify this unknown term, the following assumption has been made:
2
ΠR,ij = δij Πk
3
(16.5-145)
where δij is the Kronecker delta, and Πk represents the modified version of the original
Simonin model [317].
Πkc = Kdc (k̃dc − 2k̃c + Ṽrel · Ṽdrift )
16-76
(16.5-146)
Release 12.0 c ANSYS, Inc. January 29, 2009
16.5 Eulerian Model Theory
where K̃c represents the turbulent kinetic energy of the continuous phase, k̃dc is the
continuous-dispersed phase velocity covariance and finally, Ṽrel and Ṽdrift stand for the
relative and the drift velocities, respectively. In order to achieve full closure, the transport
equation for the turbulent kinetic energy dissipation rate (˜) is required. The modeling
of ˜ together with all other unknown terms in Equation 16.5-146 are modeled in the same
way as in [58].
RSM Mixture Turbulence Model
The main assumption for the mixture model is that all phases share the same turbulence field which consequently means that the term ΠR in the Reynolds stress transport
equations (Equation 16.5-143) is neglected. Apart from that, the equations maintain the
same form but with phase properties and phase velocities being replaced with mixture
properties and mixture velocities. The mixture density, for example, can be expressed as
ρm =
N
X
αi ρi
(16.5-147)
αi ρi Ũi
i=1 αi ρi
(16.5-148)
i=1
while mixture velocities can be expressed as
PN
Ũm = Pi=1
N
where N is the number of species.
16.5.12
Solution Method in ANSYS FLUENT
For Eulerian multiphase calculations, ANSYS FLUENT can solve the phase momentum
equations, the shared pressure, and phasic volume fraction equations in a coupled and
segregated fashion. The coupled solution for multiphase flows is discussed in detail in Section 24.7.1: Coupled Solution for Multiphase Flows in the separate User’s Guide. When
solving the equations in a segregated manner, ANSYS FLUENT uses the phase coupled
SIMPLE (PC-SIMPLE) algorithm [354] for the pressure-velocity coupling. PC-SIMPLE
is an extension of the SIMPLE algorithm [264] to multiphase flows. The velocities are
solved coupled by phases, but in a segregated fashion. The block algebraic multigrid
scheme used by the density-based solver described in [371] is used to solve a vector equation formed by the velocity components of all phases simultaneously. Then, a pressure
correction equation is built based on total volume continuity rather than mass continuity.
Pressure and velocities are then corrected so as to satisfy the continuity constraint.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-77
Multiphase Flows
The Pressure-Correction Equation
For incompressible multiphase flow, the pressure-correction equation takes the form
n
X
1
k=1
ρrk
(
n
X
∂
αk ρk + ∇ · αk ρk~vk0 + ∇ · αk ρk~vk∗ − ( (ṁlk − ṁkl )) = 0
∂t
l=1
)
(16.5-149)
where ρrk is the phase reference density for the k th phase (defined as the total volume
average density of phase k), ~vk0 is the velocity correction for the k th phase, and ~vk∗ is the
value of ~vk at the current iteration. The velocity corrections are themselves expressed as
functions of the pressure corrections.
Volume Fractions
The volume fractions are obtained from the phase continuity equations. In discretized
form, the equation of the k th volume fraction is
ap,k αk =
X
(anb,k αnb,k ) + bk = Rk
(16.5-150)
nb
In order to satisfy the condition that all the volume fractions sum to one,
n
X
αk = 1
(16.5-151)
k=1
16.5.13
Dense Discrete Phase Model
In the standard formulation of the Largangian multiphase model, described in Chapter 15: Discrete Phase, the assumption is that the volume fraction of the discrete phase is
sufficiently low: it is not taken into account when assembling the continuous phase equations. The general form of the mass and momentum conservation equations in ANSYS
FLUENT is given in Equations 16.5-152 and 16.5-153 (and also defined in Section 1.2: Continuity and Momentum Equations).
∂ρ
+ ∇ · (ρ~v ) = SDP M + Sother
∂t
∂ρ~v
+ ∇ · (ρ~v~v ) = −∇p + ∇ · τ + ρ~g + F~DP M + F~other
∂t
16-78
(16.5-152)
(16.5-153)
Release 12.0 c ANSYS, Inc. January 29, 2009
16.5 Eulerian Model Theory
To overcome this limitation of the Lagrangian multiphase model, the volume fraction of
the particulate phase is accounted for by extending Equations 16.5-152 and 16.5-153 to
the following set of equations (see also Section 16.5.3: Conservation Equations, written
for phase p):
nphases
X
∂
(αp ρp ) + ∇ · (αp ρp~vp ) =
(ṁqp − ṁpq )
∂t
q=1
(16.5-154)
h
i
∂
(αp ρp~vp ) + ∇ · (αp ρp~vp~vp ) = −αp ∇p + ∇ · αp µp ∇~vp + ∇~vpT
∂t
+αp ρp~g + Fvm,lif t,user +
nphases
X
~ qp (~vq − ~vp ) + ṁqp~vqp − ṁqp~vqp
K
q=1
+ KDP M (~vDP M − ~vp ) + SDP M,explicit
(16.5-155)
Here, Equation 16.5-154 is the mass conservation equation for an individual phase p and
Equation 16.5-155 is the corresponding momentum conservation equation. Currently,
the momentum exchange terms (denoted by DP M ) are considered only in the primary
phase equations.
In the resulting set of equations (one continuity and one momentum conservation equation
per phase), those corresponding to a discrete phase are not solved. The solution, such as
volume fraction or velocity field, is taken from the Lagrangian tracking solution.
In the context of the phase coupled SIMPLE algorithm (Section 16.5.12: Solution Method
in ANSYS FLUENT) and the coupled algorithm for pressure-velocity coupling (Section 24.7.5: Selecting the Solution Method in the separate User’s Guide), a higher degree of implicitness
is achieved in the treatment of the drag coupling terms. All drag related terms appear
as coefficients on the left hand side of the linear equation system.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-79
Multiphase Flows
Limitations
Since the given approach makes use of the Eulerian multiphase model framework, all its
limitations are adopted:
• The turbulence models: LES, DES and k − ω turbulence models are not available.
• The combustion models: PDF Transport model, Premixed, Non-premixed and partially premixed combustion models are not available.
• The radiation models are not available.
• The solidification and melting models are not available.
• The Wet Steam model is not available.
• The real gas model (pressure-based and density-based) is not available.
• The density-based solver and models dependent on it are not available.
• Parallel DPM with the shared memory option is disabled.
Granular Temperature
The solids stress acting on particles in a dense flow situation is modeled via an additional
acceleration in the particle force balance Equation 15.2-1.
dup
gx (ρp − ρ)
= FD (u − up ) +
+ Fx + Finteraction
dt
ρp
(16.5-156)
The term Finteraction models the additional acceleration acting on a particle, resulting
from interparticle interaction. It is computed from the stress tensor given by the Kinetic
Theory of Granular Flows as
Finteraction = −
1
∇ · τ̄¯s
ρp
(16.5-157)
The conservation equation for the granular temperature (kinetic energy of the fluctuating
particle motion) is solved with the averaged particle velocity field. Therefore, a sufficient
statistical representation of the particle phase is needed to ensure the stable behavior
of the granular temperature equation. For details on the Kinetic Theory of Granular
Flows, please refer to Section 16.5.3: Conservation Equations – Section 16.5.8: Granular
Temperature.
The main advantage over the Eulerian model is that, there is no need to define classes
to handle particle size distributions. This is done in a natural way in the Lagrangian
formulation [279].
16-80
Release 12.0 c ANSYS, Inc. January 29, 2009
16.5 Eulerian Model Theory
16.5.14
Immiscible Fluid Model
The immiscible fluid model for Eulerian multiphase allows you to use the Geo-Reconstruct
and CICSAM sharpening schemes with the explicict VOF option. This model should be
enabled only for cases requiring sharp interface treatment between phases. This model
might help in overcoming some limitations of the VOF model because of the shared
velocity and temperature formulation.
The immiscible fluid model for the Eulerian multiphase model provides the anisotropic
drag law, which can be used when modeling free surface flow. This drag law is also used
when there is higher drag in the normal direction to the interface and lower drag in the
tangential direction to the interface. This model may help in overcoming some limitations
of the VOF model because of the shared velocity and temperature formulation.
In some cases, where the flow for a particular phase is important in both the directions
(tangential and normal to the interface), using a higher anisotropy ratio will result in
numerical instability. Therefore, in those cases, an anisotropy ratio of up to 1000 is
recommended, where the anisotropy ratio is defined as
anisotropy ratio =
friction factornormal to interface
friction factortangential to interface
In cases, where flow for a particular phase is important only in one direction (tangential or
normal to the interface), a higher anisotropy ratio could be used. The principal directions
for this drag are based on the normal and tangential direction to the interface.
Two types of drag formulations exist within the anisotropic drag law: one that is based
on the symmetric drag law and the other is based on different viscosity options.
Formulation 1
This is based on the symmetric drag law, where the effective drag coefficient in the
principal direction p is described as follows:
K, p = Ksymmetric λ, p
(16.5-158)
where λ is the friction factor vector in the principal direction. Ksymmetric is the isotropic
drag coefficient obtained from the symmetric drag law.
Formulation 2
The effective drag coefficient in the principal direction p is described as follows:
K, p = K, visc, p ∗ vofi ∗ vofj K, p = (Kvisc , p vofi vofj
(16.5-159)
where vofi is the volume fraction for phase i and vofj is the volume fracion for phase j.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-81
Multiphase Flows
The viscous drag component in the principal direction Kvisc , p is
Kvisc , p =
µ
λ, p
(lc lc )
(16.5-160)
where the viscosity options can be any one of the following:
µ
µ
µ
µ
µ
µ
= 0.5(µi + µj )
i µj
= (µ2µi +µ
j)
µj
= (µi vofµj i+µ
j vofi )
= µi vofi + µj vofj
= µi
= µj
and lc is the length scale.
To learn how to use the immiscible fluid model and the two drag formulations, refer to
Section 24.5.8: Including the Immiscible Fluid Model in the separate User’s Guide.
16.6
Wet Steam Model Theory
Information is organized into the following subsections:
• Section 16.6.1: Overview and Limitations of the Wet Steam Model
• Section 16.6.2: Wet Steam Flow Equations
• Section 16.6.3: Phase Change Model
• Section 16.6.4: Built-in Thermodynamic Wet Steam Properties
16.6.1
Overview and Limitations of the Wet Steam Model
Overview
During the rapid expansion of steam, a condensation process will take place shortly
after the state path crosses the vapor-saturation line. The expansion process causes the
super-heated dry steam to first subcool and then nucleate to form a two-phase mixture
of saturated vapor and fine liquid droplets known as wet steam.
Modeling wet steam is very important in the analysis and design of steam turbines. The
increase in steam turbine exit wetness can cause severe erosion to the turbine blades at
the low-pressure stages, and a reduction in aerodynamic efficiency of the turbine stages
operating in the wet steam region [237].
16-82
Release 12.0 c ANSYS, Inc. January 29, 2009
16.6 Wet Steam Model Theory
ANSYS FLUENT has adopted the Eulerian-Eulerian approach for modeling wet steam
flow. The flow mixture is modeled using the compressible Navier-Stokes equations, in
addition to two transport equations for the liquid-phase mass-fraction (β), and the number of liquid-droplets per unit volume (η). The phase change model, which involves the
formation of liquid-droplets in a homogeneous nonequilibrium condensation process, is
based on the classical nonisothermal nucleation theory.
This section describes the theoretical aspects of the wet steam model. Information about
enabling the model and using your own property functions and data with the wet steam
model is provided in Section 24.6: Setting Up the Wet Steam Model in the separate
User’s Guide. Solution settings and strategies for the wet steam model can be found in
Section 24.7.6: Wet Steam Model in the separate User’s Guide. Postprocessing variables
are described in Section 24.8.1: Model-Specific Variables in the separate User’s Guide.
Limitations
The following restrictions and limitations currently apply to the wet steam model in
ANSYS FLUENT:
• The wet steam model is available for the density-based solver only.
• Pressure inlet, mass-flow inlet, and pressure outlet are the only inflow and outflow
boundary conditions available.
• When the wet steam model is active, the access to the Create/Edit Materials dialog
box is restricted because the fluid mixture properties are determined from the builtin steam property functions or from the user-defined wet steam property functions.
Therefore, if solid properties need to be set and adjusted, then it must be done in
the Create/Edit Materials dialog box before activating the wet steam model.
16.6.2
Wet Steam Flow Equations
The wet steam is a mixture of two-phases. The primary phase is the gaseous-phase
consisting of water-vapor (denoted by the subscript v) while the secondary phase is the
liquid-phase consisting of condensed-water droplets (denoted by the subscript l).
Release 12.0 c ANSYS, Inc. January 29, 2009
16-83
Multiphase Flows
The following assumptions are made in this model:
• The velocity slip between the droplets and gaseous-phase is negligible.
• The interactions between droplets are neglected.
• The mass fraction of the condensed phase, β (also known as wetness factor), is
small (β < 0.2).
• Since droplet sizes are typically very small (from approximately 0.1 microns to
approximately 100 microns), it is assumed that the volume of the condensed liquid
phase is negligible.
From the preceding assumptions, it follows that the mixture density (ρ) can be related
to the vapor density (ρv ) by the following equation:
ρ=
ρv
(1 − β)
(16.6-1)
In addition, the temperature and the pressure of the mixture will be equivalent to the
temperature and pressure of the vapor-phase.
The mixture flow is governed by the compressible Navier-Stokes equations given in vector
form by Equation 18.5-4:
I
Z
∂W ∂ Z
Q dV + [F − G] · dA =
H dV
∂Q ∂t V
V
(16.6-2)
where Q=(P,u,v,w,T) are mixture quantities. The flow equations are solved using the
same density-based solver algorithms employed for general compressible flows.
To model wet steam, two additional transport equations are needed [138]. The first
transport equation governs the mass fraction of the condensed liquid phase (β):
∂ρβ
→
+ ∇ · (ρ−
v β) = Γ
∂t
(16.6-3)
where Γ is the mass generation rate due to condensation and evaporation (kg per unit
volume per second). The second transport equation models the evolution of the number
density of the droplets per unit volume:
∂ρη
→
+ ∇ · (ρ−
v η) = ρI
∂t
(16.6-4)
where I is the nucleation rate (number of new droplets per unit volume per second).
16-84
Release 12.0 c ANSYS, Inc. January 29, 2009
16.6 Wet Steam Model Theory
To determine the number of droplets per unit volume, Equation 16.6-1 and the average
droplet volume Vd are combined in the following expression:
η=
β
(1 − β)Vd (ρl /ρv )
(16.6-5)
where ρl is the liquid density and the average droplet volume is defined as
4
Vd = πr3d
3
(16.6-6)
where rd is the droplet radius.
Together, Equation 16.6-2, Equation 16.6-3, and Equation 16.6-4 form a closed system
of equations which, along with Equation 16.6-1, permit the calculation of the wet steam
flow field.
16.6.3
Phase Change Model
The following is assumed in the phase change model:
• The condensation is homogeneous (i.e., no impurities present to form nuclei).
• The droplet growth is based on average representative mean radii.
• The droplet is assumed to be spherical.
• The droplet is surrounded by infinite vapor space.
• The heat capacity of the fine droplet is negligible compared with the latent heat
released in condensation.
The mass generation rate Γ in the classical nucleation theory during the nonequilibrium
condensation process is given by the sum of mass increase due to nucleation (the formation
of critically sized droplets) and also due to growth/demise of these droplets [138].
Therefore, Γ is written as:
4
∂r
Γ = πρl Ir∗ 3 + 4πρl ηr2
3
∂t
(16.6-7)
where r is the average radius of the droplet, and r∗ is the Kelvin-Helmholtz critical droplet
radius, above which the droplet will grow and below which the droplet will evaporate.
An expression for r∗ is given by [387].
Release 12.0 c ANSYS, Inc. January 29, 2009
16-85
Multiphase Flows
r∗ =
2σ
ρl RT ln S
(16.6-8)
where σ is the liquid surface tension evaluated at temperature T , ρl is the condensed
liquid density (also evaluated at temperature T ), and S is the super saturation ratio
defined as the ratio of vapor pressure to the equilibrium saturation pressure:
s=
P
Psat (T )
(16.6-9)
The expansion process is usually very rapid. Therefore, when the state path crosses the
saturated-vapor line, the process will depart from equilibrium, and the supersaturation
ratio S can take on values greater than one.
The condensation process involves two mechanisms, the transfer of mass from the vapor
to the droplets and the transfer of heat from the droplets to the vapor in the form of
latent heat. This energy transfer relation was presented in [385] and used in [138] and
can be written as:
∂r
P
γ+1
√
=
Cp (T0 − T )
∂t
hlv ρl 2πRT 2γ
(16.6-10)
where T0 is the droplet temperature.
The classical homogeneous nucleation theory describes the formation of a liquid-phase
in the form of droplets from a supersaturated phase in the absence of impurities or
foreign particles. The nucleation rate described by the steady-state classical homogeneous
nucleation theory [387] and corrected for nonisothermal effects, is given by:
qc
ρ2v
I=
(1 + θ) ρl
!s
2σ −
e
Mm 3 π
4πr∗ 2 σ
3Kb T
(16.6-11)
where qc is evaporation coefficient, kb is the Boltzmann constant, Mm is mass of one
molecule, σ is the liquid surface tension, and ρl is the liquid density at temperature T .
A nonisothermal correction factor, θ, is given by:
2(γ − 1)
θ=
(γ + 1)
hlv
RT
!
!
hlv
− 0.5
RT
(16.6-12)
where hlv is the specific enthalpy of evaporation at pressure p and γ is the ratio of specific
heat capacities.
16-86
Release 12.0 c ANSYS, Inc. January 29, 2009
16.6 Wet Steam Model Theory
16.6.4
Built-in Thermodynamic Wet Steam Properties
There are many equations that describe the thermodynamic state and properties of steam.
While some of these equations are accurate in generating property tables, they are not
suitable for fast CFD computations. Therefore, ANSYS FLUENT uses a simpler form of
the thermodynamic state equations [386] for efficient CFD calculations that are accurate
over a wide range of temperatures and pressures. These equations are described below.
Equation of State
The steam equation of state used in the solver, which relates the pressure to the vapor
density and the temperature, is given by [386]:
P = ρv RT (1 + Bρv + Cρv 2 )
(16.6-13)
where B, and C are the second and the third virial coefficients given by the following
empirical functions:
B = a1 (1 +
5
τ −1
) + a2 eτ (1 − e−τ ) 2 + a3 τ
α
(16.6-14)
where B is given in m3 /kg, τ = 1500
with T given in Kelvin, α = 10000.0, a1 = 0.0015,
T
a2 = -0.000942, and a3 = -0.0004882.
C = a(τ − τ0 )e−ατ + b
where C is given in m6 /kg 2 , τ =
a= 1.772, and b= 1.5E-06.
T
647.286
(16.6-15)
with T given in Kelvin, τo = 0.8978, α=11.16,
The two empirical functions that define the virial coefficients B and C cover the temperature range from 273 K to 1073 K.
The vapor isobaric specific heat capacity Cpv is given by:
Cpv = Cp0 (T ) + R [(1 − αv T )(B − B1 ) − B2 ] ρv + (1 − 2αv T )C + αv T C1 −
C2
ρv 2
2
(16.6-16)
The vapor specific enthalpy, hv is given by:
hv = h0 (T ) + RT (B − B1 )ρv + (C −
C1 2
)ρv
2
(16.6-17)
The vapor specific entropy, sv is given by:
Release 12.0 c ANSYS, Inc. January 29, 2009
16-87
Multiphase Flows
"
(C + C1 ) 2
sv = s0 (T ) − R ln ρv + (B + B1 )ρv +
ρv
2
#
(16.6-18)
The isobaric specific heat at zero pressure is defined by the following empirical equation:
Cp0 (T ) =
X6
ai T i−2
(16.6-19)
i=1
where Cp0 is in KJ/kg K, a1 = 46.0, a2 = 1.47276, a3 = 8.38930E-04, a4 = -2.19989E-07,
a5 = 2.46619E-10, and a6 = -9.70466E-14.
and
2
2
, C1 = T dC
, B2 = T 2 dB
, and C2 = T 2 dC
.
B1 = T dB
dT
dT
dT 2
dT 2
Both h0 (T ) and s0 (T ) are functions of temperature and they are defined by:
h0 (T ) =
s0 (T ) =
Z
Z
Cp0 dT + hc
(16.6-20)
Cp0
dT + sc
T
(16.6-21)
where hc and sc are arbitrary constants.
The vapor dynamic viscosity µv and thermal conductivity Ktv are also functions of
temperature and were obtained from [385].
Saturated Vapor Line
The saturation pressure equation as a function of temperature was obtained from [290].
The example provided in Section 24.6.5: UDWSPF Example in the separate User’s Guide
contains a function called wetst satP() that represents the formulation for the saturation pressure.
Saturated Liquid Line
At the saturated liquid-line, the liquid density, surface tension, specific heat Cp, dynamic
viscosity, and thermal conductivity must be defined. The equation for liquid density, ρl ,
was obtained from [290]. The liquid surface tension equation was obtained from [385].
While the values of Cpl , µl and Ktl were curve fit using published data from [83] and then
written in polynomial forms. The example provided in Section 24.6.5: UDWSPF Example
in the separate User’s Guide contains functions called wetst cpl(), wetst mul(), and
wetst ktl() that represent formulations for Cpl , µl and Ktl .
16-88
Release 12.0 c ANSYS, Inc. January 29, 2009
16.7 Modeling Mass Transfer in Multiphase Flows
Mixture Properties
The mixture properties are related to vapor and liquid properties via the wetness factor
using the following mixing law:
φm = φl β + (1 − β)φv
(16.6-22)
where φ represents any of the following thermodynamic properties: h, s, Cp, Cv, µ or
Kt.
16.7
Modeling Mass Transfer in Multiphase Flows
This section describes the modeling of mass transfer in the framework of ANSYS FLUENT’s general multiphase models (i.e., Eulerian multiphase, mixture multiphase, VOF
multiphase). There are numerous kinds of mass transfer processes that can be modeled
in ANSYS FLUENT. You can use models available in ANSYS FLUENT (e.g. ANSYS FLUENT’s cavitation model), or define your own mass transfer model via user-defined functions. See Section 16.7.3: UDF-Prescribed Mass Transfer and the separate UDF Manual
for more information about the modeling of mass transfer via user-defined functions.
Information about mass transfer is presented in the following subsections:
• Section 16.7.1: Source Terms due to Mass Transfer
• Section 16.7.2: Unidirectional Constant Rate Mass Transfer
• Section 16.7.3: UDF-Prescribed Mass Transfer
• Section 16.7.4: Cavitation Models
• Section 16.7.5: Evaporation-Condensation Model
16.7.1
Source Terms due to Mass Transfer
ANSYS FLUENT adds contributions due to mass transfer only to the momentum, species,
and energy equations. No source term is added for other scalars such as turbulence or
user-defined scalars.
Let mpi qj be the mass transfer rate per unit volume from the ith species of phase p to
the j th species of phase q. In case a particular phase does not have a mixture material
associated with it, the mass transfer will be with the bulk phase.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-89
Multiphase Flows
Mass Equation
The contribution to the mass source for phase p in a cell is
mp = −mpi qj
(16.7-1)
mq = mpi qj
(16.7-2)
and for phase q is
Momentum Equation
For VOF or mixture models, there is no momentum source.
For the Eulerian model, the momentum source in a cell for phase p is
mp~up = −mpi qj ~up
(16.7-3)
mq ~uq = mpi qj ~up
(16.7-4)
and for phase q is
Energy Equation
For all multiphase models, the following energy sources are added.
The energy source in a cell for phase p is
Hp = −mpi qj (hip )
(16.7-5)
and for phase q is
i
j
Hq = mpi qj (hip + hf p − hf q )
i
(16.7-6)
j
where hf p and hf q are the formation enthalpies of species i of phase p and species j of
phase q respectively and hip is the enthalpy of species i of phase p (with reference to the
formation enthalpy).
Species Equation
The species source in a cell for species i of phase p is
mip = −mpi qj
(16.7-7)
mjq = mpi qj
(16.7-8)
and for species j of phase q is
Other Scalar Equations
No source/sink terms are added for turbulence quantities and other scalars. The transfer
of these scalar quantities due to mass transfer could be modeled using user-defined source
terms.
16-90
Release 12.0 c ANSYS, Inc. January 29, 2009
16.7 Modeling Mass Transfer in Multiphase Flows
16.7.2
Unidirectional Constant Rate Mass Transfer
The unidirectional mass transfer model defines a positive mass flow rate per unit volume
from phase p to phase q:
m˙pq = max[0, λpq ] − max[0, −λpq ]
(16.7-9)
λpq = ṙαp ρq
(16.7-10)
where
and ṙ is a constant rate of particle shrinking or swelling, such as the rate of burning of
a liquid droplet. This is not available for the VOF model.
If phase p is a mixture material and a mass transfer mechanism is defined for species i
of phase p, then
λpq = ṙαp yp,i ρq
(16.7-11)
where yp,i is the mass fraction of species i in phase p.
16.7.3
UDF-Prescribed Mass Transfer
Because there is no universal model for mass transfer, ANSYS FLUENT provides a UDF
that you can use to input models for different types of mass transfer, e.g. evaporation,
condensation, boiling, etc. Note that when using this UDF, ANSYS FLUENT will automatically add the source contribution to all relevant momentum and scalar equations.
This contribution is based on the assumption that the mass “created” or “destroyed”
will have the same momentum and energy of the phase from which it was created or
destroyed. If you would like to input your source terms directly into momentum, energy,
or scalar equations, then the appropriate path is to use UDFs for user-defined sources
for all equations, rather than the UDF for mass transfer. See the separate UDF Manual
for more information about UDF-based mass transfer in multiphase.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-91
Multiphase Flows
16.7.4
Cavitation Models
A liquid at constant temperature can be subjected to a decreasing pressure, which may
fall below the saturated vapor pressure. The process of rupturing the liquid by a decrease
of pressure at constant temperature is called cavitation. The liquid also contains the
micro-bubbles of noncondensable (dissolved or ingested) gases, or nuclei, which under
decreasing pressure may grow and form cavities. In such processes, very large and steep
density variations happen in the low-pressure/cavitating regions.
This section provides information about the following three cavitation models used in
ANSYS FLUENT.
• Singhal et al. model: You can use this model to include cavitation effects in
two-phase flows when the mixture model is used. This is also known as the Full
Cavitaton Model, which has been implemented in ANSYS FLUENTsince Version
6.1.
• Zwart-Gerber-Belamri model: You can use this model in both the mixture and
Eulerian multiphase models.
• Schnerr and Sauer model: This is the default model. You can use this model in
both the mixture and Eulerian multiphase models.
The following assumptions are made in the standard two-phase cavitation models:
• The system under investigation must consist of a liquid and a vapor phase.
• Mass transfer between the liquid and vapor phase is assumed to take place. Both
bubble formation (evaporation) and collapse (condensation) are taken into account
in the cavitation models.
• The cavitation models are based on the Rayleigh-Plesset equation, describing the
growth of a single vapor bubble in a liquid.
• In the Singhal et al. model, noncondensable gases have been introduced into the
system. The mass fraction of the noncondensable gases is assumed to be a known
constant.
• The input material properties used in the cavitation models can be constants,
functions of temperature or user-defined.
The cavitation models offer the following capabilities:
• The Singhal et al. model can be used to account for the effect of noncondensable
gases. The Zwart-Gerber-Belamri and Schnerr and Sauer models do not include
the noncondensable gases in the basic model terms.
16-92
Release 12.0 c ANSYS, Inc. January 29, 2009
16.7 Modeling Mass Transfer in Multiphase Flows
• The Zwart-Gerber-Belamri and Schnerr and Sauer models are compatible with all
the turbulence models available in ANSYS FLUENT.
• Both the pressure-based segregated and coupled solvers are available with the cavitation models.
• They are all fully compatible with dynamic mesh and non-conformal interfaces.
• Both liquid and vapor phases can be incompressible or compressible. For compressible liquids, the density is described using a user-defined function. See the separate
UDF Manual for more information on user-defined density functions.
Limitations of the Cavitation Models
The following limitations apply to the cavitation models in ANSYS FLUENT:
• None of the cavitation models can be used with the VOF model because the surface
tracking schemes for the VOF model are incompatible with the interpenetrating
continua assumption of the cavitation models.
• They can only be used for cavitating flows occurring in a single liquid fluid.
• The Singhal et al. model requires the primary phase to be a liquid and the secondary
phase to be a vapor. This model is only compatible with the multiphase mixture
model.
• The Singhal et al. model cannot be used with the Eulerian multiphase model.
• The Singhal et al. model is not compatible with the LES turbulence model.
• The Zwart-Gerber-Belamri and Schnerr and Sauer models do not take the effect of
noncondensable gases into account by default.
Vapor Transport Equation
With the multiphase cavitation modeling approach, a basic two-phase cavitation model
consists of using the standard viscous flow equations governing the transport of mixture
(Mixture model) or phases (Eulerian multiphase), and a conventional turbulence model
(k- model). In cavitation, the liquid-vapor mass transfer (evaporation and condensation)
is governed by the vapor transport equation:
∂
~ v ) = Re − Rc
(αρv ) + ∇.(αρv V
∂t
Release 12.0 c ANSYS, Inc. January 29, 2009
(16.7-12)
16-93
Multiphase Flows
where,
v
α
ρv
V~v
Re , Rc
=
=
=
=
=
vapor phase
vapor volume fraction
vapor density
vapor phase velocity
mass transfer source terms connected to the growth and collapse of the
vapor bubbles repectively
In Equation 16.7-12, the terms Re and Rc account for the mass transfer between the
vapor and liquid phases in cavitation. In ANSYS FLUENT, they are modeled based on
the Rayleigh-Plesset equation describing the growth of a single vapor bubble in a liquid.
Bubble Dynamics Consideration
In most engineering situations we assume that there are plenty of nuclei for the inception
of cavitation. Thus, our primary focus is on proper accounting of bubble growth and
collapse. In a flowing liquid with zero velocity slip between the fluid and bubbles, the
bubble dynamics equation can be derived from the generalized Rayleigh-Plesset equation
as [37]
Tsat
ṁe→v = coef f ∗ αl ρl
(T − Tsat )
Tsat
(16.7-40)
ṁe→v = coef f ∗ αv ρv
(T − Tsat )
Tsat
(16.7-41)
If T < Tsat
ṁe→v represents the rate of mass transfer from the liquid phase to the vapor phase, with
units of kg/s/m3 . coef f is a coefficient that needs to be fine tuned and can be interpreted
as a relaxation time. α and ρ are the phase volume fraction and density, respectively.
The source term for the energy equation can be obtained by multiplying the rate of mass
transfer by the latent heat.
Consider the Hertz Knudsen formula, which gives the evaporation-condensation flux
based on the kinetic theory for a flat interface:
s
F =β
M
(P ∗ − Psat )
2πRTsat
(16.7-42)
The flux has units of kg/s/m2 , P is the pressure, T is the temperature, and R is the
universal gas constant. The coefficient β is the so-called accommodation coefficient that
shows the portion of vapor molecules going into the liquid surface and adsorbed by this
surface. P ∗ represents the vapor partial pressure at the interface on the gas side. The
Clapeyron-Clausius equation relates the pressure to the temperature for the saturation
condition. (It is obtained by equating the vapor and liquid chemical potentials):
16-104
Release 12.0 c ANSYS, Inc. January 29, 2009
16.7 Modeling Mass Transfer in Multiphase Flows
Figure 16.7.1: The Stability Phase Diagram
dP
L
=
dT
T (vg − vl )
(16.7-43)
vg and vl are the inverse of the density for the gas and liquid (volume per mass unit),
respectively. L is the latent heat (J/kg).
Based on this differential expression, we can obtain variation of temperature from variation of pressure close to the saturation condition.
The Clausius Clapeyron equation yields the following formula as long as P ∗ and T ∗ are
close to the saturation condition:
(P ∗ − Psat ) = −
L
(T ∗ − Tsat )
T (vg − vl )
(16.7-44)
Using this relation in the above Hertz Knudsen equation yields [346]
s
M
ρg ρl
L
F =β
2πRTsat
ρl − ρg
!
(T ∗ − Tsat )
Tsat
(16.7-45)
The factor β is defined by means of the accomodation coefficient and the physical characteristics of the gas. β approaches 1.0 at near equilibrium conditions.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-105
Multiphase Flows
In the Eulerian and mixture multiphase models, the flow regime is assumed to be dispersed. If we assume that all vapor bubbles, for example, have the same diameter, then
the interfacial area density is given by the following formula:
Ai
6αv
=
Vcell
d
(16.7-46)
where Vcell is the cell volume and the phase source term (kg/s/m3 ) should be of the form:
s
Ai
6
M
ρl
F
= β
L
Vcell
d
2πRTsat
ρl − ρg
(T ∗ − Tsat
ρg αv
Tsat
!"
#
(16.7-47)
From the above equation, coef f , which is the inverse of the relaxation time (1/s) is
defined as
s
M
ρl
6
L
coef f = β
2πRTsat
ρl − ρg
d
!
(16.7-48)
This leads to the final expression for the vaporization, defined in Equation 16.7-41. It
can be treated implicitly as a source term in the phase conservation equation.
A similar expression can be obtained for condensation. In this case, we consider small
droplets in a continuous vapor phase even if your primary phase is a liquid.
Note that the coefficient coef f should theoretically be different for the condensation and
evaporation expression. Furthermore, the theoretical expression is based on a few strong
assumptions:
• flat interface
• dispersed regime with constant diameter
• known β
The bubble diameter and accommodation coefficient are usually not very well known,
which is why the coefficient coef f can be fine tuned to match experimental data. By
default, the coefficient for both evaporation and condensation is 0.1.
16-106
Release 12.0 c ANSYS, Inc. January 29, 2009
16.8 Modeling Species Transport in Multiphase Flows
16.8
Modeling Species Transport in Multiphase Flows
Species transport, as described in Chapter 7: Species Transport and Finite-Rate Chemistry,
can also be applied to multiphase flows. You can choose to solve the conservation equations for chemical species in multiphase flows by having ANSYS FLUENT, for each phase k,
predict the local mass fraction of each species, Yi k , through the solution of a convectiondiffusion equation for the ith species. The generalized chemical species conservation
equation (Equation 7.1-1), when applied to a multiphase mixture can be represented in
the following form:
n
X
q
∂ q q q
(ρ α Yi )+∇·(ρq αq~v q Yi q ) = −∇·αq J~i +αq Ri q +αq Si q + (ṁpi qj − ṁqj pi )+R (16.8-1)
∂t
p=1
where Ri q is the net rate of production of homogeneous species i by chemical reaction for
phase q, ṁqj pi is the mass transfer source between species i and j from phase q to p, and
R is the heterogeneous reaction rate. In addition, αq is the volume fraction for phase q
and Si q is the rate of creation by addition from the dispersed phase plus any user-defined
sources.
ANSYS FLUENT treats homogeneous gas phase chemical reactions the same as a singlephase chemical reaction. The reactants and the products belong to the same mixture
material (set in the Species Model dialog box), and hence the same phase. The reaction
rate is scaled by the volume fraction of the particular phase in the cell.
The set-up of a homogeneous gas phase chemical reaction in ANSYS FLUENT is the
same as it is for a single phase. For more information, see Chapter 7: Species Transport
and Finite-Rate Chemistry. For most multiphase species transport problems, boundary
conditions for a particular species are set in the associated phase boundary condition
dialog box (see Section 24.2.9: Defining Multiphase Cell Zone and Boundary Conditions
in the separate User’s Guide), and postprocessing and reporting of results is performed
on a per-phase basis (see Section 24.8: Postprocessing for Multiphase Modeling in the
separate User’s Guide).
For multiphase species transport simulations, the Species Model dialog box allows you to
include Volumetric, Wall Surface, and Particle Surface reactions. ANSYS FLUENT treats
multiphase surface reactions as it would a single-phase reaction. The reaction rate is
scaled with the volume fraction of the particular phase in the cell. For more information,
see Chapter 7: Species Transport and Finite-Rate Chemistry.
i
To turn off reactions for a particular phase, while keeping the reactions
active for other phases. turn on Volumetric under Reactions in the Species
Model dialog box. Then, in the Create/Edit Materials dialog box, select
none from the Reactions drop-down list.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-107
Multiphase Flows
The species of different phases is entirely independent. There is no implicit relationship
between them even if they share the same name. Explicit relationships between species of
different phases can be specified through mass transfer and heterogeneous reactions. For
more information on mass transfer and heterogeneous reactions, see Section 24.2.8: Including Mass Transfer Effects and Section 24.2.7: Specifying Heterogeneous Reactions in
the separate User’s Guide, respectively.
Some phases may have a fluid material associated with them instead of a mixture material. The species equations are solved in those phases that are assigned a mixture
material. The species equation above is solved for the mass fraction of the species in a
particular phase. The mass transfer and heterogeneous reactions will be associated with
the bulk fluid for phases with a single fluid material.
Additional information about modeling species transport is presented in the following
subsections:
• Section 16.8.1: Limitations
• Section 16.8.2: Mass and Momentum Transfer with Multiphase Species Transport
• Section 16.8.3: The Stiff Chemistry Solver
16.8.1
Limitations
The following limitations exist for the modeling of species transport for multiphase flows:
• The nonpremixed, premixed, partially-premixed combustion, or the composition
PDF transport species transport models are not available for multiphase species
reactions.
• Only the laminar finite-rate, finite-rate/eddy-dissipation and eddy-dissipation
turbulence-chemistry models of homogeneous reactions are available for multiphase
species transport.
• The discrete phase model (DPM) is not compatible with multiphase species transport.
16.8.2
Mass and Momentum Transfer with Multiphase Species Transport
The ANSYS FLUENT multiphase mass transfer model accommodates mass transfer between species belonging to different phases. Instead of a matrix-type input, multiple mass
transfer mechanisms need to be input. Each mass transfer mechanism defines the mass
transfer phenomenon from one entity to another entity. An entity is either a particular
species in a phase, or the bulk phase itself if the phase does not have a mixture material associated with it. The mass transfer phenomenon could be specified either through
16-108
Release 12.0 c ANSYS, Inc. January 29, 2009
16.8 Modeling Species Transport in Multiphase Flows
the inbuilt unidirectional “constant-rate” mass transfer (Section 16.7.2: Unidirectional
Constant Rate Mass Transfer) or through user-defined functions.
ANSYS FLUENT loops through all the mass transfer mechanisms to compute the net
mass source/sink of each species in each phase. The net mass source/sink of a species is
used to compute species and mass source terms. ANSYS FLUENT will also automatically
add the source contribution to all relevant momentum and energy equations based on
that assumption that the momentum and energy carried along with the transferred mass.
For other equations, the transport due to mass transfer needs to be explicitly modeled
by the user.
Source Terms due to Heterogeneous Reactions
Consider the following reaction:
aA + bB → cC + dD
(16.8-2)
Let as assume that A and C belong to phase 1 and B and D to phase 2.
Mass Transfer
Mass source for the phases are given by:
S1 = R(cMc − aMa )
S2 = R(dMd − bMb )
(16.8-3)
(16.8-4)
where S is the mass source, M is the molecular weight, and R is the reaction rate.
The general expression for the mass source for the ith phase is
Sri = −R
X
γjr Mjr
(16.8-5)
ri
Spi = R
X
γjp Mjp
(16.8-6)
pi
Si = Spi + Sri
(16.8-7)
where γ is the stoichiometric coefficient, p represents the product, and r represents the
reactant.
Momentum Transfer
Momentum transfer is more complicated, but we can assume that the reactants mix
(conserving momentum) and the products take momentum in the ratio of the rate of
their formation.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-109
Multiphase Flows
The net velocity, ~unet , of the reactants is given by:
~unet =
aMa~u1 + bMb~u2
aMa + bMb
(16.8-8)
The general expression for the net velocity of the reactants is given by:
r
r
ur
rγ M ~
~unet = P j r j r j
r γj Mj
P
(16.8-9)
where j represents the j th item (either a reactant or a product).
Momentum transfer for the phases is then given by:
S1~u = R(cMc~unet − aMa~u1 )
S2~u = R(dMd~unet − bMb~u2 )
(16.8-10)
(16.8-11)
Si~u = Spi ~unet − R
(16.8-12)
The general expression is
X
γjr Mjr ~ui
ri
If we assume that there is no momentum transfer, then the above term will be zero.
Species Transfer
The general expression for source for k th species in the j th phase is
Srik = −R
Spki = R
X
k
γjr Mjr
(16.8-13)
rik
X
k
k
γjp Mjp
(16.8-14)
pki
Sik = Spki + Srik
16-110
k
(16.8-15)
Release 12.0 c ANSYS, Inc. January 29, 2009
16.8 Modeling Species Transport in Multiphase Flows
Heat Transfer
For heat transfer, we need to consider the formation enthalpies of the reactants and
products as well:
The net enthalpy of the reactants is given by:
Hnet =
aMa (Ha + hfa ) + bMb (Hb + hfb )
aMa + bMb
(16.8-16)
where hf represents the formation enthalpy, and H represents the enthalpy.
The general expression for Hnet is:
r
P
Hnet =
r
γjr Mjr (Hjr + hf j )
P r r
r γj Mj
(16.8-17)
If we assume that this enthalpy gets distributed to the products in the ratio of their mass
production rates, heat transfer for the phases are given by:
S1H = R(cMc Hnet − aMa H a − cMc hcf )
(16.8-18)
S2H
(16.8-19)
b
= R(dMd Hnet − bMb H −
dMd hdf )
The last term in the above equations appears because our enthalpy is with reference to
the formation enthalpy.
The general expression for the heat source is:
SiH
= Spi Hnet − R
X
γjr Mjr Hjr
+
ri
X
p
γjp Mjp hf j
!
(16.8-20)
pi
If we assume that there is no heat transfer, we can assume that the different species only
carry their formation enthalpies with them. Thus the expression for Hnet will be:
r
γjr Mjr hf j
P r r
r γj Mj
P
Hnet =
r
(16.8-21)
The expression SiH will be
SiH = Spi Hnet − R
X
p
γjp Mjp hf j
(16.8-22)
pi
16.8.3
The Stiff Chemistry Solver
ANSYS FLUENT has the option of solving intraphase and inter phase chemical reactions
with a stiff chemistry solver. This option is only available for unsteady cases, where
a fractional step scheme is applied. In the first fractional step, the multiphase species
Equation 16.8-1 is solved spatially with the reaction term Ri q set to zero. In the second
fractional step, the reaction term is integrated in every cell using a stiff ODE solver.
Release 12.0 c ANSYS, Inc. January 29, 2009
16-111
Multiphase Flows
16-112
Release 12.0 c ANSYS, Inc. January 29, 2009
Chapter 17.
Solidification and Melting
This chapter describes how you can model solidification and melting in ANSYS FLUENT.
For information about using the model, see Chapter 25: Modeling Solidification and
Melting in the separate User’s Guide. Information about the theory behind the model is
organized into the following sections:
• Section 17.1: Overview
• Section 17.2: Limitations
• Section 17.3: Introduction
• Section 17.4: Energy Equation
• Section 17.5: Momentum Equations
• Section 17.6: Turbulence Equations
• Section 17.7: Species Equations
• Section 17.8: Pull Velocity for Continuous Casting
• Section 17.9: Contact Resistance at Walls
17.1
Overview
ANSYS FLUENT can be used to solve fluid flow problems involving solidification and/or
melting taking place at one temperature (e.g., in pure metals) or over a range of temperatures (e.g., in binary alloys). Instead of tracking the liquid-solid front explicitly, ANSYS
FLUENT uses an enthalpy-porosity formulation. The liquid-solid mushy zone is treated
as a porous zone with porosity equal to the liquid fraction, and appropriate momentum
sink terms are added to the momentum equations to account for the pressure drop caused
by the presence of solid material. Sinks are also added to the turbulence equations to
account for reduced porosity in the solid regions.
Release 12.0 c ANSYS, Inc. January 29, 2009
17-1
Solidification and Melting
ANSYS FLUENT provides the following capabilities for modeling solidification and melting:
• calculation of liquid-solid solidification/melting in pure metals as well as in binary
alloys
• modeling of continuous casting processes (i.e., “pulling” of solid material out of the
domain)
• modeling of the thermal contact resistance between solidified material and walls
(e.g., due to the presence of an air gap)
• modeling of species transport with solidification/melting
• postprocessing of quantities related to solidification/melting (i.e., liquid fraction
and pull velocities)
These modeling capabilities allow ANSYS FLUENT to simulate a wide range of solidification/melting problems, including melting, freezing, crystal growth, and continuous casting. The physical equations used for these calculations are described in Section 17.3: Introduction, and instructions for setting up and solving a solidification/melting
problem are provided in Section 25: Modeling Solidification and Melting in the separate
User’s Guide.
