FLUENT 6.0 Tutorial Guide Volume 2
December 2001
Licensee acknowledges that use of Fluent Inc.’s products can only provide an imprecise estimation of possible future performance and that additional testing and analysis, independent of the Licensor’s products, must be conducted before any product can be finally developed or commercially introduced. As a result, Licensee agrees that it will not rely upon the results of any usage of Fluent Inc.’s products in determining the final design, composition or structure of any product.
c 2001 by Fluent Inc. Copyright All rights reserved. No part of this document may be reproduced or otherwise used in any form without express written permission from Fluent Inc.
Airpak, FIDAP , FLUENT, GAMBIT , Icepak, MixSim , and POLYFLOW are registered trademarks of Fluent Inc. All other products or name brands are trademarks of their respective holders.
Fluent Inc. Centerra Resource Park 10 Cavendish Court Lebanon, NH 03766
Contents
Volume 1 1 Introduction to Using FLUENT
1-1
2 Modeling Periodic Flow and Heat Transfer
2-1
3 Modeling External Compressible Flow
3-1
4 Modeling Unsteady Compressible Flow
4-1
5 Modeling Radiation and Natural Convection
5-1
6 Using a Non-Conformal Mesh
6-1
7 Using a Single Rotating Reference Frame
7-1
8 Using Multiple Rotating Reference Frames
8-1
9 Using the Mixing Plane Model
9-1
10 Using Sliding Meshes
10-1
⇒ Volume 2 11 Modeling Species Transport and Gaseous Combustion 11-1 12 Using the Non-Premixed Combustion Model
c