17.2
Limitations
As mentioned in Section 17.1: Overview, the formulation in ANSYS FLUENT can be used
to model the solidification/melting of pure materials, as well as alloys. ANSYS FLUENT
offers two rules to determine the liquid fraction versus temperature relationship, namely
the linear Lever rule and the non-linear Scheil rule.
The following limitations apply to the solidification/melting model in ANSYS FLUENT:
• The solidification/melting model can be used only with the pressure-based solver;
it is not available with the density-based solvers.
• The solidification/melting model cannot be used for compressible flows.
• Of the general multiphase models (VOF, mixture, and Eulerian), only the VOF
model can be used with the solidification/melting model.
• With the exception of species diffusivities, you cannot specify material properties
separately for the solid and liquid materials.
• When using the solidification/melting model in conjunction with modeling species
transport with reactions, there is no mechanism to restrict the reactions to only
the liquid region; i.e., the reactions are solved everywhere.
17-2
Release 12.0 c ANSYS, Inc. January 29, 2009
17.3 Introduction
17.3
Introduction
An enthalpy-porosity technique [358, 360, 361] is used in ANSYS FLUENT for modeling
the solidification/melting process. In this technique, the melt interface is not tracked
explicitly. Instead, a quantity called the liquid fraction, which indicates the fraction of
the cell volume that is in liquid form, is associated with each cell in the domain. The
liquid fraction is computed at each iteration, based on an enthalpy balance.
The mushy zone is a region in which the liquid fraction lies between 0 and 1. The mushy
zone is modeled as a “pseudo” porous medium in which the porosity decreases from 1 to
0 as the material solidifies. When the material has fully solidified in a cell, the porosity
becomes zero and hence the velocities also drop to zero.
In this section, an overview of the solidification/melting theory is given. Refer to Voller
and Prakash [361] for details on the enthalpy-porosity method.
17.4
Energy Equation
The enthalpy of the material is computed as the sum of the sensible enthalpy, h, and the
latent heat, ∆H:
H = h + ∆H
(17.4-1)
where
h = href +
and href
Tref
cp
Z
T
Tref
cp dT
(17.4-2)
= reference enthalpy
= reference temperature
= specific heat at constant pressure
The liquid fraction, β, can be defined as
β = 0 if T < Tsolidus
β = 1 if T > Tliquidus
β=
T − Tsolidus
if Tsolidus < T < Tliquidus
Tliquidus − Tsolidus
(17.4-3)
The latent heat content can now be written in terms of the latent heat of the material,
L:
∆H = βL
Release 12.0 c ANSYS, Inc. January 29, 2009
(17.4-4)
17-3
Solidification and Melting
The latent heat content can vary between zero (for a solid) and L (for a liquid).
For solidification/melting problems, the energy equation is written as
∂
(ρH) + ∇ · (ρ~v H) = ∇ · (k∇T ) + S
∂t
where
H
ρ
~v
S
(17.4-5)
= enthalpy (see Equation 17.4-1)
= density
= fluid velocity
= source term
The solution for temperature is essentially an iteration between the energy equation
(Equation 17.4-5) and the liquid fraction equation (Equation 17.4-3). Directly using
Equation 17.4-3 to update the liquid fraction usually results in poor convergence of
the energy equation. In ANSYS FLUENT, the method suggested by Voller and Swaminathan [362] is used to update the liquid fraction. For pure metals, where Tsolidus and
Tliquidus are equal, a method based on specific heat, given by Voller and Prakash [361], is
used instead.
17.5
Momentum Equations
The enthalpy-porosity technique treats the mushy region (partially solidified region) as a
porous medium. The porosity in each cell is set equal to the liquid fraction in that cell.
In fully solidified regions, the porosity is equal to zero, which extinguishes the velocities
in these regions. The momentum sink due to the reduced porosity in the mushy zone
takes the following form:
S=
(1 − β)2
Amush (~v − ~vp )
(β 3 + )
(17.5-1)
where β is the liquid volume fraction, is a small number (0.001) to prevent division by
zero, Amush is the mushy zone constant, and ~vp is the solid velocity due to the pulling of
solidified material out of the domain (also referred to as the pull velocity).
The mushy zone constant measures the amplitude of the damping; the higher this value,
the steeper the transition of the velocity of the material to zero as it solidifies. Very large
values may cause the solution to oscillate.
The pull velocity is included to account for the movement of the solidified material as
it is continuously withdrawn from the domain in continuous casting processes. The
presence of this term in Equation 17.5-1 allows newly solidified material to move at the
pull velocity. If solidified material is not being pulled from the domain, ~vp = 0. More
details about the pull velocity are provided in Section 17.8: Pull Velocity for Continuous
Casting.
17-4
Release 12.0 c ANSYS, Inc. January 29, 2009
17.6 Turbulence Equations
17.6
Turbulence Equations
Sinks are added to all of the turbulence equations in the mushy and solidified zones to
account for the presence of solid matter. The sink term is very similar to the momentum
sink term (Equation 17.5-1):
S=
(1 − β)2
Amush φ
(β 3 + )
(17.6-1)
where φ represents the turbulence quantity being solved (k, , ω, etc.), and the mushy
zone constant, Amush , is the same as the one used in Equation 17.5-1.
17.7
Species Equations
For solidification and melting of a pure substance, phase change occurs at a distinct melting temperature, Tmelt . For a multicomponent mixture, however, a mushy freeze/melt
zone exists between a lower solidus and an upper liquidus temperature. When a multicomponent liquid solidifies, solutes diffuse from the solid phase into the liquid phase.
This effect is quantified by the partition coefficient of solute i, denoted Ki , which is the
ratio of the mass fraction in the solid to that in the liquid at the interface.
ANSYS FLUENT computes the solidus and liquidus temperatures in a species mixture as,
Tsolidus = Tmelt +
X
mi Yi /Ki
(17.7-1)
m i Yi
(17.7-2)
solutes
Tliquidus = Tmelt +
X
solutes
where Ki is the partition coefficient of solute i, Yi is the mass fraction of solute i, and mi
is the slope of the liquidus surface with respect to Yi . It is assumed that the last species
material of the mixture is the solvent and that the other species are the solutes.
The liquidus slope of species i, mi , is calculated from the Eutectic temperature and the
Eutectic mass fraction as,
mi =
TEut − Tmelt
Yi,Eut
(17.7-3)
Updating the liquid fraction via Equation 17.4-3 can cause numerical errors and convergence difficulties in multicomponent mixtures. Instead, the liquid fraction is updated
as,
β n+1 = β n − λ
Release 12.0 c ANSYS, Inc. January 29, 2009
ap (T − T ∗ ) ∆t
∗
ρV L − ap ∆tL ∂T
∂β
(17.7-4)
17-5
Solidification and Melting
where the superscript n indicates the iteration number, λ is a relaxation factor with a
default value if 0.9, ap is the cell matrix co-efficient, ∆t is the time-step, ρ is the current
density, V is the cell volume, T is the current cell temperature and T ∗ is the interface
temperature.
ANSYS FLUENT offers two models for species segregation at the micro-scale, namely the
Lever and Scheil rules. The former assumes infinite diffusion of the solute species in the
solid, and the latter assumes zero diffusion. For the Lever rule, the interface temperature,
T ∗ , is calculated for a binary mixture as,
T∗ =
Tliquidus − Tmelt (1 − β)(1 − P )
1 − Tmelt (1 − β)(1 − P )
(17.7-5)
Tmelt − Tliquidus
Tmelt − Tsolidus
(17.7-6)
where
P =
The Scheil rule evaluates T ∗ as,
T ∗ = Tmelt − (Tmelt − Tliquidus )β (P −1)
(17.7-7)
For the Lever rule, species transport equations are solved for the total mass fraction of
species i, Yi :
∂
(ρYi ) + ∇ · (ρ [β~vliq Yi,liq + (1 − β)~vp Yi,sol ]) = −∇ · J~i + Ri
∂t
(17.7-8)
where Ri is the reaction rate and J~i is given by
J~i = −ρ[βDi,m,liq ∇Yi,liq + (1 − β)Di,m,sol ∇Yi,sol ]
(17.7-9)
~vliq is the velocity of the liquid and ~vp is the solid (pull) velocity. ~vp is set to zero if pull
velocities are not included in the solution. The liquid velocity can be found from the
average velocity (as determined by the flow equation) as
~vliq =
(~v − ~vp (1 − β))
β
(17.7-10)
The liquid (Yi,liq ) and solid (Yi,sol ) mass fractions are related to each other by the partition
coefficient Ki :
Yi,sol = Ki Yi,liq
17-6
(17.7-11)
Release 12.0 c ANSYS, Inc. January 29, 2009
17.8 Pull Velocity for Continuous Casting
When the Scheil model is selected, ANSYS FLUENT solves for Yi,liq as the dependent
variable [359]:
∂
(ρYi,liq ) + ∇ · (ρ [β~vliq Yi,liq + (1 − β)~vp Yi,sol ]) = Ri +
∂t
∂
∂
∇ · (ρβDi,m,liq ∇Yi,liq ) − Ki Yi,liq (ρ(1 − β)) + (ρ(1 − β)Yi,liq )
∂t
∂t
17.8
(17.7-12)
Pull Velocity for Continuous Casting
In continuous casting processes, the solidified matter is usually continuously pulled out
from the computational domain, as shown in Figure 17.8.1. Consequently, the solid
material will have a finite velocity that needs to be accounted for in the enthalpy-porosity
technique.
mushy zone
solidified shell
vp
liquid pool
wall
Figure 17.8.1: “Pulling” a Solid in Continuous Casting
As mentioned in Section 17.5: Momentum Equations, the enthalpy-porosity approach
treats the solid-liquid mushy zone as a porous medium with porosity equal to the liquid
fraction. A suitable sink term is added in the momentum equation to account for the
pressure drop due to the porous structure of the mushy zone. For continuous casting
applications, the relative velocity between the molten liquid and the solid is used in the
momentum sink term (Equation 17.5-1) rather than the absolute velocity of the liquid.
The exact computation of the pull velocity for the solid material is dependent on the
Young’s modulus and Poisson’s ratio of the solid and the forces acting on it. ANSYS
FLUENT uses a Laplacian equation to approximate the pull velocities in the solid region
based on the velocities at the boundaries of the solidified region:
∇2~vp = 0
Release 12.0 c ANSYS, Inc. January 29, 2009
(17.8-1)
17-7
Solidification and Melting
ANSYS FLUENT uses the following boundary conditions when computing the pull velocities:
• At a velocity inlet, a stationary wall, or a moving wall, the specified velocity is
used.
• At all other boundaries (including the liquid-solid interface between the liquid and
solidified material), a zero-gradient velocity is used.
The pull velocities are computed only in the solid region.
Note that ANSYS FLUENT can also use a specified constant value or custom field function
for the pull velocity, instead of computing it. See Section 25.2: Procedures for Modeling
Continuous Casting in the separate User’s Guide for details.
17.9
Contact Resistance at Walls
ANSYS FLUENT’s solidification/melting model can account for the presence of an air gap
between the walls and the solidified material, using an additional heat transfer resistance
between walls and cells with liquid fractions less than 1. This contact resistance is
accounted for by modifying the conductivity of the fluid near the wall. Thus, the wall
heat flux, as shown in Figure 17.9.1, is written as
q=
(T − Tw )
(l/k + Rc (1 − β))
(17.9-1)
where T , Tw , and l are defined in Figure 17.9.1, k is the thermal conductivity of the fluid,
β is the liquid volume fraction, and Rc is the contact resistance, which has the same units
as the inverse of the heat transfer coefficient.
17-8
Release 12.0 c ANSYS, Inc. January 29, 2009
17.9 Contact Resistance at Walls
wall
near-wall cell
Tw
●
T
l
T
Tw
●
●
Rc
●
l/k
Figure 17.9.1: Circuit for Contact Resistance
Release 12.0 c ANSYS, Inc. January 29, 2009
17-9
Solidification and Melting
17-10
Release 12.0 c ANSYS, Inc. January 29, 2009
Chapter 18.
Solver Theory
This chapter describes the ANSYS FLUENT solver theory. Details about the solver algorithms used by ANSYS FLUENT are provided in Sections 18.1–18.6. For more information
about using the solver, see Chapter 26: Using the Solver in the separate User’s Guide.
• Section 18.1: Overview of Flow Solvers
• Section 18.2: General Scalar Transport Equation: Discretization and Solution
• Section 18.3: Discretization
• Section 18.4: Pressure-Based Solver
• Section 18.5: Density-Based Solver
• Section 18.6: Multigrid Method
• Section 18.7: Full Multigrid (FMG) Initialization
18.1
Overview of Flow Solvers
ANSYS FLUENT allows you to choose one of the two numerical methods:
• pressure-based solver (see Section 18.1.1: Pressure-Based Solver)
• density-based solver (see Section 18.1.2: Density-Based Solver)
Historically speaking, the pressure-based approach was developed for low-speed incompressible flows, while the density-based approach was mainly used for high-speed compressible flows. However, recently both methods have been extended and reformulated to
solve and operate for a wide range of flow conditions beyond their traditional or original
intent.
In both methods the velocity field is obtained from the momentum equations. In the
density-based approach, the continuity equation is used to obtain the density field while
the pressure field is determined from the equation of state.
On the other hand, in the pressure-based approach, the pressure field is extracted by
solving a pressure or pressure correction equation which is obtained by manipulating
continuity and momentum equations.
Release 12.0 c ANSYS, Inc. January 29, 2009
18-1
Solver Theory
Using either method, ANSYS FLUENT will solve the governing integral equations for
the conservation of mass and momentum, and (when appropriate) for energy and other
scalars such as turbulence and chemical species. In both cases a control-volume-based
technique is used that consists of:
• Division of the domain into discrete control volumes using a computational grid.
• Integration of the governing equations on the individual control volumes to construct algebraic equations for the discrete dependent variables (“unknowns”) such
as velocities, pressure, temperature, and conserved scalars.
• Linearization of the discretized equations and solution of the resultant linear equation system to yield updated values of the dependent variables.
The two numerical methods employ a similar discretization process (finite-volume), but
the approach used to linearize and solve the discretized equations is different.
The general solution methods are described in Sections 18.1.1 and 18.1.2. To learn how
to apply the solvers, see Section 26.1.1: Choosing the Solver in the separate User’s Guide.
18.1.1
Pressure-Based Solver
The pressure-based solver employs an algorithm which belongs to a general class of methods called the projection method [54]. In the projection method, wherein the constraint
of mass conservation (continuity) of the velocity field is achieved by solving a pressure
(or pressure correction) equation. The pressure equation is derived from the continuity
and the momentum equations in such a way that the velocity field, corrected by the pressure, satisfies the continuity. Since the governing equations are nonlinear and coupled to
one another, the solution process involves iterations wherein the entire set of governing
equations is solved repeatedly until the solution converges.
Two pressure-based solver algorithms are available in ANSYS FLUENT. A segregated
algorithm, and a coupled algorithm. These two approaches are discussed in the sections
below.
The Pressure-Based Segregated Algorithm
The pressure-based solver uses a solution algorithm where the governing equations are
solved sequentially (i.e., segregated from one another). Because the governing equations
are non-linear and coupled, the solution loop must be carried out iteratively in order to
obtain a converged numerical solution.
18-2
Release 12.0 c ANSYS, Inc. January 29, 2009
18.1 Overview of Flow Solvers
In the segregated algorithm, the individual governing equations for the solution variables
(e.g., u, v, w, p, T , k, , etc.) are solved one after another . Each governing equation,
while being solved, is “decoupled” or “segregated” from other equations, hence its name.
The segregated algorithm is memory-efficient, since the discretized equations need only
be stored in the memory one at a time. However, the solution convergence is relatively
slow, inasmuch as the equations are solved in a decoupled manner.
With the segregated algorithm, each iteration consists of the steps illustrated in Figure 18.1.1 and outlined below:
1. Update fluid properties (e,g, density, viscosity, specific heat) including turbulent
viscosity (diffusivity) based on the current solution.
2. Solve the momentum equations, one after another, using the recently updated values of pressure and face mass fluxes.
3. Solve the pressure correction equation using the recently obtained velocity field and
the mass-flux.
4. Correct face mass fluxes, pressure, and the velocity field using the pressure correction obtained from Step 3.
5. Solve the equations for additional scalars, if any, such as turbulent quantities,
energy, species, and radiation intensity using the current values of the solution
variables.
6. Update the source terms arising from the interactions among different phases (e.g.,
source term for the carrier phase due to discrete particles).
7. Check for the convergence of the equations.
These steps are continued until the convergence criteria are met.
Release 12.0 c ANSYS, Inc. January 29, 2009
18-3
Solver Theory
Pressure−Based Segregated Algorithm
Pressure−Based Coupled Algorithm
Update properties
Update properties
Solve sequentially:
Uvel Vvel Wvel
Solve simultaneously:
system of momentum
and pressure−based
continuity equations
Solve pressure−correction
(continuity) equation
Update mass flux,
pressure, and velocity
Update mass flux
Solve energy, species,
turbulence, and other
scalar equations
Solve energy, species,
turbulence, and other
scalar equations
No
Converged?
Yes
Stop
No
Converged?
Yes
Stop
Figure 18.1.1: Overview of the Pressure-Based Solution Methods
18-4
Release 12.0 c ANSYS, Inc. January 29, 2009
18.1 Overview of Flow Solvers
The Pressure-Based Coupled Algorithm
Unlike the segregated algorithm described above, the pressure-based coupled algorithm
solves a coupled system of equations comprising the momentum equations and the pressurebased continuity equation. Thus, in the coupled algorithm, Steps 2 and 3 in the segregated solution algorithm are replaced by a single step in which the coupled system of
equations are solved. The remaining equations are solved in a decoupled fashion as in
the segregated algorithm.
Since the momentum and continuity equations are solved in a closely coupled manner,
the rate of solution convergence significantly improves when compared to the segregated
algorithm. However, the memory requirement increases by 1.5 – 2 times that of the segregated algorithm since the discrete system of all momentum and pressure-based continuity
equations needs to be stored in the memory when solving for the velocity and pressure
fields (rather than just a single equation, as is the case with the segregated algorithm).
18.1.2
Density-Based Solver
The density-based solver solves the governing equations of continuity, momentum, and
(where appropriate) energy and species transport simultaneously (i.e., coupled together).
Governing equations for additional scalars will be solved afterward and sequentially (i.e.,
segregated from one another and from the coupled set) using the procedure described in
Section 18.2: General Scalar Transport Equation: Discretization and Solution. Because
the governing equations are non-linear (and coupled), several iterations of the solution
loop must be performed before a converged solution is obtained. Each iteration consists
of the steps illustrated in Figure 18.1.2 and outlined below:
1. Update the fluid properties based on the current solution. (If the calculation has
just begun, the fluid properties will be updated based on the initialized solution.)
2. Solve the continuity, momentum, and (where appropriate) energy and species equations simultaneously.
3. Where appropriate, solve equations for scalars such as turbulence and radiation
using the previously updated values of the other variables.
4. When interphase coupling is to be included, update the source terms in the appropriate continuous phase equations with a discrete phase trajectory calculation.
5. Check for convergence of the equation set.
These steps are continued until the convergence criteria are met.
Release 12.0 c ANSYS, Inc. January 29, 2009
18-5
Solver Theory
Update properties
Solve continuity, momentum, energy, and
species equations simultaneously
Solve turbulence and other scalar equations
No
Converged?
Yes
Stop
Figure 18.1.2: Overview of the Density-Based Solution Method
In the density-based solution method, you can solve the coupled system of equations (continuity, momentum, energy and species equations if available) using, either the coupledexplicit formulation or the coupled-implicit formulation. The main distinction between
the density-based explicit and implicit formulations is described next.
In the density-based solution methods, the discrete, non-linear governing equations are
linearized to produce a system of equations for the dependent variables in every computational cell. The resultant linear system is then solved to yield an updated flow-field
solution.
The manner in which the governing equations are linearized may take an “implicit” or
“explicit” form with respect to the dependent variable (or set of variables) of interest.
By implicit or explicit we mean the following:
• implicit: For a given variable, the unknown value in each cell is computed using
a relation that includes both existing and unknown values from neighboring cells.
Therefore each unknown will appear in more than one equation in the system, and
these equations must be solved simultaneously to give the unknown quantities.
• explicit: For a given variable, the unknown value in each cell is computed using a
relation that includes only existing values. Therefore each unknown will appear in
only one equation in the system and the equations for the unknown value in each
cell can be solved one at a time to give the unknown quantities.
18-6
Release 12.0 c ANSYS, Inc. January 29, 2009
18.1 Overview of Flow Solvers
In the density-based solution method you have a choice of using either an implicit or explicit linearization of the governing equations. This choice applies only to the coupled set
of governing equations. Transport equations for additional scalars are solved segregated
from the coupled set (such as turbulence, radiation, etc.). The transport equations are
linearized and solved implicitly using the method described in section Section 18.2: General Scalar Transport Equation: Discretization and Solution. Regardless of whether you
choose the implicit or explicit methods, the solution procedure shown in Figure 18.1.2 is
followed.
If you choose the implicit option of the density-based solver, each equation in the coupled
set of governing equations is linearized implicitly with respect to all dependent variables
in the set. This will result in a system of linear equations with N equations for each cell
in the domain, where N is the number of coupled equations in the set. Because there are
N equations per cell, this is sometimes called a “block” system of equations.
A point implicit linear equation solver (Incomplete Lower Upper (ILU) factorization
scheme or a symmetric block Gauss-Seidel) is used in conjunction with an algebraic
multigrid (AMG) method to solve the resultant block system of equations for all N
dependent variables in each cell. For example, linearization of the coupled continuity, x-,
y-, z-momentum, and energy equation set will produce a system of equations in which
p, u, v, w, and T are the unknowns. Simultaneous solution of this equation system
(using the block AMG solver) yields at once updated pressure, u-, v-, w-velocity, and
temperature fields.
In summary, the coupled implicit approach solves for all variables (p, u, v, w, T ) in all
cells at the same time.
If you choose the explicit option of the density-based solver, each equation in the coupled
set of governing equations is linearized explicitly. As in the implicit option, this too will
result in a system of equations with N equations for each cell in the domain and likewise,
all dependent variables in the set will be updated at once. However, this system of
equations is explicit in the unknown dependent variables. For example, the x-momentum
equation is written such that the updated x velocity is a function of existing values of
the field variables. Because of this, a linear equation solver is not needed. Instead,
the solution is updated using a multi-stage (Runge-Kutta) solver. Here you have the
additional option of employing a full approximation storage (FAS) multigrid scheme to
accelerate the multi-stage solver.
In summary, the density-based explicit approach solves for all variables (p, u, v, w, T )
one cell at a time.
Note that the FAS multigrid is an optional component of the explicit approach, while
the AMG is a required element in both the pressure-based and density-based implicit
approaches.
Release 12.0 c ANSYS, Inc. January 29, 2009
18-7
Solver Theory
18.2
General Scalar Transport Equation: Discretization and Solution
ANSYS FLUENT uses a control-volume-based technique to convert a general scalar transport equation to an algebraic equation that can be solved numerically. This control
volume technique consists of integrating the transport equation about each control volume, yielding a discrete equation that expresses the conservation law on a control-volume
basis.
Discretization of the governing equations can be illustrated most easily by considering the
unsteady conservation equation for transport of a scalar quantity φ. This is demonstrated
by the following equation written in integral form for an arbitrary control volume V as
follows:
Z
V
I
I
Z
∂ρφ
~ = Γφ ∇φ · dA
~ + Sφ dV
dV + ρφ ~v · dA
∂t
V
(18.2-1)
where
ρ
~v
~
A
Γφ
∇φ
Sφ
=
=
=
=
=
=
density
velocity vector (= u ı̂ + v ̂ in 2D)
surface area vector
diffusion coefficient for φ
gradient of φ (= ∂φ/∂x) ı̂ + (∂φ/∂y) ̂ in 2D)
source of φ per unit volume
Equation 18.2-1 is applied to each control volume, or cell, in the computational domain.
The two-dimensional, triangular cell shown in Figure 18.2.1 is an example of such a
control volume. Discretization of Equation 18.2-1 on a given cell yields
NX
NX
faces
faces
∂ρφ
~
~ f + Sφ V
V +
ρf ~vf φf · Af =
Γφ ∇φf · A
∂t
f
f
(18.2-2)
where
Nfaces
φf
~f
ρf ~vf · A
~f
A
∇φf
V
=
=
=
=
=
=
number of faces enclosing cell
value of φ convected through face f
mass flux through the face
area of face f , |A| (= |Ax ı̂ + Ay ̂| in 2D)
gradient of φ at face f
cell volume
Where ∂ρφ
V is defined in Section 18.3.2: Temporal Discretization. The equations solved
∂t
by ANSYS FLUENT take the same general form as the one given above and apply readily
to multi-dimensional, unstructured meshes composed of arbitrary polyhedra.
18-8
Release 12.0 c ANSYS, Inc. January 29, 2009
18.2 General Scalar Transport Equation: Discretization and Solution
Af
f
r1
c1
r0
c0
Figure 18.2.1: Control Volume Used to Illustrate Discretization of a Scalar
Transport Equation
18.2.1 Solving the Linear System
The discretized scalar transport equation (Equation 18.2-2) contains the unknown scalar
variable φ at the cell center as well as the unknown values in surrounding neighbor cells.
This equation will, in general, be non-linear with respect to these variables. A linearized
form of Equation 18.2-2 can be written as
aP φ =
X
anb φnb + b
(18.2-3)
nb
where the subscript nb refers to neighbor cells, and aP and anb are the linearized coefficients for φ and φnb .
The number of neighbors for each cell depends on the mesh topology, but will typically
equal the number of faces enclosing the cell (boundary cells being the exception).
Similar equations can be written for each cell in the mesh. This results in a set of
algebraic equations with a sparse coefficient matrix. For scalar equations, ANSYS FLUENT solves this linear system using a point implicit (Gauss-Seidel) linear equation solver
in conjunction with an algebraic multigrid (AMG) method which is described in Section 18.6.3: Algebraic Multigrid (AMG).
Release 12.0 c ANSYS, Inc. January 29, 2009
18-9
Solver Theory
18.3
Discretization
Information is organized into the following subsections:
• Section 18.3.1: Spatial Discretization
• Section 18.3.2: Temporal Discretization
• Section 18.3.3: Evaluation of Gradients and Derivatives
• Section 18.3.4: Gradient Limiters
18.3.1
Spatial Discretization
By default, ANSYS FLUENT stores discrete values of the scalar φ at the cell centers
(c0 and c1 in Figure 18.2.1). However, face values φf are required for the convection
terms in Equation 18.2-2 and must be interpolated from the cell center values. This is
accomplished using an upwind scheme.
Upwinding means that the face value φf is derived from quantities in the cell upstream, or
“upwind,” relative to the direction of the normal velocity vn in Equation 18.2-2. ANSYS
FLUENT allows you to choose from several upwind schemes: first-order upwind, secondorder upwind, power law, and QUICK. These schemes are described in Sections 18.3.1–
18.3.1.
The diffusion terms in Equation 18.2-2 are central-differenced and are always secondorder accurate.
For information on how to use the various spatial discretization schemes, see Section 26.2: Choosing the Spatial Discretization Scheme in the separate User’s Guide.
First-Order Upwind Scheme
When first-order accuracy is desired, quantities at cell faces are determined by assuming
that the cell-center values of any field variable represent a cell-average value and hold
throughout the entire cell; the face quantities are identical to the cell quantities. Thus
when first-order upwinding is selected, the face value φf is set equal to the cell-center
value of φ in the upstream cell.
i
18-10
First-order upwind is available in the pressure-based and density-based
solvers.
Release 12.0 c ANSYS, Inc. January 29, 2009
18.3 Discretization
Power-Law Scheme
The power-law discretization scheme interpolates the face value of a variable, φ, using
the exact solution to a one-dimensional convection-diffusion equation
∂
∂ ∂φ
(ρuφ) =
Γ
∂x
∂x ∂x
(18.3-1)
where Γ and ρu are constant across the interval ∂x. Equation 18.3-1 can be integrated
to yield the following solution describing how φ varies with x:
exp(Pe Lx ) − 1
φ(x) − φ0
=
φL − φ0
exp(Pe) − 1
(18.3-2)
where
φ0
φL
= φ|x=0
= φ|x=L
and Pe is the Peclet number:
Pe =
ρuL
Γ
(18.3-3)
The variation of φ(x) between x = 0 and x = L is depicted in Figure 18.3.1 for a range
of values of the Peclet number. Figure 18.3.1 shows that for large Pe, the value of φ at
x = L/2 is approximately equal to the upstream value. This implies that when the flow
is dominated by convection, interpolation can be accomplished by simply letting the face
value of a variable be set equal to its “upwind” or upstream value. This is the standard
first-order scheme for ANSYS FLUENT.
If the power-law scheme is selected, ANSYS FLUENT uses Equation 18.3-2 in an equivalent
“power law” format [264], as its interpolation scheme.
As discussed in Section 18.3.1: First-Order Upwind Scheme, Figure 18.3.1 shows that for
large Pe, the value of φ at x = L/2 is approximately equal to the upstream value. When
Pe=0 (no flow, or pure diffusion), Figure 18.3.1 shows that φ may be interpolated using
a simple linear average between the values at x = 0 and x = L. When the Peclet number
has an intermediate value, the interpolated value for φ at x = L/2 must be derived by
applying the “power law” equivalent of Equation 18.3-2.
i
The power-law scheme is available in the pressure-based solver and when
solving additional scalar equations in the density-based solver.
Release 12.0 c ANSYS, Inc. January 29, 2009
18-11
Solver Theory
φL
Pe < -1
Pe = -1
φ
Pe= 0
Pe = 1
Pe > 1
φ0
0
L
X
Figure 18.3.1: Variation of a Variable φ Between x = 0 and x = L (Equation 18.3-1)
Second-Order Upwind Scheme
When second-order accuracy is desired, quantities at cell faces are computed using a
multidimensional linear reconstruction approach [14]. In this approach, higher-order
accuracy is achieved at cell faces through a Taylor series expansion of the cell-centered
solution about the cell centroid. Thus when second-order upwinding is selected, the face
value φf is computed using the following expression:
φf,SOU = φ + ∇φ · ~r
(18.3-4)
where φ and ∇φ are the cell-centered value and its gradient in the upstream cell, and
~r is the displacement vector from the upstream cell centroid to the face centroid. This
formulation requires the determination of the gradient ∇φ in each cell, as discussed in
Section 18.3.3: Evaluation of Gradients and Derivatives. Finally, the gradient ∇φ is
limited so that no new maxima or minima are introduced.
i
18-12
Second-order upwind is available in the pressure-based and density-based
solvers.
Release 12.0 c ANSYS, Inc. January 29, 2009
18.3 Discretization
First-to-Higher Order Blending
In some instances, and at certain flow conditions, a converged solution to steady-state
may not be possible with the use of higher-order discretization schemes due to local flow
fluctuations (physical or numerical). On the other hand, a converged solution for the
same flow conditions maybe possible with a first-order discretization scheme. For this
type of flow and situation, if a better than first-order accurate solution is desired, then
first-to-higher-order blending can be used to obtain a converged steady-state solution.
The first-order to higher-order blending is applicable only when higher-order discretization is used. It is applicable with the following discretization schemes: second-order upwinding, central-differencing schemes, QUICK, and third-order MUSCL. The blending is
not applicable to first-order, power-law, modified HRIC schemes, or the Geo-reconstruct
and CICSAM schemes.
In the density-based solver, the blending is applied as a scaling factor to the reconstruction gradients. While in the pressure-based solver, the blending is applied to the
higher-order terms for the convective transport variable.
To learn how to apply this option, refer to Section 26.2.1: First-to-Higher Order Blending
in the separate User’s Guide.
Central-Differencing Scheme
A second-order-accurate central-differencing discretization scheme is available for the momentum equations when you are using the LES turbulence model. This scheme provides
improved accuracy for LES calculations.
The central-differencing scheme calculates the face value for a variable (φf ) as follows:
φf,CD =
1
1
(φ0 + φ1 ) + (∇φ0 · ~r0 + ∇φ1 · ~r1 )
2
2
(18.3-5)
where the indices 0 and 1 refer to the cells that share face f , ∇φr,0 and ∇φr,1 are the
reconstructed gradients at cells 0 and 1, respectively, and ~r is the vector directed from
the cell centroid toward the face centroid.
It is well known that central-differencing schemes can produce unbounded solutions and
non-physical wiggles, which can lead to stability problems for the numerical procedure.
These stability problems can often be avoided if a deferred approach is used for the
central-differencing scheme. In this approach, the face value is calculated as follows:
φf =
φf,UP
| {z }
implicit part
Release 12.0 c ANSYS, Inc. January 29, 2009
+
(φf,CD − φf,UP )
|
{z
explicit part
(18.3-6)
}
18-13
Solver Theory
where UP stands for upwind. As indicated, the upwind part is treated implicitly while
the difference between the central-difference and upwind values is treated explicitly. Provided that the numerical solution converges, this approach leads to pure second-order
differencing.
i
The central differencing scheme is available only in the pressure-based
solver.
Bounded Central Differencing Scheme
The central differencing scheme described in Section 18.3.1: Central-Differencing Scheme
is an ideal choice for LES in view of its meritoriously low numerical diffusion. However,
it often leads to unphysical oscillations in the solution fields. In LES, the situation
is exacerbated by usually very low subgrid-scale turbulent diffusivity. The bounded
central differencing scheme is essentially based on the normalized variable diagram (NVD)
approach [187] together with the convection boundedness criterion (CBC). The bounded
central differencing scheme is a composite NVD-scheme that consists of a pure central
differencing, a blended scheme of the central differencing and the second-order upwind
scheme, and the first-order upwind scheme. It should be noted that the first-order scheme
is used only when the CBC is violated.
18-14
i
The bounded central differencing scheme is the default convection scheme
for LES. When you select LES, the convection discretization schemes for
all transport equations are automatically switched to the bounded central
differencing scheme.
i
The bounded central differencing scheme is available only in the pressurebased solver.
Release 12.0 c ANSYS, Inc. January 29, 2009
18.3 Discretization
QUICK Scheme
For quadrilateral and hexahedral meshes, where unique upstream and downstream faces
and cells can be identified, ANSYS FLUENT also provides the QUICK scheme for computing a higher-order value of the convected variable φ at a face. QUICK-type schemes [188]
are based on a weighted average of second-order-upwind and central interpolations of the
variable. For the face e in Figure 18.3.2, if the flow is from left to right, such a value can
be written as
φe = θ
Sd
Sc
Su + 2Sc
Sc
φP +
φE + (1 − θ)
φP −
φW
Sc + S d
Sc + S d
S u + Sc
S u + Sc
Su
Sc
W
∆x w P
∆x e E
w
e
(18.3-7)
Sd
Figure 18.3.2: One-Dimensional Control Volume
θ = 1 in the above equation results in a central second-order interpolation while θ = 0
yields a second-order upwind value. The traditional QUICK scheme is obtained by setting
θ = 1/8. The implementation in ANSYS FLUENT uses a variable, solution-dependent
value of θ, chosen so as to avoid introducing new solution extrema.
The QUICK scheme will typically be more accurate on structured meshes aligned with
the flow direction. Note that ANSYS FLUENT allows the use of the QUICK scheme
for unstructured or hybrid meshes as well; in such cases the usual second-order upwind
discretization scheme (described in Section 18.3.1: Second-Order Upwind Scheme) will be
used at the faces of non-hexahedral (or non-quadrilateral, in 2D) cells. The second-order
upwind scheme will also be used at partition boundaries when the parallel solver is used.
i
The QUICK scheme is available in the pressure-based solver and when
solving additional scalar equations in the density-based solver.
Release 12.0 c ANSYS, Inc. January 29, 2009
18-15
Solver Theory
Third-Order MUSCL Scheme
This third-order convection scheme was conceived from the original MUSCL (Monotone
Upstream-Centered Schemes for Conservation Laws) [352] by blending a central differencing scheme and second-order upwind scheme as
φf = θφf,CD + (1 − θ)φf,SOU
(18.3-8)
where φf,CD is defined in Equation 18.3-5, and φf,SOU is computed using the second-order
upwind scheme as described in Section 18.3.1: Second-Order Upwind Scheme.
Unlike the QUICK scheme which is applicable to structured hex meshes only, the MUSCL
scheme is applicable to arbitrary meshes. Compared to the second-order upwind scheme,
the third-order MUSCL has a potential to improve spatial accuracy for all types of meshes
by reducing numerical diffusion, most significantly for complex three-dimensional flows,
and it is available for all transport equations.
i
The third-order MUSCL currently implemented in ANSYS FLUENT does
not contain any flux-limiter. As a result, it can produce undershoots and
overshoots when the flow-field under consideration has discontinuities such
as shock waves.
i
The MUSCL scheme is available in the pressure-based and density-based
solvers.
Modified HRIC Scheme
For simulations using the VOF multiphase model, upwind schemes are generally unsuitable for interface tracking because of their overly diffusive nature. Central differencing
schemes, while generally able to retain the sharpness of the interface, are unbounded and
often give unphysical results. In order to overcome these deficiencies, ANSYS FLUENT
uses a modified version of the High Resolution Interface Capturing (HRIC) scheme. The
modified HRIC scheme is a composite NVD scheme that consists of a non-linear blend
of upwind and downwind differencing [243].
First, the normalized cell value of volume fraction, φ˜c , is computed and is used to find
the normalized face value, φ̃f , as follows:
φD − φU
φ˜c =
φA − φU
18-16
(18.3-9)
Release 12.0 c ANSYS, Inc. January 29, 2009
18.3 Discretization
φf
φU
φD
φA
Figure 18.3.3: Cell Representation for Modified HRIC Scheme
where A is the acceptor cell, D is the donor cell, and U is the upwind cell, and
φ̃f =
˜
φc
2φ˜c
1
φ˜c < 0 or φ˜c > 1
0 ≤ φ˜c ≤ 0.5
0.5 ≤ φ˜c ≤ 1
(18.3-10)
Here, if the upwind cell is not available (e.g., unstructured mesh), an extrapolated value
is used for φU . Directly using this value of φ̃f causes wrinkles in the interface, if the flow
is parallel to the interface. So, ANSYS FLUENT switches to the ULTIMATE QUICKEST
scheme (the one-dimensional bounded version of the QUICK scheme [187]) based on the
angle between the face normal and interface normal:
φ˜c
φ˜c < 0 or φ˜c > 1
φUf˜Q =
˜
M IN φ̃f , 6φc8+3 0 ≤ φ˜c ≤ 1
(18.3-11)
This leads to a corrected version of the face volume fraction, φ̃∗f :
√
√
φ̃∗f = φ̃f cos θ + (1 − cos θ)φUf˜Q
(18.3-12)
where
cos θ =
∇φ · ~d
|∇φ||~d|
(18.3-13)
and ~d is a vector connecting cell centers adjacent to the face f .
Release 12.0 c ANSYS, Inc. January 29, 2009
18-17
Solver Theory
The face volume fraction is now obtained from the normalized value computed above as
follows:
φf = φ̃∗f (φA − φU ) + φU
(18.3-14)
The modified HRIC scheme provides improved accuracy for VOF calculations when compared to QUICK and second-order schemes, and is less computationally expensive than
the Geo-Reconstruct scheme.
18.3.2 Temporal Discretization
For transient simulations, the governing equations must be discretized in both space
and time. The spatial discretization for the time-dependent equations is identical to
the steady-state case. Temporal discretization involves the integration of every term in
the differential equations over a time step ∆t. The integration of the transient terms is
straightforward, as shown below.
A generic expression for the time evolution of a variable φ is given by
∂φ
= F (φ)
∂t
(18.3-15)
where the function F incorporates any spatial discretization. If the time derivative is
discretized using backward differences, the first-order accurate temporal discretization is
given by
φn+1 − φn
= F (φ)
∆t
(18.3-16)
and the second-order discretization is given by
3φn+1 − 4φn + φn−1
= F (φ)
2∆t
(18.3-17)
where
φ
= a scalar quantity
n + 1 = value at the next time level, t + ∆t
n
= value at the current time level, t
n − 1 = value at the previous time level, t − ∆t
Once the time derivative has been discretized, a choice remains for evaluating F (φ): in
particular, which time level values of φ should be used in evaluating F ?
18-18
Release 12.0 c ANSYS, Inc. January 29, 2009
18.3 Discretization
Implicit Time Integration
One method is to evaluate F (φ) at the future time level:
φn+1 − φn
= F (φn+1 )
∆t
(18.3-18)
This is referred to as “implicit” integration since φn+1 in a given cell is related to φn+1
in neighboring cells through F (φn+1 ):
φn+1 = φn + ∆tF (φn+1 )
(18.3-19)
This implicit equation can be solved iteratively at each time level before moving to the
next time step.
The advantage of the fully implicit scheme is that it is unconditionally stable with respect
to time step size.
Explicit Time Integration
A second method is available when the density-based explicit solver is used. This method
evaluates F (φ) at the current time level:
φn+1 − φn
= F (φn )
∆t
(18.3-20)
and is referred to as “explicit” integration since φn+1 can be expressed explicitly in terms
of the existing solution values, φn :
φn+1 = φn + ∆tF (φn )
(18.3-21)
Here, the time step ∆t is restricted to the stability limit of the underlying solver (i.e.,
a time step is limited by the Courant-Friedrich-Lewy condition). In order to be timeaccurate, all cells in the domain must use the same time step. For stability, this time
step must be the minimum of all the local time steps in the domain. This method is also
referred to as “global time stepping”.
Release 12.0 c ANSYS, Inc. January 29, 2009
18-19
Solver Theory
The use of explicit time stepping is fairly restrictive. It is used primarily to capture the
transient behavior of moving waves, such as shocks, because it is more accurate and less
expensive than the implicit time stepping methods in such cases. You cannot use explicit
time stepping in the following cases:
• Calculations with the pressure-based solver or density-based implicit formulation.
The explicit time stepping formulation is available only with the density-based
explicit formulation. ANSYS FLUENT also uses multi-stage Runge-Kutta explicit
time integration for the density-based solver, as detailed in Sections 18.5.4 and
18.5.5
• Incompressible flow. Explicit time stepping cannot be used to compute timeaccurate incompressible flows (i.e., gas laws other than ideal gas). Incompressible
solutions must be iterated to convergence within each time step.
• Convergence acceleration. FAS multigrid and residual smoothing cannot be used
with explicit time stepping because they destroy the time accuracy of the underlying
solver.
18.3.3
Evaluation of Gradients and Derivatives
Gradients are needed not only for constructing values of a scalar at the cell faces, but
also for computing secondary diffusion terms and velocity derivatives. The gradient ∇φ
of a given variable φ is used to discretize the convection and diffusion terms in the flow
conservation equations. The gradients are computed in ANSYS FLUENT according to
the following methods:
• Green-Gauss Cell-Based
• Green-Gauss Node-Based
• Least Squares Cell-Based
To learn how to apply the various gradients, see Section 26.2: Choosing the Spatial
Discretization Scheme in the separate User’s Guide.
Green-Gauss Theorem
When the Green-Gauss theorem is used to compute the gradient of the scalar φ at the
cell center c0, the following discrete form is written as
(∇φ)c0 =
1X
~f
φ A
V f f
(18.3-22)
where φf is the value of φ at the cell face centroid, computed as shown in the sections
below. The summation is over all the faces enclosing the cell.
18-20
Release 12.0 c ANSYS, Inc. January 29, 2009
18.3 Discretization
Green-Gauss Cell-Based Gradient Evaluation
By default, the face value, φf , in Equation 18.3-22 is taken from the arithmetic average
of the values at the neighboring cell centers, i.e.,
φf =
φc0 + φc1
2
(18.3-23)
Green-Gauss Node-Based Gradient Evaluation
Alternatively, φf can be computed by the arithmetic average of the nodal values on the
face.
φf =
Nf
1 X
φ
Nf n n
(18.3-24)
where Nf is the number of nodes on the face.
The nodal values, φn in Equation 18.3-24, are constructed from the weighted average
of the cell values surrounding the nodes, following the approach originally proposed by
Holmes and Connel[132] and Rauch et al.[286]. This scheme reconstructs exact values of a
linear function at a node from surrounding cell-centered values on arbitrary unstructured
meshes by solving a constrained minimization problem, preserving a second-order spatial
accuracy.
The node-based gradient is known to be more accurate than the cell-based gradient particularly on irregular (skewed and distorted) unstructured meshes, however, it is relatively
more expensive to compute than the cell-based gradient scheme.
i
The node-based gradient method is not available with polyhedral meshes.
Release 12.0 c ANSYS, Inc. January 29, 2009
18-21
Solver Theory
Least Squares Cell-Based Gradient Evaluation
In this method the solution is assumed to vary linearly. In Figure 18.3.4, the change in
cell values between cell c0 and ci along the vector δri from the centroid of cell c0 to cell
ci, can be expressed as
(∇φ)c0 · ∆ri = (φci − φc0 )
co
(18.3-25)
ci
r
i
Figure 18.3.4: Cell Centroid Evaluation
If we write similar equations for each cell surrounding the cell c0, we obtain the following
system written in compact form:
[J](∇φ)c0 = ∆φ
(18.3-26)
Where [J] is the coefficient matrix which is purely a function of geometry.
The objective here is to determine the cell gradient (∇φ0 = φx ı̂+φy ĵ+φz k̂) by solving
the minimization problem for the system of the non-square coefficient matrix in a leastsquares sense.
The above linear-system of equation is over-determined and can be solved by decomposing
the coefficient matrix using the Gram-Schmidt process [6]. This decomposition yields a
matrix of weights for each cell. Thus for our cell-centered scheme this means that the
three components of the weights (W x i0 , W y i0 , W z i0 ) are produced for each of the faces of
cell c0.
18-22
Release 12.0 c ANSYS, Inc. January 29, 2009
18.3 Discretization
Therefore, the gradient at the cell center can then be computed by multiplying the weight
factors by the difference vector ∆φ = (φc1 − φc0 ),
(φx )c0 =
(φy )c0 =
(φz )c0 =
n
X
i=1
n
X
i=1
n
X
W x i0 · (φci − φc0 )
(18.3-27)
W y i0 · (φci − φc0 )
(18.3-28)
W z i0 · (φci − φc0 )
(18.3-29)
i=1
On irregular (skewed and distorted) unstructured meshes, the accuracy of the leastsquares gradient method is comparable to that of the node-based gradient (and both are
much more superior compared to the cell-based gradient). However, it is less expensive
to compute the least-squares gradient than the node-based gradient. Therefore, it has
been selected as the default gradient method in the ANSYS FLUENT solver.
18.3.4
Gradient Limiters
Gradient limiters, also known as slope limiters, are used on the second-order upwind
(SOU) scheme to prevent spurious oscillations, which would otherwise appear in the
solution flow field near shocks, discontinuities, or near rapid local changes in the flow
field. The gradient limiter attempts to invoke and enforce the monotonicity principle
by prohibiting the linearly reconstructed field variable on the cell faces to exceed the
maximum or minimum values of the neighboring cells.
There are three gradient limiters in the ANSYS FLUENT solvers:
• Standard limiter
• Multidimensional limiter
• Differentiable limiter
Gradient limiters can be categorized into two general groups: non-differentiable limiters
and differentiable limiters. Both, the standard limiter and multidimensional limiter are
of the non-differentiable form, since they use minimum and maximum types of functions
for limiting the solution variables. The third limiter in ANSYS FLUENT, as the name
indicates, is a differentiable type of limiter, which uses a smooth function to impose the
monotonicity principle.
Release 12.0 c ANSYS, Inc. January 29, 2009
18-23
Solver Theory
For each of the above mentioned limiter methods, ANSYS FLUENT provides two limiting
directions:
• cell to face limiting, where the limited value of the reconstruction gradient is determined at cell face centers. This is the default method.
• cell to cell limiting, where the limited value of the reconstruction gradient is determined along a scaled line between two adjacent cell centroids. On an orthogonal
mesh (or when cell-to-cell direction is parallel to face area direction) this method
becomes equivalent to the default cell to face method. For smooth field variation,
cell to cell limiting may provide less numerical dissipation on meshes with skewed
cells.
For more information about how to access the limiter functions in ANSYS FLUENT
through the GUI or TUI, see Section 26.8: Selecting Gradient Limiters in the separate
User’s Guide.
i
On unstructured meshes, ANSYS FLUENT uses the scalar form of the gradient limiter given by the following equation:
ΦfSOU = Φ + ψ∇φ · r
(18.3-30)
Where ψ is a scalar value which limits the gradient ∇Φ.
Standard Limiter
The standard limiter is the default limiter function in ANSYS FLUENT and is derived
from the work of Barth and Jespersen [14]. This limiter is of a non-differentiable type
and uses the Minmod function (Minimum Modulus) to limit and clip the reconstructed
solution overshoots and undershoots on the cell faces.
Multidimensional Limiter
The multidimensional limiter in ANSYS FLUENT [164] has a similar form to the standard
limiter. Since the multidimensional limiter uses a Minmod function for limiting the
gradient, it is also classified as a non-differentiable type of limiter. However, in the
standard limiter formulation, if limiting took place on any face of the cell, then this will
cause the cell gradient to be clipped in an equal manner, in all directions, regardless of
whether or not limiting is needed on the other cell faces. This limiting method is rather
severe and adds unnecessary dissipation to the numerical scheme. The multidimensional
limiter, on the other hand, attempts to lessen the severity of the gradient limiting by
carefully examining the gradient on each cell and clipping only the normal components
of the gradient to the cell faces. For this procedure to work on a scalar form limiter, the
normal components of gradients on cell faces are first sorted out in ascending order of
18-24
Release 12.0 c ANSYS, Inc. January 29, 2009
18.4 Pressure-Based Solver
their magnitude so that only the necessary clipping can be applied. The multidimensional
limiter is therefore less dissipative than the standard limiter.
Differentiable Limiter
One disadvantage with non-differentiable limiters is that they tend to stall the apparent
residual’s convergence after a few orders of reduction in residual magnitude. Note that
this does not mean that the solution is not converging, but rather the solution continues
to converge while the residuals are stalling. This annoying behavior can be directly traced
to the non-differentiable nature of the limiting functions. Therefore, the differentiable
limiter uses a smooth function to impose the monotonicity condition while allowing the
residuals to converge. The differentiable limiter used in ANSYS FLUENT is a modified
form [366] of a limiter which was originally proposed by Venkatakrishnan[355].
i
ANSYS FLUENT uses gradient or slope limiters and not flux limiters. Gradient limiters are applied to the gradients of the variable field being linearly
reconstructed at the cell faces, while flux limiters are used on the system
fluxes.
18.4 Pressure-Based Solver
In this section, special practices related to the discretization of the momentum and continuity equations and their solution by means of the pressure-based solver are addressed.
Information is organized into the following subsections:
• Section 18.4.1: Discretization of the Momentum Equation
• Section 18.4.2: Discretization of the Continuity Equation
• Section 18.4.3: Pressure-Velocity Coupling
• Section 18.4.4: Steady-State Iterative Algorithm
• Section 18.4.5: Time-Advancement Algorithm
These special practices are most easily described by considering the steady-state continuity and momentum equations in integral form:
I
~=−
ρ~v ~v · dA
I
~=0
ρ ~v · dA
I
~+
pI · dA
I
~+
τ · dA
(18.4-1)
Z
F~ dV
(18.4-2)
V
where I is the identity matrix, τ is the stress tensor, and F~ is the force vector.
Release 12.0 c ANSYS, Inc. January 29, 2009
18-25
Solver Theory
18.4.1
Discretization of the Momentum Equation
The discretization scheme described in Section 18.3: Discretization for a scalar transport equation is also used to discretize the momentum equations. For example, the
x-momentum equation can be obtained by setting φ = u:
aP u =
X
anb unb +
X
pf A · ı̂ + S
(18.4-3)
nb
If the pressure field and face mass fluxes are known, Equation 18.4-3 can be solved in the
manner outlined in Section 18.3: Discretization, and a velocity field obtained. However,
the pressure field and face mass fluxes are not known a priori and must be obtained as a
part of the solution. There are important issues with respect to the storage of pressure
and the discretization of the pressure gradient term; these are addressed next.
ANSYS FLUENT uses a co-located scheme, whereby pressure and velocity are both stored
at cell centers. However, Equation 18.4-3 requires the value of the pressure at the face
between cells c0 and c1, shown in Figure 18.2.1. Therefore, an interpolation scheme is
required to compute the face values of pressure from the cell values.
Pressure Interpolation Schemes
The default scheme in ANSYS FLUENT interpolates the pressure values at the faces using
momentum equation coefficients [292]:
Pf =
Pc0
ap,c0
1
ap,c0
+
+
Pc1
ap,c1
1
ap,c1
(18.4-4)
This procedure works well as long as the pressure variation between cell centers is smooth.
When there are jumps or large gradients in the momentum source terms between control volumes, the pressure profile has a high gradient at the cell face, and cannot be
interpolated using this scheme. If this scheme is used, the discrepancy shows up in
overshoots/undershoots of cell velocity.
Flows for which the standard pressure interpolation scheme will have trouble include
flows with large body forces, such as in strongly swirling flows, in high-Rayleigh-number
natural convection and the like. In such cases, it is necessary to pack the mesh in regions
of high gradient to resolve the pressure variation adequately.
Another source of error is that ANSYS FLUENT assumes that the normal pressure gradient at the wall is zero. This is valid for boundary layers, but not in the presence of body
forces or curvature. Again, the failure to correctly account for the wall pressure gradient
is manifested in velocity vectors pointing in/out of walls.
18-26
Release 12.0 c ANSYS, Inc. January 29, 2009
18.4 Pressure-Based Solver
Several alternate methods are available for cases in which the standard pressure interpolation scheme is not valid:
• The linear scheme computes the face pressure as the average of the pressure values
in the adjacent cells.
• The second-order scheme reconstructs the face pressure in the manner used for
second-order accurate convection terms (see Section 18.3.1). This scheme may
provide some improvement over the standard and linear schemes, but it may have
some trouble if it is used at the start of a calculation and/or with a bad mesh.
The second-order scheme is not applicable for flows with discontinuous pressure
gradients imposed by the presence of a porous medium in the domain or the use of
the VOF or mixture model for multiphase flow.
• The body-force-weighted scheme computes the face pressure by assuming that the
normal gradient of the difference between pressure and body forces is constant.
This works well if the body forces are known a priori in the momentum equations
(e.g., buoyancy and axisymmetric swirl calculations).
i
When a case contains porous media, the body-force-weighted scheme is
applied only for non-porous faces, where the scheme takes into account the
discontinuity of explicit body forces (e.g., gravity, swirl, Coriolis) and the
discontinuity of pressure gradients for flows with rapidly changing densities
(e.g., natural convection, VOF). All interior and exterior porous faces are
treated with a special scheme that preserves the continuity of the normal
velocity across cell faces in spite of the discontinuity of the resistance.
• The PRESTO! (PREssure STaggering Option) scheme uses the discrete continuity
balance for a “staggered” control volume about the face to compute the “staggered”
(i.e., face) pressure. This procedure is similar in spirit to the staggered-grid schemes
used with structured meshes [264]. Note that for triangular, tetrahedral, hybrid,
and polyhedral meshes, comparable accuracy is obtained using a similar algorithm.
The PRESTO! scheme is available for all meshes.
For recommendations on when to use these alternate schemes, see Section 26.2.3: Choosing the Pressure Interpolation Scheme in the separate User’s Guide.
Release 12.0 c ANSYS, Inc. January 29, 2009
18-27
Solver Theory
18.4.2
Discretization of the Continuity Equation
Equation 18.4-1 may be integrated over the control volume in Figure 18.2.1 to yield the
following discrete equation
NX
faces
J f Af = 0
(18.4-5)
f
where Jf is the mass flux through face f , ρvn .
In order to proceed further, it is necessary to relate the face values of velocity, ~vn , to the
stored values of velocity at the cell centers. Linear interpolation of cell-centered velocities to the face results in unphysical checker-boarding of pressure. ANSYS FLUENT uses
a procedure similar to that outlined by Rhie and Chow [292] to prevent checkerboarding. The face value of velocity is not averaged linearly; instead, momentum-weighted
averaging, using weighting factors based on the aP coefficient from equation 18.4-3, is
performed. Using this procedure, the face flux, Jf , may be written as
J f = ρf
ap,c0 vn,c0 + ap,c1 vn,c1
+df ((pc0 +(∇p)c0 · r~0 )−(pc1 +(∇p)c1 · r~1 )) = Jˆf +df (pc0 −pc1 )
ap,c0 + ap,c1
(18.4-6)
where pc0 , pc1 and vn,c0 , vn,c1 are the pressures and normal velocities, respectively, within
the two cells on either side of the face, and Jˆf contains the influence of velocities in these
cells (see Figure 18.2.1). The term df is a function of āP , the average of the momentum
equation aP coefficients for the cells on either side of face f .
Density Interpolation Schemes
For incompressible flows, ANSYS FLUENT uses arithmetic averaging for density. For
compressible flow calculations (i.e., calculations that use the ideal gas law for density),
ANSYS FLUENT applies upwind interpolation of density at cell faces. Several interpolation schemes are available for the density upwinding at cell faces: first-order upwind
(default), second-order-upwind, QUICK, MUSCL, and when applicable, central differencing and bounded central differencing.
The first-order upwind scheme (based on [157]) sets the density at the cell face to be the
upstream cell-center value. This scheme provides stability for the discretization of the
pressure-correction equation, and gives good results for most classes of flows. The firstorder scheme is the default scheme for compressible flows. Although this scheme provides
the best stability for compressible flow calculations, it gives very diffusive representations
of shocks.
18-28
Release 12.0 c ANSYS, Inc. January 29, 2009
18.4 Pressure-Based Solver
The second-order upwind scheme provides stability for supersonic flows and captures
shocks better than the first-order upwind scheme. The QUICK scheme for density is
similar to the QUICK scheme used for other variables. See Section 18.3.1: QUICK
Scheme for details.
i
In the case of multiphase flows, the selected density scheme is applied to
the compressible phase and arithmetic averaging is used for incompressible
phases.
i
For stability reasons, it is recommended that you achieve a solution with a
first order scheme and then switch to a higher order scheme for compressible
flow calculations.
For recommendations on choosing an appropriate density interpolation scheme for your
compressible flow, see Section 26.2.4: Choosing the Density Interpolation Scheme in the
separate User’s Guide.
18.4.3
Pressure-Velocity Coupling
Pressure-velocity coupling is achieved by using Equation 18.4-6 to derive an additional
condition for pressure by reformatting the continuity equation (Equation 18.4-5). The
pressure-based solver allows you to solve your flow problem in either a segregated or
coupled manner. ANSYS FLUENT provides the option to choose among five pressurevelocity coupling algorithms: SIMPLE, SIMPLEC, PISO, Coupled, and (for unsteady
flows using the non-iterative time advancement scheme (NITA)) Fractional Step (FSM).
All the aforementioned schemes, except the “coupled” scheme, are based on the predictorcorrector approach. For instructions on how to select these algorithms, see Section 26.3.1: Choosing the Pressure-Velocity Coupling Method in the separate User’s Guide.
Note that SIMPLE, SIMPLEC, PISO, and Fractional Step use the pressure-based segregated
algorithm, while Coupled uses the pressure-based coupled solver.
i
The pressure-velocity coupling schemes that are applicable when using the
Eulerian multiphase model are Phase Coupled SIMPLE, Multiphase Coupled, and Full Multiphase Coupled. These are discussed in detail in Section 24.7.5: Selecting the Solution Method in the separate User’s Guide.
Release 12.0 c ANSYS, Inc. January 29, 2009
18-29
Solver Theory
Segregated Algorithms
SIMPLE
The SIMPLE algorithm uses a relationship between velocity and pressure corrections to
enforce mass conservation and to obtain the pressure field.
If the momentum equation is solved with a guessed pressure field p∗ , the resulting face
flux, Jf∗ , computed from Equation 18.4-6
Jf∗ = Jˆf∗ + df (p∗c0 − p∗c1 )
(18.4-7)
does not satisfy the continuity equation. Consequently, a correction Jf0 is added to the
face flux Jf∗ so that the corrected face flux, Jf
Jf = Jf∗ + Jf0
(18.4-8)
satisfies the continuity equation. The SIMPLE algorithm postulates that Jf0 be written
as
Jf0 = df (p0c0 − p0c1 )
(18.4-9)
where p0 is the cell pressure correction.
The SIMPLE algorithm substitutes the flux correction equations (Equations 18.4-8 and
18.4-9) into the discrete continuity equation (Equation 18.4-5) to obtain a discrete equation for the pressure correction p0 in the cell:
aP p 0 =
X
anb p0nb + b
(18.4-10)
nb
where the source term b is the net flow rate into the cell:
b=
NX
faces
Jf∗ Af
(18.4-11)
f
18-30
Release 12.0 c ANSYS, Inc. January 29, 2009
18.4 Pressure-Based Solver
The pressure-correction equation (Equation 18.4-10) may be solved using the algebraic
multigrid (AMG) method described in Section 18.6.3: Algebraic Multigrid (AMG). Once
a solution is obtained, the cell pressure and the face flux are corrected using
p = p∗ + αp p0
(18.4-12)
Jf = Jf∗ + df (p0c0 − p0c1 )
(18.4-13)
Here αp is the under-relaxation factor for pressure (see Section 18.4.4: Under-Relaxation
of Variables for information about under-relaxation). The corrected face flux, Jf , satisfies
the discrete continuity equation identically during each iteration.
SIMPLEC
A number of variants of the basic SIMPLE algorithm are available in the literature.
In addition to SIMPLE, ANSYS FLUENT offers the SIMPLEC (SIMPLE-Consistent)
algorithm [353]. SIMPLE is the default, but many problems will benefit from the use of
SIMPLEC, as described in Section 26.3.1: SIMPLE vs. SIMPLEC in the separate User’s
Guide.
The SIMPLEC procedure is similar to the SIMPLE procedure outlined above. The only
difference lies in the expression used for the face flux correction, Jf0 . As in SIMPLE, the
correction equation may be written as
Jf = Jf∗ + df (p0c0 − p0c1 )
(18.4-14)
However, the coefficient df is redefined as a function of (aP − nb anb ). The use of this
modified correction equation has been shown to accelerate convergence in problems where
pressure-velocity coupling is the main deterrent to obtaining a solution.
P
Skewness Correction
For meshes with some degree of skewness, the approximate relationship between the
correction of mass flux at the cell face and the difference of the pressure corrections
at the adjacent cells is very rough. Since the components of the pressure-correction
gradient along the cell faces are not known in advance, an iterative process similar to the
PISO neighbor correction described below is desirable. After the initial solution of the
pressure-correction equation, the pressure-correction gradient is recalculated and used
to update the mass flux corrections. This process, which is referred to as “skewness
correction”, significantly reduces convergence difficulties associated with highly distorted
meshes. The SIMPLEC skewness correction allows ANSYS FLUENT to obtain a solution
on a highly skewed mesh in approximately the same number of iterations as required for
a more orthogonal mesh.
Release 12.0 c ANSYS, Inc. January 29, 2009
18-31
Solver Theory
PISO
The Pressure-Implicit with Splitting of Operators (PISO) pressure-velocity coupling
scheme, part of the SIMPLE family of algorithms, is based on the higher degree of the
approximate relation between the corrections for pressure and velocity. One of the limitations of the SIMPLE and SIMPLEC algorithms is that new velocities and corresponding
fluxes do not satisfy the momentum balance after the pressure-correction equation is
solved. As a result, the calculation must be repeated until the balance is satisfied. To
improve the efficiency of this calculation, the PISO algorithm performs two additional
corrections: neighbor correction and skewness correction.
Neighbor Correction
The main idea of the PISO algorithm is to move the repeated calculations required
by SIMPLE and SIMPLEC inside the solution stage of the pressure-correction equation [141]. After one or more additional PISO loops, the corrected velocities satisfy the
continuity and momentum equations more closely. This iterative process is called a momentum correction or “neighbor correction”. The PISO algorithm takes a little more
CPU time per solver iteration, but it can dramatically decrease the number of iterations
required for convergence, especially for transient problems.
Skewness Correction
For meshes with some degree of skewness, the approximate relationship between the
correction of mass flux at the cell face and the difference of the pressure corrections at
the adjacent cells is very rough. Since the components of the pressure-correction gradient
along the cell faces are not known in advance, an iterative process similar to the PISO
neighbor correction described above is desirable [94]. After the initial solution of the
pressure-correction equation, the pressure-correction gradient is recalculated and used
to update the mass flux corrections. This process, which is referred to as “skewness
correction”, significantly reduces convergence difficulties associated with highly distorted
meshes. The PISO skewness correction allows ANSYS FLUENT to obtain a solution on
a highly skewed mesh in approximately the same number of iterations as required for a
more orthogonal mesh.
Skewness - Neighbor Coupling
For meshes with a high degree of skewness, the simultaneous coupling of the neighbor
and skewness corrections at the same pressure correction equation source may cause
divergence or a lack of robustness. An alternate, although more expensive, method for
handling the neighbor and skewness corrections inside the PISO algorithm is to apply
one or more iterations of skewness correction for each separate iteration of neighbor
correction. For each individual iteration of the classical PISO algorithm from [141], this
technique allows a more accurate adjustment of the face mass flux correction according
to the normal pressure correction gradient.
18-32
Release 12.0 c ANSYS, Inc. January 29, 2009
18.4 Pressure-Based Solver
Fractional-Step Method (FSM)
In the FSM, the momentum equations are decoupled from the continuity equation using
a mathematical technique called operator-splitting or approximate factorization. The
resulting solution algorithm is similar to the segregated solution algorithms described
earlier. The formalism used in the approximate factorization allows you to control the
order of splitting error. Because of this, the FSM is adopted in ANSYS FLUENT as a
velocity-coupling scheme in a non-iterative time-advancement (NITA) algorithm (Section 18.4.5: Non-Iterative Time-Advancement Scheme).
Coupled Algorithm
As previously mentioned, the pressure-based solver allows you to solve your flow problem in either a segregated or coupled manner. Using the coupled approach offers some
advantages over the non-coupled or segregated approach. The coupled scheme obtains
a robust and efficient single phase implementation for steady-state flows, with superior
performance compared to the segregated solution schemes. This pressure-based coupled
algorithm offers an alternative to the density-based and pressure-based segregated algorithm with SIMPLE-type pressure-velocity coupling. For transient flows, using the
coupled algorithm is necessary when the quality of the mesh is poor, or if large time
steps are used.
The pressure-based segregated algorithm solves the momentum equation and pressure
correction equations separately. This semi-implicit solution method results in slow convergence.
The coupled algorithm solves the momentum and pressure-based continuity equations
together. The full implicit coupling is achieved through an implicit discretization of
pressure gradient terms in the momentum equations, and an implicit discretization of
the face mass flux, including the Rhie-Chow pressure dissipation terms.
In the momentum equations (18.4-3), the pressure gradient for component k is of the
form
X
p f Ak = −
X
au k p p j
(18.4-15)
j
f
Where auk p is the coefficient derived from the Gauss divergence theorem and coefficients
of the pressure interpolation schemes (Equation 18.4-4). Finally, for any ith cell, the
discretized form of the momentum equation for component uk is defined as
X
j
Release 12.0 c ANSYS, Inc. January 29, 2009
aij uk uk ukj +
X
aij uk p pj = bi uk
(18.4-16)
j
18-33
Solver Theory
In the continuity equation, Equation 18.4-5, the balance of fluxes is replaced using the
flux expression in Equation 18.4-6, resulting in the discretized form
XX
k
aij puk ukj +
X
j
aij pp pj = bi p
(18.4-17)
j
As a result, the overall system of equations (18.4-16 and 18.4-17), after being transformed
to the δ-form, is presented as
X
~j = B
~i
[A]ij X
(18.4-18)
j
where the influence of a cell i on a cell j has the form
Aij =
app
ij
aup
ij
avp
ij
awp
ij
apu
ij
auu
ij
avu
ij
awu
ij
apv
ij
auv
ij
avv
ij
awv
ij
apw
ij
auw
ij
avw
ij
aww
ij
(18.4-19)
and the unknown and residual vectors have the form
~j =
X
~i =
B
0
pi
0
ui
0
vi
0
wi
−rip
−riu
−riv
−riw
(18.4-20)
(18.4-21)
Note that Equation 18.4-18 is solved using the coupled AMG, which is detailed in Section 18.6.3: The Coupled and Scalar AMG Solvers.
Limitations
The pressure-based coupled algorithm is not compatible with
• The non-iterative time advancement solver (NITA)
• Periodic mass-flow boundary conditions
• The fixed velocity option
18-34
Release 12.0 c ANSYS, Inc. January 29, 2009
18.4 Pressure-Based Solver
18.4.4
Steady-State Iterative Algorithm
If you are performing a steady-state calculation, the governing equations for the pressurebased solver do not contain time-dependent terms. For steady-state flows,
Section 18.3: Discretization describes control-volume-based discretization of the steadystate transport equation (see Equation 18.2-1).
Under-Relaxation of Variables
The under-relaxation of variables is used in all cases for some material properties, in the
NITA solver for solution variables, and in the pressure-based coupled algorithm where
this explicit under-relaxation is used for momentum and pressure.
Because of the nonlinearity of the equation set being solved by ANSYS FLUENT, it is
necessary to control the change of φ. This is typically achieved by under-relaxation of
variables (also referred to as explicit relaxation), which reduces the change of φ produced
during each iteration. In a simple form, the new value of the variable φ within a cell
depends upon the old value, φold , the computed change in φ, ∆φ, and the under-relaxation
factor, α, as follows:
φ = φold + α∆φ
(18.4-22)
Under-Relaxation of Equations
The under-relaxation of equations, also known as implicit relaxation, is used in the
pressure-based solver to stabilize the convergence behavior of the outer nonlinear iterations by introducing selective amounts of φ in the system of discretized equations. This
is equivalent to the location-specific time step.
ap φ X
1−α
=
anb φnb + b +
ap φold
α
α
nb
(18.4-23)
The CFL number is a solution parameter in the pressure-based coupled algorithm and
can be written in terms of α:
1−α
1
=
α
CF L
Release 12.0 c ANSYS, Inc. January 29, 2009
(18.4-24)
18-35
Solver Theory
18.4.5
Time-Advancement Algorithm
For time-dependent flows, the discretized form of the generic transport equations is of
the following form:
Z
V
I
I
Z
∂ρφ
~
~
dV + ρφ ~v · dA = Γφ ∇φ · dA + Sφ dV
∂t
V
(18.4-25)
where
∂ρφ
∂t
= conservative form of transient derivative of transported variable φ
ρ
= density
~v
= velocity vector (= u ı̂ + v ̂ in 2D)
~
A
= surface area vector
Γφ = diffusion coefficient for φ
∇φ = gradient of φ (= (∂φ/∂x) ı̂ + (∂φ/∂y) ̂ in 2D)
Sφ = source of φ per unit volume
The temporal discretization of the transient derivative in the Equation 18.4-25 is described in Section 18.3.2: Temporal Discretization, including first-order and second-order
schemes in time. The pressure-based solver in ANSYS FLUENT uses an implicit discretization of the transport equation (Equation 18.4-25). As a standard default approach, all
convective, diffusive, and source terms are evaluated from the fields for time level n+1.
Z
V
I
I
Z
∂ρφ
n+1
n+1 n+1 n+1
n+1
~
~
dV + ρ φ
~v
· dA = Γφ
∇φ
· dA + Sφ n+1 dV
∂t
V
(18.4-26)
In the pressure-based solver, the overall time-discretization error is determined by both
the choice of temporal discretization (e.g., first-order, second-order) and the manner
in which the solutions are advanced to the next time step (time-advancement scheme).
Temporal discretization introduces the corresponding truncation error; O(∆t), O [(∆t)2 ],
for first-order and second-order, respectively. The segregated solution process by which
the equations are solved one by one introduces splitting error. There are two approaches
to the time-advancement scheme depending on how you want to control the splitting
error.
18-36
Release 12.0 c ANSYS, Inc. January 29, 2009
18.4 Pressure-Based Solver
Iterative Time-Advancement Scheme
In the iterative scheme, all the equations are solved iteratively, for a given time-step, until
the convergence criteria are met. Thus, advancing the solutions by one time-step normally requires a number of outer iterations as shown in Figure 18.1.1 and Figure 18.4.1.
With this iterative scheme, non-linearity of the individual equations and inter-equation
couplings are fully accounted for, eliminating the splitting error. The iterative scheme is
the default in ANSYS FLUENT.
t = t + n∆ t
Solve Momentum Equations
Solve Pressure Correction
Outer
Iterations
Correct Velocity
Pressure Flux
Solve Scalars (T, κ , ε , etc.)
Converged?
no
yes
Next Time Step
n += 1
Figure 18.4.1: Overview of the Iterative Time Advancement Solution Method
For the Segregate Solver
Release 12.0 c ANSYS, Inc. January 29, 2009
18-37
Solver Theory
The Frozen Flux Formulation
The standard fully-implicit discretization of the convective part of Equation 18.4-26 produces non-linear terms in the resulting equations. In addition, solving these equations
generally requires numerous iterations per time step. As an alternative, ANSYS FLUENT
provides an optional way to discretize the convective part of Equation 18.4-25 using the
mass flux at the cell faces from the previous time level n.
I
~=
ρφ ~v · dA
I
~
ρn φn+1 ~v n · dA
(18.4-27)
The solution still has the same order of accuracy but the non-linear character of the
discretized transport equation is essentially reduced and the convergence within each
time step is improved.
The Frozen Flux Formulation option is accessible from the Solution Methods dialog box.
i
This option is only available for single-phase transient problems that use
the segregated iterative solver and do not use a moving/deforming mesh
model.
Non-Iterative Time-Advancement Scheme
The iterative time-advancement scheme requires a considerable amount of computational
effort due to a large number of outer iterations performed for each time-step. The idea
underlying the non-iterative time-advancement (NITA) scheme is that, in order to preserve overall time accuracy, you do not really need to reduce the splitting error to zero,
but only have to make it the same order as the truncation error. The NITA scheme, as
seen in Figure 18.4.2, does not need the outer iterations, performing only a single outer
iteration per time-step, which significantly speeds up transient simulations. However, the
NITA scheme still allows for an inner iteration to solve the individual set of equations.
ANSYS FLUENT offers two versions of NITA schemes; the non-iterative fractional step
method (FSM) ([8], [81], [142], and [143]) and the non-iterative PISO method [140]. Both
NITA schemes are available for first-order and second-order time integration.
i
18-38
In general, the NITA solver is not recommended for highly viscous fluid
flow.
Release 12.0 c ANSYS, Inc. January 29, 2009
18.4 Pressure-Based Solver
t = t + n∆ t
Solve U, V, and W Equations
Converged?
Inner
Iterations
No
Yes
Solve Pressure Correction
Inner
Iterations
Correct Velocity
Pressure Flux
Converged?
No
Yes
Solve κ and ε
Converged?
Inner
Iterations
No
Yes
Solve Other Scalars
Next Time Step
n = n+1
Figure 18.4.2: Overview of the Non-Iterative Time Advancement Solution
Method
Release 12.0 c ANSYS, Inc. January 29, 2009
18-39
Solver Theory
18.5
Density-Based Solver
The density-based solver in ANSYS FLUENT solves the governing equations of continuity, momentum, and (where appropriate) energy and species transport simultaneously as
a set, or vector, of equations. Governing equations for additional scalars will be solved
sequentially (i.e., segregated from one another and from the coupled set), in a manner described in Section 18.2: General Scalar Transport Equation: Discretization and Solution.
Two algorithms are available for solving the coupled set of equations, the coupled-explicit
formulation and the coupled-implicit formulation.
Information is organized into the following subsections:
• Section 18.5.1: Governing Equations in Vector Form
• Section 18.5.2: Preconditioning
• Section 18.5.3: Convective Fluxes
• Section 18.5.4: Steady-State Flow Solution Methods
• Section 18.5.5: Unsteady Flows Solution Methods
18.5.1
Governing Equations in Vector Form
The system of governing equations for a single-component fluid, written to describe the
mean flow properties, is cast in integral Cartesian form for an arbitrary control volume
V with differential surface area dA as follows:
I
Z
∂ Z
W dV + [F − G] · dA =
H dV
∂t V
V
(18.5-1)
where the vectors W, F, and G are defined as
W=
ρ
ρu
ρv
ρw
ρE
, F=
ρv
ρvu + pî
ρvv + pĵ
ρvw
+
p
k̂
ρvE + pv
, G=
0
τxi
yi
τ
zi
τ
τij vj + q
and the vector H contains source terms such as body forces and energy sources.
Here ρ, v, E, and p are the density, velocity, total energy per unit mass, and pressure of
the fluid, respectively. τ is the viscous stress tensor, and q is the heat flux.
18-40
Release 12.0 c ANSYS, Inc. January 29, 2009
18.5 Density-Based Solver
Total energy E is related to the total enthalpy H by
E = H − p/ρ
(18.5-2)
H = h + |v|2 /2
(18.5-3)
where
The Navier-Stokes equations as expressed in Equation 18.5-1 become (numerically) very
stiff at low Mach number due to the disparity between the fluid velocity v and the acoustic
speed c (speed of sound). This is also true for incompressible flows, regardless of the fluid
velocity, because acoustic waves travel infinitely fast in an incompressible fluid (speed of
sound is infinite). The numerical stiffness of the equations under these conditions results
in poor convergence rates. This difficulty is overcome in ANSYS FLUENT’s density-based
solver by employing a technique called (time-derivative) preconditioning [372].
18.5.2
Preconditioning
Time-derivative preconditioning modifies the time-derivative term in Equation 18.5-1 by
pre-multiplying it with a preconditioning matrix. This has the effect of re-scaling the
acoustic speed (eigenvalue) of the system of equations being solved in order to alleviate
the numerical stiffness encountered in low Mach numbers and incompressible flow.
Derivation of the preconditioning matrix begins by transforming the dependent variable
in Equation 18.5-1 from conserved quantities W to primitive variables Q using the chainrule as follows:
I
Z
∂W ∂ Z
Q dV + [F − G] · dA =
H dV
∂Q ∂t V
V
(18.5-4)
where Q is the vector {p, u, v, w, T }T and the Jacobian ∂W/∂Q is given by
∂W
=
∂Q
ρp
ρp u
ρp v
ρp w
ρp H − δ
0
ρ
0
0
ρu
0
0
ρ
0
ρv
0
0
0
ρ
ρw
ρT
ρT u
ρT v
ρT w
ρT H + ρCp
(18.5-5)
where
ρp =
Release 12.0 c ANSYS, Inc. January 29, 2009
∂ρ
∂p
, ρT =
T
∂ρ
∂T
p
18-41
Solver Theory
and δ = 1 for an ideal gas and δ = 0 for an incompressible fluid.
The choice of primitive variables Q as dependent variables is desirable for several reasons.
First, it is a natural choice when solving incompressible flows. Second, when we use
second-order accuracy we need to reconstruct Q rather than W in order to obtain more
accurate velocity and temperature gradients in viscous fluxes, and pressure gradients in
inviscid fluxes. And finally, the choice of pressure as a dependent variable allows the
propagation of acoustic waves in the system to be singled out [356].
We precondition the system by replacing the Jacobian matrix ∂W/∂Q (Equation 18.5-5)
with the preconditioning matrix Γ so that the preconditioned system in conservation form
becomes
Γ
I
Z
∂ Z
Q dV + [F − G] · dA =
H dV
∂t V
V
(18.5-6)
where
Γ=
Θ
Θu
Θv
Θw
ΘH − δ
0
ρ
0
0
ρu
0
0
ρ
0
ρv
0
0
0
ρ
ρw
ρT
ρT u
ρT u
ρT u
ρT H + ρCp
(18.5-7)
The parameter Θ is given by
Θ=
1
ρT
−
2
Ur
ρCp
!
(18.5-8)
The reference velocity Ur appearing in Equation 18.5-8 is chosen locally such that the
eigenvalues of the system remain well conditioned with respect to the convective and
diffusive time scales [372].
The resultant eigenvalues of the preconditioned system (Equation 18.5-6) are given by
u, u, u, u0 + c0 , u0 − c0
(18.5-9)
where
u = v · n̂
u0 = u (1 − α)
c0 =
18-42
q
α2 u2 + Ur2
Release 12.0 c ANSYS, Inc. January 29, 2009
18.5 Density-Based Solver
α =
β =
1 − βUr2 /2
ρT
ρp +
ρCp
!
For an ideal gas, β = (γRT )−1 = 1/c2 . Thus, when Ur = c (at sonic speeds and above),
α = 0 and the eigenvalues of the preconditioned system take their traditional form, u ± c.
At low speed, however, as Ur → 0, α → 1/2 and all eigenvalues become of the same order
as u. For constant-density flows, β = 0 and α = 1/2 regardless of the values of Ur . As
long as the reference velocity is of the same order as the local velocity, all eigenvalues
remain of the order u. Thus, the eigenvalues of the preconditioned system remain well
conditioned at all speeds.
Note that the non-preconditioned Navier-Stokes equations are recovered exactly from
Equation 18.5-6 by setting 1/Ur2 to ρp , the derivative of density with respect to pressure.
In this case Γ reduces exactly to the Jacobian ∂W/∂Q.
Although Equation 18.5-6 is conservative in the steady state, it is not, in a strict sense,
conservative for time-dependent flows. This is not a problem, however, since the preconditioning has already destroyed the time accuracy of the equations and we will not
employ them in this form for unsteady calculations.
For unsteady calculations, an unsteady preconditioning is available when the dual-time
stepping method is used (Section 18.5.5: Implicit Time Stepping (Dual-Time formulation)).
The unsteady preconditioning enhances the solution accuracy by improving the scaling
of the artificial dissipation and maximizes the efficiency by optimizing the number of
sub-iterations required at each physical time step [263]. For low Mach number flows
in particular, for both low frequency problems (large time steps) and high frequency
problems (small time step), significant savings in computational time are possible when
compared with the non-preconditioned case.
The unsteady preconditioning adapts the level of preconditioning based on the user specified time-step and on the local advective and acoustic time scales of the flow. For acoustic
problems, the physical time-step size is small as it is based on the acoustic CFL number.
In this case the preconditioning parameter Ur2 will approach c2 , which in effect will turn
off the low-Mach preconditioning almost completely. For advection dominated problems,
like the transport of turbulent vortical structures, etc., the physical time-step is large as
it is based on the particle CFL number. The corresponding unsteady preconditioning
parameter Ur2 will then approach u2 , which corresponds to the steady preconditioning
choice. For intermediate physical time-step sizes, the unsteady preconditioning parameter
will be adapted to provide optimum convergence efficiency of the pseudo-time iterations
and accurate scaling of the artificial dissipation terms, regardless of the choice of the
physical time step.
Release 12.0 c ANSYS, Inc. January 29, 2009
18-43
Solver Theory
18.5.3
Convective Fluxes
Roe Flux-Difference Splitting Scheme
The inviscid flux vector F appearing in Equation 18.5-6 is evaluated by a standard
upwind, flux-difference splitting [296]. This approach acknowledges that the flux vector
F contains characteristic information propagating through the domain with speed and
direction according to the eigenvalues of the system. By splitting F into parts, where
each part contains information traveling in a particular direction (i.e., characteristic
information), and upwind differencing the split fluxes in a manner consistent with their
corresponding eigenvalues, we obtain the following expression for the discrete flux at each
face:
F=
1
1
(FR + FL ) − Γ |Â| δQ
2
2
(18.5-10)
Here δQ is the spatial difference QR − QL . The fluxes FR = F (QR ) and FL = F (QL )
are computed using the (reconstructed) solution vectors QR and QL on the “right” and
“left” side of the face. The matrix |Â| is defined by
|Â| = M |Λ| M −1
(18.5-11)
where Λ is the diagonal matrix of eigenvalues and M is the modal matrix that diagonalizes
Γ−1 A, where A is the inviscid flux Jacobian ∂F/∂Q.
For the non-preconditioned system (and an ideal gas) Equation 18.5-10 reduces to Roe’s
flux-difference splitting [296] when Roe-averaged values are used to evaluate Γ |Â|. At
present, arithmetic averaging of states QR and QL is used.
In its current form, Equation 18.5-10 can be viewed as a second-order central difference
plus an added matrix dissipation. The added matrix dissipation term is not only responsible for producing an upwinding of the convected variables, and of pressure and flux
velocity in supersonic flow, but it also provides the pressure-velocity coupling required
for stability and efficient convergence of low-speed and incompressible flows.
18-44
Release 12.0 c ANSYS, Inc. January 29, 2009
18.5 Density-Based Solver
AUSM+ Scheme
An alternative way to compute the flux vector F appearing in Equation 18.5-6 is by using a flux-vector splitting scheme [53]. The scheme, called Advection Upstream Splitting
Method (AUSM), was first introduced by Liou and Steffen in 1993 [202]. The AUSM
scheme first computes a cell interface Mach number based on the characteristic speeds
from the neighboring cells. The interface Mach number is then used to determine the
upwind extrapolation for the convection part of the inviscid fluxes. A separate Mach
number splitting is used for the pressure terms. Generalized Mach number based convection and pressure splitting functions were proposed by Liou [201] and the new scheme
was termed AUSM+. The AUSM+ scheme has several desirable properties:
1. Provides exact resolution of contact and shock discontinuities
2. Preserves positivity of scalar quantities
3. Free of oscillations at stationary and moving shocks
The AUSM+ scheme avoids using an explicit artificial dissipation, by proposing a numerical flux of the form:
F = mf φ + pi
(18.5-12)
Here mf is the mass flux through the interface, which is computed using the fourth order
polynomial functions of the left and right side (of the interface) Mach numbers.
ANSYS FLUENT utilizes an all-speed version of the AUSM+ scheme based on the lowMach preconditioning.
Low Diffusion Roe Flux Difference Splitting Scheme
In order to reduce dissipation in LES calculations, ANSYS FLUENT uses a modified
version of the Roe Flux Difference Splitting scheme, called the Low Diffusion Roe Flux
Difference Splitting scheme. The scheme includes low Mach number preconditioning, in
which the artificial dissipation term has been reduced [43] through the use of a hybrid
scheme that combines a central scheme and a second-order upwind scheme (Roe’s Flux
Difference scheme).
i
The low diffusion discretization must be used only for subsonic flows. For
high Mach number flows, you should switch to the second-order upwind
scheme.
Release 12.0 c ANSYS, Inc. January 29, 2009
18-45
Solver Theory
i
The low diffusion discretization is only available with the implicit-time
formulation (dual-time-stepping). When running LES with the explicit
time formulation, you will need to use the second-order upwind scheme.
To learn how to apply the different convective fluxes, see Section 26.4.2: Convective Flux
Types in the separate User’s Guide.
18.5.4
Steady-State Flow Solution Methods
The coupled set of governing equations (Equation 18.5-6) in ANSYS FLUENT is discretized in time for both steady and unsteady calculations. In the steady case, it is
assumed that time marching proceeds until a steady-state solution is reached. Temporal discretization of the coupled equations is accomplished by either an implicit or an
explicit time-marching algorithm. These two algorithms are described below. To learn
how to apply the two formulations, see Section 26.4: Density-Based Solver Settings in
the separate User’s Guide.
Explicit Formulation
In the explicit scheme a multi-stage, time-stepping algorithm [146] is used to discretize
the time derivative in Equation 18.5-6. The solution is advanced from iteration n to
iteration n + 1 with an m-stage Runge-Kutta scheme, given by
Q0 = Qn
∆Qi = −αi ∆tΓ−1 Ri−1
Qn+1 = Qm
where ∆Qi ≡ Qi − Qn and i = 1, 2, . . . , m is the stage counter for the m-stage scheme.
αi is the multi-stage coefficient for the ith stage. The residual Ri is computed from the
intermediate solution Qi and, for Equation 18.5-6, is given by
Ri =
NX
faces
F(Qi ) − G(Qi ) · A − V H
(18.5-13)
The time step ∆t is computed from the CFL (Courant-Friedrichs-Lewy) condition
2CFL · V
∆t = P
max
Af
f λf
(18.5-14)
where V is the cell volume, Af is the face area, and λf max is the maximum of the local
eigenvalues defined by Equation 18.5-9.
18-46
Release 12.0 c ANSYS, Inc. January 29, 2009
18.5 Density-Based Solver
For steady-state solutions, convergence acceleration of the explicit formulation can be
achieved with the use of local time stepping, residual smoothing, and full-approximation
storage multigrid.
Local time stepping is a method by which the solution at each control volume is advanced
in time with respect to the cell time step, defined by the local stability limit of the timestepping scheme.
Residual smoothing, on the other hand, increases the bound of stability limits of the
time-stepping scheme and hence allows for the use of a larger CFL value to achieve fast
convergence (Section 18.5.4: Implicit Residual Smoothing).
The convergence rate of the explicit scheme can be accelerated through use of the
full-approximation storage (FAS) multigrid method described in Section 18.6.4: FullApproximation Storage (FAS) Multigrid.
By default, ANSYS FLUENT uses a 3-stage Runge-Kutta scheme based on the work by
Lynn [211] for steady-state flows that use the density-based explicit solver.
Implicit Residual Smoothing
The maximum time step can be further increased by increasing the support of the scheme
through implicit averaging of the residuals with their neighbors. The residuals are filtered
through a Laplacian smoothing operator:
R̄i = Ri +
X
(R̄j − R̄i )
(18.5-15)
This equation can be solved with the following Jacobi iteration:
Ri + R̄jm−1
=
P
1+ 1
P
R̄im
(18.5-16)
Two Jacobi iterations are usually sufficient to allow doubling the time step with a value
of = 0.5.
Implicit Formulation
In the implicit scheme, an Euler implicit discretization in time of the governing equations
(Equation 18.5-6) is combined with a Newton-type linearization of the fluxes to produce
the following linearized system in delta form [370]:
D +
NX
faces
Sj,k ∆Qn+1 = −Rn
(18.5-17)
j
The center and off-diagonal coefficient matrices, D and Sj,k are given by
Release 12.0 c ANSYS, Inc. January 29, 2009
18-47
Solver Theory
NX
faces
V
Γ+
Sj,i
D =
∆t
j
(18.5-18)
!
Sj,k =
∂Fj
∂Gj
−
Aj
∂Qk ∂Qk
(18.5-19)
and the residual vector Rn and time step ∆t are defined as in Equation 18.5-13 and
Equation 18.5-14, respectively.
Equation 18.5-17 is solved using either Incomplete Lower Upper factorization (ILU) by
default or symmetric point Gauss-Seidel algorithm, in conjunction with an algebraic
multigrid (AMG) method (see Section 18.6.3: Algebraic Multigrid (AMG)) adapted for
coupled sets of equations.
Explicit relaxation can improve the convergence to steady state of the implicit formulation. By default, explicit relaxation is enabled for the implicit solver and uses a factor
of 0.75. You can specify a factor α to control the amount that the solution vector Q
changes between iterations after the end of the algebraic multigrid (AMG) cycle:
Qnew = Qold + α∆Q
(18.5-20)
By specifying a value less than the default value of 1 for α, the variables in the solution
vector will be under-relaxed and the convergence history can be improved. For information on how to set this value, see Section 26.4.3: Specifying the Explicit Relaxation in
the separate User’s Guide.
i
18.5.5
Note that explicit relaxation is available for the density-based implicit
solver in steady state mode only.
Unsteady Flows Solution Methods
For time-accurate calculations, explicit and implicit time-stepping schemes are available.
(The time-implicit approach is also referred to as “dual time stepping”.)
Explicit Time Stepping
The explicit time stepping approach, is available only for the explicit scheme described
above. The time step is determined by the CFL condition. To maintain time accuracy
of the solution the explicit time stepping employs the same time step in each cell of the
domain (this is also known as global-time step), and with preconditioning disabled. By
default, ANSYS FLUENT uses a 4-stage Runge-Kutta scheme for unsteady flows.
18-48
Release 12.0 c ANSYS, Inc. January 29, 2009
18.5 Density-Based Solver
Implicit Time Stepping (Dual-Time formulation)
The implicit-time stepping method (also known as dual-time formulation) is available in
the density-based explicit and implicit formulation.
When performing unsteady simulations with implicit-time stepping (dual-time stepping),
ANSYS FLUENT uses a low Mach number time-derivative unsteady preconditioner to
provide accurate results both for pure convective processes (e.g., simulating unsteady
turbulence) and for acoustic processes (e.g., simulating wave propagation) [350, 263].
Here we introduce a preconditioned pseudo-time-derivative term into Equation 18.5-1 as
follows:
I
Z
∂ Z
∂ Z
W dV + Γ
Q dV + [F − G] · dA =
H dV
∂t V
∂τ V
V
(18.5-21)
where t denotes physical-time and τ is a pseudo-time used in the time-marching procedure. Note that as τ → ∞, the second term on the left side of Equation 18.5-21 vanishes
and Equation 18.5-1 is recovered.
The time-dependent term in Equation 18.5-21 is discretized in an implicit fashion by
means of either a first- or second-order accurate, backward difference in time.
The dual-time formulation is written in semi-discrete form as follows:
"
#
Γ
0 ∂W
1 I
k+1
+
∆Q
+
[F − G] · dA
∆τ
∆t ∂Q
V
1
=H −
0 Wk − 1 Wn + 2 Wn−1
∆t
where {0 = 1 = 1/2, 2 = 0} gives first-order time accuracy, and {0 = 3/2, 1 = 2, 2 =
1/2} gives second-order. k is the inner iteration counter and n represents any given
physical-time level.
The pseudo-time-derivative is driven to zero at each physical time level by a series of
inner iterations using either the implicit or explicit time-marching algorithm.
Throughout the (inner) iterations in pseudo-time, Wn and Wn−1 are held constant and
Wk is computed from Qk . As τ → ∞, the solution at the next physical time level Wn+1
is given by W(Qk ).
Note that the physical time step ∆t is limited only by the level of desired temporal
accuracy. The pseudo-time-step ∆τ is determined by the CFL condition of the (implicit
or explicit) time-marching scheme.
Release 12.0 c ANSYS, Inc. January 29, 2009
18-49
Solver Theory
Table 18.5.1 summarizes all operation modes for the density-based solver from the iterative scheme in steady-state calculations to time-marching schemes for transient calculations.
Table 18.5.1: Summary of the Density-Based Solver
Solution
Method
Steady-State
Unsteady Explicit Time
Stepping
Unsteady Implicit Time
Stepping
(dual-time
formulation)
First Order
Unsteady Implicit Time
Stepping
(dual-time
formulation)
Second Order
18-50
Density-Based Solver Explicit Formulation
– 3-stages Runge-Kutta
– local time step
– time-derivative
preconditioning
– FAS
– 4-stages Runge-Kutta
– global time step
– no time-derivative
preconditioning
– No FAS
– dual-time formulation
– Physical time: first order
Euler backward
– preconditioned
pseudo-time derivative
– inner iteration: explicit
pseudo-time marching,
3-stage Runge-Kutta
– dual-time formulation
– Physical time: second
order Euler backward
– preconditioned
pseudo-time derivative
– inner iteration: explicit
pseudo-time marching,
3-stage Runge-Kutta
Density-Based Solver Implicit Formulation
– local time step
– time-derivative
preconditioning
N/A
– dual-time formulation
– Physical time: first order
Euler backward
– preconditioned
pseudo-time derivative
– inner iteration: implicit
pseudo-time marching
– dual-time formulation
– Physical time: second
order Euler backward
– preconditioned
pseudo-time derivative
– inner iteration: implicit
pseudo-time marching
Release 12.0 c ANSYS, Inc. January 29, 2009
18.6 Multigrid Method
18.6
Multigrid Method
The ANSYS FLUENT solver contains two forms of multigrid: algebraic (AMG) and fullapproximation storage (FAS). AMG is an essential component of both the pressure-based
and density-based implicit solvers, while FAS is an important, but optional, component
of the density-based explicit solver. (Note that when the density-based explicit solver
is used, AMG will also be used, since the scalar equations (e.g., turbulence) are solved
using the approach described in Section 18.2: General Scalar Transport Equation: Discretization and Solution.)
This section describes the mathematical basis of the multigrid approach. Common aspects of AMG and FAS are presented first, followed by separate sections that provide
details unique to each method.
Information is organized into the following subsections:
• Section 18.6.1: Approach
• Section 18.6.2: Multigrid Cycles
• Section 18.6.3: Algebraic Multigrid (AMG)
• Section 18.6.4: Full-Approximation Storage (FAS) Multigrid
For information about user inputs and controls for the multigrid solver, see
Section 26.18.3: Modifying Algebraic Multigrid Parameters and Section 26.5.2: Setting
FAS Multigrid Parameters in the separate User’s Guide.
18.6.1
Approach
ANSYS FLUENT uses a multigrid scheme to accelerate the convergence of the solver
by computing corrections on a series of coarse grid levels. The use of this multigrid
scheme can greatly reduce the number of iterations and the CPU time required to obtain
a converged solution, particularly when your model contains a large number of control
volumes.
The Need for Multigrid
Implicit solution of the linearized equations on unstructured meshes is complicated by
the fact that there is no equivalent of the line-iterative methods that are commonly
used on structured meshes. Since direct matrix inversion is out of the question for
realistic problems and “whole-field” solvers that rely on conjugate-gradient (CG) methods
have robustness problems associated with them, the methods of choice are point implicit
solvers like Gauss-Seidel and ILU. Although the Gauss-Seidel and ILU schemes rapidly
remove local (high-frequency) errors in the solution, global (low-frequency) errors are
Release 12.0 c ANSYS, Inc. January 29, 2009
18-51
Solver Theory
reduced at a rate inversely related to the mesh size. Thus, for a large number of nodes,
the solver “stalls” and the residual reduction rate becomes prohibitively low.
The multi-stage scheme used in the density-based explicit solver can efficiently remove
local (high-frequency) errors as well. That is, the effect of the solution in one cell is
communicated to adjacent cells relatively quickly. However, the scheme is less effective
at reducing global (low-frequency) errors–errors which exist over a large number of control
volumes. Thus, global corrections to the solution across a large number of control volumes
occur slowly, over many iterations. This implies that performance of the multi-stage
scheme will deteriorate as the number of control volumes increases.
Multigrid techniques allow global error to be addressed by using a sequence of successively
coarser meshes. This method is based upon the principle that global (low-frequency)
error existing on a fine mesh can be represented on a coarse mesh where it again becomes
accessible as local (high-frequency) error: because there are fewer coarse cells overall,
the global corrections can be communicated more quickly between adjacent cells. Since
computations can be performed at an exponentially decaying expense in both CPU time
and memory storage on coarser meshes, there is the potential for very efficient elimination
of global error. The fine-grid relaxation scheme or “smoother”, in this case either the
point-implicit linear solvers (Section 18.6.3: The Coupled and Scalar AMG Solvers) or
the explicit multi-stage scheme, is not required to be particularly effective at reducing
global error and can be tuned for efficient reduction of local error.
The Basic Concept in Multigrid
Consider the set of discretized linear (or linearized) equations given by
A φe + b = 0
(18.6-1)
where φe is the exact solution. Before the solution has converged there will be a defect
d associated with the approximate solution φ:
Aφ + b = d
(18.6-2)
We seek a correction ψ to φ such that the exact solution is given by
φe = φ + ψ
(18.6-3)
Substituting Equation 18.6-3 into Equation 18.6-1 gives
A (φ + ψ) + b = 0
A ψ + (A φ + b) = 0
18-52
(18.6-4)
(18.6-5)
Release 12.0 c ANSYS, Inc. January 29, 2009
18.6 Multigrid Method
Now using Equations 18.6-2 and 18.6-5 we obtain
Aψ + d = 0
(18.6-6)
which is an equation for the correction in terms of the original fine level operator A and
the defect d. Assuming the local (high-frequency) errors have been sufficiently damped
by the relaxation scheme on the fine level, the correction ψ will be smooth and therefore
more effectively solved on the next coarser level.
Restriction and Prolongation
Solving for corrections on the coarse level requires transferring the defect down from
the fine level (restriction), computing corrections, and then transferring the corrections
back up from the coarse level (prolongation). We can write the equations for coarse level
corrections ψ H as
AH ψ H + R d = 0
(18.6-7)
where AH is the coarse level operator and R the restriction operator responsible for
transferring the fine level defect down to the coarse level. Solution of Equation 18.6-7 is
followed by an update of the fine level solution given by
φnew = φ + P ψ H
(18.6-8)
where P is the prolongation operator used to transfer the coarse level corrections up to
the fine level.
Unstructured Multigrid
The primary difficulty with using multigrid on unstructured meshes is the creation and
use of the coarse grid hierarchy. On a structured mesh, the coarse meshes can be formed
simply by removing every other mesh line from the fine meshes and the prolongation and
restriction operators are simple to formulate (e.g., injection and bilinear interpolation).
The difficulties of applying multigrid on unstructured meshes are overcome in a separate
fashion by each of the two multigrid methods used in ANSYS FLUENT. While the basic
principles discussed so far and the cycling strategy described in Section 18.6.2: Multigrid
Cycles are the same, the techniques for construction of restriction, prolongation, and
coarse mesh operators are different, as discussed in Section 18.6.3: Algebraic Multigrid
(AMG) and Section 18.6.4: Full-Approximation Storage (FAS) Multigrid for the AMG
and FAS methods, respectively.
Release 12.0 c ANSYS, Inc. January 29, 2009
18-53
Solver Theory
18.6.2
Multigrid Cycles
A multigrid cycle can be defined as a recursive procedure that is applied at each grid
level as it moves through the grid hierarchy. Four types of multigrid cycles are available
in ANSYS FLUENT: the V, W, F, and flexible (“flex”) cycles. The V and W cycles are
available in both AMG and FAS, while the F and flexible cycles are restricted to the
AMG method only. (The W and flexible AMG cycles are not available for solving the
coupled equation set due to the amount of computation required.)
The V and W Cycles
Figures 18.6.1 and 18.6.2 show the V and W multigrid cycles (defined below). In each
figure, the multigrid cycle is represented by a square, and then expanded recursively to
show the individual steps that are performed within the cycle. The individual steps are
represented by a circle, one or more squares, and a triangle, connected by lines: circlesquare-triangle for a V cycle, or circle-square-square-triangle for a W cycle. The squares
in this group expand again, into circle-square-triangle or circle-square-square-triangle,
and so on. You may want to follow along in the figures as you read the steps below.
For the V and W cycles, the traversal of the hierarchy is governed by three parameters,
β1 , β2 , and β3 , as follows:
1. First, iterations are performed on the current grid level to reduce the high-frequency
components of the error (local error). For AMG, one iteration consists of one forward and one backward Gauss-Seidel sweep. For FAS, one iteration consists of one
pass of the multi-stage scheme (described in Section 18.5.4: Explicit Formulation).
These iterations are referred to as pre-relaxation sweeps because they are performed
before moving to the next coarser grid level. The number of pre-relaxation sweeps
is specified by β1 .
In Figures 18.6.1 and 18.6.2 this step is represented by a circle and marks the start
of a multigrid cycle. The high-wave-number components of error should be reduced
until the remaining error is expressible on the next coarser mesh without significant
aliasing.
If this is the coarsest grid level, then the multigrid cycle on this level is complete. (In
Figures 18.6.1 and 18.6.2 there are 3 coarse grid levels, so the square representing
the multigrid cycle on level 3 is equivalent to a circle, as shown in the final diagram
in each figure.)
i
In the AMG method, the default value of β1 is zero (i.e., no pre-relaxation
sweeps are performed).
2. Next, the problem is “restricted” to the next coarser grid level using Equation 18.6-7.
In Figures 18.6.1 and 18.6.2, the restriction from a finer grid level to a coarser grid
level is designated by a downward-sloping line.
18-54
Release 12.0 c ANSYS, Inc. January 29, 2009
18.6 Multigrid Method
grid
level
multigrid cycle
0
pre-relaxation sweeps
0
post-relaxation sweeps and/or
Laplacian smoothings
1
0
1
2
0
1
2
3
0
1
2
3
Figure 18.6.1: V-Cycle Multigrid
grid
level
multigrid cycle
0
pre-relaxation sweeps
0
post-relaxation sweeps and/or
Laplacian smoothings
1
0
1
2
0
1
2
3
0
1
2
3
Figure 18.6.2: W-Cycle Multigrid
Release 12.0 c ANSYS, Inc. January 29, 2009
18-55
Solver Theory
3. The error on the coarse grid is reduced by performing a specified number (β2 ) of
multigrid cycles (represented in Figures 18.6.1 and 18.6.2 as squares). Commonly,
for fixed multigrid strategies β2 is either 1 or 2, corresponding to V-cycle and Wcycle multigrid, respectively.
4. Next, the cumulative correction computed on the coarse grid is “interpolated”
back to the fine grid using Equation 18.6-8 and added to the fine grid solution. In
the FAS method, the corrections are additionally smoothed during this step using
the Laplacian smoothing operator discussed in Section 18.5.4: Implicit Residual
Smoothing.
In Figures 18.6.1 and 18.6.2 the prolongation is represented by an upward-sloping
line.
The high-frequency error now present at the fine grid level is due to the prolongation
procedure used to transfer the correction.
5. In the final step, iterations are performed on the fine grid to remove the highfrequency error introduced on the coarse grid by the multigrid cycles. These iterations are referred to as post-relaxation sweeps because they are performed after
returning from the next coarser grid level. The number of post-relaxation sweeps
is specified by β3 .
In Figures 18.6.1 and 18.6.2, this relaxation procedure is represented by a single
triangle.
For AMG, the default value of β3 is 1.
i
Note, however, that if you are using AMG with V-cycle to solve an energy equation with a solid conduction model presented with anisotropic
or very high conductivity coefficient, there is a possibility of divergence
with a default post-relaxation sweep of 1. In such cases you should increase the post-relaxation sweep (e.g., to 2) in the AMG section for better convergence, or change the cycle type to F-cycle or W-cycle, with an
under-relaxation factor set to 1. This is especially effective when calculating pure heat conduction or conjugate heat transfer. Any instability
observed when using the F-cycle or W-cycle can be remedied by increasing
the pre-relaxation sweep count to 1. Although the default value of 0 is
optimal for most cases, increasing the pre-relaxation sweep value to 1 or 2
can improve convergence.
Since the default value for β1 is 0 (i.e., pre-relaxation sweeps are not performed),this
procedure is roughly equivalent to using the solution from the coarse level as the
initial guess for the solution at the fine level.
18-56
Release 12.0 c ANSYS, Inc. January 29, 2009
18.6 Multigrid Method
For FAS, the default value of β3 is zero (i.e., post-relaxation sweeps are not performed); post-relaxation sweeps are never performed at the end of the cycle for
the finest grid level, regardless of the value of β3 . This is because for FAS, postrelaxation sweeps at the fine level are equivalent to pre-relaxation sweeps during
the next cycle.
18.6.3
Algebraic Multigrid (AMG)
This algorithm is referred to as an “algebraic” multigrid scheme because, as we shall
see, the coarse level equations are generated without the use of any geometry or rediscretization on the coarse levels; a feature that makes AMG particularly attractive
for use on unstructured meshes. The advantage being that no coarse meshes have to
be constructed or stored, and no fluxes or source terms need to be evaluated on the
coarse levels. This approach is in contrast with FAS (sometimes called “geometric”)
multigrid in which a hierarchy of meshes is required and the discretized equations are
evaluated on every level. In theory, the advantage of FAS over AMG is that the former
should perform better for non-linear problems since non-linearities in the system are
carried down to the coarse levels through the re-discretization; when using AMG, once
the system is linearized, non-linearities are not “felt” by the solver until the fine level
operator is next updated.
AMG Restriction and Prolongation Operators
The restriction and prolongation operators used here are based on the additive correction
(AC) strategy described for structured meshes by Hutchinson and Raithby [136]. Interlevel transfer is accomplished by piecewise constant interpolation and prolongation. The
defect in any coarse level cell is given by the sum of those from the fine level cells it
contains, while fine level corrections are obtained by injection of coarse level values. In
this manner the prolongation operator is given by the transpose of the restriction operator
P = RT
(18.6-9)
The restriction operator is defined by a coarsening or “grouping” of fine level cells into
coarse level ones. In this process each fine level cell is grouped with one or more of
its “strongest” neighbors, with a preference given to currently ungrouped neighbors.
The algorithm attempts to collect cells into groups of fixed size, typically two or four,
but any number can be specified. In the context of grouping, strongest refers to the
neighbor j of the current cell i for which the coefficient Aij is largest. For sets of coupled
equations Aij is a block matrix and the measure of its magnitude is simply taken to be
the magnitude of its first element. In addition, the set of coupled equations for a given
cell are treated together and not divided amongst different coarse cells. This results in
the same coarsening for each equation in the system.
Release 12.0 c ANSYS, Inc. January 29, 2009
18-57
Solver Theory
AMG Coarse Level Operator
The coarse level operator AH is constructed using a Galerkin approach. Here we require that the defect associated with the corrected fine level solution must vanish when
transferred back to the coarse level. Therefore we may write
R dnew = 0
(18.6-10)
Upon substituting Equations 18.6-2 and 18.6-8 for dnew and φnew we have
R [A φnew + b] = 0
h
R A φ + P ψH + b
i
= 0
(18.6-11)
Now rearranging and using Equation 18.6-2 once again gives
R A P ψ H + R (A φ + b) = 0
R A P ψH + R d = 0
(18.6-12)
Comparison of Equation 18.6-12 with Equation 18.6-7 leads to the following expression
for the coarse level operator:
AH = R A P
(18.6-13)
The construction of coarse level operators thus reduces to a summation of diagonal and
corresponding off-diagonal blocks for all fine level cells within a group to form the diagonal
block of that group’s coarse cell.
18-58
Release 12.0 c ANSYS, Inc. January 29, 2009
18.6 Multigrid Method
The F Cycle
The multigrid F cycle is essentially a combination of the V and W cycles described in
Section 18.6.2: The V and W Cycles.
Recall that the multigrid cycle is a recursive procedure. The procedure is expanded to
the next coarsest grid level by performing a single multigrid cycle on the current level.
Referring to Figures 18.6.1 and 18.6.2, this means replacing the square on the current
level (representing a single cycle) with the procedure shown for the 0-1 level cycle (the
second diagram in each figure). We see that a V cycle consists of:
pre sweep → restrict → V cycle → prolongate → post sweep
and a W cycle:
pre sweep → restrict → W cycle → W cycle → prolongate → post sweep
An F cycle is formed by a W cycle followed by a V cycle:
pre sweep → restrict → W cycle → V cycle → prolongate → post sweep
As expected, the F cycle requires more computation than the V cycle, but less than the
W cycle. However, its convergence properties turn out to be better than the V cycle and
roughly equivalent to the W cycle. The F cycle is the default AMG cycle type for the
coupled equation set.
The Flexible Cycle
For the flexible cycle, the calculation and use of coarse grid corrections is controlled in
the multigrid procedure by the logic illustrated in Figure 18.6.3. This logic ensures that
coarser grid calculations are invoked when the rate of residual reduction on the current
grid level is too slow. In addition, the multigrid controls dictate when the iterative
solution of the correction on the current coarse grid level is sufficiently converged and
should thus be applied to the solution on the next finer grid. These two decisions are
controlled by the parameters α and β shown in Figure 18.6.3, as described in detail
below. Note that the logic of the multigrid procedure is such that grid levels may be
visited repeatedly during a single global iteration on an equation. For a set of 4 multigrid
levels, referred to as 0, 1, 2, and 3, the flex-cycle multigrid procedure for solving a given
transport equation might consist of visiting grid levels as 0-1-2-3-2-3-2-1-0-1-2-1-0, for
example.
The main difference between the flexible cycle and the V and W cycles is that the
satisfaction of the residual reduction tolerance and termination criterion determine when
and how often each level is visited in the flexible cycle, whereas in the V and W cycles
the traversal pattern is explicitly defined.
Release 12.0 c ANSYS, Inc. January 29, 2009
18-59
Solver Theory
level
Solve for φ on level 0 (fine) grid
0
R0
relaxation
0
0
R i> β R i-1
1
1
return R 0i< α R 00 or
i > i max,fine
R i< α R 0 or
i > i max,coarse
Solve for φ′ on level 1 grid
1
1
R i> β R i-1
2
2
R i< α R 0 or
i > i max,coarse
Solve for φ′ on level 2 grid
2
2
R i> β R i-1
3
3
R i< α R 0 or
i > i max,coarse
etc.
Figure 18.6.3: Logic Controlling the Flex Multigrid Cycle
The Residual Reduction Rate Criteria
The multigrid procedure invokes calculations on the next coarser grid level when the
error reduction rate on the current level is insufficient, as defined by
Ri > βRi−1
(18.6-14)
Here Ri is the absolute sum of residuals (defect) computed on the current grid level after
the ith relaxation on this level. The above equation states that if the residual present in
the iterative solution after i relaxations is greater than some fraction, β (between 0 and
1), of the residual present after the (i − 1)th relaxation, the next coarser grid level should
be visited. Thus β is referred to as the residual reduction tolerance, and determines when
to “give up” on the iterative solution at the current grid level and move to solving the
correction equations on the next coarser grid. The value of β controls the frequency with
which coarser grid levels are visited. The default value is 0.7. A larger value will result
in less frequent visits, and a smaller value will result in more frequent visits.
18-60
Release 12.0 c ANSYS, Inc. January 29, 2009
18.6 Multigrid Method
The Termination Criteria
Provided that the residual reduction rate is sufficiently rapid, the correction equations
will be converged on the current grid level and the result applied to the solution field on
the next finer grid level.
The correction equations on the current grid level are considered sufficiently converged
when the error in the correction solution is reduced to some fraction, α (between 0 and
1), of the original error on this grid level:
Ri < αR0
(18.6-15)
Here, Ri is the residual on the current grid level after the ith iteration on this level,
and R0 is the residual that was initially obtained on this grid level at the current global
iteration. The parameter α, referred to as the termination criterion, has a default value
of 0.1. Note that the above equation is also used to terminate calculations on the lowest
(finest) grid level during the multigrid procedure. Thus, relaxations are continued on each
grid level (including the finest grid level) until the criterion of this equation is obeyed
(or until a maximum number of relaxations has been completed, in the case that the
specified criterion is never achieved).
The Coupled and Scalar AMG Solvers
The scalar AMG solver is used for the solution of linear systems obtained from the
discretization of the individual transport equations.
aij xj = bi
(18.6-16)
where the above equation contains scalar variables.
The coupled AMG solver is used to solve linear transport equations using implicit discretization from coupled systems such as flow variables for the density-based solver,
pressure-velocity variables for the coupled pressure-based schemes and inter-phase coupled individual equations for Eulerian multiphase flows.
~j = B
~i
[A]ij X
(18.6-17)
where the influence of a cell i on a cell j has the form
Aij =
Release 12.0 c ANSYS, Inc. January 29, 2009
a12
... a1N
a11
ij
ij
ij
a21
.
.
ij
:
. .
1
N
aN
aN
ij
ij
(18.6-18)
18-61
Solver Theory
and the unknown and source vectors have the form
~j =
X
~i =
B
x1j
.
.
xN
j
b1i
.
.
bN
i
(18.6-19)
(18.6-20)
The above resultant system of equations is solved in ANSYS FLUENT using either the
Gauss-Seidel smoother or the Incomplete Lower Upper decomposition (ILU) smoother. If
a scalar system of equations is to be solved then the point-method (Gauss-Seidel or ILU)
smoother is used, while for a coupled system of equations the block-method (Gauss-Seidel
or ILU) smoother is used.
Gauss-Seidel
The Gauss-Seidel method is a technique for solving a linear system of equations one at
a time and in sequence. It uses the previously computed results as soon as they become
available. It performs two sweeps on the unknowns in forward and backward directions.
Both point or block method Gauss-Seidel smoothers are available in ANSYS FLUENT
to solve for either the scalar AMG system of equations or the coupled AMG system of
equations.
The Gauss-Seidel procedure can be illustrated using the scalar system, Equation 18.6-16.
The forward sweep can be written as:
xi k+1/2 = (bi −
X
aij xj k+1/2 −
ji
(i = 1, ..., N )
where N is the number of unknowns. The forward sweep is followed by a backward sweep
which can be written as:
xi k+1 = (bi −
X
ji
Release 12.0 c ANSYS, Inc. January 29, 2009
18.6 Multigrid Method
Following from Equations 18.6-21 and 18.6-22, symmetric Gauss-Seidel can be expressed
in matrix form as a two-step recursive solution of the system
(DA + LA )DA −1 (DA + UA )(xk+1 − xk ) = b − Axk
(18.6-23)
where DA , LA , and UA represent diagonal, lower tridiagonal, and upper tridiagonal parts
of matrix A, respectively.
Symmetric Gauss-Seidel has a somewhat limited rate of smoothing of residuals between
levels of AMG, unless the coarsening factor is set to 2.
Incomplete Lower Upper (ILU)
A more effective AMG smoother is based on the ILU decomposition technique. In general,
any iterational method can be represented as
M (xk+1 − xk ) = b − Axk
(18.6-24)
where matrix M is some approximation of the original matrix A from
Ax = b
(18.6-25)
M should be close to A and the calculation of M −1 should have a low operation count.
We consider M as an incomplete lower upper factorization of the matrix A such that
M = LU = (D + LA )D−1 (D + UA )
(18.6-26)
where LA and UA are the lower tridiagonal and upper tridiagonal parts of matrix A. The
diagonal matrix D is calculated in a special way to satisfy the following condition for
diagonal DM of matrix M:
DM = DA
(18.6-27)
In this case, the ith element of the diagonal of D will be calculated using
dii = aii −
X aij aji
(
j<1
Release 12.0 c ANSYS, Inc. January 29, 2009
djj
)
(18.6-28)
18-63
Solver Theory
The calculation of the new solution xk+1 is then performed in two symmetric recursive
sweeps, similar to Gauss-Seidel sweeps. Diagonal elements dii of the ILU decomposition
are calculated during the construction of levels and stored in the memory. ILU smoother
is slightly more expensive compared to Gauss-Seidel, but has better smoothing properties,
especially for block-coupled systems solved by coupled AMG. In this case, coarsening of
levels can be more aggressive using coarsening factors between 8 and 12 for 3D problems
compared to 2 for Gauss-Seidel.
i
18.6.4
When solving the coupled systems, shorter solution times and more robust
performance can be obtained by using the default ILU smoother, rather
than the Gauss-Seidel smoother, which is the default for scalar systems.
ILU is recommended whenever the coupled AMG solver is used.
Full-Approximation Storage (FAS) Multigrid
ANSYS FLUENT’s approach to forming the multigrid grid hierarchy for FAS is simply
to coalesce groups of cells on the finer grid to form coarse grid cells. Coarse grid cells
are created by agglomerating the cells surrounding a node, as shown in Figure 18.6.4.
Depending on the grid topology, this can result in cells with irregular shapes and variable
numbers of faces. The grid levels are, however, simple to construct and are embedded,
resulting in simple prolongation and relaxation operators.
Figure 18.6.4: Node Agglomeration to Form Coarse Grid Cells
It is interesting to note that although the coarse grid cells look very irregular, the discretization cannot “see” the jaggedness in the cell faces. The discretization uses only the
area projections of the cell faces and therefore each group of “jagged” cell faces separating two irregularly-shaped cells is equivalent to a single straight line (in 2D) connecting
the endpoints of the jagged segment. (In 3D, the area projections form an irregular, but
continuous, geometrical shape.) This optimization decreases the memory requirement
and the computation time.
18-64
Release 12.0 c ANSYS, Inc. January 29, 2009
18.6 Multigrid Method
FAS Restriction and Prolongation Operators
FAS requires restriction of both the fine grid solution φ and its residual (defect) d. The
restriction operator R used to transfer the solution to the next coarser grid level is formed
using a full-approximation scheme [35]. That is, the solution for a coarse cell is obtained
by taking the volume average of the solution values in the embedded fine grid cells.
Residuals for the coarse grid cell are obtained by summing the residuals in the embedded
fine grid cells.
The prolongation operator P used to transfer corrections up to the fine level is constructed
to simply set the fine grid correction to the associated coarse grid value.
The coarse grid corrections ψ H , which are brought up from the coarse level and applied to
the fine level solution, are computed from the difference between the solution calculated
on the coarse level φH and the initial solution restricted down to the coarse level Rφ.
Thus correction of the fine level solution becomes
φnew = φ + P φH − Rφ
(18.6-29)
FAS Coarse Level Operator
The FAS coarse grid operator AH is simply that which results from a re-discretization
of the governing equations on the coarse level mesh. Since the discretized equations
presented in Sections 18.3 and 18.5 place no restrictions on the number of faces that
make up a cell, there is no problem in performing this re-discretization on the coarse
grids composed of irregularly shaped cells.
There is some loss of accuracy when the finite-volume scheme is used on the irregular
coarse grid cells, but the accuracy of the multigrid solution is determined solely by the
finest grid and is therefore not affected by the coarse grid discretization.
In order to preserve accuracy of the fine grid solution, the coarse level equations are
modified to include source terms [145] which insure that corrections computed on the
coarse grid φH will be zero if the residuals on the fine grid dh are zero as well. Thus, the
coarse grid equations are formulated as
AH φH + dH = dH (Rφ) − Rdh
(18.6-30)
Here dH is the coarse grid residual computed from the current coarse grid solution φH ,
and dH (Rφ) is the coarse grid residual computed from the restricted fine level solution
Rφ. Initially, these two terms will be the same (because initially we have φH = Rφ) and
cancel from the equation, leaving
AH φH = −Rdh
Release 12.0 c ANSYS, Inc. January 29, 2009
(18.6-31)
18-65
Solver Theory
So there will be no coarse level correction when the fine grid residual dh is zero.
18.7
Full Multigrid (FMG) Initialization
For many complex flow problems such as those found in rotating machinery, or flows in
expanding or spiral ducts, flow convergence can be accelerated if a better initial solution
is used at the start of the calculation. The Full Multigrid initialization (FMG initialization) can provide this initial and approximate solution at a minimum cost to the overall
computational expense.
For more information about using FMG initialization in ANSYS FLUENT, see Section 26.10: Using Full Multigrid (FMG) Initialization in the separate User’s Guide.
18.7.1
Overview of FMG Initialization
FMG initialization utilizes the ANSYS FLUENT FAS Multigrid technology (see Section 18.6.4: Full-Approximation Storage (FAS) Multigrid) to obtain the initial solution.
Starting from a uniform solution (after performing standard initialization), the FMG
initialization procedure constructs the desirable number of geometric grid levels using
the procedure outlined in Section 18.6.4: Full-Approximation Storage (FAS) Multigrid.
To begin the process, the initial solution is restricted all the way down to the coarsest
level. The FAS multigrid cycle is then applied until a given order of residual reduction is
obtained or the maximum number of cycles is reached. The solution is then interpolated
one grid level up and the FAS multigrid cycle is applied again between the current level
all the way down to the coarsest level. This process will repeat until the finest level is
reached. The FMG initialization iteration is illustrated in Figure 18.7.1.
Grid Level
Fine
1 multistage sweep on
fine mesh
0
1
2
Coarse 3
n cycles in
level 3
n cycles in level 2
n cycles in level 1
Figure 18.7.1: The FMG Initialization
18-66
Release 12.0 c ANSYS, Inc. January 29, 2009
18.7 Full Multigrid (FMG) Initialization
Since FMG initialization does most of the work on coarse levels, this initialization procedure is computationally inexpensive and, for large problems, a good initial solution can
be obtained in a fraction of the time spent to converge on a final solution. Note that
FMG initialization can be used with the pressure-based and density-based solvers.
When FMG initialization is started, the algorithm will perform the following steps:
1. Records the current solver selection and all current solver parameters.
2. Switches from the selected solver to the density-based explicit formulation.
3. Performs one FMG iteration using the FMG parameters given in the text command
interface (see below).
4. Switches back to the initially selected solver and resets all solver parameters back
to the original solver settings.
In the FMG iteration, the inviscid Euler equations are solved using first order-discretization
to obtain the approximate solution. If species are present, then the FMG initialization
will solve the species equations. However, turbulence equations or any other transport
scalars are not solved in the FMG initialization.
18.7.2
Limitations of FMG Initialization
• FMG initialization is not available for unsteady flows.
i
If an initial solution is needed for an unsteady calculation, then you must
first switch to the steady state solver, perform FMG initialization and other
necessary iterations to get an initial solution, and then perform unsteady
calculations.
• FMG will not initialize turbulence or other transport equations field variables.
i
If your are solving for turbulent flow, then you can still use FMG initialization, however the FMG will not initialize the turbulence field variables.
For this reason, a good initial guess of the turbulence field quantities are
important for achieving fast convergence after the FMG initialization has
been performed.
• FMG should not be used with multiphase flow.
Release 12.0 c ANSYS, Inc. January 29, 2009
18-67
Solver Theory
18-68
Release 12.0 c ANSYS, Inc. January 29, 2009
Chapter 19.
Adapting the Mesh
The solution-adaptive mesh refinement feature of ANSYS FLUENT allows you to refine
and/or coarsen your mesh based on geometric and numerical solution data. In addition,
ANSYS FLUENT provides tools for creating and viewing adaption fields customized to
particular applications. For information about using mesh adaption in ANSYS FLUENT,
see Chapter 27: Adapting the Mesh in the separate User’s Guide. Theoretical information
about the adaption process is described in detail in the following sections.
• Section 19.1: Static Adaption Process
• Section 19.2: Boundary Adaption
• Section 19.3: Gradient Adaption
• Section 19.4: Dynamic Gradient Adaption
• Section 19.5: Isovalue Adaption
• Section 19.6: Region Adaption
• Section 19.7: Volume Adaption
• Section 19.8: Yplus/Ystar Adaption
• Section 19.9: Anisotropic Adaption
• Section 19.10: Geometry-Based Adaption
• Section 19.11: Registers
Release 12.0 c ANSYS, Inc. January 29, 2009
19-1
Adapting the Mesh
19.1
Static Adaption Process
The adaption process is separated into two distinct tasks.
1. The individual cells are marked for refinement or coarsening based on the adaption
function, which is created from geometric and/or solution data.
2. The cell is refined or considered for coarsening based on these adaption marks.
The primary advantages of this modularized approach are the abilities to create
sophisticated adaption functions and to experiment with various adaption functions
without modifying the existing mesh.
i
19.1.1
Write a case and data file before starting the adaption process. If you
generate an undesirable mesh, you can restart the process with the saved
files.
Hanging Node Adaption
Hanging node adaption is the procedure used in ANSYS FLUENT. Meshes produced by
this method are characterized by nodes on edges and faces that are not vertices of all the
cells sharing those edges or faces, as shown in Figure 19.1.1.
Hanging
Node
Figure 19.1.1: Example of a Hanging Node
Hanging node mesh adaption provides the ability to operate on meshes with a variety
of cell shapes, including hybrid meshes. Although the hanging node scheme provides
significant mesh flexibility, it requires additional memory to maintain the mesh hierarchy
which is used by the rendering and mesh adaption operations.
19-2
Release 12.0 c ANSYS, Inc. January 29, 2009
19.1 Static Adaption Process
Hanging Node Refinement
The cells marked for refinement are divided as described here:
• A triangle is split into 4 triangles.
• A quadrilateral is split into 4 quadrilaterals.
• A tetrahedron is split into eight tetrahedra. The subdivision consists of trimming
each corner of the tetrahedron, and subdividing the enclosed octahedron by introducing the shortest diagonal.
• A hexahedron is split into 8 hexahedra.
• A wedge (prism) is split into 8 wedges.
• A pyramid is split into 6 pyramids and 4 tetrahedra.
Figures 19.1.2 and 19.1.3 illustrate the division of the supported cell shapes.
To maintain accuracy, neighboring cells are not allowed to differ by more than one level of
refinement. This prevents the adaption from producing excessive cell volume variations
(reducing truncation error) and ensures that the positions of the parent (original) and
child (refined) cell centroids are similar (reducing errors in the flux evaluations).
Triangle
Quadrilateral
Figure 19.1.2: Hanging Node Adaption of 2D Cell Types
Hanging Node Coarsening
The mesh is coarsened by reintroducing inactive parent cells (uniting the child cells to
reclaim the previously subdivided parent cell). An inactive parent cell is reactivated if all
its children are marked for coarsening. You will eventually reclaim the original mesh with
repeated application of the hanging node coarsening. Using the hanging node adaption
process, you cannot coarsen the mesh further than the original mesh.
Release 12.0 c ANSYS, Inc. January 29, 2009
19-3
Adapting the Mesh
Tetrahedron
Hexahedron
Prism/Wedge
Pyramid
Figure 19.1.3: Hanging Node Adaption of 3D Cell Types
19-4
Release 12.0 c ANSYS, Inc. January 29, 2009
19.2 Boundary Adaption
19.2
Boundary Adaption
If more cells are required on a boundary, they can be added using boundary adaption,
which allows you to mark or refine cells in the proximity of the selected boundary zones.
The ability to refine the mesh near one or more boundary zones is provided because
important fluid interactions often occur in these regions. Example, development of strong
velocity gradients in the boundary layer near a wall.
An example of a mesh that can be improved with boundary adaption is shown in Figure 19.2.1. This mesh has only two cells on the vertical face of a step. Boundary adaption
on the zone corresponding to the face of the step can be used to increase the number
of cells, as shown in Figure 19.2.2. This procedure cannot increase the resolution of a
curved surface. Therefore, if more cells are required on a curved surface where the shape
of the surface is important, create the mesh with sufficient surface nodes before reading
it into the solver.
19.3
Gradient Adaption
The gradient adaption function allows you to mark cells or adapt the mesh based on the
gradient, curvature, or isovalue of the selected field variables.
Information can be found in the following subsections:
• Section 19.3.1: Gradient Adaption Approach
• Section 19.3.2: Example of Steady Gradient Adaption
19.3.1
Gradient Adaption Approach
Solution-adaptive mesh refinement is performed to efficiently reduce the numerical error in the digital solution, with minimal numerical cost. Unfortunately, direct error
estimation for point-insertion adaption schemes is difficult because of the complexity of
accurately estimating and modeling the error in the adapted meshes. A comprehensive
mathematically rigorous theory for error estimation and convergence is not yet available
for CFD simulations. Assuming that maximum error occurs in high-gradient regions,
the readily available physical features of the evolving flow field may be used to drive the
mesh adaption process.
Release 12.0 c ANSYS, Inc. January 29, 2009
19-5
Adapting the Mesh
Grid
Figure 19.2.1: Mesh Before Adaption
Grid
Figure 19.2.2: Mesh after Boundary Adaption
19-6
Release 12.0 c ANSYS, Inc. January 29, 2009
19.3 Gradient Adaption
Three approaches for using this information for mesh adaption are available in ANSYS
FLUENT:
• Gradient approach: In this approach, ANSYS FLUENT multiplies the Euclidean
norm of the gradient of the selected solution variable by a characteristic length
scale [68]. For example, the gradient function in two dimensions has the following
form:
r
|ei1 | = (Acell ) 2 |∇f |
(19.3-1)
where ei1 is the error indicator, Acell is the cell area, r is the gradient volume weight,
and ∇f is the Euclidean norm of the gradient of the desired field variable, f .
The default value of the gradient volume weight is unity, which corresponds to full
volume weighting. A value of zero will eliminate the volume weighting, and values
between 0 and 1 will use proportional weighting of the volume.
If you specify adaption based on the gradient of a scalar, then the value of |ei1 | is
displayed when you plot contours of the adaption function.
This approach is recommended for problems with strong shocks, e.g., supersonic
inviscid flows.
• Curvature approach: This is the equidistribution adaption technique formerly
used by ANSYS FLUENT, that multiplies the undivided Laplacian of the selected
solution variable by a characteristic length scale [368].
For example, the gradient function in two dimensions has the following form:
r
|ei2 | = (Acell ) 2 |∇2 f |
(19.3-2)
where ei2 is the error indicator, Acell is the cell area, r is the gradient volume weight,
and ∇2 f is the undivided Laplacian of the desired field variable (f ).
The default value of the gradient volume weight is unity, which corresponds to full
volume weighting. A value of zero will eliminate the volume weighting, and values
between 0 and 1 will use proportional weighting of the volume.
This approach is recommended for problems with smooth solutions.
Release 12.0 c ANSYS, Inc. January 29, 2009
19-7
Adapting the Mesh
• Isovalue approach: This approach is not based on derivatives. Instead, the isovalues of the required field variable f , are used to control the adaption. Therefore,
the function is of the form:
ei3 = f
(19.3-3)
where ei3 is the error indicator. This approach is recommended for problems where
derivatives are not helpful. For example, if you want to refine the mesh where the
reaction is taking place, you can use the isovalues of the reaction rate and mark
for refinement at high reaction rates. This approach also allows you to customize
the criteria for controlling the adaption using custom field functions, user-defined
scalars, etc.
The length scale is the square (2D) or cube (3D) root of the cell volume. Introducing
the length scale allows resolution of both strong and weak disturbances, increasing the
potential for more accurate solutions. However, you can reduce or eliminate the volume
weighting by changing the gradient Volume Weight in the Mesh Adaption Controls
dialog box (see Section 27.12: Mesh Adaption Controls in the separate User’s Guide for
details).
Any of the field variables available for contouring can be used in the gradient adaption
function. These scalar functions include, both geometric and physical features of the
numerical solution. Therefore, in addition to traditional adaption to physical features,
such as the velocity, you may choose to adapt to the cell volume field to reduce rapid
variations in cell volume.
In addition to the Standard (no normalization) approach formerly used by ANSYS FLUENT, two options are available for Normalization [107]:
• Scale, which scales the values of ei1 , ei2 , or ei3 by their average value in the domain,
i.e.:
|ei |
|ei |
(19.3-4)
when using the Scale option, suitable first-cut values for the Coarsen Threshold and
the Refine Threshold are 0.3 to 0.5, and 0.7 to 0.9, respectively. Smaller values will
result in larger adapted regions.
• Normalize, which scales the values of ei1 , ei2 , or ei3 by their maximum value in the
domain, therefore always returning a problem-independent range of [0, 1] for any
variable used for adaption, i.e.:
|ei |
max |ei |
19-8
(19.3-5)
Release 12.0 c ANSYS, Inc. January 29, 2009
19.4 Dynamic Gradient Adaption
when using the Normalize option, suitable first-cut values for the Coarsen Threshold
and the Refine Threshold are 0.2 to 0.4, and 0.5 to 0.9, respectively. Smaller values
will result in larger adapted regions.
19.3.2
Example of Steady Gradient Adaption
An example of the use of steady gradient adaption is the solution of the supersonic flow
over a circular cylinder. The initial mesh, shown in Figure 19.3.1, is very coarse, even
though it contains sufficient cells to adequately describe the shape of the cylinder. The
mesh ahead of the cylinder is too coarse to resolve the shock wave that forms in front
of the cylinder. In this instance, pressure is a suitable variable to be used in gradient
adaption. This is because there will be a jump in pressure across the shock. However,
several adaptions are necessary before the shock can be properly resolved. After several
adaptions the mesh will be as shown in Figure 19.3.2.
A typical application of gradient adaption for an incompressible flow might be a mixing
layer, which involves a discontinuity.
19.4
Dynamic Gradient Adaption
In contrast with the static gradient adaption (Section 19.3: Gradient Adaption) dynamic
gradient adaption is a fully automated process. For time dependent and for steady state
problems, you can perform the entire solution without changing the initial settings. That
is, you can let the solver periodically perform adaptions without changing/entering any
parameter.
19.5
Isovalue Adaption
Some flows may contain flow features that are easy to identify based on values of a certain
quantity. For instance, wakes represent a total pressure deficit, and jets are identifiable
by a region of relatively high-velocity fluid. Since it is known that these regions also
contain large gradients of important flow quantities (such as k and in turbulent flows),
it is convenient to perform an isovalue adaption on the relevant flow quantity than to
refine on gradients of the individual flow variables.
The isovalue adaption function allows you to mark or refine cells inside or outside a
specified range of a selected field variable function. The mesh can be refined or marked
for refinement based on geometric and/or solution vector data. Specifically, any quantity
in the display list of field variables can be used for the isovalue adaption. Some examples
of how you might use the isovalue marking/adaption feature include the following:
Release 12.0 c ANSYS, Inc. January 29, 2009
19-9
Adapting the Mesh
Grid
Figure 19.3.1: Bluff-Body Mesh Before Adaption
Grid
Figure 19.3.2: Bluff-Body Mesh after Gradient Adaption
19-10
Release 12.0 c ANSYS, Inc. January 29, 2009
19.6 Region Adaption
• Create masks using coordinate values or the quadric function.
• Refine cells that have a velocity magnitude within a specified range.
• Mark and display cells with a pressure or continuity residual outside of a desired
range to determine where the numerical solution is changing rapidly.
The approach used in isovalue adaption function is to compute the specified value for
each cell (velocity, quadric function, centroid x coordinate, etc.), and then visit each cell,
marking for refinement the cells that have values inside (or outside) the specified ranges.
An example of a problem in which isovalue adaption is useful is shown in Figure 19.5.1.
The mesh for an impinging jet is displayed along with contours of x velocity. An isovalue
adaption based on x velocity allows refinement of the mesh only in the jet (Figure 19.5.2).
Note: When adapting to isovalues take care to prevent large gradients in cell volume.
This can affect accuracy and impede convergence (Section 27.1: Using Adaption
in the separate User’s Guide). To rectify large gradients in cell volume, adapt to
cell-volume change, as demonstrated in Section 19.7.2: Volume Adaption Example.
19.6
Region Adaption
Many mesh generators create meshes with cell volumes that grow very rapidly with
distance from boundaries. While this avoids a dense mesh as a matter of course, it might
also create problems if the mesh is not fine enough to resolve the flow. But if it is known
a priori that a finer mesh is required in a certain region of the solution domain, the mesh
can be refined using region adaption.
The region adaption function marks or refines cells inside or outside a region defined
by text or mouse input. Presently, the mesh can be refined or marked inside or outside
a hexahedron (quadrilateral in 2D), a sphere (circle in 2D), or a cylinder. The regionbased marking/adaption feature is particularly useful for refining regions that intuitively
require good resolution: e.g., the wake region of a blunt-body flow field. In addition, you
can use the region marking to create mask adaption registers that can be used to limit
the extent of the refinement and coarsening.
Information can be found in the following subsections:
• Section 19.6.1: Defining a Region
• Section 19.6.2: Region Adaption Example
Release 12.0 c ANSYS, Inc. January 29, 2009
19-11
Adapting the Mesh
1.00e+00
9.00e-01
8.00e-01
7.00e-01
6.00e-01
5.00e-01
4.00e-01
3.00e-01
2.00e-01
1.00e-01
Contours of X-Velocity (m/s)
Figure 19.5.1: Impinging Jet Mesh Before Adaption
Grid
Figure 19.5.2: Impinging Jet Mesh after Isovalue Adaption
19-12
Release 12.0 c ANSYS, Inc. January 29, 2009
19.6 Region Adaption
19.6.1
Defining a Region
The basic approach to the region adaption function is to first define a region:
• The hexahedron (quadrilateral) is defined by entering the coordinates of two points
defining the diagonal.
• The sphere (circle) is defined by entering the coordinates of the center of the sphere
and its radius.
• To define a cylinder, specify the coordinates of the points defining the cylinder axis,
and the radius. In 3D this will define a cylinder. In 2D, you will have an arbitrarily
oriented rectangle with length equal to the cylinder axis length and width equal to
the radius.
A rectangle defined using the cylinder option differs from one defined with the
quadrilateral option in that the former can be arbitrarily oriented in the domain
while the latter must be aligned with the coordinate axes.
You can either enter the exact coordinates into the appropriate real entry fields
or select the locations with the mouse on displays of the mesh or solution field.
After the region is defined, each cell that has a centroid inside/outside the specified
region is marked for refinement.
19.6.2
Region Adaption Example
Figure 19.6.1 shows a mesh that was created for solving the flow around a flap airfoil.
The mesh is very fine near the surface of the airfoil so that the viscous-affected region
may be resolved. However, the mesh grows very rapidly away from the airfoil, because
of which the flow separation known to occur on the suction surface of the flap will not be
properly predicted. To avoid this problem, the mesh is adapted within circular regions
(selected by mouse probe) surrounding the flap. The result is shown in Figure 19.6.2.
When the region adaption is performed, the minimum cell volume for adaption is limited
(as described in Section 27.12: Mesh Adaption Controls in the separate User’s Guide) to
prevent the very small cells near the surface from being refined further.
Release 12.0 c ANSYS, Inc. January 29, 2009
19-13
Adapting the Mesh
Grid
Figure 19.6.1: Flap-Airfoil Mesh Before Adaption
Grid
Figure 19.6.2: Flap-Airfoil Mesh after Region Adaption
19-14
Release 12.0 c ANSYS, Inc. January 29, 2009
19.7 Volume Adaption
19.7
Volume Adaption
As mentioned in Section 27.1: Using Adaption in the separate User’s Guide, it is best for
both accuracy and convergence to have a mesh in which the changes in cell volume are
gradual. If the mesh creation or adaption process results in a mesh that does not have
this property, the mesh can be improved by using volume adaption with the option of
refining, based on either the cell volume or the change in volume between the cell and
its neighbors.
Information can be found in the following subsections:
• Section 19.7.1: Volume Adaption Approach
• Section 19.7.2: Volume Adaption Example
19.7.1
Volume Adaption Approach
Marking or refining the mesh based on volume magnitude is often used to remove large
cells or to globally refine the mesh. The procedure is to mark for refinement any cell
with a volume greater than the specified threshold value.
Marking or refining the mesh based on the change in cell volume is used to improve
the smoothness of the mesh. The procedure is to mark for refinement any cell that
has a volume change greater than the specified threshold value. The volume change is
computed by looping over the faces and comparing the ratio of the cell neighbors to the
face.
For example, in Figure 19.7.1 the ratio of V1/V2 and the ratio of V2/V1 is compared
to the threshold value. If V2/V1 is greater than the threshold, then C2 is marked for
refinement.
Figure 19.7.1: Volume Change—Ratio of the Volumes of the Cells
Release 12.0 c ANSYS, Inc. January 29, 2009
19-15
Adapting the Mesh
19.7.2
Volume Adaption Example
The mesh in Figure 19.7.2 was created for computing a turbulent jet. Local refinement
was used in TGrid to create a mesh that is fine in the region of the jet, but coarse
elsewhere. This created a very sharp change in cell volume at the edge of the jet.
To improve the mesh, it was refined using volume adaption with the criterion that the
maximum cell volume change should be less than 50%. The minimum cell volume for
adaption was also limited. The resulting mesh, after smoothing and swapping, is shown
in Figure 19.7.3. It can be seen that the interface between the refined region within the
jet and the surrounding mesh is no longer as sharp.
19.8
Yplus/Ystar Adaption
ANSYS FLUENT provides three different options for near-wall modeling of turbulence,
standard wall functions, nonequilibrium wall functions, and the enhanced wall treatment.
As described in Section 12.3: Mesh Considerations for Turbulent Flow Simulations in the
separate User’s Guide, there are certain mesh requirements for each of these near-wall
modeling options.
It is often difficult to gauge the near-wall resolution requirements when creating the mesh.
Hence, Yplus and Ystar adaption have been provided to appropriately refine or coarsen
the mesh along the wall during the solution process.
19.8.1
Yplus/Ystar Adaption Approach
The approach is to compute y + or y ∗ for boundary cells on the specified viscous wall
zones, define the minimum and maximum allowable y + or y ∗ , and mark and/or adapt
the appropriate cells. Cells with y + or y ∗ values below the minimum allowable threshold
will be marked for coarsening and cells with y + or y ∗ values above the maximum allowable threshold will be marked for refinement (unless coarsening or refinement has been
disabled).
Figure 19.8.1 shows the mesh for a duct flow, where the top boundary is the wall and
the bottom boundary is the symmetry plane. After an initial solution, it was determined
that y + values of the cells on the wall boundary were too large, and y + adaption was
used to refine them. The resulting mesh is shown in Figure 19.8.2. This figure shows that
the height of the cells along the wall boundary has been reduced during the refinement
process. However, the cell-size distribution on the wall after refinement is much less
uniform than in the original mesh, which is an adverse effect of y + adaption.
See Section 12.3: Mesh Considerations for Turbulent Flow Simulations in the separate
User’s Guide for guidelines on recommended values of y + or y ∗ for different near-wall
treatments.
19-16
Release 12.0 c ANSYS, Inc. January 29, 2009
19.8 Yplus/Ystar Adaption
Grid
Figure 19.7.2: Jet Mesh Before Adaption
Grid
Figure 19.7.3: Jet Mesh after Volume Adaption Based on Change in Cell
Volume
Release 12.0 c ANSYS, Inc. January 29, 2009
19-17
Adapting the Mesh
Grid
Figure 19.8.1: Duct Flow Mesh Before Adaption
Grid
Figure 19.8.2: Duct Flow Mesh after y + Adaption
19-18
Release 12.0 c ANSYS, Inc. January 29, 2009
19.9 Anisotropic Adaption
19.9
Anisotropic Adaption
The purpose of anisotropic adaption is to refine hexahedral or prism layer cells in 3D
meshes. Anisotropic adaption is considered to be more of a mesh manipulation tool
rather than an adaption feature, allowing you to refine some hexahedral or prism cells
that are adjacent to one or a few boundary face zones using the GUI. The hexahedral or
prism cells are split in one direction each time, giving you control of the different splitting
ratios, thus achieving anisotropic refinement.
i
Note that anisotropic adaption is different from other mesh adaption features because it only refines the mesh and cannot be coarsened after refinement.
For information on how to use anisotropic adaption, see Section 27.9: Anisotropic Adaption
in the separate User’s Guide
19.10 Geometry-Based Adaption
The purpose of adaption is to produce a mesh that is fine enough and adequately represents all important features of the geometry. However, when you have a coarse mesh
of a geometry that has curved profiles and sharp corners, the adapted mesh may not
recover the curved profiles and corners at the perimeter of the geometry. In such cases,
use geometry-based adaption to reconstruct the geometry (or to recover the finer details
of the geometry at its extends) along with performing the adaption process.
19.10.1
Geometry-Based Adaption Approach
Geometry-based adaption works on the principle of geometry reconstruction. In this
approach, the cell count of the mesh is increased by creating the new nodes in the domain
in between the existing nodes of the mesh. The newly created nodes are projected in such
a way that the resulting mesh is finer and it’s shape is closer to the original geometry.
The following sections explain how nodes are projected and the parameters that control
the node propagation.
Node Projection
Consider a coarse mesh created for a circular geometry. A section of the mesh close to
the circular edge is shown in Figure 19.10.1. The edge is not smooth and has sharp
corners, because of which its shape is not closer to that of the original geometry. Using
boundary adaption along with the geometry reconstruction option will result in a mesh
with smoother edges as shown in Figure 19.10.2.
Release 12.0 c ANSYS, Inc. January 29, 2009
19-19
Adapting the Mesh
In Figure 19.10.2, the dotted lines represent the original edge of the mesh. The boundary
adaption process creates new nodes in between the original nodes. These nodes are
projected towards the edge of the geometry, because of which the resulting mesh has
smooth edges and its shape is closer to the original geometry.
i
Only the nodes created in the adaption process (newly created nodes) are
projected and the original nodes retain their positions.
The following parameters control node projection and are specified in Geometry Based
Adaption dialog box.
• Levels of Projection Propagation: This parameter allows you to specify the number
of node layers across which node propagation should take place for geometry reconstruction. A value of 1 means only the nodes at the boundary will be projected, a
value of 2 means the nodes at the boundary and the nodes in the next layer will
be projected, and so on.
Note: The nodes in the first level are projected by a maximum magnitude and the
node in the last level are projected by a minimum magnitude. The magnitude
of projection decreases gradually from the first level to the last level.
For example, a value of 3 for Levels of Projection Propagation means, the level
1 node is projected by maximum magnitude and level 3 node is projected by
minimum magnitude. Figure 19.10.3 illustrates the level of propagation and
magnitude of projection of newly created nodes.
• Direction of Projection: This parameter allows you to specify the direction, X, Y,
or Z (for 3D), for node projection. If you do not specify any direction, the node
projection takes place at the nearest point of the newly created node.
• Background Mesh: This option allows you to use a fine surface mesh as a background mesh, based on which the geometry is reconstructed. When you read the
surface mesh, the node projection will take place based on the node positions of
the background mesh.
This option is useful when the mesh you want to adapt is very coarse and geometry is
highly curved. In such cases, node projection, only by specifying the parameters may
not result in a good quality mesh. However, you can also modify the propagation
criteria by specifying the parameters.
i
19-20
You can read only one surface mesh at a time. The various zones of the
surface mesh will be listed in the Background Mesh drop-down list.
Release 12.0 c ANSYS, Inc. January 29, 2009
19.10 Geometry-Based Adaption
Figure 19.10.1: Mesh Before Adaption
Figure 19.10.2: Projection of Nodes
Release 12.0 c ANSYS, Inc. January 29, 2009
19-21
Adapting the Mesh
Figure 19.10.3: Levels Projection Propagation and Magnitude
Example of Geometry-Based Adaption
Consider a mesh created for a spherical geometry. The initial mesh is very coarse, because
of which it has sharp corners (as in Figure 19.10.4). It does not represent the spherical
geometry accurately. To recover the original spherical geometry from this coarse mesh
use geometry-based adaption.
If you adapt boundaries of the domain without activating the Reconstruct Geometry option, the resulting mesh (see Figure 19.10.5) has sufficient number of cells, but the boundary of the domain still contains sharp corners.
Boundary adaption only creates new nodes in between the existing nodes to increase the
cell count of the mesh. Since it does not project the nodes, the shape of the mesh remains
as it is.
If you adapt the boundary with Reconstruct Geometry option. The resulting mesh (Figure 19.10.6) has more number of cells and less sharp corners at boundary. In addition,
the newly created nodes are projected in a direction such that it’s shape is closer to the
original geometry (i.e., sphere with smooth boundary).
19-22
Release 12.0 c ANSYS, Inc. January 29, 2009
19.10 Geometry-Based Adaption
Figure 19.10.4: Coarse Mesh of a Sphere
Release 12.0 c ANSYS, Inc. January 29, 2009
19-23
Adapting the Mesh
19.11 Registers
A register is the group of cells that are marked for refinement/coarsening but not adapted.
There are two types of registers:
• Adaption Register
• Mask Register
Adaption Register
An adaption register is basically a list of identifiers for each cell in the domain. The
identifiers designate whether a cell is neutral (not marked), marked for refinement, or
marked for coarsening. Invoking the Mark command creates an adaption register. It is
called a register because it is used in a manner similar to the way memory registers are
used in calculators. For example, one adaption register holds the result of an operation,
another register holds the results of a second operation, and these registers can be used
to produce a third register.
The adaption function is used to set the appropriate identifier. For example, to refine the
cells based on pressure gradient, the solver computes the gradient adaption function for
each cell. The cell value is compared with the refining and coarsening threshold values
and assigned the appropriate identifier.
• If the cell value < coarsen threshold value, the cell is marked for coarsening.
• If the coarsen threshold value < cell value < refine threshold value, the cell is
neutral (not marked).
• If the cell value > refine threshold value, the cell is marked for refinement.
Adaption registers can be created using geometric data, physical features of the flow field,
and combinations of these information. After they are created, the adaption registers
can be listed, displayed, deleted, combined, exchanged, inverted, and changed to mask
registers.
19-24
Release 12.0 c ANSYS, Inc. January 29, 2009
19.11 Registers
Figure 19.10.5: Adapted Mesh Without Geometry Reconstruction
Figure 19.10.6: Mesh after Geometry-Based Adaption
Release 12.0 c ANSYS, Inc. January 29, 2009
19-25
Adapting the Mesh
Hybrid Adaption Functions
The hybrid adaption functions are created to confine the adaption to a specific region
(using masks) and/or create a more accurate error indicator. ANSYS FLUENT provides
a few basic tools to aid in creating hybrid adaption functions.
1. Create the initial adaption registers using geometric and/or solution vector information.
2. Manipulate these registers and their associated refinement and coarsening marks.
• Manipulate the registers by changing the type and/or combining them to
create the desired hybrid function.
• Manipulate the marks by using Exchange, Invert, Limit, and Fill operations.
3. Delete, display adapt to the hybrid adaption functions.
For example, you can capture the shock wave generated on a wedge in a supersonic flow
field by adapting the mesh to the gradients of pressure. The pressure gradient near the
surface of the wedge, however, is relatively small. You can therefore use the velocity field
to resolve the equally important boundary layer near the surface of the wedge.
• If you adapt to pressure, regions near the surface might be coarsened.
• If you subsequently adapted to velocity, these regions may be refined, but the net
result will not gain in resolution.
• If you combine the velocity and pressure gradient adaption functions, the new
adaption function will allow increased resolution in both regions.
The relative weight of the two functions in the hybrid function is determined by the
values of the refinement and coarsening thresholds you specify for each of the flow field
variables.
To refine the shock and boundary layer only near the leading edge of the wedge, create
a circle at the leading edge of the wedge using the region adaption function, change this
new register to a mask, and combine it with the hybrid gradient function.
The GUI and text interface commands generate adaption registers that designate the cells
marked for refinement or coarsening. These registers can be converted to mask registers.
19-26
Release 12.0 c ANSYS, Inc. January 29, 2009
19.11 Registers
Mask Register
Mark registers maintain only two states: ACTIVE and INACTIVE. If the adaption
register is converted to a mask, cells marked for refinement become ACTIVE cells, while
those that are unmarked or marked for coarsening become INACTIVE.
You can use a mask register to limit adaption to cells within a certain region.
This process is illustrated in Figures 19.11.1, 19.11.2, and 19.11.3.
Figure 19.11.1 shows a cloud of cells representing an adaption register (shaded cells are
marked cells). Figure 19.11.2 illustrates the active cells associated with a mask register.
If the mask is applied to (combined with) the adaption register, the new adaption register
formed from the combination has the marked cells shown in Figure 19.11.3.
Figure 19.11.1: Adaption Register with Marked Cells
Figure 19.11.2: Mask Register with Active Cells
Release 12.0 c ANSYS, Inc. January 29, 2009
19-27
Adapting the Mesh
Figure 19.11.3: New Adaption Register Created from Application of Mask
This example does not differentiate between refinement or coarsening marks because the
mask is applied to both types of marks. For more information on combining registers,
see Section 27.11.1: Manipulating Adaption Registers in the separate User’s Guide.
19-28
Release 12.0 c ANSYS, Inc. January 29, 2009
Chapter 20.
Reporting Alphanumeric Data
ANSYS FLUENT provides tools for computing and reporting integral quantities at surfaces
and boundaries. These tools enable you to find the mass flow rate and heat transfer rate
through boundaries, the forces and moments on boundaries, and the area, integral, flow
rate, average, and mass average (among other quantities) on a surface or in a volume. In
addition, you can print histograms of geometric and solution data, set reference values
for the calculation of nondimensional coefficients, and compute projected surface areas.
You can also print or save a summary report of the models, boundary conditions, and
solver settings in the current case.
This chapter describes some of the background behind ANSYS FLUENT’s reporting features. These features are described in the following sections.
• Section 20.1: Fluxes Through Boundaries
• Section 20.2: Forces on Boundaries
• Section 20.3: Surface Integration
• Section 20.4: Volume Integration
Additional information about using these reporting tools can be found in Chapter 30: Reporting Alphanumeric Data in the separate User’s Guide. Reporting tools for the discrete
phase are described in Section 23.7: Postprocessing for the Discrete Phase in the separate
User’s Guide.
Release 12.0 c ANSYS, Inc. January 29, 2009
20-1
Reporting Alphanumeric Data
20.1
Fluxes Through Boundaries
This section describes the quantities that you can compute for boundaries. For more
information about generating flux reports, see Section 30.3.1: Generating a Flux Report
in the separate User’s Guide.
For selected boundary zones, you can compute the following quantities:
• The mass flow rate through a boundary is computed by summing the dot product
of the density times the velocity vector and the area projections over the faces of
the zone.
• The total heat transfer rate through a boundary is computed by summing the total
heat transfer rate, q = qc +qr , over the faces, where qc is the convective heat transfer
rate and qr is the radiation heat transfer rate. The computation of the heat transfer
through the face depends on the specified boundary condition. For example, the
conduction heat transfer on a constant-temperature wall face would be the product
of the thermal conductivity with the dot product of the area projection and the
temperature gradient. For flow boundaries, the total heat transfer rate is the flow
rate of the conserved quantity. Depending on the models that are being used, the
total heat transfer rate may include the convective flow of sensible or total enthalpy,
diffusive flux of energy, etc. Note that the reference temperature in all enthalpy
calculations is always 298.15K
• The radiation heat transfer rate through a boundary is computed by summing the
radiation heat transfer rate qr over the faces. The computation of the radiation
heat transfer depends on the radiation model used.
For example, you might use flux reporting to compute the resulting mass flow through a
duct with pressure boundaries specified at the inlet and exit.
20.2
Forces on Boundaries
For selected wall zones, you can compute and report the forces along a specified vector,
the moments about a specified center and along a specified axis, and the coordinates of
the center of pressure. This feature is useful for reporting, for instance, aerodynamic
quantities such as lift, drag, and moment coefficients, as well as the center of pressure
for an airfoil.
For information about how ANSYS FLUENT computes forces, moments, and centers of
pressure, see Section 20.2.1: Computing Forces, Moments, and the Center of Pressure.
Otherwise, for more information about generating a report on forces, moments, or centers
of pressure, see Section 30.4.1: Generating a Force, Moment, or Center of Pressure Report
in the separate User’s Guide.
20-2
Release 12.0 c ANSYS, Inc. January 29, 2009
20.2 Forces on Boundaries
20.2.1
Computing Forces, Moments, and the Center of Pressure
The total force component along the specified force vector ~a on a wall zone is computed
by summing the dot product of the pressure and viscous forces on each face with the
specified force vector. The terms in this summation represent the pressure and viscous
force components in the direction of the vector ~a:
F
~a · F~p
=
a
|{z}
total f orce component
~a · F~v
+
(20.2-1)
| {z }
| {z }
pressure f orce component
viscous f orce component
where
~a
F~p
F~v
=
=
=
specified force vector
pressure force vector
viscous force vector
In addition to the actual pressure, viscous, and total forces, the associated force coefficients are also computed for each of the selected wall zones, using the reference values
(as described in Section 30.11: Reference Values in the separate User’s Guide). The force
coefficient is defined as force divided by 12 ρv 2 A, where ρ, v, and A are the density, velocity, and area. Finally, the net values of the pressure, viscous, and total forces and
coefficients for all of the selected wall zones are also computed.
The total moment vector about a specified center A is computed by summing the cross
products of the pressure and viscous force vectors for each face with the moment vector
~rAB , which is the vector from the specified moment center A to the force origin B (see
Figure 20.2.1). The terms in this summation represent the pressure and viscous moment
vectors:
~A
M
|{z}
total moment
=
~rAB × F~p
|
{z
}
pressure moment
+
~rAB × F~v
|
{z
(20.2-2)
}
viscous moment
where
A
B
~rAB
F~p
F~v
= specified moment center
= force origin
= moment vector
= pressure force vector
= viscous force vector
Direction of the total moment vector follows the right hand rule for cross products.
Release 12.0 c ANSYS, Inc. January 29, 2009
20-3
Reporting Alphanumeric Data
Line of action of F
Moment center
A
rAB
F = Fp + Fv
B
z
Force origin
MA= rΑΒ
O
F
y
x
Figure 20.2.1: Moment About a Specified Moment Center
20-4
Release 12.0 c ANSYS, Inc. January 29, 2009
20.2 Forces on Boundaries
Along with the actual components of the pressure, viscous, and total moments, the
moment coefficients are computed for each of the selected wall zones, using the reference
values (as described in Section 30.11: Reference Values in the separate User’s Guide).
The moment coefficient is defined as the moment divided by 12 ρv 2 AL, where ρ, v, A, and
L are the density, velocity, area, and length. The coefficient values for the individual
wall zones are also summed to yield the net values of the pressure, viscous, and total
moments and coefficients for all of the selected wall zones.
Furthermore, the moments along a specified axis are computed. These moments, also
known as torques, are defined as the dot product of a unit vector in the direction of
the specified axis and the individual and net values of the pressure, viscous, and total
moments and coefficients.
To reduce round-off error, a reference pressure is used to normalize the cell pressure for
computation of the pressure force. For example, the net pressure force vector, acting on
a wall zone, is computed as the vector sum of the individual force vectors for each cell
face:
F~p =
=
n
X
i=1
n
X
(p − pref )An̂
pAn̂ − pref
i=1
n
X
(20.2-3)
An̂
(20.2-4)
i=1
where n is the number of faces, A is the area of the face, and n̂ is the unit normal to the
face.
The center of pressure is the average location of the pressure. The pressure varies around
the surface of an object, such that P = p(x). The general expression for determining the
center of pressure is
R
cp = R
xp(x)dx
p(x)dx
(20.2-5)
However, the center of pressure of a wall is also defined as the point about which the
moment on the wall(s) will be zero, that is, the point on the wall where all of the forces
balance. It is computed as follows:
~ = ~r × F~
M
~ = 0
M
(20.2-6)
(20.2-7)
where F~ is the force acting on the selected wall and ~r is the position vector from the
center of pressure to the point where the force is applied.
Release 12.0 c ANSYS, Inc. January 29, 2009
20-5
Reporting Alphanumeric Data
20.3
Surface Integration
You can compute the area or mass flow rate, or the integral, standard deviation, flow
rate, volume flow rate, area-weighted average, flow rate, mass-weighted average, sum,
facet average, facet maximum, facet minimum, vertex average, vertex minimum, and
vertex maximum for a selected field variable on selected surfaces in the domain. These
surfaces are sets of data points created by ANSYS FLUENT for each of the zones in your
model, or defined by you using the methods described in Chapter 28: Creating Surfaces
for Displaying and Reporting Data in the separate User’s Guide, or by using the Text
User Interface, described in Chapter 3: Text User Interface (TUI) in the separate User’s
Guide.
The following list provides information on the data reported for the various surface
integrals:
• For the vertex average, vertex maximum, and the vertex minimum, ANSYS FLUENT
reports the node values of the selected variable on the selected surface.
• For mass flow rate, volume flow rate, and flow rate, ANSYS FLUENT reports the
rate. Of these, flow rate is the only one associated with a selected variable. The
values used in the computation depend on the kind of surface selected:
– The face flux values are used for face zone surfaces.
– The cell values are used for postprocessing surfaces.
• For all other surface integrals, ANSYS FLUENT reports the integral, using values
that are appropriate for the particular surface:
– For face zone surfaces, the face values are used when they are available, that
is, when they are calculated by the solver or specified as a boundary condition.
Otherwise, the cell values are used. The cell value for noninternal faces (i.e.,
faces that only have c0 and no c1) is the c0 value. The cell value for internal
faces (i.e., faces that have c0 and c1) is the average of the c0 and c1 values.
– For postprocessing surfaces, the cell values are used. See Section 31.1.1: Cell
Values in the separate User’s Guide for further details.
Example uses of several types of surface integral reports are given below:
• Area: You can compute the area of a velocity inlet zone, and then estimate the
velocity from the mass flow rate:
v=
20-6
ṁ
ρA
(20.3-1)
Release 12.0 c ANSYS, Inc. January 29, 2009
20.3 Surface Integration
• Area-weighted average: You can find the average value on a solid surface, such as
the average heat flux on a heated wall with a specified temperature.
• Mass average: You can find the average value on a surface in the flow, such as
average enthalpy at a velocity inlet.
• Mass flow rate: You can compute the mass flow rate through a velocity inlet zone,
and then estimate the velocity from the area, as described above.
• Flow rate: To calculate the heat transfer rate through a surface, you can calculate
the flow rate of enthalpy.
• Integral: You can use integrals for more complex calculations, which may involve
the use of the Custom Field Function Calculator dialog box, described in
Section 31.5: Custom Field Functions in the separate User’s Guide, to calculate a
function that requires integral computations (e.g., swirl number).
• Standard deviation: You can find the standard deviation of a specified field variable
on a surface, such as enthalpy, viscosity, and velocity.
• Volume flow rate: This will report the volume flow rate through the specified
surface.
For information about how ANSYS FLUENT computes surface integrals, see Section 20.3.1: Computing Surface Integrals. Otherwise, for more information about generating a surface
integral report, see Section 30.6.1: Generating a Surface Integral Report in the separate
User’s Guide.
20.3.1
Computing Surface Integrals
Area
The area of a surface is computed by summing the areas of the facets that define the
surface. Facets on a surface are either triangular or quadrilateral in shape.
Z
dA =
n
X
|Ai |
(20.3-2)
i=1
Integral
An integral on a surface is computed by summing the product of the facet area and
the selected field variable facet value, such as density or pressure. For details on the
computation of the facet values, see Section 20.3: Surface Integration.
Release 12.0 c ANSYS, Inc. January 29, 2009
20-7
Reporting Alphanumeric Data
Area-Weighted Average
The area-weighted average of a quantity is computed by dividing the summation of the
product of the selected field variable and facet area by the total area of the surface:
n
1Z
1X
φdA =
φi |Ai |
A
A i=1
(20.3-3)
Flow Rate
The flow rate of a quantity through a surface is computed by summing the value of the
selected field variable multiplied by the density and the dot product of the facet area
vector and the facet velocity vector.
Z
~=
φρ~v · dA
n
X
~i
φi ρi v~i · A
(20.3-4)
i=1
Mass Flow Rate
The mass flow rate through a surface is computed by summing the value of the selected
field variable multiplied by the density and the dot product of the facet area vector and
the facet velocity vector.
Z
n
X
~
~i
ρ~v · dA =
ρi v~i · A
(20.3-5)
i=1
Mass-Weighted Average
The mass-weighted average of a quantity is computed by dividing the summation of the
value of the selected field variable multiplied by the absolute value of the dot product of
the facet area and momentum vectors by the summation of the absolute value of the dot
product of the facet area and momentum vectors (surface mass flux):
Z
Z
n
X
~
φρ ~v · dA
~
ρ ~v · dA
=
~i
φi ρi v~i · A
i=1
n
X
(20.3-6)
~i
ρi v~i · A
i=1
20-8
Release 12.0 c ANSYS, Inc. January 29, 2009
20.3 Surface Integration
Sum of Field Variable
The sum of a specified field variable on a surface is computed by summing the value of
the selected variable at each facet:
n
X
φi
(20.3-7)
i=1
Facet Average
The facet average of a specified field variable on a surface is computed by dividing the
summation of the facet values of the selected variable by the total number of facets. See
Section 31.1: Node, Cell, and Facet Values in the separate User’s Guide for definitions of
facet values.
n
X
φi
i=1
n
(20.3-8)
Facet Minimum
The facet minimum of a specified field variable on a surface is the minimum facet value
of the selected variable on the surface. See Section 31.1: Node, Cell, and Facet Values in
the separate User’s Guide for definitions of facet values.
Facet Maximum
The facet maximum of a specified field variable on a surface is the maximum facet value
of the selected variable on the surface. See Section 31.1: Node, Cell, and Facet Values in
the separate User’s Guide for definitions of facet values.
Vertex Average
The vertex average of a specified field variable on a surface is computed by dividing the
summation of the vertex values of the selected variable by the total number of vertices.
See Section 31.1: Node, Cell, and Facet Values in the separate User’s Guide for definitions
of vertex values.
n
X
φi
i=1
n
Release 12.0 c ANSYS, Inc. January 29, 2009
(20.3-9)
20-9
Reporting Alphanumeric Data
Vertex Minimum
The vertex minimum of a specified field variable on a surface is the minimum vertex value
of the selected variable on the surface. See Section 31.1: Node, Cell, and Facet Values in
the separate User’s Guide for definitions of vertex values.
Vertex Maximum
The vertex maximum of a specified field variable on a surface is the maximum vertex
value of the selected variable on the surface. See Section 31.1: Node, Cell, and Facet
Values in the separate User’s Guide for definitions of vertex values.
Standard-Deviation
The standard deviation of a specified field variable on a surface is computed using the
mathematical expression below:
v
uX
u n
u
(x − x0 )2
u
t i=1
n
(20.3-10)
where x is the cell value of the selected variables at each facet, x0 is the mean of x
n
X
x0 =
x
i=1
n
and n is the total number of facets. See Section 31.1: Node, Cell, and Facet Values in
the separate User’s Guide for definitions of facet values.
Volume Flow Rate
The volume flow rate through a surface is computed by summing the value of the facet
area vector multiplied by the facet velocity vector:
Z
~=
~v · dA
n
X
~i
v~i · A
(20.3-11)
i=1
20-10
Release 12.0 c ANSYS, Inc. January 29, 2009
20.4 Volume Integration
20.4
Volume Integration
The volume, sum, maximum, minimum, volume integral, volume-weighted average, mass
integral, and mass-weighted average can be obtained for a selected field variable in selected cell zones in the domain.
Example uses of the different types of volume integral reports are given below:
• Volume: You can compute the total volume of a fluid region.
• Sum: You can add up the discrete-phase mass or energy sources to determine the
net transfer from the discrete phase. You can also sum user-defined sources of mass
or energy.
• Maximum: The maximum value of the selected variable at each cell in the selected
zone.
• Minimum: The minimum value of the selected variable at each cell in the selected
zone.
• Volume Integral: For quantities that are stored per unit volume, you can use volume
integrals to determine the net value (e.g., integrate density to determine mass).
• Volume-Average: You can obtain volume averages of mass sources, energy sources,
or discrete-phase exchange quantities.
• Mass Integral: You can determine the total mass of a particular species by integrating its mass fraction.
• Mass-Average: You can find the average value (such as average temperature) in a
fluid zone.
For information about how ANSYS FLUENT computes volume integrals, see Section 20.4.1: Computing Volume Integrals. Otherwise, for more information about generating a volume
integral report, see Section 30.7.1: Generating a Volume Integral Report in the separate
User’s Guide.
Release 12.0 c ANSYS, Inc. January 29, 2009
20-11
Reporting Alphanumeric Data
20.4.1
Computing Volume Integrals
Volume
The volume of a cell zone is computed by summing the volumes of the cells that comprise
the zone:
Z
dV =
n
X
|Vi |
(20.4-1)
i=1
Sum
The sum of a specified field variable in a cell zone is computed by summing the value of
the selected variable at each cell in the selected zone:
n
X
φi
(20.4-2)
i=1
Volume Integral
A volume integral is computed by summing the product of the cell volume and the
selected field variable:
Z
φdV =
n
X
φi |Vi |
(20.4-3)
i=1
Volume-Weighted Average
The volume-weighted average of a quantity is computed by dividing the summation of
the product of the selected field variable and cell volume by the total volume of the cell
zone:
n
1 Z
1 X
φdV =
φi |Vi |
V
V i=1
(20.4-4)
Mass-Weighted Integral
The mass-weighted integral is computed by summing the product of density, cell volume,
and the selected field variable:
Z
φρdV =
n
X
φi ρi |Vi |
(20.4-5)
i=1
20-12
Release 12.0 c ANSYS, Inc. January 29, 2009
20.4 Volume Integration
Mass-Weighted Average
The mass-weighted average of a quantity is computed by dividing the summation of the
product of density, cell volume, and the selected field variable by the summation of the
product of density and cell volume:
Z
Z
n
X
φρdV
=
ρdV
φi ρi |Vi |
i=1
n
X
(20.4-6)
ρi |Vi |
i=1
Release 12.0 c ANSYS, Inc. January 29, 2009
20-13
Reporting Alphanumeric Data
20-14
Release 12.0 c ANSYS, Inc. January 29, 2009
Nomenclature
A
Area (m2 , ft2 )
~a
Acceleration (m/s2 , ft/s2 )
a
Local speed of sound (m/s, ft/s)
c
Concentration (mass/volume, moles/volume)
CD
Drag coefficient, defined different ways (dimensionless)
cp , cv Heat capacity at constant pressure, volume (J/kg-K, Btu/lbm -◦ F)
d
Diameter; dp , Dp , particle diameter (m, ft)
DH
Hydraulic diameter (m, ft)
Dij , D Mass diffusion coefficient (m2 /s, ft2 /s)
E
Total energy, activation energy (J, kJ, cal, Btu)
f
F~
Mixture fraction (dimensionless)
FD
Drag force (N, lbf )
~g
Gravitational acceleration (m/s2 , ft/s2 ); standard values = 9.80665 m/s2 , 32.1740 ft/s2
Gr
Grashof number ≡ ratio of buoyancy forces to viscous forces (dimensionless)
H
Total enthalpy (energy/mass, energy/mole)
h
Heat transfer coefficient (W/m2 -K, Btu/ft2 -h-◦ F)
h
Species enthalpy; h0 , standard state enthalpy of formation (energy/mass, energy/mole)
I
Radiation intensity (energy per area of emitting surface per unit solid angle)
J
Mass flux; diffusion flux (kg/m2 -s, lbm /ft2 -s)
K
Equilibrium constant = forward rate constant/backward rate constant (units vary)
k
Kinetic energy per unit mass (J/kg, Btu/lbm )
k
Reaction rate constant, e.g., k1 , k−1 ,kf,r , kb,r (units vary)
k
Thermal conductivity (W/m-K, Btu/ft-h-◦ F)
kB
Boltzmann constant (1.38 × 10−23 J/molecule-K)
k,kc
Mass transfer coefficient (units vary); also K, Kc
Force vector (N, lbf )
`, l, L Length scale (m, cm, ft, in)
Release 12.0 c ANSYS, Inc. January 29, 2009
Nom-1
Nomenclature
Le
Lewis number ≡ ratio of thermal diffusivity to mass diffusivity (dimensionless)
m
Mass (g, kg, lbm )
ṁ
Mass flow rate (kg/s, lbm /s)
Mw
Molecular weight (kg/kgmol, lbm /lbm mol)
M
Mach number ≡ ratio of fluid velocity magnitude to local speed of sound (dimensionless)
Nu
Nusselt number ≡ dimensionless heat transfer or mass transfer coefficient (dimensionless); usually a function of other dimensionless groups
p
Pressure (Pa, atm, mm Hg, lbf /ft2 )
Pe
Peclet number ≡ Re × Pr for heat transfer, and ≡ Re × Sc for mass transfer
(dimensionless)
Pr
Prandtl number ≡ ratio of momentum diffusivity to thermal diffusivity (dimensionless)
Q
Flow rate of enthalpy (W, Btu/h)
q
Heat flux (W/m2 , Btu/ft2 -h)
R
Gas-law constant (8.31447 × 103 J/kgmol-K, 1.98588 Btu/lbm mol-◦ F)
r
Radius (m, ft)
R
Reaction rate (units vary)
Ra
Rayleigh number ≡ Gr × Pr; measure of the strength of buoyancy-induced flow in
natural (free) convection (dimensionless)
Re
Reynolds number ≡ ratio of inertial forces to viscous forces (dimensionless)
S
Total entropy (J/K, J/kgmol-K, Btu/lbm mol-◦ F)
s
Species entropy; s0 , standard state entropy (J/kgmol-K, Btu/lbm mol-◦ F)
Sc
Schmidt number ≡ ratio of momentum diffusivity to mass diffusivity (dimensionless)
Sij
Mean rate-of-strain tensor (s−1 )
T
Temperature (K, ◦ C, ◦ R, ◦ F)
t
Time (s)
U
Free-stream velocity (m/s, ft/s)
u, v, w Velocity magnitude (m/s, ft/s); also written with directional subscripts (e.g., vx ,
vy , vz , vr )
V
Volume (m3 , ft3 )
~v
Overall velocity vector (m/s, ft/s)
We
Weber number ≡ ratio of aerodynamic forces to surface tension forces (dimensionless)
Nom-2
Release 12.0 c ANSYS, Inc. January 29, 2009
Nomenclature
X
Mole fraction (dimensionless)
Y
Mass fraction (dimensionless)
α
Permeability (m2 , ft2 )
α
Thermal diffusivity (m2 /s, ft2 /s)
α
Volume fraction (dimensionless)
β
Coefficient of thermal expansion (K−1 )
γ
Porosity (dimensionless)
γ
Ratio of specific heats, cp /cv (dimensionless)
∆
Change in variable, final − initial (e.g., ∆p, ∆t, ∆H, ∆S, ∆T )
δ
Delta function (units vary)
Emissivity (dimensionless)
Lennard-Jones energy parameter (J/molecule)
Turbulent dissipation rate (m2 /s3 , ft2 /s3 )
Void fraction (dimensionless)
η
Effectiveness factor (dimensionless)
η 0 , η 00 Rate exponents for reactants, products (dimensionless)
θr
Radiation temperature (K)
λ
Molecular mean free path (m, nm, ft)
λ
Wavelength (m, nm, Å, ft)
µ
Dynamic viscosity (cP, Pa-s, lbm /ft-s)
ν
Kinematic viscosity (m2 /s, ft2 /s)
ν 0 , ν 00 Stoichiometric coefficients for reactants, products (dimensionless)
ρ
Density (kg/m3 , lbm /ft3 )
σ
Stefan-Boltzmann constant (5.67 ×108 W/m2 -K4 )
σ
Surface tension (kg/m, dyn/cm, lbf /ft)
σs
Scattering coefficient (m−1 )
τ
Stress tensor (Pa, lbf /ft2 )
τ
Shear stress (Pa, lbf /ft2 )
τ
Time scale, e.g., τc , τp , τc (s)
τ
Tortuosity, characteristic of pore structure (dimensionless)
φ
Equivalence ratio (dimensionless)
φ
Thiele modulus (dimensionless)
Ω
Angular velocity; Ωij , Mean rate of rotation tensor (s−1 )
Release 12.0 c ANSYS, Inc. January 29, 2009
Nom-3
Nomenclature
ω
Specific dissipation rate (s−1 )
Ω, Ω0 Solid angle (degrees, radians, gradians)
ΩD
Nom-4
Diffusion collision integral (dimensionless)
Release 12.0 c ANSYS, Inc. January 29, 2009
Bibliography
[1] User manual for 1993 version pulverized coal gasification and combustion 3dimensional (pcgc-3).
Advanced Combustion Engineering Research Center,
Brigham Young University, 1993.
[2] T. Ahmad, S. L. Plee, and J. P. Myers. Computation of Nitric Oxide and Soot
Emissions from Turbulent Diffusion Flames. J. of Engineering for Gas Turbines
and Power, 107:48–53, 1985.
[3] B. J. Alder and T. E. Wainwright. Studies in Molecular Dynamics II: Behaviour
of a Small Number of Elastic Spheres. J. Chem. Phys., 33:1439, 1960.
[4] A. A. Amsden. KIVA-3: A KIVA Program with Block-Structured Mesh for Complex Geometries. Technical Report LA-12503-MS, UC-361, Los Alamos National
Laboratory, Los Alamos, New Mexico, March 1993.
[5] T. B. Anderson and R. Jackson. A Fluid Mechanical Description of Fluidized Beds.
I & EC Fundam., 6:527–534, 1967.
[6] W. Anderson and D. L. Bonhus. An Implicit Upwind Algorithm for Computing
Turbulent Flows on Unstructured Grids. Computers Fluids, 23(1):1–21, 1994.
[7] A. Antifora, M. Sala, A. Perera, and L. Vigevano. NOx Emissions in Combustion
Systems of Coal Fired Furnaces with a Reducing Environment: Predictions and
Measurements. In Fourth International Conference on Technologies and Combustion for a Clean Environment, Lisbon, Portugal, 1997.
[8] S. Armsfield and R. Street. The Fractional-Step Method for the Navier-Stokes
Equations on Staggered Grids: Accuracy of Three Variations. Journal of Computational Physics, 153:660–665, 1999.
[9] F. Backmier, K. H. Eberius, and T. Just. Comb. Sci. Tech., 7:77, 1973.
[10] S. Badzioch and P. G. W. Hawksley. Kinetics of Thermal Decomposition of Pulverized Coal Particles. Ind. Eng. Chem. Process Design and Development, 9:521–530,
1970.
[11] J. Baldyga. Turbulent mixer model with application to homogenous instantaneous
chemical reactions. Chem. Eng. Sci., 44:1175–1182, 1989.
Release 12.0 c ANSYS, Inc. January 29, 2009
Bib-1
BIBLIOGRAPHY
[12] R. S. Barlow, G. J. Fiechtner, C. D. Carter, and J. Y. Chen. Experiments on
the Scalar Structure of Turbulent CO/H2 /N2 Jet Flames. Combustion and Flame,
120:549–569, 2000.
[13] F. J. Barnes, J. H. Bromly, T. J. Edwards, and R. Madngezewsky. NOx Emissions
from Radiant Gas Burners. Journal of the Institute of Energy, 155:184–188, 1988.
[14] T. J. Barth and D. Jespersen. The design and application of upwind schemes
on unstructured meshes. Technical Report AIAA-89-0366, AIAA 27th Aerospace
Sciences Meeting, Reno, Nevada, 1989.
[15] H. Barths, C. Antoni, and N. Peters. Three-Dimensional Simulation of Pollutant
Formation in a DI-Diesel Engine Using Multiple Interactive Flamelets. SAE Paper,
SAE, 1998.
[16] H. Barths, N. Peters, N. Brehm, A. Mack, M. Pfitzner, and V. Smiljanowski. Simulation of pollutant formation in a gas turbine combustor using unsteady flamelets.
In 27th Symp. (Int’l.) on Combustion, pages 1841–1847. The Combustion Institute,
1998.
[17] G. K. Batchelor. An Introduction to Fluid Dynamics. Cambridge Univ. Press,
Cambridge, England, 1967.
[18] D. L. Baulch, D. D. Drysdall, D. G. Horne, and A. C. Lloyd. Evaluated Kinetic
Data for High Temperature Reactions, volume 1,2,3. Butterworth, 1973.
[19] D. L. Baulch et al. Evaluated Kinetic Data for Combustion Modelling. J. Physical
and Chemical Reference Data, 21(3), 1992.
[20] M. M. Baum and P. J. Street. Predicting the Combustion Behavior of Coal Particles. Combust. Sci. Tech., 3(5):231–243, 1971.
[21] L. L. Baxter. Turbulent Transport of Particles. PhD thesis, Brigham Young University, Provo, Utah, 1989.
[22] L. L. Baxter and P. J. Smith. Turbulent Dispersion of Particles: The STP Model.
Energy & Fuels, 7:852–859, 1993.
[23] W. Bechara, C. Bailly, P. Lafon, and S. Candel. Stochastic Approach to Noise
Modeling for Free Turbulent Flows. AIAA Journal, 32:3, 1994.
[24] M. Behnia, S. Parneix, Y. Shabany, and P. A. Durbin. Numerical Study of Turbulent Heat Transfer in Confined and Unconfined Impinging Jets. International
Jounal of Heat and Fluid Flow, 20:1–9, 1999.
[25] R. W. Bilger and R. E. Beck. In 15th Symp. (Int’l.) on Combustion, page 541. The
Combustion Institute, 1975.
Bib-2
Release 12.0 c ANSYS, Inc. January 29, 2009
BIBLIOGRAPHY
[26] R. W. Bilger, M. B. Esler, and S. H. Starner. On Reduced Mechanisms for MethaneAir Combustion. In Lecture Notes in Physics, volume 384, page 86. Springer-Verlag,
1991.
[27] B. Binniger, M. Chan, G. Paczkko, and M. Herrmann. Numerical Simulation of
Turbulent Partially Premixed Hydrogen Flames with the Flamelet Model. Technical report, Advanced Combustion Gmbh, Internal Report, 1998.
[28] G. A. Bird. Molecular Gas Dynamics and the direct Simulation of Gas Flows.
Oxford University Press, New York, 1994.
[29] J. Blauvens, B. Smets, and J. Peters. In 16th Symp. (Int’l.) on Combustion. The
Combustion Institute, 1977.
[30] Blint. Principles of Combustion. Wiley-Interscience, New York, 1988.
[31] R. M. Bowen. Theory of Mixtures. In A. C. Eringen, editor, Continuum Physics,
pages 1–127. Academic Press, New York, 1976.
[32] C. T. Bowman. Chemistry of Gaseous Pollutant Formation and Destruction. In
W. Bartok and A. F. Sarofim, editors, Fossil Fuel Combustion. J. Wiley and Sons,
Canada, 1991.
[33] R. K. Boyd and J. H. Kent. Three-dimensional furnace computer modeling. In 21st
Symp. (Int’l.) on Combustion, pages 265–274. The Combustion Institute, 1986.
[34] J. U. Brackbill, D. B. Kothe, and C. Zemach. A Continuum Method for Modeling
Surface Tension. J. Comput. Phys., 100:335–354, 1992.
[35] A. Brandt. Multi-level Adaptive Computations in Fluid Dynamics. Technical
Report AIAA-79-1455, AIAA, Williamsburg, VA, 1979.
[36] K. N. Bray and N. Peters. Laminar Flamelets in Turbulent Flames. In P. A. Libby
and F. A. Williams, editors, Turbulent Reacting Flows, pages 63–114. Academic
Press, 1994.
[37] C.E. Brennen. Cavitation and Bubble Dynamics. Oxford University Press, 1995.
[38] K. S. Brentner and F. Farassat. An Analytical Comparison of the Acoustic Analogy
and Kirchhoff Formulations for Moving Surfaces. AIAA Journal, 36(8), 1998.
[39] S. J. Brookes and J. B. Moss. Prediction of Soot and Thermal Radiation in Confined
Turbulent Jet Diffusion Flames. Combustion and Flame, 116:486–503, 1999.
[40] J. Brouwer, M. P. Heap, D. W. Pershing, and P. J. Smith. A Model for Prediction
of Selective Non-Catalytic Reduction of Nitrogen Oxides by Ammonia, Urea, and
Cyanuric Acid with Mixing Limitations in the Presence of CO. In 26th Symposium
(Int’l) on Combustion, The Combustion Institute, 1996.
Release 12.0 c ANSYS, Inc. January 29, 2009
Bib-3
BIBLIOGRAPHY
[41] A. L. Brown. Modeling Soot in Pulverized Coal Flames. MSc thesis, Brigham Young
University, Utah, USA, 1997.
[42] S. Brunauer. The Absorption of Gases and Vapors. Princeton University Press,
Princeton, NJ, 1943.
[43] Trong T. Bui. A Parallel, Finite-Volume Algorithm for Large-Eddy Simulation of
Turbulent Flows. Technical Memorandum NASA/TM-1999-206570, 1999.
[44] S. Candel and T. Poinsot. Flame stretch and the balance equation for the flame
area. Combustion Science and Technology, 70:1–15, 1990.
[45] R. Cao and S. B. Pope. Numerical Integration of Stochastic Differential Equations:
Weak Second-Order Mid-Point Scheme for Application in the Composition PDF
Method. Journal of Computational Physics, 185(1):194–212, 2003.
[46] N. F. Carnahan and K. E. Starling. Equations of State for Non-Attracting Rigid
Spheres. J. Chem. Phys., 51:635–636, 1969.
[47] M. G. Carvalho, T. Farias, and P. Fontes. Predicting Radiative Heat Transfer in
Absorbing, Emitting, and Scattering Media Using the Discrete Transfer Method.
In W. A. Fiveland et al., editor, Fundamentals of Radiation Heat Transfer, volume
160, pages 17–26. ASME HTD, 1991.
[48] J. R. Cash and A. H. Karp. A variable order Runge-Kutta method for initial value
problems with rapidly varying right-hand sides. ACM Transactions on Mathematical Software, 16:201–222, 1990.
[49] S. Chapman and T. G. Cowling. The Mathematical Theory of Non-Uniform Gases.
Cambridge University Press, Cambridge, England, 3rd edition, 1990.
[50] S. Charpenay, M. A. Serio, and P. R. Solomon. In 24th Symp. (Int’l.) on Combustion, pages 1189–1197. The Combustion Institute, 1992.
[51] H. C. Chen and V. C. Patel. Near-Wall Turbulence Models for Complex Flows
Including Separation. AIAA Journal, 26(6):641–648, 1988.
[52] P. Cheng. Two-Dimensional Radiating Gas Flow by a Moment Method. AIAA
Journal, 2:1662–1664, 1964.
[53] R. V. Chima and M. S. Liou. Comparison of the AUSM+ and H-CUSP schemes
for turbomachinery applications. NASA TM-2003-212457, 2003.
[54] A. J. Chorin. Numerical solution of navier-stokes equations. Mathematics of Computation, 22:745–762, 1968.
[55] B. H. Chowdhury. Emission Control Alternatives for Electric Utility Power Plants.
Energy Sources, 18(4):393–406, October 1996.
Bib-4
Release 12.0 c ANSYS, Inc. January 29, 2009
BIBLIOGRAPHY
[56] E. H. Chui and G. D. Raithby. Computation of Radiant Heat Transfer on a NonOrthogonal Mesh Using the Finite-Volume Method. Numerical Heat Transfer, Part
B, 23:269–288, 1993.
[57] Clift, Grace, and Weber. Bubbles, Drops, and Particles. Technical report, Academic
Press, 1978.
[58] D. Cokljat, V. A. Ivanov, F. J. Sarasola, and S. A. Vasquez. Multiphase k-epsilon
Models for Unstructured Meshes. In ASME 2000 Fluids Engineering Division Summer Meeting, Boston, USA, 2000.
[59] D. Cokljat, M. Slack, and S. A. Vasquez. Reynolds-Stress Model for Eulerian
Multiphase. In Y. Nagano K. Hanjalic and M. J. Tummers, editors, Proceedings
of the 4th International Symposium on Turbulence Heat and Mass Transfer, pages
1047–1054. Begell House, Inc., 2003.
[60] A. Coppalle and P. Vervisch. The Total Emissivities of High-Temperature Flames.
Combustion and Flame, 49:101–108, 1983.
[61] S. M. Correa. A Review of NOx Formation Under Gas-Turbine Combustion Conditions. Combustion Science and Technology, 87:329–362, 1992.
[62] C. Crowe, M. Sommerfield, and Yutaka Tsuji. Multiphase Flows with Droplets and
Particles. CRC Press, 1998.
[63] G. T. Csanady. Turbulent Diffusion of Heavy Particles in the Atmosphere. J.
Atmos. Science, 20:201–208, 1963.
[64] N. Curle. The Influence of Solid Boundaries upon Aerodynamic Sound. Proceedings
of the Royal Society of London. Series A, Mathematical and Physical Sciences,
231:505–514, 1955.
[65] J. Dacles-Mariani, G. G. Zilliac, J. S. Chow, and P. Bradshaw. Numerical/Experimental Study of a Wingtip Vortex in the Near Field. AIAA Journal,
33(9):1561–1568, 1995.
[66] J. M. Dalla Valle. Micromeritics. Pitman, London, 1948.
[67] B. J. Daly and F. H. Harlow. Transport Equations in Turbulence. Phys. Fluids,
13:2634–2649, 1970.
[68] J. F. Daunenhofer and J. R. Baron. Grid Adaption for the 2D Euler Equations.
Technical Report AIAA-85-0484, American Institute of Aeronautics and Astronautics, 1985.
[69] G. G. De Soete. Overall Reaction Rates of NO and N2 Formation from Fuel Nitrogen. In 15th Symp. (Int’l.) on Combustion, pages 1093–1102. The Combustion
Institute, 1975.
Release 12.0 c ANSYS, Inc. January 29, 2009
Bib-5
BIBLIOGRAPHY
[70] M. K. Denison and B. W. Webb. A Spectral Line-Based Weighted-Sum-of-GrayGases Model for Arbitrary RTE Solvers. J. Heat Transfer, 115:1002–1012, 1993.
[71] J. Ding and D. Gidaspow. A Bubbling Fluidization Model Using Kinetic Theory
of Granular Flow. AIChE J., 36(4):523–538, 1990.
[72] G. Dixon-Lewis. Structure of Laminar Flames. In 23rd Symp. (Int’l.) on Combustion, pages 305–324. The Combustion Institute, 1990.
[73] N. Dombrowski and P. C. Hooper. The effect of ambient density or drop formation
in sprays. Chemical Engineering Science, 17:291–305, 1962.
[74] N. Dombrowski and W. R. Johns. The aerodynamic Instability and Disintegration
of Viscous Liquid Sheets. Chemical Engineering Science, 18:203, 1963.
[75] C. Dopazo and E. E. O’Brien. Functional formulation of nonisothermal turbulent
reactive flows. Phys. Fluids, 17:1968, 1975.
[76] A. M. Douaud and P. Eyzat. Four-Octane-Number Method for Predicting the
Anti-Knock Behavior of Fuels in Engines. SAE Technical Paper, v87 780080, SAE,
1978.
[77] M. C. Drake and R. J. Blint. Relative Importance of Nitrogen Oxide Formation
Mechanisms in Laminar Opposed-Flow Diffusion Flames. Combustion and Flame,
83:185–203, 1991.
[78] M. C. Drake, S. M. Correa, R. W. Pitz, W. Shyy, and C. P. Fenimore. Superequilibrium and Thermal Nitric Oxide Formation in Turbulent Diffusion Flames. Combustion and Flame, 69:347–365, 1987.
[79] M. C. Drake, R. W. Pitz, M. Lapp, C. P. Fenimore, R. P. Lucht, D. W. Sweeney,
and N. M. Laurendeau. In 20th Symp. (Int’l.) on Combustion, page 327. The
Combustion Institute, 1984.
[80] D. A. Drew and R. T. Lahey. In Particulate Two-Phase Flow, pages 509–566.
Butterworth-Heinemann, Boston, 1993.
[81] J. K. Dukowwicz and A. S. Dvinsky. Approximate Factorization as a High-Order
Splitting for the Implicit Incompressible Flow Equations. Journal of Computational
Physics, 102:336–347, 1992.
[82] P. A. Durbin. Separated Flow Computations with the k--v 2 Model. AIAA Journal,
33(4):659–664, 1995.
[83] E. R. G. Eckert and R. M. Drake. Analysis of Heat and Mass Transfer. McGrawHill Co., 1972.
Bib-6
Release 12.0 c ANSYS, Inc. January 29, 2009
BIBLIOGRAPHY
[84] D. K. Edwards and R. Matavosian. Scaling Rules for Total Absorptivity and Emissivity of Gases. J. Heat Transfer, 106:684–689, 1984.
[85] J. K. Edwards, B. S. McLaury, and S. A. Shirazi. Supplementing a CFD Code with
Erosion Prediction Capabilities. In Proceedings of ASME FEDSM’98: ASME 1998
Fluids Engineering Division Summer Meeting, Washington DC, June 1998.
[86] J. K. Edwards, B. S. McLaury, and S. A. Shirazi. Evaluation of Alternative Pipe
Bend Fittings in Erosive Service. In Proceedings of ASME FEDSM’00: ASME
2000 Fluids Engineering Division Summer Meeting, Boston, June 2000.
[87] S. E. Elgobashi and T. W. Abou-Arab. A Two-Equation Turbulence Model for
Two-Phase Flows. Phys. Fluids, 26(4):931–938, 1983.
[88] S. Ergun. Fluid Flow through Packed Columns. Chem. Eng. Prog., 48(2):89–94,
1952.
[89] G. Erlebacher, M. Y. Hussaini, C. G. Speziale, and T. A. Zang. Toward the LargeEddy Simulation of Compressible Turbulent Flows. J. Fluid Mech., 238:155–185,
1992.
[90] R. F. Fedors and R. F. Landell. An Empirical Method of Estimating the Void
Fraction in Mixtures of Uniform Particles of Different Size. Powder Technology,
23:225–231.
[91] C. P. Fenimore. Formation of Nitric Oxide in Premixed Hydrocarbon Flames. In
13th Symp. (Int’l.) on Combustion, page 373. The Combustion Institute, 1971.
[92] C. P. Fenimore. Destruction of NO by NH3 in Lean Burnt Gas. Combustion and
Flame, 37:245, 1980.
[93] C. P. Fenimore and G. W. Jones. Oxidation of soot by hydroxyl radicals. J. Phys.
Chem., 71:593–597, 1967.
[94] J. L. Ferzieger and M. Peric. Computational Methods for Fluid Dynamics. SpringerVerlag, Heidelberg, 1996.
[95] J. E. Ffowcs-Williams and D. L. Hawkings. Sound Generation by Turbulence and
Surfaces in Arbitrary Motion. Proc. Roy. Soc. London, A264:321–342, 1969.
[96] M. A. Field. Rate of Combustion Of Size-Graded Fractions of Char from a Low
Rank Coal between 1200 K–2000 K. Combustion and Flame, 13:237–252, 1969.
[97] I. Finnie. Erosion of Surfaces by Solid Particles. Wear, 3:87–103, 1960.
[98] W. A. Fiveland and A. S. Jamaluddin. Three-Dimensional Spectral Radiative Heat
Transfer Solutions by the Discrete Ordinates Method. HTD Vol. 106, Heat Transfer
Phenomena in Radiation, Combustion and Fires, pp. 43–48, 1989.
Release 12.0 c ANSYS, Inc. January 29, 2009
Bib-7
BIBLIOGRAPHY
[99] T. H. Fletcher and D. R. Hardesty. Compilation of Sandia coal devolatilization
data: Milestone report. Sandia Report SAND92-8209, 1992.
[100] T. H. Fletcher and A. R. Kerstein. Chemical percolation model for devolatilization:
3. Direct use of 13 C NMR data to predict effects of coal type. Energy and Fuels,
6:414, 1992.
[101] T. H. Fletcher, A. R. Kerstein, R. J. Pugmire, and D. M. Grant. Chemical percolation model for devolatilization: 2. Temperature and heating rate effects on product
yields. Energy and Fuels, 4:54, 1990.
[102] W. L. Flower, R. K. Hanson, and C. H. Kruger. In 15th Symp. (Int’l.) on Combustion, page 823. The Combustion Institute, 1975.
[103] R. O. Fox. Computational Models for Turbulent Reacting Flows. Cambridge University Press, Cambridge, England, 2003.
[104] S. Fu, B. E. Launder, and M. A. Leschziner. Modeling Strongly Swirling Recirculating Jet Flow with Reynolds-Stress Transport Closures. In Sixth Symposium on
Turbulent Shear Flows, Toulouse, France, 1987.
[105] J. Garside and M. R. Al-Dibouni. Velocity-Voidage Relationships for Fluidization
and Sedimentation. I & EC Process Des. Dev., 16:206–214, 1977.
[106] M. Germano, U. Piomelli, P. Moin, and W. H. Cabot. Dynamic Subgrid-Scale
Eddy Viscosity Model. In Summer Workshop, Center for Turbulence Research,
Stanford, CA, 1996.
[107] T. Gessner. Dynamic Mesh Adaption for Supersonic Combustion Waves Modeled
with Detailed Reaction Mechanisms. PhD thesis, University of Freiburg, Freiburg,
Germany, 2001.
[108] M. M. Gibson and B. E. Launder. Ground Effects on Pressure Fluctuations in the
Atmospheric Boundary Layer. J. Fluid Mech., 86:491–511, 1978.
[109] D. Gidaspow. Multiphase Flow and Fluidization. Academic Press, Boston, 1994.
[110] D. Gidaspow, R. Bezburuah, and J. Ding. Hydrodynamics of Circulating Fluidized Beds, Kinetic Theory Approach. In Fluidization VII, Proceedings of the 7th
Engineering Foundation Conference on Fluidization, pages 75–82, 1992.
[111] R. G. Gilbert, K. Luther, and J. Troe. Ber. Bunsenges. Phys. Chem., 87, 1983.
[112] P. Glarborg, J. E. Johnsson, and K. Dam-Johansen. Kinetics of Homogeneous
Nitrous Oxide Decomposition. Combustion and Flame, 99:523–532, 1994.
[113] M. E. Goldstein and B. Rosenbaum. Effect of Anisotropic Turbulence on Aerodynamic Noise. Journal of the Acoustical Society of America, 54:630–645, 1973.
Bib-8
Release 12.0 c ANSYS, Inc. January 29, 2009
BIBLIOGRAPHY
[114] J. Gottgens, F. Mauss, and N. Peters. Analytic Approximations of Burning Velocities and Flame Thicknesses of Lean Hydrogen, Methane, Ethylene, Ethane,
Acetylene and Propane Flames. In Twenty-Fourth Symposium (Int.) on Combustion, pages 129–135, Pittsburgh, 1992.
[115] I. R. Gran and B. F. Magnussen. A numerical study of a bluff-body stabilized
diffusion flame. part 2. influence of combustion modeling and finite-rate chemistry.
Combustion Science and Technology, 119:191, 1996.
[116] D. M. Grant, R. J. Pugmire, T. H. Fletcher, and A. R. Kerstein. Chemical percolation model of coal devolatilization using percolation lattice statistics. Energy
and Fuels, 3:175, 1989.
[117] D. J. Gunn. Transfer of Heat or Mass to Particles in Fixed and Fluidized Beds.
Int. J. Heat Mass Transfer, 21:467–476, 1978.
[118] W. W. Hagerty and J. F. Shea. A Study of the Stability of Plane Fluid Sheets.
Journal of Applied Mechanics, 22:509, 1955.
[119] A. Haider and O. Levenspiel. Drag Coefficient and Terminal Velocity of Spherical
and Nonspherical Particles. Powder Technology, 58:63–70, 1989.
[120] R. J. Hall, M. D. Smooke, and M. B. Colket. Physical and Chemical Aspects of
Combustion. Gordon and Breach, 1997.
[121] M. P. Halstead, L. J. Kirsch, and C. P. Quinn. Autoignition of Hydrocarbon Fuels at
High Temperatures and Pressures – Fitting of a Mathematical Model. Combustion
and Flame, 30:45–60, 1977.
[122] Z. Han, S. Perrish, P. V. Farrell, and R. D. Reitz. Modeling Atomization Processes
of Pressure-Swirl Hollow-Cone Fuel Sprays. Atomization and Sprays, 7(6):663–684,
Nov.-Dec. 1997.
[123] G. Hand, M. Missaghi, M. Pourkashanian, and A. Williams. Experimental Studies
and Computer Modelling of Nitrogen Oxides in a Cylindrical Furnace. In Proceedings of the Ninth Members Conference, volume 2. IFRF Doc No K21/g/30,
1989.
[124] R. K. Hanson and S. Salimian. Survey of Rate Constants in H/N/O Systems. In
W. C. Gardiner, editor, Combustion Chemistry, page 361, 1984.
[125] H. O. Hardenburg and F. W. Hase. An Empirical Formula for Computing the
Pressure Rise Delay of a Fuel from its Cetane Number and from the Relevant
Parameters of Direct Injection Diesel Engines. SAE Technical Paper 790493, SAE,
1979.
[126] K. Haugen, O. Kvernvold, A. Ronald, and R. Sandberg. Sand Erosion of Wearresistant Materials: Erosion in Choke Valves. Wear, 186-187:179–188, 1995.
Release 12.0 c ANSYS, Inc. January 29, 2009
Bib-9
BIBLIOGRAPHY
[127] R. A. W. M. Henkes, F. F. van der Flugt, and C. J. Hoogendoorn. Natural Convection Flow in a Square Cavity Calculated with Low-Reynolds-Number Turbulence
Models. Int. J. Heat Mass Transfer, 34:1543–1557, 1991.
[128] J. B. Heywood. Internal Combustion Engine Fundamentals. McGraw-Hill, New
York, rev. edition, 1988.
[129] T. Hibiki and M. Ishii. One-group Interfacial Area Transport of Bubbly Flows in
Vertical Round Tubes. International Journal of Heat and Mass Transfer, 43:2711–
2726, 2000.
[130] J. O. Hinze. Turbulence. McGraw-Hill Publishing Co., New York, 1975.
[131] C. W. Hirt and B. D. Nichols. Volume of Fluid (VOF) Method for the Dynamics
of Free Boundaries. J. Comput. Phys., 39:201–225, 1981.
[132] D. G. Holmes and S. D. Connell. Solution of the 2D Navier-Stokes Equations on
Unstructured Adaptive Grids. Presented at the AIAA 9th Computational Fluid
Dynamics Conference, June, 1989.
[133] T. J. Houser, M. Hull, R. Alway, and T. Biftu. Int. Journal of Chem. Kinet.,
12:579, 1980.
[134] P. Huang, P. Bradshaw, and T. Coakley. Skin Friction and Velocity Profile Family
for Compressible Turbulent Boundary Layers. AIAA Journal, 31(9):1600–1604,
September 1993.
[135] S. C. Hunter. Formation of so3 in gas turbines. Transactions of the ASME, 104:44–
51, 1982.
[136] B. R. Hutchinson and G. D. Raithby. A Multigrid Method Based on the Additive
Correction Strategy. Numerical Heat Transfer, 9:511–537, 1986.
[137] H. Ibdir and H. Arastoopour. Modeling of multi-type particle flow using kinetic
approach. AICHE Journal, May 2005.
[138] K. Ishazaki, T. Ikohagi, and H. Daiguji. A High-Resolution Numerical Method for
Transonic Non-equilibrium Condensation Flows Through a Steam Turbine Cascade. In Proceedings of the 6th International Symposium on Computational Fluid
Dynamics, volume 1, pages 479–484, 1995.
[139] M. Ishii and S. Kim. Micro Four-Sensor Probe Measurement of Interfacial Area
Transport for Bubbly Flow in Round Pipes. Nuclear Engineering and Design,
205:123–131, 2001.
[140] R. I. Issa. Solution of the Implicitly Discretized Fluid Flow Equations by OperatorSplitting. Journal of Computational Physics, 62:40–65, 1985.
Bib-10
Release 12.0 c ANSYS, Inc. January 29, 2009
BIBLIOGRAPHY
[141] R. I. Issa. Solution of Implicitly Discretized Fluid Flow Equations by Operator
Splitting. J. Comput. Phys., 62:40–65, 1986.
[142] H. M. Glaz J. B. Bell, P. Colella. Second-Order Projection Method for the Incompressible Navier-Stokes Equations. Journal of Computational Physics, 85:257,
1989.
[143] H. M. Glaz J. B. Bell, P. Colella. An Analysis of the Fractional-Step Method.
Journal of Computational Physics, 108:51–58, 1993.
[144] S. Jain. Three-Dimensional Simulation of Turbulent Particle Dispersion. PhD
thesis, University of Utah, Utah, 1995.
[145] A. Jameson. Solution of the Euler Equations for Two Dimensional Transonic Flow
by a Multigrid Method. MAE Report 1613, Princeton University, June 1983.
[146] A. Jameson, W. Schmidt, and E. Turkel. Numerical Solution of the Euler Equations
by Finite Volume Methods Using Runge-Kutta Time-Stepping Schemes. Technical
Report AIAA-81-1259, AIAA 14th Fluid and Plasma Dynamics Conference, Palo
Alto, California, June 1981.
[147] J. Janicka, W. Kolbe, and W. Kollmann. Closure of the transport equation for
the pdf of turbulent scalar fields. Journal Non-Equilibrium Thermodynamics, 4:47,
1978.
[148] J. Janicka and W. Kollmann. A Two-Variable Formulation for the Treatment of
Chemical Reactions in Turbulent H2 -Air Diffusion Flames. In 17th Symp. (Int’l.)
on Combustion. The Combustion Institute, 1978.
[149] J. Janicka and W. Kollmann. A Numerical Study of Oscillating Flow Around a
Circular Cylinder. Combustion and Flame, 44:319–336, 1982.
[150] C. Jayatillaka. The Influence of Prandtl Number and Surface Roughness on the
Resistance of the Laminar Sublayer to Momentum and Heat Transfer. Prog. Heat
Mass Transfer, 1:193–321, 1969.
[151] P. C. Johnson and R. Jackson. Frictional-Collisional Constitutive Relations for
Granular Materials, with Application to Plane Shearing. J. Fluid Mech., 176:67–
93, 1987.
[152] W. P. Jones and J. H. Whitelaw. Calculation Methods for Reacting Turbulent
Flows: A Review. Combustion and Flame, 48:1–26, 1982.
[153] T. Jongen. Simulation and Modeling of Turbulent Incompressible Flows. PhD
thesis, EPF Lausanne, Lausanne, Switzerland, 1992.
[154] T. Just and S. Kelm. Die Industry, 38:76, 1986.
Release 12.0 c ANSYS, Inc. January 29, 2009
Bib-11
BIBLIOGRAPHY
[155] B. Kader. Temperature and Concentration Profiles in Fully Turbulent Boundary
Layers. Int. J. Heat Mass Transfer, 24(9):1541–1544, 1981.
[156] N. Kandamby, G. Lazopoulos, F. C. Lockwood, A. Perera, and L. Vigevano. Mathematical Modeling of NOx Emission Reduction by the Use of Reburn Technology in
Utility Boilers. In ASME Int. Joint Power Generation Conference and Exhibition,
Houston, Texas, 1996.
[157] K. C. Karki and S. V. Patankar. Pressure-Based Calculation Procedure for Viscous
Flows at All Speeds in Arbitrary Configurations. AIAA Journal, 27:1167–1174,
1989.
[158] W. M. Kays. Loss coefficients for abrupt changes in flow cross section with low
reynolds number flow in single and multiple tube systems. Transactions of the
ASME, 72:1067–1074, January 1950.
[159] W. M. Kays. Turbulent Prandtl Number - Where Are We?
116:284–295, 1994.
J. Heat Transfer,
[160] W. M. Kays and A. L. London. Compact Heat Exchangers. McGraw-Hill, New
York, 1964.
[161] R. J. Kee, F. M. Rupley, J. A. Miller, M. E. Coltrin, J. F. Grcar, E. Meeks, H. K.
Moffat, A. E. Lutz, G. Dixon-Lewis, M. D. Smooke, J. Warnatz, G. H. Evans,
R. S. Larson, R. E. Mitchell, L. R. Petzold, W. C. Reynolds, M. Caracotsios,
W. E. Stewart, P. Glarborg, C. Wang, O. Adigun, W. G. Houf, C. P. Chou, S. F.
Miller, P. Ho, and D. J. Young. CHEMKIN v. 4.0. Technical Report San Diego,
CA, Reaction Design, Inc., 2004.
[162] I. M. Khan and G. Greeves. A Method for Calculating the Formation and Combustion of Soot in Diesel Engines. In N. H. Afgan and J. M. Beer, editors, Heat
Transfer in Flames, chapter 25. Scripta, Washington DC, 1974.
[163] J. S. Kim and F. A. Williams. Extinction of Diffusion Flames with Non-Unity
Lewis Number. Eng. Math, 31:101–118, 1997.
[164] S. Kim, D. Caraeni, and B. Makarov. A Multidimensional Linear Reconstruction
Scheme for Arbitrary Unstructured Grids. Technical report, American Institute of
Aeronautics and Astronautics, AIAA 16th Computational Fluid Dynamics Conference, Orlando, Florida, June 2003.
[165] S.-E. Kim. Large eddy simulation using unstructured meshes and dynamic subgridscale turbulence models. Technical Report AIAA-2004-2548, American Institute of
Aeronautics and Astronautics, 34th Fluid Dynamics Conference and Exhibit, June
2004.
Bib-12
Release 12.0 c ANSYS, Inc. January 29, 2009
BIBLIOGRAPHY
[166] S.-E. Kim and D. Choudhury. A Near-Wall Treatment Using Wall Functions Sensitized to Pressure Gradient. In ASME FED Vol. 217, Separated and Complex Flows.
ASME, 1995.
[167] S.-E. Kim, D. Choudhury, and B. Patel. Computations of Complex Turbulent Flows Using the Commercial Code ANSYS FLUENT. In Proceedings of the
ICASE/LaRC/AFOSR Symposium on Modeling Complex Turbulent Flows, Hampton, Virginia, 1997.
[168] W.-W. Kim and S. Menon. Application of the localized dynamic subgrid-scale
model to turbulent wall-bounded flows. Technical Report AIAA-97-0210, American
Institute of Aeronautics and Astronautics, 35th Aerospace Sciences Meeting, Reno,
NV, January 1997.
[169] H. Kobayashi, J. B. Howard, and A. F. Sarofim. Coal Devolatilization at High
Temperatures. In 16th Symp. (Int’l.) on Combustion. The Combustion Institute,
1976.
[170] N.I. Kolev. Multiphase Flow Dynamics 2: Thermal and Mechanical Interactions.
Springer, Berlin, Germany, 2nd edition edition, 20051994.
[171] R. Kraichnan. Diffusion by a Random Velocity Field. Physics of Fluids, 11:21–31,
1970.
[172] J. C. Kramlich. The Fate and Behavior of Fuel-Sulfur in Combustion Systems.
PhD thesis, Washington State University, Washington, USA, 1980.
[173] K. K. Y. Kuo. Principles of Combustion. John Wiley and Sons, New York, 1986.
[174] H. Lamb. Hydrodynamics, Sixth Edition. Dover Publications, New York, 1945.
[175] M. E. Larsen and J. R. Howell. Least Squares Smoothing of Direct Exchange Areas
in Zonal Analysis. J. Heat Transfer, 108:239–242, 1986.
[176] B. E. Launder. Second-Moment Closure and Its Use in Modeling Turbulent Industrial Flows. International Journal for Numerical Methods in Fluids, 9:963–985,
1989.
[177] B. E. Launder. Second-Moment Closure: Present... and Future? Inter. J. Heat
Fluid Flow, 10(4):282–300, 1989.
[178] B. E. Launder, G. J. Reece, and W. Rodi. Progress in the Development of a
Reynolds-Stress Turbulence Closure. J. Fluid Mech., 68(3):537–566, April 1975.
[179] B. E. Launder and N. Shima. Second-Moment Closure for the Near-Wall Sublayer:
Development and Application. AIAA Journal, 27(10):1319–1325, 1989.
Release 12.0 c ANSYS, Inc. January 29, 2009
Bib-13
BIBLIOGRAPHY
[180] B. E. Launder and D. B. Spalding. Lectures in Mathematical Models of Turbulence.
Academic Press, London, England, 1972.
[181] B. E. Launder and D. B. Spalding. The Numerical Computation of Turbulent Flows.
Computer Methods in Applied Mechanics and Engineering, 3:269–289, 1974.
[182] N. M. Laurendeau. Heterogeneous Kinetics of Coal Char Gasification and Combustion. Prog. Energy Comb. Sci., 4:221–270, 1978.
[183] J. L. Lebowitz. Exact Solution of Generalized Percus-Yevick Equation for a Mixture
of Hard Spheres. The Phy. Rev., 133(4A):A895–A899, 1964.
[184] K. B. Lee, M. W. Thring, and J. M. Beer. Combustion and Flame, 6:137–145, 1962.
[185] W.H. Lee. A Pressure Iteration Scheme for Two-Phase Modeling. Technical Report
LA-UR 79-975, Los Alamos Scientific Laboratory, Los Alamos, New Mexico, 1979.
[186] A. H. Lefebvre. Atomization and Sprays. Hemisphere Publishing Corporation,
1989.
[187] B. P. Leonard. The ULTIMATE conservative difference scheme applied to unsteady
one-dimensional advection. Comp. Methods Appl. Mech. Eng., 88:17–74, 1991.
[188] B. P. Leonard and S. Mokhtari. ULTRA-SHARP Nonoscillatory Convection
Schemes for High-Speed Steady Multidimensional Flow. NASA TM 1-2568
(ICOMP-90-12), NASA Lewis Research Center, 1990.
[189] K. M. Leung and R. P. Lindsted. Detailed Kinetic Modeling of C1-C3 Alkane
Diffusion Flames. Combustion and Flame, 102:129–160, 1995.
[190] J. M. Levy, L. K. Chen, A. F. Sarofim, and J. M. Beer. NO/Char Reactions at
Pulverized Coal Flame Conditions. In 18th Symp. (Int’l.) on Combustion. The
Combustion Institute, 1981.
[191] A. Li and G. Ahmadi. Dispersion and Deposition of Spherical Particles from Point
Sources in a Turbulent Channel Flow. Aerosol Science and Technology, 16:209–226,
1992.
[192] X. Li and R. S. Tankin. On the Temporal Instability of a Two-Dimensional Viscous
Liquid Sheet. Journal of Fluid Mechanics, 226:425, 1991.
[193] A. K. Lichtarowicz, R. K. Duggins, and E. Markland. Discharge Coefficients for
Incompressible Non-Cavitating Flow Through Long Orifices. Journal of Mechanical
Engineering Science, 7:2, 1965.
[194] F. S. Lien and M. A. Leschziner. Assessment of Turbulent Transport Models Including Non-Linear RNG Eddy-Viscosity Formulation and Second-Moment Closure.
Computers and Fluids, 23(8):983–1004, 1994.
Bib-14
Release 12.0 c ANSYS, Inc. January 29, 2009
BIBLIOGRAPHY
[195] M. J. Lighthill. On Sound Generated Aerodynamically. Proc. Roy. Soc. London,
A211:564–587, 1952.
[196] G. M. Lilley. The radiated noise from isotropic turbulence revisited. NASA Contract Report 93-75, NASA Langley Research Center, Hampton, VA, 1993.
[197] D. K. Lilly. A Proposed Modification of the Germano Subgrid-Scale Closure Model.
Physics of Fluids, 4:633–635, 1992.
[198] F. Lindemann. Trans. Faraday Soc., 7, 1922.
[199] R. P. Lindstedt. In Proc. IUTAM Conf. on Aerothermo-Chemistry in Combustion,
Taipei, Taiwan, 1991.
[200] R. P. Lindstedt. Soot Formation in Combustion. Springer-Verlag, Berlin, 1994.
[201] M. S. Liou. A sequel to AUSM: AUSM+. Journal of Computational Physics,
129:364–382, 1996.
[202] M. S. Liou and C. J. Steffen, Jr. A new flux splitting scheme. Journal of Computational Physics, 107(1):23–39, 1993.
[203] A. N. Lipatnikov and J. Chomiak. Turbulent Flame Speed and Thickness:
Phenomenology, Evaluation and Application in Multi-dimensional Simulations.
Progress in Energy & Combustion Science, 28:1–74, January 2002.
[204] R. J. Litchford and S. M. Jeng. Efficient Statistical Transport Model for Turbulent
Particle Dispersion in Sprays. AIAA Journal, 29:1443, 1991.
[205] A. B. Liu, D. Mather, and R. D. Reitz. Modeling the Effects of Drop Drag and
Breakup on Fuel Sprays. SAE Technical Paper 930072, SAE, 1993.
[206] H. Liu and B. M. Gibbs. Modeling of NO and N2 O Emissions from Biomass-Fired
Circulating Fluidized Bed Combustors. Fuel, 81:271–280, 2002.
[207] F. C. Lockwood and C. A. Romo-Millanes. Mathematical Modelling of Fuel - NO
Emissions From PF Burners. J. Int. Energy, 65:144–152, September 1992.
[208] C. K. K. Lun, S. B. Savage, D. J. Jeffrey, and N. Chepurniy. Kinetic Theories for
Granular Flow: Inelastic Particles in Couette Flow and Slightly Inelastic Particles
in a General Flow Field. J. Fluid Mech., 140:223–256, 1984.
[209] J. Y. Luo, R. I. Issa, and A. D. Gosman. Prediction of Impeller-Induced Flows in
Mixing Vessels Using Multiple Frames of Reference. In IChemE Symposium Series,
number 136, pages 549–556, 1994.
[210] A. E. Lutz, R. J. Kee, J. F. Grcar, and F. M. Rupley. OPPDIF: A FORTRAN
Program for Computing Opposed-Flow Diffusion Flames. Sandia National Laboratories Report SAND96-8243, 1997.
Release 12.0 c ANSYS, Inc. January 29, 2009
Bib-15
BIBLIOGRAPHY
[211] J. F. Lynn. Multigrid Solution of the Euler Equations with Local Preconditioning.
PhD thesis, University of Michigan, 1995.
[212] R. K. Lyon. The NH3 -NO-O2 Reaction. Int. Journal of Chem. Kinetics, 8:315–318,
1976.
[213] D. Ma and G. Ahmadi. A Thermodynamical Formulation for Dispersed Multiphase
Turbulent Flows. Int. J. Multiphase Flow, 16:323–351, 1990.
[214] J. Ma. Soot Formation and Soot Secondary Reactions During Coal Pyrolysis. PhD
thesis, Brigham Young University, Utah, USA, 1996.
[215] B. F. Magnussen. On the Structure of Turbulence and a Generalized Eddy Dissipation Concept for Chemical Reaction in Turbulent Flow. Nineteeth AIAA Meeting,
St. Louis, 1981.
[216] B. F. Magnussen and B. H. Hjertager. On mathematical models of turbulent combustion with special emphasis on soot formation and combustion. In 16th Symp.
(Int’l.) on Combustion. The Combustion Institute, 1976.
[217] M. Manninen, V. Taivassalo, and S. Kallio. On the mixture model for multiphase
flow. VTT Publications 288, Technical Research Centre of Finland, 1996.
[218] D. L. Marchisio and R. O. Fox. Solution of Population Balance Equations Using the
Direct Quadrature Method of Moments. Aerosol Science and Technology, 36:43–73,
2005.
[219] F. Mathey, D. Cokljat, J. P. Bertoglio, and E. Sergent. Specification of LES Inlet Boundary Condition Using Vortex Method. In K. Hanjalić, Y. Nagano, and
M. Tummers, editors, 4th International Symposium on Turbulence, Heat and Mass
Transfer, Antalya, Turkey, 2003. Begell House, Inc.
[220] S. R. Mathur and J. Y. Murthy. Coupled ordinates method for multigrid acceleration of radiation calculations. J. of Thermophysics and Heat Transfer, 13(4):467–
473, 1999.
[221] B. S. McLaury, J. Wang, S. A. Shirazi, J. R. Shadley, and E. F. Rybicki. Solid
Particle Erosion in Long Radius Elbows and Straight Pipes. SPE Paper 38842,
SPE Annual Technical Conference and Exhibition, II Production Operations and
Engineering/General, San Antonio, Texas, October 1997.
[222] P. C. Melte and D. T. Pratt. Measurement of Atomic Oxygen and Nitrogen Oxides in Jet Stirred Combustion. In 15th Symposium (Int’l) on Combustion, The
Combustion Institute, pages 1061–1070, 1974.
[223] C. Meneveau and T. Poinsot. Stretching and Quenching of Flamelets in Premixed
Turbulent Combustion. Combustion and Flame, 86:311–332, 1991.
Bib-16
Release 12.0 c ANSYS, Inc. January 29, 2009
BIBLIOGRAPHY
[224] F. R. Menter. Two-Equation Eddy-Viscosity Turbulence Models for Engineering
Applications. AIAA Journal, 32(8):1598–1605, August 1994.
[225] F. R. Menter, M. Kuntz, and R. Langtry. Ten Years of Experience with the SST
Turbulence Model. In K. Hanjalic, Y. Nagano, and M. Tummers, editors, Turbulence, Heat and Mass Transfer 4, pages 625–632. Begell House Inc., 2003.
[226] F. R. Menter, R. B. Langtry, S. R. Likki, Y. B. Suzen, P. G. Huang, and S. Volker.
A Correlation Based Transition Model Using Local Variables Part 1 - Model Formulation. (ASME-GT2004-53452), 2004.
[227] M. Metghalchi and J. C. Keck. Burning velocities of mixtures of air with methanol,
isooctane and indolene at high pressures and temperatures. Combustion and Flame,
48:191–210, 1982.
[228] J. A. Miller and C. T. Bowman. Mechanism and Modeling of Nitrogen Chemistry
in Combustion. Prog. in Energy and Comb. Sci., 15:287–338, 1989.
[229] J. A. Miller, M. C. Branch, W. J. McLean, D. W. Chandler, M. D. Smooke, and
R. J. Kee. In 20th Symp. (Int’l.) on Combustion, page 673. The Combustion
Institute, 1985.
[230] J. A. Miller and G. A. Fisk. Chemical and Engineering News, 31, 1987.
[231] M. Missaghi. Mathematical Modelling of Chemical Sources in Turbulent Combustion. PhD thesis, The University of Leeds, England, 1987.
[232] M. Missaghi, M. Pourkashanian, A. Williams, and L. Yap. In Proceedings of American Flame Days Conference, USA, 1990.
[233] M. F. Modest. The Weighted-Sum-of-Gray-Gases Model for Arbitrary Solution
Methods in Radiative Transfer. J. Heat Transfer, 113:650–656, 1991.
[234] M. F. Modest. Radiative Heat Transfer. Series in Mechanical Engineering. McGrawHill, 1993.
[235] L. J. Molero de Blas. Pollutant Formation and Interaction in the Combustion of
Heavy Liquid Fuels. PhD thesis, University of London, London, England, 1998.
[236] J. P. Monat, R. K. Hanson, and C. H. Kruger. In 17th Symp. (Int’l.) on Combustion,
page 543. The Combustion Institute, 1979.
[237] M. J. Moore and C. H. Sieverding. Two-Phase Steam Flow in Turbines and Separator. McGraw-Hill, 1976.
[238] S. A. Morsi and A. J. Alexander. An Investigation of Particle Trajectories in TwoPhase Flow Systems. J. Fluid Mech., 55(2):193–208, September 26 1972.
Release 12.0 c ANSYS, Inc. January 29, 2009
Bib-17
BIBLIOGRAPHY
[239] J. B. Moss, S. A. L. Perera, C. D. Stewart, and M. Makida. Radiation Heat Transfer
in Gas Turbine Combustors. In Proc. 16th (Int’l.) Symp. on Airbreathing Engines,
Cleveland, OH, 2003.
[240] C. M. Muller, H. Breitbach, and N. Peters. Partially Premixed Turbulent Flame
Propagation in Jet Flames. Technical report, 25th Symposium (Int) on Combustion, The Combustion Institute, 1994.
[241] C. Mundo, M. Sommerfeld, and C. Tropea. Droplet-Wall Collisions: Experimental
Studies of the Deformation and Breakup Process. International Journal of Multiphase Flow, 21(2):151–173, 1995.
[242] J. Y. Murthy and S. R. Mathur. A Finite Volume Method For Radiative Heat
Transfer Using Unstructured Meshes. AIAA-98-0860, January 1998.
[243] S. Muzaferija, M. Peric, P. Sames, and T. Schellin. A Two-Fluid Navier-Stokes
Solver to Simulate Water Entry. In Proc 22nd Symposium on Naval Hydrodynamics,
pages 277–289, Washington, DC, 1998.
[244] J. D. Naber and R. D. Reitz. Modeling Engine Spray/Wall Impingement. Technical Report 880107, Society of Automotive Engineers, General Motors Research
Laboratories, Warren, MI, 1988.
[245] M. Namazian and J. B. Heywood. Flow in the Piston Cylinder Ring Crevices of
a Spark Ignition Engine: Effect on Hydrocarbon Emissions, Efficiency, and Power.
SAE Technical Paper 820088, SAE, 1982.
[246] I. Naruse, Y. Yamamoto, Y. Itoh, and K. Ohtake. Fundamental Study on N2 O
Formation/Decomposition Characteristics by Means of Low-Temperature Pulverized Coal Combustion. In 26th Symposium (Int’l) on Combustion, The Combustion
Institute, pages 3213–3221, 1996.
[247] P. F. Nelson, A. N. Buckley, and M. D. Kelly. Functional Forms of Nitrogen in
Coals and the Release of Coal Nitrogen as NOx Precursors (HCN and NH3 ). In 24th
Symposium (Int’l) on Combustion, The Combustion Institute, page 1259, 1992.
[248] F. Nicoud and F. Ducros. Subgrid-Scale Stress Modelling Based on the Square of
the Velocity Gradient Tensor. Flow, Turbulence, and Combustion, 62(3):183–200,
1999.
[249] L. Nokleberg and T. Sontvedt. Erosion of Oil and Gas Industry Choke Valves
Using Computational Fluid Dynamics and Experiment. International Journal of
Heat and Fluid Flow, 19:636–643, 1998.
[250] P. A. Nooren, H. A. Wouters, T. W. J. Peeters, D. Roekaerts, U. Maas, and
D. Schmidt. Monte carlo pdf modeling of a turbulent natural-gas diffusion flame.
Combustion Theory and Modeling, 1:79–96, 1997.
Bib-18
Release 12.0 c ANSYS, Inc. January 29, 2009
BIBLIOGRAPHY
[251] J. Norman, M. Porkashanian, and A. Williams. Modelling the Formation and Emission of Environmentally Unfriendly Coal Species in Some Gasification Processes.
Fuel, 76(13):1201–1216, October 1997.
[252] W. H. Nurick. Orifice Cavitation and Its Effects on Spray Mixing. Journal of Fluids
Engineering, page 98, 1976.
[253] R. Ocone, S. Sundaresan, and R. Jackson. Gas-particle flow in a duct of arbitrary
inclination with particle-particle interaction. AIChE J., 39:1261–1271, 1993.
[254] S. Ogawa, A. Umemura, and N. Oshima. On the Equation of Fully Fluidized
Granular Materials. J. Appl. Math. Phys., 31:483, 1980.
[255] P. J. O’Rourke. Collective Drop Effects on Vaporizing Liquid Sprays. PhD thesis,
Princeton University, Princeton, New Jersey, 1981.
[256] P. J. O’Rourke and A. A. Amsden. The TAB Method for Numerical Calculation
of Spray Droplet Breakup. SAE Technical Paper 872089, SAE, 1987.
[257] P. J. O’Rourke and A. A. Amsden. A Particle Numerical Model for Wall Film
Dynamics in Port-Fuel Injected Engines. SAE Paper 961961, 1996.
[258] P. J. O’Rourke and A. A. Amsden. A Spray/Wall Interaction Submodel for the
KIVA-3 Wall Film Model. SAE Paper 2000-01-0271, 2000.
[259] S.A. Orszag, V. Yakhot, W.S. Flannery, F. Boysan, D. Choudhury, J. Maruzewski,
and B. Patel. Renormalization Group Modeling and Turbulence Simulations. In
International Conference on Near-Wall Turbulent Flows, Tempe, Arizona, 1993.
[260] M. Ostberg and K. Dam-Johansen. Empirical Modeling of the Selective NonCatalytic Reduction of NO: Comparison with Large-Scale Experiments and Detailed Kinetic Modeling. Chem. Engineering Science, 49(12):1897–1904, 1994.
[261] H. Ounis, G. Ahmadi, and J. B. McLaughlin. Brownian Diffusion of Submicrometer Particles in the Viscous Sublayer. Journal of Colloid and Interface Science,
143(1):266–277, 1991.
[262] M. N. Ozisik. Radiative Transfer and Interactions with Conduction and Convection.
Wiley, New York, 1973.
[263] S. A. Pandya, S. Venkateswaran, and T. H. Pulliam. Implementation of dual-time
procedures in overflow. Technical Report AIAA-2003-0072, American Institute of
Aeronautics and Astronautics, 2003.
[264] S. V. Patankar. Numerical Heat Transfer and Fluid Flow. Hemisphere, Washington,
DC, 1980.
Release 12.0 c ANSYS, Inc. January 29, 2009
Bib-19
BIBLIOGRAPHY
[265] D.Y. Peng and D.B. Robinson. A New Two-Constant Equation of State. Industrial
and Engineering Chemistry: Fundamentals, 15:59–64, 1976.
[266] R. H. Perry, D. W. Gree, and J. O. Maloney. Perry’s Chemical Engineers’ Handbook. McGraw-Hill, New York, 6th edition, 1984.
[267] N. Peters. Laminar Diffusion Flamelet Models in Non Premixed Combustion. Prog.
Energy Combust. Sci., 10:319–339, 1984.
[268] N. Peters. Laminar Flamelet Concepts in Turbulent Combustion. In 21st Symp.
(Int’l.) on Combustion, pages 1231–1250. The Combustion Institute, 1986.
[269] N. Peters and S. Donnerhack. In 18th Symp. (Int’l.) on Combustion, page 33. The
Combustion Institute, 1981.
[270] N. Peters and B. Rogg. Reduced Kinetic Mechanisms for Applications in Combustion Systems. In Lecture Notes in Physics, volume m15. Springer-Verlag, 1992.
[271] K. K. Pillai. The Influence of Coal Type on Devolatilization and Combustion in
Fluidized Beds. J. Inst. Energy, page 142, 1981.
[272] H. Pitsch, H. Barths, and N. Peters. Three-Dimensional Modeling of NOx and Soot
Formation in DI-Diesel Engines Using Detailed Chemistry Based on the Interactive
Flamelet Approach. SAE Paper 962057, SAE, 1996.
[273] H. Pitsch and N. Peters. A Consistent Flamelet Formulation for Non-Premixed
Combustion Considering Differential Diffusion Effects. Combustion and Flame,
114:26–40, 1998.
[274] T. Poinsot and D. Veynante. Theoretical and Numerical Combustion. McGraw-Hill,
New York, 2001.
[275] B.E. Poling, J.M. Prausnitz, and J.P. OConnell. The properties of Gases and
Liquids. McGraw-Hill, New York, 5th edition, 2001.
[276] S. B. Pope. Pdf methods for turbulent reactive flows. Progress Energy Combustion
Science, 11:119, 1985.
[277] S. B. Pope. Computationally efficient implementation of combustion chemistry
using in-situ adaptive tabulation. Combustion Theory and Modeling, 1:41–63, 1997.
[278] S. B. Pope. Turbulent Flows. Cambridge University Press, Cambridge, England,
2000.
[279] B. Popoff and M. Braun. A Lagrangian Approach to Dense Particulate Flows. In
International Conference on Multiphase Flow, Leipzig, Germany, 2007.
[280] I. Proudman. The Generation of Noise by Isotropic Turbulence. Proc. Roy. Soc.,
A214:119, 1952.
Bib-20
Release 12.0 c ANSYS, Inc. January 29, 2009
BIBLIOGRAPHY
[281] S.Kim Q. Wu and M. Ishii. One-group Interfacial Area Transport in Vertical Bubbly
Flow. International Journal of Heat and Mass Transfer, 41:1103–1112, 1997.
[282] G. D. Raithby and E. H. Chui. A Finite-Volume Method for Predicting a Radiant
Heat Transfer in Enclosures with Participating Media. J. Heat Transfer, 112:415–
423, 1990.
[283] W. E. Ranz. Some Experiments on Orifice Sprays. Canadian Journal of Chemical
Engineering, page 175, 1958.
[284] W. E. Ranz and W. R. Marshall, Jr. Evaporation from Drops, Part I. Chem. Eng.
Prog., 48(3):141–146, March 1952.
[285] W. E. Ranz and W. R. Marshall, Jr. Evaporation from Drops, Part II. Chem. Eng.
Prog., 48(4):173–180, April 1952.
[286] R. D. Rauch, J. T. Batira, and N. T. Y. Yang. Spatial Adaption Procedures on
Unstructured Meshes for Accurate Unsteady Aerodynamic Flow Computations.
Technical Report AIAA-91-1106, aiaa, 1991.
[287] R. D. Reitz. Mechanisms of Atomization Processes in High-Pressure Vaporizing
Sprays. Atomization and Spray Technology, 3:309–337, 1987.
[288] R. D. Reitz and F. V. Bracco. Mechanism of Atomization of a Liquid Jet. Phys.
Fluids., 26(10), 1982.
[289] R. D. Reitz and F. V. Bracco. Mechanisms of Breakup of Round Liquid Jets. The
Encyclopedia of Fluid Mechanics, ed. N. Cheremisnoff, 3:223–249, 1986.
[290] W. C. Reynolds. Thermodynamic Properties in SI: Graphs, Tables, and Computational Equations for 40 Substances. Department of Mechanical Engineering,
Stanford University, 1979.
[291] W. C. Reynolds. Fundamentals of turbulence for turbulence modeling and simulation. Lecture Notes for Von Karman Institute Agard Report No. 755, 1987.
[292] C. M. Rhie and W. L. Chow. Numerical Study of the Turbulent Flow Past an Airfoil
with Trailing Edge Separation. AIAA Journal, 21(11):1525–1532, November 1983.
[293] H. S. Ribner. The Generation of Sound by turbulent jets. In Advances in Applied
Mathematics. Academic, New York, 1964.
[294] J. R. Richardson and W. N. Zaki. Sedimentation and Fluidization: Part I. Trans.
Inst. Chem. Eng., 32:35–53, 1954.
[295] C. E. Roberts and R. D. Matthews. Development and Application of an Improved
Ring Pack Model for Hydrocarbon Emissions Studies. SAE Technical Paper 961966,
SAE, 1996.
Release 12.0 c ANSYS, Inc. January 29, 2009
Bib-21
BIBLIOGRAPHY
[296] P. L. Roe. Characteristic based schemes for the Euler equations. Annual Review
of Fluid Mechanics, 18:337–365, 1986.
[297] R. Rota, D. Antos, E. F. Zanoelo, and M. Morbidelli. Experimental and Modeling
Analysis of the NOxOUT Process. Chemical Engineering Science, 57:27–38, 2002.
[298] P. G. Saffman. The Lift on a Small Sphere in a Slow Shear Flow. J. Fluid Mech.,
22:385–400, 1965.
[299] M. M. Salama and E. S. Venkatesh. Evaluation of api rp14e erosional velocity
limitations for offshore gas wells. In OTC Conference, pages 371–376. Houston,
May 1983.
[300] S. Sarkar and L. Balakrishnan. Application of a Reynolds-Stress Turbulence Model
to the Compressible Shear Layer. ICASE Report 90-18, NASA CR 182002, 1990.
[301] S. Sarkar and M. Y. Hussaini. Computation of the sound generated by isotropic turbulence. NASA Contract Report 93-74, NASA Langley Research Center, Hampton,
VA, 1993.
[302] S. S. Sazhin. An Approximation for the Absorption Coefficient of Soot in a Radiating Gas. Manuscript, Fluent Europe, Ltd., 1994.
[303] D. G. Schaeffer. Instability in the Evolution Equations Describing Incompressible
Granular Flow. J. Diff. Eq., 66:19–50, 1987.
[304] R. W. Schefer, M. Namazian, and J. Kelly. In Combustion Research Facility News,
volume 3, number 4. Sandia, 1991.
[305] L. Schiller and Z. Naumann. Z. Ver. Deutsch. Ing., 77:318, 1935.
[306] D. P. Schmidt and M. L. Corradini. Analytical Prediction of the Exit Flow of
Cavitating Orifices. Atomization and Sprays, 7:6, 1997.
[307] D. P. Schmidt, M. L. Corradini, and C. J. Rutland. A Two-Dimensional, NonEquilibrium Model of Flashing Nozzle Flow. In 3rd ASME/JSME Joint Fluids
Engineering Conference, 1999.
[308] D. P. Schmidt, I. Nouar, P. K. Senecal, C. J. Rutland, J. K. Martin, and R. D.
Reitz. Pressure-Swirl Atomization in the Near Field. SAE Paper 01-0496, SAE,
1999.
[309] G.H. Schnerr and J. Sauer. Physical and Numerical Modeling of Unsteady Cavitation Dynamics. In Fourth International Conference on Multiphase Flow, New
Orleans, USA,, 2001.
[310] P. K. Senecal, D. P. Schmidt, I. Nouar, C. J. Rutland, and R. D. Reitz. Modeling
High Speed Viscous Liquid Sheet Atomization. International Journal of Multiphase
Flow, in press.
Bib-22
Release 12.0 c ANSYS, Inc. January 29, 2009
BIBLIOGRAPHY
[311] E. Sergent. Vers une methodologie de couplage entre la Simulation des Grandes
Echelles et les modeles statistiques. PhD thesis, L’Ecole Centrale de Lyon, Lyon,
France, 2002.
[312] N. G. Shah. A New Method of Computation of Radiant Heat Transfer in Combustion Chambers. PhD thesis, Imperial College of Science and Technology, London,
England, 1979.
[313] T.-H. Shih, W. W. Liou, A. Shabbir, Z. Yang, and J. Zhu. A New k- EddyViscosity Model for High Reynolds Number Turbulent Flows - Model Development
and Validation. Computers Fluids, 24(3):227–238, 1995.
[314] M. Shur, P. R. Spalart, M. Strelets, and A. Travin. Detached-Eddy Simulation of
an Airfoil at High Angle of Attack. In 4th Int. Symposium on Eng. Turb. Modeling
and Experiments, Corsica, France, May 1999.
[315] R. Siegel and J. R. Howell. Thermal Radiation Heat Transfer. Hemisphere Publishing Corporation, Washington DC, 1992.
[316] R. Siegel and C. M. Spuckler. Effect of Refractive Index and Diffuse or Specular
Boundaries on a Radiating Isothermal Layer. J. Heat Transfer, 116:787–790, 1994.
[317] C. Simonin and P. L. Viollet. Predictions of an Oxygen Droplet Pulverization
in a Compressible Subsonic Coflowing Hydrogen Flow. Numerical Methods for
Multiphase Flows, FED91:65–82, 1990.
[318] A. K. Singhal, H. Y. Li, M. M. Athavale, and Y. Jiang. Mathematical Basis
and Validation of the Full Cavitation Model. ASME FEDSM’01, New Orleans,
Louisiana, 2001.
[319] Y. R. Sivathanu and G. M. Faeth. Generalized State Relationships for Scalar
Properties in Non-Premixed Hydrocarbon/Air Flames. Combustion and Flame,
82:211–230, 1990.
[320] J. Smagorinsky. General Circulation Experiments with the Primitive Equations. I.
The Basic Experiment. Month. Wea. Rev., 91:99–164, 1963.
[321] R. Smirnov, S. Shi, and I. Celik. Random Flow Generation Technique for Large
Eddy Simulations and Particle-Dynamics Modeling. Journal of Fluids Engineering,
123:359–371, 2001.
[322] I. W. Smith. Combustion and Flame, 17:421, 1971.
[323] I. W. Smith. The Intrinsic Reactivity of Carbons to Oxygen. Fuel, 57:409–414,
1978.
[324] I. W. Smith. The Combustion Rates of Coal Chars: A Review. In 19th Symp.
(Int’l.) on Combustion, pages 1045–1065. The Combustion Institute, 1982.
Release 12.0 c ANSYS, Inc. January 29, 2009
Bib-23
BIBLIOGRAPHY
[325] J. M. Smith and H. C. Van Ness. Introduction to Chemical Engineering Thermodynamics. McGraw Hill, New Jersey, 1986.
[326] T. F. Smith, Z. F. Shen, and J. N. Friedman. Evaluation of Coefficients for the
Weighted Sum of Gray Gases Model. J. Heat Transfer, 104:602–608, 1982.
[327] L. D. Smoot and P. J. Smith. NOx Pollutant Formation in a Turbulent Coal System.
In Coal Combustion and Gasification, page 373, Plenum, Plenum, NY, 1985.
[328] D. O. Snyder, E. K. Koutsavdis, and J. S. R. Anttonen. Transonic store separation
using unstructured cfd with dynamic meshing. Technical Report AIAA-2003-3913,
American Institute of Aeronautics and Astronautics, 33th AIAA Fluid Dynamics
Conference and Exhibit, 2003.
[329] M. S. Solum, R. J. Pugmire, and D. M. Grant. Energy and Fuels, 3:187, 1989.
[330] C. Soteriou, R. Andrews, and M. Smith. Direct Injection Diesel Sprays and the
Effect of Cavitation and Hydraulic Flip on Atomization. SAE Paper 950080, SAE,
1995.
[331] P. Spalart and S. Allmaras. A one-equation turbulence model for aerodynamic
flows. Technical Report AIAA-92-0439, American Institute of Aeronautics and
Astronautics, 1992.
[332] P. R. Spalart, S. Deck, M. L. Shur, K. D. Squires, M. K. Strelets, and A. Travin.
A new version of detached-eddy simulation, resistant to ambiguous grid densities.
Theoretical and Computational Fluid Dynamics, 20:181–195, 2006.
[333] D. B. Spalding. Mixing and chemical reaction in steady confined turbulent flames.
In 13th Symp. (Int’l.) on Combustion. The Combustion Institute, 1970.
[334] C. G. Speziale, S. Sarkar, and T. B. Gatski. Modelling the Pressure-Strain Correlation of Turbulence: An Invariant Dynamical Systems Approach. J. Fluid Mech.,
227:245–272, 1991.
[335] H. B. Squire. Investigation of the Instability of a Moving Liquid Film. British
Journal of Applied Physics, 4:167, 1953.
[336] D. W. Stanton and C. J. Rutland. Modeling Fuel Film Formation and Wall Interaction in Diesel Engines. SAE Paper 960628, 1996.
[337] D. W. Stanton and C. J. Rutland. Multi-Dimensional Modeling of Thin Liquid
Films and Spray-Wall Interactions Resulting from Impinging Sprays. International
Journal of Heat and Mass Transfer, 41:3037–3054, 1998.
[338] R. C. Steele, P. C. Malte, D. G. Nichol, and J. C. Kramlich. NOx and N2 O in
Lean-Premixed Jet-Stirred Flames. Combustion and Flame, 100:440–449, 1995.
Bib-24
Release 12.0 c ANSYS, Inc. January 29, 2009
BIBLIOGRAPHY
[339] P. H. Steward, C. W. Larson, and D. Golden. Combustion and Flame, 75, 1989.
[340] S. Subramaniam and S. B. Pope. A Mixing Model for Turbulent Reactive Flows
Based on Euclidean Minimum Spanning Trees. Combustion and Flame, 115:487–
514, 1998.
[341] M. Syamlal. The Particle-Particle Drag Term in a Multiparticle Model of
Fluidization. National Technical Information Service, Springfield, VA, 1987.
DOE/MC/21353-2373, NTIS/DE87006500.
[342] M. Syamlal and T. J. O’Brien. Computer Simulation of Bubbles in a Fluidized
Bed. AIChE Symp. Series, 85:22–31, 1989.
[343] M. Syamlal, W. Rogers, and O’Brien T. J. MFIX Documentation: Volume 1,
Theory Guide. National Technical Information Service, Springfield, VA, 1993.
DOE/METC-9411004, NTIS/DE9400087.
[344] D. Tabacco, C. Innarella, and C. Bruno. Theoretical and Numerical Investigation
on Flameless Combustion. Combustion Science and Technology, 2002.
[345] L. Talbot et al. Thermophoresis of Particles in a Heated Boundary Layer. J. Fluid
Mech., 101(4):737–758, 1980.
[346] I. Tanasawa. Advances in Condensation Heat Transfer. Advances in Heat Transfer,
21:55–139, 1991.
[347] G. I. Taylor. The Shape and Acceleration of a Drop in a High Speed Air Stream.
Technical report, In the Scientific Papers of G. I. Taylor, ed., G. K. Batchelor,
1963.
[348] P. B. Taylor and P. J. Foster. Some Gray Weighting Coefficients for CO2 -H2 O-Soot
Mixtures. Int. J. Heat Transfer, 18:1331–1332, 1974.
[349] P. A. Tesner, T. D. Snegiriova, and V. G. Knorre. Kinetics of Dispersed Carbon
Formation. Combustion and Flame, 17:253–260, 1971.
[350] E. Turkel and V. N. Vatsa. Choice of variables and preconditioning for time dependent problems. Technical Report AIAA-2003-3692, American Institute of Aeronautics and Astronautics, 16th AIAA Computational Fluid Dynamics Conference,
Orlando, Florida, June 2003.
[351] O. Ubbink. Numerical Prediction of Two Fluid Systems With Sharp Interfaces. PhD
thesis, Imperial College of Science, Technology and Medicine, London, England,
1997.
[352] B. Van Leer. Toward the Ultimate Concervative Difference Scheme. IV. A Second
Order Sequel to Godunov’s Method. Jounal of Computational Physics, 32:101–136,
1979.
Release 12.0 c ANSYS, Inc. January 29, 2009
Bib-25
BIBLIOGRAPHY
[353] J. P. Vandoormaal and G. D. Raithby. Enhancements of the SIMPLE Method for
Predicting Incompressible Fluid Flows. Numer. Heat Transfer, 7:147–163, 1984.
[354] S. A. Vasquez and V. A. Ivanov. A Phase Coupled Method for Solving Multiphase
Problems on Unstructured Meshes. In Proceedings of ASME FEDSM’00: ASME
2000 Fluids Engineering Division Summer Meeting, Boston, June 2000.
[355] V. Venkatakrishnan. On The Accuracy of Limiters and Convergence to Steady State
Solutions. Technical Report AIAA-93-0880, American Institute of Aeronautics and
Astronautics, January 1993.
[356] S. Venkateswaran, J. M. Weiss, and C. L. Merkle. Propulsion Related Flowfields
Using the Preconditioned Navier-Stokes Equations. Technical Report AIAA-923437, AIAA/ASME/SAE/ASEE 28th Joint Propulsion Conference, Nashville, TN,
July 1992.
[357] J. R. Viegas, M. W. Rubesin, and C. C. Horstman. On the Use of Wall Functions as
Boundary Conditions for Two-Dimensional Separated Compressible Flows. Technical Report AIAA-85-0180, AIAA 23rd Aerospace Sciences Meeting, Reno, Nevada,
1985.
[358] V. R. Voller. Modeling Solidification Processes. Technical report, Mathematical
Modeling of Metals Processing Operations Conference, American Metallurgical Society, Palm Desert, CA, 1987.
[359] V. R. Voller, A. D. Brent, and C. Prakash. The Modeling of Heat, Mass and Solute
Transport in Solidification Systems. Int. J. Heat Mass Transfer, 32(9):1719–1731,
1989.
[360] V. R. Voller, A. D. Brent, and K. J. Reid. A Computational Modeling Framework
for the Analysis of Metallurgical Solidification Process and Phenomena. Technical report, Conference for Solidification Processing, Ranmoor House, Sheffield,
September 1987.
[361] V. R. Voller and C. Prakash. A Fixed-Grid Numerical Modeling Methodology for
Convection-Diffusion Mushy Region Phase-Change Problems. Int. J. Heat Mass
Transfer, 30:1709–1720, 1987.
[362] V. R. Voller and C. R. Swaminathan. Generalized Source-Based Method for Solidification Phase Change. Numer. Heat Transfer B, 19(2):175–189, 1991.
[363] K. S. Vorres. User’s handbook for the Argonne premium coal sample bank. Argonne
National Laboratory, supported by DOE contract W-31-109-ENG-38, September
1989. Also K. S. Vorres, ACS Div. Fuel Chem. preprint, 32:4, 1987.
[364] D. Keith Walters and Davor Cokljat. A three-equation eddy-viscosity model for
reynolds-averaged navier-stokes simulations of transitional flows. Journal of Fluids
Engineering, 130, December 2008.
Bib-26
Release 12.0 c ANSYS, Inc. January 29, 2009
BIBLIOGRAPHY
[365] L. P. Wang. On the Dispersion of Heavy Particles by Turbulent Motion. PhD
thesis, Washington State University, 1990.
[366] Z. J. Wang. A Fast Nested Multi-grid Viscous Flow Solver for Adaptive Cartesian/Quad Grids. International Journal for Numerical Methods in Fluids, 33:657–
680, 2000.
[367] J. Warnatz. NOx Formation in High Temperature Processes.
Stuttgart, Germany.
University of
[368] G. P. Warren, W. K. Anderson, J. L. Thomas, and S. L. Krist. Grid convergence for
adaptive methods. Technical Report AIAA-91-1592, American Institute of Aeronautics and Astronautics, AIAA 10th Computational Fluid Dynamics Conference,
Honolulu, Hawaii, June 1991.
[369] C. Weber. Zum Zerfall eines Flüssigkeitsstrahles. ZAMM, 11:136–154, 1931.
[370] J. M. Weiss, J. P. Maruszewski, and W. A. Smith. Implicit Solution of the NavierStokes Equations on Unstructured Meshes. Technical Report AIAA-97-2103, 13th
AIAA CFD Conference, Snowmass, CO, July 1997.
[371] J. M. Weiss, J. P. Maruszewski, and W. A. Smith. Implicit Solution of Preconditioned Navier-Stokes Equations Using Algebraic Multigrid. AIAA Journal,
37(1):29–36, 1999.
[372] J. M. Weiss and W. A. Smith. Preconditioning Applied to Variable and Constant
Density Flows. AIAA Journal, 33(11):2050–2057, November 1995.
[373] C.-Y. Wen and Y. H. Yu. Mechanics of Fluidization. Chem. Eng. Prog. Symp.
Series, 62:100–111, 1966.
[374] Z. Wen, S. Yun, M. J. Thomson, and M. F. Lightstone. Modeling Soot Formation
in Turbulent Kerosene/Air Jet Diffusion Flames. Combustion and Flame, 135:323–
340, 2003.
[375] H. Werner and H. Wengle. Large-Eddy Simulation of Turbulent Flow Over and
Around a Cube in a Plate Channel. In Eighth Symposium on Turbulent Shear
Flows, Munich, Germany, 1991.
[376] C. Westbrook and F. Dryer. Chemical Kinetic Modelling of Hydrocarbon Combustion. Prog. Energy Comb. Sci., page 1, 1984.
[377] A. A. Westenberg. Comb. Sci. Tech., 4:59, 1971.
[378] F. White and G. Christoph. A Simple New Analysis of Compressible Turbulent
Skin Friction Under Arbitrary Conditions. Technical Report AFFDL-TR-70-133,
February 1971.
Release 12.0 c ANSYS, Inc. January 29, 2009
Bib-27
BIBLIOGRAPHY
[379] D. C. Wilcox. Turbulence Modeling for CFD. DCW Industries, Inc., La Canada,
California, 1998.
[380] F. A. Williams. Turbulent Mixing in Nonreactive and Reactive Flows. Plenum
Press, New York, 1975.
[381] F. Winter, C. Wartha, G. Loffler, and H. Hofbauer. The NO and N2 O Formation
Mechanism During Devolatilization and Char Combustion Under Fluidized Bed
Conditions. In 26th Symposium (Int’l) on Combustion, The Combustion Institute,
pages 3325–3334, 1996.
[382] M. Wolfshtein. The Velocity and Temperature Distribution of One-Dimensional
Flow with Turbulence Augmentation and Pressure Gradient. Int. J. Heat Mass
Transfer, 12:301–318, 1969.
[383] P.-K. Wu, L.-K. Tseng, and G. M. Faeth. Primary Breakup in Gas/Liquid Mixing
Layers for Turbulent Liquids. Atomization and Sprays, 2:295–317, 1995.
[384] V. Yakhot and S. A. Orszag. Renormalization Group Analysis of Turbulence: I.
Basic Theory. Journal of Scientific Computing, 1(1):1–51, 1986.
[385] J. B. Young. The Spontaneous Condensation od Steam in Supersonic Nozzles.
Physico Chemical Hydrodynamics, 3(2):57–82, July 1982.
[386] J. B. Young. An Equation of State for Steam for Turbomachinery and Other
Flow Calculations. Journal of Engineering for Gas Turbines and Power, 110:1–7,
January 1988.
[387] J. B. Young. Two-Dimensional, Nonequilibrium, Wet-Steam Calculations for Nozzles and Turbine Cascades. Journal of Turbomachinery, 114:569–579, July 1992.
[388] D. L. Youngs. Time-Dependent Multi-Material Flow with Large Fluid Distortion.
In K. W. Morton and M. J. Baines, editors, Numerical Methods for Fluid Dynamics.
Academic Press, 1982.
[389] Q. Zhou and M. A. Leschziner. Technical report, 8th Turbulent Shear Flows Symp.,
Munich, 1991.
[390] V. Zimont. Gas Premixed Combustion at High Turbulence. Turbulent Flame Closure Model Combustion Model. Experimental Thermal and Fluid Science, 21:179–
186, 2000.
[391] V. Zimont, W. Polifke, M. Bettelini, and W. Weisenstein. An Efficient Computational Model for Premixed Turbulent Combustion at High Reynolds Numbers
Based on a Turbulent Flame Speed Closure. J. of Gas Turbines Power, 120:526–
532, 1998.
Bib-28
Release 12.0 c ANSYS, Inc. January 29, 2009
BIBLIOGRAPHY
[392] V. L. Zimont, F. Biagioli, and K. J. Syed. Modelling Turbulent Premixed Combustion in the Intermediate Steady Propagation Regime. Progress in Computational
Fluid Dynamics, 1(1):14–28, 2001.
[393] V. L. Zimont and A. N. Lipatnikov. A Numerical Model of Premixed Turbulent
Combustion of Gases. Chem. Phys. Report, 14(7):993–1025, 1995.
[394] P.J. Zwart. Numerical Modelling of Free Surface and Cavitating Flows. VKI Lecture
Series, 2005.
[395] P.J. Zwart, A.G. Gerber, and T. Belamri. A Two-Phase Flow Model for Predicting Cavitation Dynamics. In Fifth International Conference on Multiphase Flow,
Yokohama, Japan, 2004.
Release 12.0 c ANSYS, Inc. January 29, 2009
Bib-29
BIBLIOGRAPHY
Bib-30
Release 12.0 c ANSYS, Inc. January 29, 2009
Index
absolute velocity, 2-13
absolute velocity formulation, 2-5, 2-13
absorption coefficient, 5-13
composition-dependent, 5-13, 5-46
effect of particles on, 5-49
effect of soot on, 5-48
WSGGM, 5-46
accuracy
diffusion terms, 18-10
first-order, 18-10
first-to-higher order, 18-13
second-order, 18-12
acoustic signals, 14-2
acoustics model, 14-1
acoustic analogy, 14-2
boundary layer noise, 14-9
broadband noise, 14-3, 14-7
direct method, 14-2
FW-H
formulation, 14-5
integral method, 14-2
jet noise, 14-8
Lilley’s equation, 14-11
linearized Euler equation, 14-10
Proudman’s formula, 14-7
quadrupoles, 14-3
adaption, 19-1
adaption registers, 19-24
anisotropic, 19-19
boundary, 19-5
coarsening, 19-3
dynamic gradient, 19-9
geometry-based, 19-19
gradient, 19-5
hanging node, 19-2
Release 12.0 c ANSYS, Inc. January 29, 2009
hybrid adaption, 19-26
isovalue, 19-9
marking, 19-2
mask registers, 19-27
process, 19-2
refinement, 19-3
region, 19-11
volume, 19-15
y + , y ∗ , 19-16
added mass effect, 16-46
aerodynamic noise, 14-1
algebraic multigrid (AMG), see also multigrid solver, 18-9, 18-51, 18-57
algebraic slip mixture model, see mixture
multiphase model
alloys, solidification of, 17-1
alphanumeric reporting, 20-1
ammonia
injection, 13-30
production, 13-35
angular discretization, 5-26
angular momentum, 1-14
anisotropic adaption, 19-19
anisotropic diffusivity, 1-5
anisotropic scattering
discrete ordinates radiation model, 5-29
DO radiation model, 5-29
P-1 model, 5-14
Rosseland model, 5-18
anisotropic thermal conductivity, 5-6
area averaging, 2-17
area-weighted average, 20-7
Arrhenius reaction rate, 7-4
atomizer models, 15-60
Index-1
Index
autoignition
flamelet model for, 8-39
model, 12-3
ignition delay modeling, 12-7
knock modeling, 12-6
limitations, 12-4
overview, 12-4
axisymmetric flow
modeling with swirl or rotation, 1-11
axisymmetric swirl flows, 1-11
beam width, 5-40
blending
first-to-higher order, 18-13
blowers, 3-6
body forces, 18-26
boiling, 15-21
rate equation, 15-24
boundary adaption, 19-5
boundary conditions
discrete ordinates (DO)
radiation model
opaque walls, 5-30
periodic boundaries, 5-42
specular walls, 5-42
symmetry boundaries, 5-42
low-pressure gas slip, 7-15
radiation
discrete ordinates (DO)
model, 5-31, 5-32, 5-42
discrete transfer radiation
model (DTRM), 5-21
P-1 model, 5-16, 5-17
Rosseland model, 5-18, 5-19
species, 7-14
surface reaction, 7-14
turbulence, 4-57, 4-68
boundary layers, 19-5
deformation, 3-14
Bounded Central Differencing
Scheme, 18-14
Boussinesq hypothesis, 4-5
Brinkman number, 5-4
broadband noise, 14-7
Index-2
Brownian force, 15-5
bubble columns, 16-7
bubbles, see also discrete phase,
multiphase flow
bubbly flow, 16-2, 16-5, 16-7
buoyancy forces, 5-6
buoyancy-driven flows, 5-6
theory, 5-6
burnt mixture, 9-3
calculations, see also solution, solver
capabilities, 1-2
capillary number, 16-24
cavitation model, 16-92, 16-95
additional guidelines, 16-100
Schnerr and Sauer, 16-99
Singhal et al., 16-95
Zwart-Gerber-Belamri, 16-97
CCP, see compute cluster package (CCP)
cell
values, 18-10
volume
change, 19-11
center of pressure, 20-2
computing, 20-3
CFL condition, 18-46
CFX-RIF, 8-30
char, 13-20, 13-45
burnout, 15-36
characteristic strain rate, 8-28
chemical database, 8-2
chemical reaction, 5-5
equilibrium chemistry, 8-1, 8-7
non-equilibrium chemistry, 8-7, 8-33
laminar flamelet model, 8-26
steady laminar flamelet model, 8-32
unsteady laminar flamelet
model, 8-36
non-premixed combustion model, 8-2
reversible, 7-6
chemical reactions, see reactions
chemical species, see species
chemical vapor deposition, 7-11
CICSAM, 16-20
Release 12.0 c ANSYS, Inc. January 29, 2009
Index
circumferential average, 2-16
cloud tracking, 15-9
clustering, 5-20, 5-45
co-located scheme, 18-26
coal combustion, 15-37
char burnout, 15-36
devolatilization, 13-54, 15-25
models for, 15-36
particle heating, 15-35
swelling, 15-35
coal-derived soot model, 13-54
coalescence
discrete phase, 15-89
coarsening, 19-3
coefficient of restitution, 16-54
color scale, see colormap
combusting flow radiation models, 5-46
combustion, see also reacting flows
applications, 1-5
coal, 8-20, 15-25
ECFM, 9-9
equilibrium chemistry, 8-1
finite-rate model, 7-4
flamelet model
theory, 8-26
inert model, 8-24
laminar flamelet model, 8-26
liquid fuel, 8-20, 15-21
non-equilibrium chemistry, 8-7
laminar flamelet model, 8-26
steady laminar flamelet model, 8-32
unsteady laminar flamelet
model, 8-36
non-premixed, 8-2
partially premixed, 10-1
pollutant formation, 13-1
premixed, 9-1
steady laminar flamelet model, 8-32
unsteady laminar flamelet model, 8-36
combustors, gaseous, 8-36
COMET, 5-22
composition PDF transport
Eulerian, 11-9
Release 12.0 c ANSYS, Inc. January 29, 2009
composition PDF transport model, 11-2
IEM model, 11-5
ISAT algorithm, 11-8
Modified Curl model, 11-5
Monte Carlo method, 11-3
Lagrangian method, 11-3
compressible flows, 1-16
equations for, 1-18
gas law equation, 1-19
higher-order density
interpolation, 18-28
model usage of, 1-17
physics of, 1-18
turbulence modeling, 4-24
compression-ignition engines, 8-39
computing
centers of pressure, 20-3
forces and force coefficients, 20-3
moments and moment coefficients, 20-3
conduction, 5-2, 5-5
conductive heat transfer
energy equation, 5-2
modeling, 5-2
theory, 5-2
conical mesh interface, 3-8
conjugate-gradient methods, 18-51
conservation equations, 1-3
discretization of, 18-10
in integral form, 18-25, 18-40
contact resistance in solidification
and melting, 17-8
continuity equation, 1-3
continuous casting, 17-2, 17-7
control volume technique, 18-2
convection in moving solids, 5-5
convective flux, 1-5, 1-6
convective heat transfer
energy equation, 5-2
modeling, 5-2
theory, 5-2
conventions used in this guide, UTM-3
convergence, 19-11, 19-15
criteria, 18-3, 18-5
Index-3
Index
coupled ordinates method, 5-22
Courant number, 18-46
CPD model, 15-28
crevice model, 12-9
theory, 12-13
crystal growth, 17-2
CVD, 7-11
low-pressure gas slip, 7-15
cyclones, 4-49
define/models/energy?, 5-3, 5-6
define/models/viscous/turbulence-expert/rke-cmurotation-term?, 4-22
Delta-Eddington scattering phase
function, 5-29
dense disctrete phase model
granular temperature, 16-80
density
for premixed turbulent
combustion, 9-14
interpolation schemes, 18-28
density-based solver, 18-5, 18-40
discretization, 18-46
explicit, 18-7
flux difference splitting, 18-44
flux vector splitting, 18-45
implicit, 18-7
preconditioning, 18-41
temporal discretization, 18-46
derivative evaluation, 18-20
detached eddy simulation (DES)
model, 4-58
devolatilization
coal, 13-54
models, 15-25
diesel engines, 12-10
diesel unsteady laminar flamelet
model, 8-39
differentiable limiter, 18-25
diffuse semi-transparent walls, 5-38
diffusion, see also diffusivity, binary
species, 7-2
diffusion coefficient, 1-5, 7-2
diffusion flame stretching, 8-8
Index-4
diffusion flames, 8-2
direct numerical simulation, 4-62
discrete ordinates (DO) radiation
model, see also radiative heat transfer, 5-8
advantages, 5-10
angular discretization, 5-26
anisotropic scattering, 5-29
boundary conditions
diffuse semi-transparent walls, 5-38
exterior semi-transparent walls, 5-39
flow inlets and exits, 5-42
gray-diffuse walls, 5-31
periodic boundaries, 5-42
semi-transparent walls, 5-32
solid semi-transparent media, 5-42
specular semi-transparent walls, 5-34
specular walls, 5-42
symmetry boundaries, 5-42
COMET, 5-22
coupled ordinates method, 5-22
energy coupling
limitations, 5-25
theory, 5-24
finite-volume scheme, 5-22
irradiation, 5-39
limitations, 5-10
non-gray, 5-23
angular discretization, 5-26
diffuse walls, 5-32
limitations, 5-10
particulate effects, 5-30
opaque walls, 5-30
particulate effects, 5-29
pixelation, 5-26
semi-transparent wall limitations, 5-42
theory, 5-22
discrete phase, 15-1
air-blast atomizer, 15-74
atomizer models, 15-60
boiling, 15-21
Brownian force, 15-5
cloud tracking, 15-9
Release 12.0 c ANSYS, Inc. January 29, 2009
Index
coalescence, 15-89
coupled calculations, 15-90, 15-95,
18-3, 18-5
devolatilization, 15-25
drag coefficient, 15-15
drag force, 15-2
droplet
collision model, 15-86
droplet breakup models, 15-77
dynamic drag model, 15-16
effervescent atomizer, 15-76
flat-fan atomizer, 15-75
heat transfer, 15-19, 15-90, 15-91
high mach number, 15-16
injections, 15-60
lift force, 15-5
limitations of, 16-43
mass transfer, 15-23, 15-90, 15-92
multicomponent particles, 15-43
numerics, 15-12
one-way, 15-90
particle cloud tracking, 15-9
Peng-Robinson real gas model, 15-43
plain-orifice atomizer, 15-61
pressure-swirl atomizer, 15-69
primary breakup, 15-60
radiation heat transfer to, 15-20,
15-23, 15-41
Raoult’s law, 15-42
rotating reference frames, 15-3
secondary breakup models, 15-77
spray modeling
atomizers, 15-60
breakup, 15-77
droplet collision, 15-86
dynamic drag, 15-16
wall-film, 15-47
wall-jet, 15-46
stochastic tracking, 15-6
thermophoretic force, 15-4
time step, 15-91
trajectory calculations, 15-2
turbulent dispersion, 15-6, 15-9
Release 12.0 c ANSYS, Inc. January 29, 2009
two-way, 15-90
vapor pressure, 15-23
vaporization, 15-21
wall-film model, 15-47
wall-jet model, 15-46
discrete random walk (DRW)
model, 15-6, 15-7
discrete transfer radiation model (DTRM),
see also radiative heat transfer, 5-8
advantages, 5-9
boundary conditions
inlets/outlets, 5-22
walls, 5-21
clustering, 5-20
limitations, 5-9
ray tracing, 5-20
theory, 5-19
discrete values, storage points for, 18-10
discretization, 18-10, 18-26
bounded central differencing
scheme, 18-14
first-order scheme, 18-10
first-to-higher order blending, 18-13
frozen flux formulation, 18-38
iterative time advancement, 18-36
low diffusion second-order
scheme, 18-45
modified HRIC scheme, 18-16
node vs. cell, 18-20
non-iterative time advancement, 18-36
power-law scheme, 18-11
QUICK scheme, 18-15
second-order scheme, 18-12
temporal, 18-18, 18-35, 18-46, 18-48
third-order MUSCL scheme, 18-16
dispersion angle
atomizers, 15-60
effervescent atomizer, 15-76
flat-fan atomizer, 15-75
display, see also graphics, plots
DNS, 4-62
DO radiation model, see discrete ordinates
(DO) radiation model
Index-5
Index
donor-acceptor scheme, 16-19
drag coefficient, see also forces, 20-2
discrete phase, 15-15
in Eulerian multiphase model, 16-7
drift flux model, 16-34
drift velocity, 16-33
droplet, see also discrete phase,
multiphase flow
boiling, 15-24
devolatilization, 15-25
inert heating or cooling, 15-19
multicomponent, 15-42
surface combustion, 15-36
vaporization, 15-21
droplet flow, 16-2, 16-5, 16-7
DRW model, 15-6, 15-7
DTRM, see discrete transfer
radiation model (DTRM)
dual cell
heat rejection, 6-15
ntu relations, 6-13
restrictions, 6-12
dual time stepping, 18-19, 18-49
dynamic kinetic energy
subgrid-scale model, 4-67
dynamic layering method, 3-15
dynamic meshes, 3-11
boundary layer smoothing, 3-14
crevice model, 12-9
dynamic layering method, 3-15
Laplacian smoothing, 3-14
mesh motion methods, 3-11
feature detection, 3-31
remeshing methods, 3-19
2.5D surface, 3-24
face region, 3-21
local, 3-21
local face, 3-22
spring-based smoothing method, 3-12
theory, 3-3
dynamic Smagorinsky-Lilly
subgrid-scale model, 4-66
Index-6
EDC model, 7-10
eddy-dissipation model, 7-9
effective density, 16-44
effectiveness
heat exchangers, 6-8
effectiveness factor, 7-19
eight-step reduced mechanism, 13-42
emissivity, 5-49
weighted-sum-of-gray-gases
model (WSGGM), 5-46
energy
equation, 5-2
in solid regions, 5-5
sources, 5-5
due to radiation, 5-5
due to reaction, 5-5
interphase, 5-5
energy coupling, 5-24
energy equation
convection and conduction, 5-2
in solids, 5-5
engine ignition
auto, 12-3
spark, 12-1
engines, diesel, 8-39
enhanced wall functions, 4-84
enthalpy
equation, 5-3
enthalpy-porosity method, 17-3
equilibrium chemistry, 8-1, 8-2, 8-7
partial equilibrium, 8-7
equivalence ratio, 8-6
error reduction
rate, 18-60
using multigrid, 18-51, 18-52
Euler equations, 1-20
Euler scheme, 15-12
Euler-Euler multiphase modeling, 16-6
Euler-Lagrange multiphase modeling, 15-2
Eulerian composition PDF transport, 11-9
Eulerian multiphase model, see also multiphase flow, 16-7, 16-42
k- dispersed turbulence model, 16-69
Release 12.0 c ANSYS, Inc. January 29, 2009
Index
k- mixture turbulence model, 16-68
k- per-phase turbulence model, 16-73
added mass effect, 16-46
bulk viscosity, 16-62
conservation equations, 16-44
exchange coefficients, 16-49
frictional viscosity, 16-62
granular temperature, 16-64
heat exchange coefficient, 16-66
heat transfer, 16-66
immiscible fluid model, 16-81
interfacial area concentration, 16-66
kinetic viscosity, 16-61
lift forces, 16-45
limitations of, 16-43
mass transfer, 16-89
overview, 16-42
RSM turbulence models, 16-75
dispersed turbulence model, 16-76
mixture turbulence model, 16-77
solids pressure, 16-57
solids shear stresses, 16-61
theory, 16-41
turbulence in, 16-43, 16-67
virtual mass force, 16-46
volume fraction, 16-43
Eulerian unsteady laminar flamelet
model, 8-36
evaporation, 15-21
evaporation-condensation model, 16-104
explicit interpolation scheme, 16-16
explicit time stepping, 18-19, 18-48
exponential scheme, 15-12
extended coherent flamelet model
(ECFM), 9-9
exterior semi-transparent walls, 5-39
external radiation, 5-50
F-cycle multigrid, 18-59
face flux, 18-28
face region remeshing method, 3-21
FAS multigrid, see also multigrid
solver, 18-64
feature detection, 3-31
Release 12.0 c ANSYS, Inc. January 29, 2009
finite-rate reactions, 7-4
particle surface, 7-17
volumetric, 7-1
wall surface, 7-11
finite-volume scheme, 5-22, 18-10
first-order accuracy, 18-10
first-to-higher order blending, 18-13
flame front, 9-3
thickening, 9-4
flame speed, 9-4
flame stretching, 8-8, 9-7
flamelet model, see also non-premixed
combustion model, 8-7, 8-26
approaches
generation, 8-30
import, 8-31
assumptions, 8-26
CFX-RIF format files, 8-32
flamelet generation approach, 8-30
flamelet import approach, 8-31
multiple flamelet libraries, 8-34
multiple-flamelet import approach
CFX-RIF files, 8-32
OPPDIF files, 8-32
standard format files, 8-32
OPPDIF files, 8-32
predicting slow-forming
product species, 8-36
restrictions, 8-26
scalar dissipation, 8-28
single-flamelet import approach
CFX-RIF files, 8-31
OPPDIF files, 8-31
standard format files, 8-31
standard format files, 8-32
steady laminar, 8-32
assumptions and limitations, 8-32
automated grid refinement, 8-34
introduction, 8-33
non-adiabatic, 8-35
strain rate, 8-28
theory, 8-26
Index-7
Index
unsteady laminar, 8-36
diesel, 8-39
Eulerian, 8-36
flames, slow-chemistry, 8-33
flexible-cycle multigrid, 18-59
flow rate, 20-7
flue gas recycle, non-premixed
model with, 8-23
fluid flow
compressible, 1-16
equations
continuity and momentum, 1-3
mass conservation, 1-3
momentum conservation, 1-4
UDS transport, 1-5
inviscid, 1-19
overview, 1-2
periodic, 1-7
physical models of, 1-2
swirling and rotating, 1-11
fluid-fluid multiphase flows, 16-48
fluidized beds, 16-3, 16-5, 16-7
flux
reports, 20-2
through boundaries, 20-2
flux-difference splitting, 18-44
flux-vector splitting, 18-45
FMG multigrid, 18-66
limitations, 18-67
forces
coefficients of, 20-2
computing, 20-3
on boundaries, 20-2
Fractional Step algorithm
non-iterative scheme (NITA), 18-38
free vortex, 1-14
free-surface flow, 16-2, 16-5, 16-7
freezing, 17-2
frictional viscosity, 16-62
frozen flux formulation, 18-38
FSI simulations, see fluid-structure
interaction (FSI) simulations
fuel rich flames, 8-7
Index-8
full multigrid (FMG), 18-66
limitations, 18-67
full-approximation storage (FAS)
multigrid, see also multigrid solver,
18-51, 18-64
fully-developed flow, 1-8
FW-H acoustics model, 14-4
gaseous combustors, 8-36
gaseous solid catalyzed reactions, 7-21
Gauss-Seidel method, 18-51
Gauss-Seidel smoother, 18-62
geometric reconstruction scheme, 16-19
geometry-based adaption, 19-19
Gidaspow model, 16-54
global time stepping, 18-19
governing equations, 1-3
discretization of, 18-10
in integral form, 18-25, 18-40
gradient adaption, 19-5
dynamic, 19-9
gradient limiters, 18-23
differentiable limiter, 18-25
multidimensional limiter, 18-24
standard limiter, 18-24
gradient option, 18-20
granular flows, 16-6, 16-7, 16-48
stresses in, 16-48
granular temperature, 16-37, 16-64
graphics, see also display, plots
Grashof number, 5-6
gravitational acceleration, 15-3
gray band model
see also non-gray discrete ordinates
(DO) radiation model 1
gray-band model, 5-23
gray-diffuse model, 5-43
gray-diffuse walls, 5-31
Green-Gauss cell-based, 18-21
Green-Gauss node-based, 18-21
grid
reading, see also grid importing
Release 12.0 c ANSYS, Inc. January 29, 2009
Index
hanging node adaption, 19-2
hanging nodes, 19-2
heat capacity, see also specific heat capacity
heat exchanger
dual cell
ntu relations, 6-13
heat exchanger groups, 6-1, 6-11
heat exchanger models, 6-1
dual cell
heat rejection, 6-15
restrictions, 6-12
effectiveness, 6-8
group connectivity, 6-11
heat rejection, 6-9
macros, 6-2
ntu-model, 6-1
features, 6-4
restrictions, 6-4
restrictions, 6-4, 6-12
simple-effectiveness-model, 6-1
features, 6-4
restrictions, 6-4
heat flux, 20-2
heat rejection, 6-9, 6-15
dual cell, 6-15
heat exchangers, 6-9
heat sources, 5-5
heat transfer, 5-2
buoyancy-driven flows, 5-6
convective and conductive, 5-2
theory, 5-2
modeling, 5-1
natural convection flows, 5-6
overview of models, 5-1
radiation, see also radiative
heat transfer, 5-7
radiative theory, 5-12
heterogeneous reactions
source terms, 16-109
high mach number
discrete phase, 15-16
HNCO production, 13-35
hydrotransport, 16-3, 16-5, 16-7
Release 12.0 c ANSYS, Inc. January 29, 2009
ILU method, 18-51
ILU smoother, 18-63
immiscible fluid model, 16-81
impeller-baffle interaction, 2-9
impellers, multiple, 2-9
implicit Euler scheme, 15-12
implicit interpolation scheme, 16-16
implicit time stepping, 18-19, 18-49
in-cylinder model
crevice model
theory, 12-13
inert model
combustion, 8-24
integral reporting, 20-6, 20-11
integral time scale, 15-7
interface zone, 3-6
interfacial area concentration, 16-38, 16-66
interphase exchange coefficients, 16-49
interpolation, 18-10, 18-26
inviscid flows, 1-19
continuity equation, 1-20
energy equation, 1-21
equations, 1-20
momentum equation, 1-20
irradiation, 5-40
ISAT algorithm, 11-8
isotropic diffusivity, 1-5
isovalue
adaption, 19-9
iterative procedure, 18-5
iterative time advancement, 18-36
jet breakup, 16-6, 16-14
k- model, 4-11
realizable, 4-18
RNG, 4-14
standard, 4-12
k-kl-ω model
transition, 4-37
k-ω model
SST, 4-31
standard, 4-26
Index-9
Index
kinetic theory
in granular flows, 16-6
Knudsen number, 7-15, 15-4
Kobayashi model, 15-27
Mach number, 1-17
macros, 6-2
manuals, using the, UTM-1
mass and momentum transfer, 16-108
mass average, 20-7
mass averaging, 2-17
Lagrangian discrete phase model,
see also discrete phase
mass diffusion, 7-2
Lagrangian method, 11-3
mass flow rate, 1-6, 20-7
laminar finite-rate model, 7-4
through a surface, 20-8
laminar flamelet model, see flamelet model mass flux, 20-2
Laplacian smoothing, 3-14
mass transfer, see also discrete phase,
multiphase flow, 16-89
large eddy simulation (LES), 4-61
mass-average quantities, 20-8
boundary conditions, 4-68
mass-averaged quantities, 20-13
no perturbations, 4-68
mean beam length, 5-47
spectral synthesizer, 4-70
mean free path, 7-15, 15-4
subgrid-scale models, 4-64
mean reaction rate
dynamic kinetic energy model, 4-67
NOx, 13-37
dynamic Smagorinsky-Lilly
soot, 13-59
model, 4-66
SOx, 13-46
Smagorinsky-Lilly model, 4-65
melting and solidification,
WALE model, 4-67
see solidification and melting
vortex method, 4-69
mesh,
see
grid
least squares cell-based, 18-22
adaption, 19-1
LES, see also large eddy simulation
coarsening, 19-3
(LES), 4-3, 4-61
near walls, 19-16
Lewis number, 7-3
interfaces, 3-6, 3-10
lift coefficient, see also forces, 20-2
shapes of, 3-8
lift force, 15-5
motion of, 2-1, 3-4, 3-11
in multiphase flow, 16-45
refinement, 19-3
line solvers, 18-51
at boundaries, 19-5
linear pressure-strain model, 4-50
based on cell volume, 19-15
linear-anisotropic scattering phase
function, 5-14, 5-18, 5-29
based on gradient, 19-5
liquid fraction, 17-3
based on isovalue, 19-9
liquid fuel combustion, 15-21
dynamic, 19-9
liquid reactions, 11-6
in a region, 19-11
liquid reactors, 8-36, 8-38
near walls, 19-16
local face remeshing method, 3-22
rotating reference frames, 2-1
local remeshing
spacing at walls
method, 3-21
in turbulent flows, 19-16
Low Diffusion Second-Order scheme, 18-45
storage points, 18-10
low-Re stress-omega, 4-53
mesh motion methods, 3-11
low-Reynolds-number flows, 4-15
feature detection, 3-31
Index-10
Release 12.0 c ANSYS, Inc. January 29, 2009
Index
metallurgy, 17-1
mixed convection, see also natural
convection, 5-6
mixed-out averaging, 2-18
mixing plane model, 2-11, 2-13
area averaging, 2-17
mass averaging, 2-17
mass conservation, 2-19
mixed-out averaging, 2-18
swirl conservation, 2-20
theory, 2-14
total enthalpy conservation, 2-21
mixing tanks, 2-9
mixture diffusivity, 1-7
mixture fraction, 8-2
conservation of, 8-5
limitations on, 8-19
variance, 8-5
mixture multiphase model,
see also multiphase flow, 16-6
cavitation model, 16-92
collisional viscosity, 16-36
drift flux model, 16-34
drift velocity, 16-33
evaporation-condensation
model, 16-104
granular temperature, 16-37
interfacial area concentration, 16-38
kinetic viscosity, 16-36
limitations, 16-31
mass transfer, 16-89
momentum equation, 16-32
overview, 16-30
relative velocity, 16-33
slip velocity, 16-33
solids shear stresses, 16-36
theory, 16-30
volume fraction, 16-35
modified HRIC scheme, 18-16
moment coefficient, see also forces
moments
coefficients of, 20-2
Release 12.0 c ANSYS, Inc. January 29, 2009
computing, 20-3
reporting, 20-2
momentum equation, 1-4
Monte Carlo method, 11-3
Morsi and Alexander model, 16-50
Moss-Brookes soot formation model
theory, 13-52
coal-derived soot, 13-54
turbulence-chemistry
interaction, 13-58
Moss-Brookes-Hall soot formation
model
theory, 13-56
turbulence-chemistry
interaction, 13-58
moving mesh, 2-1
moving reference frames, 2-1
multi-stage scheme, 18-46
multicomponent droplet, 15-42
Raoult’s Law, 15-42
multicomponent particle, 15-42
Raoult’s Law, 15-42
multicomponent particles, 15-43
multidimensional limiter, 18-24
multigrid solver, 18-51
algebraic (AMG), 18-57
cycles, 18-54
F cycle, 18-59
flexible cycle, 18-59
full (FMG), 18-66
limitations, 18-67
full-approximation storage
(FAS), 18-64
prolongation, 18-53
residual reduction rate, 18-59, 18-60
restriction, 18-53
termination criteria, 18-61
V cycle, 18-54, 18-56
W cycle, 18-54, 18-56
multiphase flows
cavitation model, 16-92, 16-95, 16-97,
16-99
choosing a model for, 16-5
Index-11
Index
Euler-Euler approach, 16-6
Euler-Lagrange approach, 15-2
Eulerian model, see also Eulerian multiphase model, 16-7, 16-41, 16-42
evaporation-condensation
model, 16-104
examples, 16-5
fluid-fluid, 16-48
fluid-solid, 16-48
gas-liquid, 16-2
gas-solid, 16-3
granular, 16-48
homogeneous, 16-35
immiscible fluid model, 16-81
interphase exchange coefficients, 16-49
liquid-liquid, 16-2
liquid-solid, 16-3
mixture model, see also mixture
multiphase model, 16-6, 16-30
particulate loading, 16-9
regimes, 16-2
second-order time scheme, 16-11
Stokes number, 16-10
volume of fluid (VOF) model, see also
volume of fluid (VOF) model, 16-6,
16-13, 16-14
wet steam model, 16-82
properties, 16-87
restrictions, 16-83
multiphase species transport, 16-107
heterogeneous reactions, 16-109
limitations, 16-108
momentum transfer, 16-108
stiff chemistry, 16-111
multiple reference frames, 2-8
restrictions of, 2-9
steady flow approximation, 2-8, 2-9
theory of, 2-9
multiple surface reactions model, 15-40
mushy zone, 17-3, 17-4
natural convection, 5-6, 18-26
Navier-Stokes equations, 1-3
filtered, 4-63
Index-12
near-wall flows, 4-15
near-wall treatments, 4-71
neighbor correction, 18-32
node values, 18-10
noise, 14-3
non-equilibrium chemistry, 8-7
laminar flamelet model, 8-26
steady laminar flamelet model, 8-32
unsteady laminar flamelet model, 8-36
non-equilibrium wall functions, 4-79, 4-80
non-gray discrete ordinates (DO) radiation
model, 5-23
angular discretization, 5-26
diffuse walls, 5-32
limitations, 5-10
particulate effects, 5-30
pixelation, 5-26
non-gray radiation, 5-23, 5-50
boundary conditions, 5-32
limitations, 5-10
particulate effects, 5-30
non-iterative time advancement
(NITA), 18-36
non-premixed combustion model, 8-2
equilibrium chemistry, 8-1, 8-7
flamelet model, see also flamelet model
theory, 8-26
flue gas recycle, 8-23
laminar flamelet model, 8-26
limitations of, 8-19
look-up tables, 8-12, 8-13, 8-15
multiple fuel inlets, 8-14, 8-19
non-adiabatic form, 8-12
non-equilibrium chemistry, 8-7
laminar flamelet model, 8-26
steady laminar flamelet model, 8-32
unsteady laminar flamelet
model, 8-36
PDF functions in, 8-10
rich flammability limit, 8-8
steady laminar flamelet model, 8-32
unsteady laminar flamelet
model, 8-36
Release 12.0 c ANSYS, Inc. January 29, 2009
Index
NOx, 8-33
reduction, 13-30
ammonia, 13-30
urea, 13-32
NOx model, 13-1
coal, 13-18
formation, 13-3
fuel, 13-12
liquid fuel, 13-13
PDF functions in, 13-36
prompt, 13-8
reburn, 13-26
selective noncatalytic
reduction (SNCR), 13-30
thermal, 13-4
turbulence-chemistry interaction, 13-36
NRBCs, see non-reflecting boundary
conditions
ntu relations, 6-13
ntu-model, 6-1
features, 6-4
restrictions, 6-4
nuclei formation, 13-51
numerical scheme, 18-1
boundary conditions
inlets/outlets, 5-17
walls, 5-16
limitations, 5-9
particulate effects in, 5-14
theory, 5-13
partially premixed combustion model, 10-1
limitations of, 10-1
overview, 10-1
theory, 10-2
partially premixed flames, 9-2, 10-1
partially-specular boundaries, 5-50
particle, see also discrete phase,
multiphase flow
boiling, 15-24
cloud tracking, 15-9
coupling, 15-90
devolatilization, 15-25
inert heating or cooling, 15-19
laws, 15-18
multicomponent particles, 15-42, 15-43
radiation, 15-20, 15-23
sub-micron, 15-5, 15-16
surface combustion, 15-36
trajectory calculations, 15-2
one-step soot formation model
turbulent dispersion, 15-6
theory, 13-48
vaporization, 15-21
opaque walls, 5-30
particle motion, 15-2
open channel boundary condition, 16-25
particle surface reactions, 7-17
open channel flow, 16-25
gaseous solid catalyzed reactions, 7-21
downstream boundary condition, 16-27
solid decomposition reactions, 7-21
mass flow rate, 16-27
solid deposition reactions, 7-21
upstream boundary condition, 16-26
solid-solid reactions, 7-20
wave boundary condition, 16-28
theory, 7-17
Operating Conditions dialog box, 15-3
particle-laden flow, 16-3, 16-5, 16-7
OPPDIF, 8-30
particulate effects
opposed-flow diffusion flamelet, 8-26
absorption coefficient, 5-49
optical thickness, 5-49
DO model, 5-29
P-1 radiation model, 5-14
P-1 radiation model, see also radiative
radiation, 5-50
heat transfer, 5-8
particulate loading, 16-9
advantages, 5-9
anisotropic scattering, 5-14
PDF reaction, 11-6
Release 12.0 c ANSYS, Inc. January 29, 2009
Index-13
Index
PDF/mixture fraction model, see nonpremixed combustion model
Peclet number, 18-11
Peng-Robinson real gas model, 15-43
periodic flows, 1-7
limitations, 1-9
overview, 1-8
pressure, 1-9
theory, 1-9
phase, 16-2
phase change, see solidification and melting
PISO algorithm, 18-32
neighbor correction, 18-32
non-iterative scheme (NITA), 18-38
skewness correction, 18-32
skewness-neighbor coupling, 18-32
pixelation, 5-26
planar sector, 3-10
plasma-enhanced surface reaction
modeling, 1-5
plots, see also display, graphics
pneumatic transport, 16-3, 16-5, 16-7
pollutant formation, 13-1
NOx, 13-1
soot, 13-47
SOx, 13-39, 13-40
postprocessing
reports, 20-1
power-law scheme, 18-11
preconditioning, 18-41
matrix, 18-41
premixed flame model
Zimont, 12-2
premixed flames, 9-2
premixed turbulent combustion, 9-1
adiabatic, 9-13
density, 9-14
flame front, 9-3
wrinkling, 9-4
flame speed, 9-4
flame stretching, 9-7
non-adiabatic, 9-13
product formation, 9-3
Index-14
progress variable, 9-3
restrictions, 9-2
stretch factor, 9-7
wall damping, 9-8
Zimont
theory, 9-3
pressure
drop
heat exchanger, 6-6
interpolation schemes, 18-26
pressure work, 5-3
pressure-based coupled algorithm, 18-33
pressure-based solver, 18-2, 18-25
density interpolation schemes, 18-28
discretization, 18-26
frozen flux formulation, 18-38
iterative time advancement, 18-36
non-iterative time
advancement (NITA), 18-36
pressure interpolation schemes, 18-26
pressure-velocity coupling, 18-29
steady-state flows, 18-35
time-dependent flows, 18-35
pressure-correction equation, 18-30
pressure-velocity coupling, 18-29
coupled algorithm, 18-33
PRESTO, 18-27
primary breakup, 15-60
probability density function, 8-8
product formation, 9-3
slowly forming, 8-8, 8-36
production of
ammonia, 13-35
HNCO, 13-35
urea, 13-34
progress variable, 9-3
prolongation, 18-53
properties
database, 8-2
Proudman’s formula, 14-7
pull velocity, 17-4, 17-7
Release 12.0 c ANSYS, Inc. January 29, 2009
Index
quadratic pressure-strain model, 4-52
quadrupoles, 14-3
QUICK scheme, 18-15
radiation, see radiative heat transfer
DO/energy coupling
limitations, 5-25
theory, 5-24
radiation heat flux, 20-2
radiation models
about, 5-7
combusting flows, 5-46
discrete ordinates (DO), see also discrete ordinates (DO) radiation
model, 5-10
discrete transfer radiation model
(DTRM), see also discrete transfer radiation model (DTRM), 5-9,
5-19
P-1, see also P-1 radiation model, 5-9
Rosseland, see also Rosseland radiation
model, 5-10
S2S, 5-11
surface-to-surface (S2S), see also
surface-to-surface (S2S) radiation
model, 5-11
theory, 5-12
radiative heat transfer
applications, 5-8
choosing a model, 5-49
discrete ordinates (DO) model, see also
discrete ordinates (DO) radiation
model, 5-22
discrete transfer radiation model
(DTRM), see also discrete transfer radiation model (DTRM), 5-19
emissivity, 5-49
external radiation, 5-50
modeling, 5-7
non-gray, 5-23, 5-50
non-gray discrete ordinates (DO) model
limitations, 5-10
optical thickness, 5-49
overview of, 5-8
Release 12.0 c ANSYS, Inc. January 29, 2009
P-1 model, see also P-1 radiation
model, 5-13
particulate effects, 5-49, 5-50
radiative transfer equation (RTE), 5-12
Rosseland model, see also Rosseland
radiation model, 5-17
scattering, 5-49
semi-transparent media, 5-32
semi-transparent walls, 5-50
soot effects on, 5-48
surface-to-surface
(S2S)
radiation
model, see also surface-to-surface
(S2S) radiation model, 5-43
smoothing, 5-46
theory, 5-12
radiative transfer equation, 5-12
radiosity, 5-45
RANS model
realizable k-, 4-60
Spalart-Allmaras, 4-59
SST k-ω, 4-61
Raoult’s law, 15-42
ray tracing, 5-20
Rayleigh number, 5-7
reacting flows, see also combustion, 7-1
equilibrium chemistry, 8-2
heterogeneous reactions, 15-37
non-premixed combustion model, 8-2
partially premixed combustion, 10-1
pollutant formation in, 13-1
premixed combustion, 9-1
reaction progress variable, 9-3
reaction rate
surface reactions, 7-12
reactions
liquid, 11-6
pressure-dependent, 7-7
reversible, 7-6
reactors, liquid, 8-36, 8-38
realizable k-
RANS model, 4-60
realizable k- model, 4-18
reburning, 13-26
Index-15
Index
reference frames
multiple, 2-8, 2-9
single, 2-6
reference pressure, 20-5
reference values
for force and moment
coefficient reports, 20-3
refinement, 19-3
refractive index, 5-12
region adaption, 19-11
registers, 19-24
adaption, 19-24
mask, 19-27
types, 19-24
relative velocity, 2-13
for mixture model, 16-33
relative velocity formulation, 2-5, 2-11
relaxation scheme, 18-51, 18-56
relaxation sweeps, 18-54, 18-56
remeshing methods, 3-19
2.5D surface, 3-24
face region, 3-21
local, 3-21
using size functions, 3-26
local face, 3-22
renormalization group (RNG) theory, 4-14
reporting
center of pressure, 20-2
data, 20-1
drag coefficients, 20-2
fluxes through boundaries, 20-2
forces, 20-2
heat flux, 20-2
lift coefficients, 20-2
mass flux, 20-2
moments and moment coefficients, 20-2
radiation heat flux, 20-2
surface integrals, 20-6
volume integrals, 20-11, 20-12
residual reduction rate criteria, 18-60
residual smoothing, 18-47
Index-16
residuals, reduction rate, 18-61
restriction, 18-53
reversible reactions, 7-6
Reynolds averaging, 4-3, 4-4
Reynolds number, 5-6, 20-2
Reynolds stress model (RSM), 4-48
boundary conditions, 4-57
linear pressure-strain model, 4-50
low-Re stress-omega, 4-53
pressure-strain term in, 4-50
quadratic pressure-strain model, 4-52
Reynolds stresses, 4-5
RFL option, see rich flammability
limit option
rich flammability limit option, 8-8
rich limit, 8-7
risers, 16-7
RNG k- model, 4-14
swirl modification, 4-16
Rosseland radiation model,
see also radiative heat transfer, 5-8
advantages, 5-10
anisotropic scattering, 5-18
boundary conditions
inlets/outlets, 5-19
walls, 5-18
limitations, 5-10
theory, 5-17
rotating flows, see also swirling flows, 1-11
multiple reference frames, 2-9
overview, 1-11
physics of, 1-14
rotating reference frame, 1-14
three-dimensional, 1-13
turbulence modeling in, 4-19, 4-49
rotating reference frame, 2-8
discrete phase, 15-3
mathematical equations, 2-3
RSM, see also Reynolds stress model
(RSM), 4-48
RTE, 5-12
RUN-1DL, 8-30
Runge Kutta, 15-12
Release 12.0 c ANSYS, Inc. January 29, 2009
Index
S2S radiation model, see also radiative
heat transfer
advantages, 5-11
clustering, 5-45
equations, 5-43
gray-diffuse model, 5-43
limitations, 5-11
theory, 5-43
Saffman’s lift force, 15-5
saving
data files, see also automatic file saving
scalar dissipation, 8-28
scalar transport equations, 1-5
scale, color, see colormap
scattering, 5-49
phase function
Delta-Eddington, 5-29
linear-anisotropic, 5-14, 5-18, 5-29
user-defined, 5-29
Schiller and Naumann model, 16-50
Schmidt number, 7-3
Schnerr and Sauer
cavitation model, 16-99
second-order accuracy, 18-12
secondary breakup
discrete phase, 15-77
secondary mixture fraction, 8-3
sedimentation, 16-3, 16-5–16-7
segregated algorithm, 18-2, 18-3
segregated solver
density interpolation schemes, 18-28
frozen flux formulation, 18-38
pressure interpolation schemes, 18-26
selective noncatalytic reduction
(SNCR), 13-30
ammonia injection, 13-30
urea injection, 13-32
semi-transparent interior walls, 5-33
semi-transparent media, 5-32
semi-transparent walls, 5-50
sensible enthalpy, 5-2
sequential solution, 18-2, 18-3
seven-step reduced mechanism, 13-33
Release 12.0 c ANSYS, Inc. January 29, 2009
shell conduction
DO/energy coupling, 5-25
shock waves, 19-9
SIMPLE algorithm, 18-30
simple-effectiveness-model, 6-1
features, 6-4
restrictions, 6-4
SIMPLEC algorithm, 18-31
skewness correction, 18-31
Singhal et al.
cavitation model, 16-95
single rotating reference frame, 2-6
site species, 7-14
Six DOF solver, 3-11
size functions, local remeshing using, 3-26
skewness
correction, 18-31, 18-32
skewness-neighbor coupling, 18-32
sliding meshes, 3-4
constraints, 3-8
initial conditions for, 2-9
mesh interface shapes, 3-8
mesh setup, 3-6
theory, 3-10
slip velocity, 16-33
sloshing, 16-6
slow-chemistry flames, 8-33
slug flow, 16-2, 16-5, 16-7
slurry flow, 16-3, 16-5, 16-7
Smagorinsky-Lilly subgrid-scale
model, 4-65
smoother
Gauss-Seidel, 18-62
ILU, 18-63
smoothing, 5-46
boundary layer, 3-14
residuals, 18-47
solid decomposition reactions, 7-21
solid deposition reactions, 7-21
solid species, 7-14
solid zone
convection in a moving, 5-5
solid-solid reactions, 7-20
Index-17
Index
solidification and melting, 17-1
limitations, 17-2
overview, 17-1
theory, 17-3
solids pressure, 16-57
radial distribution function, 16-59
solution, see also calculations, solver, 18-1
accuracy, 18-10
numerical scheme, 18-1
process, 18-1
under-relaxation, 18-35
solver, see also calculations, solution, 18-1
density-based, 18-5, 18-40
explicit, 18-7
implicit, 18-7
differentiable limiter, 18-25
discretization, 18-10
gradient limiters, 18-23
differentiable limiter, 18-25
multidimensional limiter, 18-24
standard limiter, 18-24
Green-Gauss cell-based, 18-21
Green-Gauss node-based, 18-21
least squares cell-based, 18-22
linearization
explicit, 18-6
implicit, 18-6
multi-stage scheme, 18-46
multidimensional limiter, 18-24
multigrid, 18-9, 18-51
algebraic (AMG), 18-51, 18-57
full (FMG), 18-66
full (FMG), limitations on, 18-67
full-approximation storage
(FAS), 18-51, 18-64
node vs. cell discretization, 18-20
numerical scheme, 18-1
overview of, 18-1
pressure-based, 18-2, 18-3, 18-25
standard limiter, 18-24
soot model, 13-47
coal-derived, 13-54
Moss-Brookes, 13-52
Index-18
coal-derived soot extension, 13-54
turbulence-chemistry
interaction, 13-58
Moss-Brookes-Hall, 13-56
turbulence-chemistry
interaction, 13-58
one-step, 13-48
radiation effects, 5-48
restrictions, 13-48
theory, 13-48
two-step, 13-50
source terms
heterogeneous reactions, 16-109
SOx model, 13-39
coal, 13-44
formation, 13-39, 13-40
gaseous fuel, 13-44
liquid fuel, 13-44
PDF functions in, 13-46
turbulence-chemistry interaction, 13-45
Spalart-Allmaras
RANS model, 4-59
Spalart-Allmaras model, 4-6
spark model, 12-1
limitations, 12-1
overview, 12-1
species, see also product formation
diffusion, 5-4, 7-2
slow-forming product, 8-8
sources, 7-11
transport, 7-1
species diffusion terms, 5-4
species transport
multiphase, 16-107
heterogeneous reactions, 16-109
limitations, 16-108
momentum transfer, 16-108
specular boundaries, 5-50
specular semi-transparent walls, 5-34
specular walls, 5-50
spray modeling
atomizers, 15-60
breakup, 15-77
Release 12.0 c ANSYS, Inc. January 29, 2009
Index
droplet collision, 15-86
dynamic drag, 15-16
wall-film, 15-47
wall-jet, 15-46
spring-based smoothing method, 3-12
SST k-ω
RANS model, 4-61
SST k-ω model, 4-31
SST transition model, 4-41
stability, 18-35
stagnation pressure, 1-18
stagnation temperature, 1-18
standard deviation, 20-7
on a surface, 20-10
standard k- model, 4-12
standard k-ω model, 4-26
standard limiter, 18-24
steady laminar flamelet model,
see also flamelet model, 8-32
assumptions and limitations, 8-32
introduction, 8-33
non-adiabatic, 8-35
stiff chemistry
multiphase, 16-111
stochastic particle tracking, 15-6
stoichiometric ratio, 8-7
Stokes number, 16-10
Stokes-Cunningham law, 15-16
strain rate, 8-28
stratified flow, 16-2, 16-5–16-7
streamwise-periodic flow, 1-7
stretch factor, 9-7
sub-micron particles, 15-5, 15-16
subgrid-scale models, 4-64
dynamic kinetic energy model, 4-67
dynamic Smagorinsky-Lilly model, 4-66
Smagorinsky-Lilly model, 4-65
WALE model, 4-67
subsonic, 1-18
supersonic, 1-18
surface coverage reaction
rate modification, 7-13
surface deposition, 7-14
Release 12.0 c ANSYS, Inc. January 29, 2009
surface integrals, 20-6
area, 20-7
area-weighted average, 20-8
computing, 20-7
facet field variables, 20-9
facet maximum, 20-9
facet minimum, 20-9
field variable sum, 20-9
flow rate, 20-8
integral, 20-7
mass flow rate, 20-8
mass-weighted average, 20-8
standard deviation, 20-10
vertex field variables, 20-9
vertex maximum, 20-10
vertex minimum, 20-10
volume flow rate, 20-10
surface integration, 20-6
surface reactions, see particle surface reactions, wall surface reactions
surface tension, 16-22
surface-to-surface (S2S) radiation model,
see also radiative heat
transfer, 5-8
advantages, 5-11
clustering, 5-45
equations, 5-43
gray-diffuse model, 5-43
limitations, 5-11
theory, 5-43
surfaces
computing integrals, 20-7
swelling
coefficient, 15-35
swirl velocity, 1-13
swirling flows, see also rotating flows, 1-11,
18-26
overview, 1-11
physics of, 1-14
rotating reference frame, 1-14
swirl velocity, 1-13
Index-19
Index
three-dimensional, 1-13
turbulence modeling in, 4-14, 4-16,
4-19, 4-49
Syamlal-O’Brien model, 16-52
symmetric model, 16-51
choosing a model, 4-3
compressibility effects, 4-24
DES model, 4-58
discrete phase interaction, 15-6
enhanced wall functions, 4-84
k- model, 4-11
TAB model, 15-78
realizable, 4-18
tar, 13-54
RNG, 4-14
Taylor analogy breakup model, 15-78
standard, 4-12
Taylor-Foster approximation, 5-49
k-kl-ω model
temporal discretization, 18-35, 18-46, 18-48
transition, 4-37
solver, 18-18
k-ω model
termination criteria, 18-61
SST, 4-31
text user interface, see also text interface
standard, 4-26
thermal conductivity
large eddy simulation (LES), 4-61
anisotropic, 5-6
mesh considerations for, 19-16
thermal mixing, 5-2
modeling, 4-1, 4-5
thermophoretic force, 15-4
in multiphase flows, 16-43
third-body efficiencies, 7-6
near-wall treatments, 4-71
third-order MUSCL scheme, 18-16
no perturbations, 4-68
time advancement schemes, 18-36
production, 4-8, 4-22
time step, 18-49
realizable k- model, 4-18
discrete phase, 15-91
Reynolds stress model (RSM), 4-48
time stepping
RNG k- model, 4-14
dual, 18-19, 18-49
Spalart-Allmaras model, 4-6
explicit, 18-19, 18-48
spectral synthesizer, 4-70
global, 18-19
SST k-ω model, 4-31
implicit, 18-19, 18-49
SST transition model, 4-41
torque, 20-5
standard k- model, 4-12
total pressure, 1-18
standard k-ω model, 4-26
total temperature, 1-18
two-layer model, 4-73, 4-82
trajectory calculations, 15-2
v 2 -f model, 4-47
transient flows, see time-dependent
vortex method, 4-69
problems
wall functions, 4-73, 4-74
translating
limitations of, 4-81
reference frames, 2-8
non-equilibrium, 4-79
transonic, 1-18
standard, 4-74
transport equations
turbulence-chemistry interaction, 7-9, 8-2,
user-defined scalar, 1-5
8-8, 13-36
trapezoidal Euler scheme, 15-12
NOx, 13-36
TUI, see also text interface
soot, 13-58
turbulence, 4-1
k-kl-ω transition model, 4-37
SOx, 13-45
buoyancy effects, 4-23, 4-55
Index-20
Release 12.0 c ANSYS, Inc. January 29, 2009
Index
v 2 -f model, 4-47
V-cycle multigrid, 18-54, 18-56
vaporization, 15-19, 15-21, 15-25
temperature, 15-19
velocity, see also absolute velocity, relative
velocity
swirl, 1-13
view factors, 5-44
UDS
virtual mass force, 15-3, 16-46
isotropic diffusivity, 1-5
viscosity
UDS transport equations, 1-5
turbulent, see turbulent viscosity
about, 1-5
viscous dissipation, 5-4
anisotropic diffusivity, 1-5
viscous dissipation terms, 5-4
diffusion coefficient, 1-5
VOF
model, see volume of fluid (VOF)
multiphase flows, 1-6
model
multiphase mass flux, 1-6
volatile fraction, 15-19
single phase flow, 1-5
volatiles, 13-21, 13-23, 13-45
unburnt mixture, 9-3
volume adaption, 19-15
under-relaxation, 18-35
volume flow rate, 20-7
discrete phase, 15-93
through a surface, 20-10
unsteady flows, see also time-dependent
volume fraction, 16-6, 16-43
problems
in Eulerian multiphase model, 16-43
unsteady laminar flamelet model, see also
in mixture model, 16-35
flamelet model, 8-36
in VOF model, 16-15
diesel approach, 8-39
volume integrals
Eulerian approach, 8-36
computing, 20-12
upwind schemes, 18-10
mass-weighted average, 20-13
first-order, 18-10
mass-weighted integral, 20-12
second-order, 18-12
sum, 20-12
urea
volume-weighted average, 20-12
injection, 13-32
volume integration, 20-11
production, 13-34
volume of fluid (VOF) model,
seven-step reduced mechanism, 13-33
see also multiphase flow, 16-6
user-defined functions (UDFs), see also
CICSAM, 16-20
UDF Manual
donor-acceptor scheme, 16-19
in multiphase models, 16-7
explicit scheme, 16-16
user-defined mass flux, 1-6
user-defined scalar (UDS) equations, 1-5
geometric reconstruction scheme, 16-19
user-defined scalars
implicit scheme, 16-16
theory, multiphase flow, 1-6
interpolation, 16-17
theory, single phase flow, 1-5
CICSAM, 16-20
using the manual, UTM-1
donor-acceptor scheme, 16-19
utilities, see filters
explicit scheme, 16-16
turbulent viscosity
in the k- model, 4-13
two-layer model, 4-73, 4-82
two-step soot formation model
theory, 13-50
2.5D surface remeshing method, 3-24
Release 12.0 c ANSYS, Inc. January 29, 2009
Index-21
Index
geometric reconstruction
scheme, 16-19
implicit scheme, 16-16
limitations, 16-14
mass transfer, 16-89
momentum equation, 16-21
open channel flow, 16-25
overview, 16-14
properties, 16-20
steady-state calculations, 16-15
surface tension, 16-22
theory, 16-13
time-dependent calculations, 16-15
volume fraction, 16-15
wall adhesion, 16-25
volumetric heat sources, 5-5
WSGGM, see weighted-sum-of-gray-gases
model (WSGGM)
y ∗ , 4-75
adaption, 19-16
+
y , 4-75
adaption, 19-16
zones
deforming, 3-11
moving, 2-1, 3-4
Zwart-Gerber-Belamri
cavitation model, 16-97
W-cycle multigrid, 18-54, 18-56
WALE subgrid-scale model, 4-67
wall
adhesion, 16-25
functions, 4-73, 4-74
limitations of, 4-78, 4-81
non-equilibrium, 4-79
standard, 4-74
rotation, 1-15
wall damping, 9-8
wall surface reactions, 7-11
boundary conditions, 7-14
reaction rate, 7-12
site species, 7-14
solid species, 7-14
wave breakup model, 15-83
wavelength bands, 5-23
Weber number, 15-67, 16-24
weighted-sum-of-gray-gases model
(WSGGM), 5-13
combusting flows, 5-46
mean beam length, 5-47
Wen and Yu model, 16-53
wet steam multiphase model
limitations, 16-83
properties, 16-87
theory, 16-82
Index-22
Release 12.0 c ANSYS, Inc. January 29, 2009
Source Exif Data:
File Type : PDF File Type Extension : pdf MIME Type : application/pdf PDF Version : 1.6 Linearized : No Encryption : Standard V2.3 (128-bit) User Access : Print, Extract, Print high-res Author : ANSYS, Inc. Subject : Modify Date : 2009:03:12 15:18:23-04:00 Create Date : 2009:01:29 17:51:00Z Page Mode : UseOutlines Page Count : 816 XMP Toolkit : 3.1-702 Creator Tool : TeX Metadata Date : 2009:03:12 15:18:23-04:00 Format : application/pdf Description : Creator : ANSYS, Inc. Title : Keywords : Producer : pdfTeX14.h Document ID : uuid:2b5d659e-f6f4-4183-b9a2-c2d1d04f8b21 Instance ID : uuid:f77ea6e1-9950-407a-beb7-8e09d5570a3bEXIF Metadata provided by EXIF.tools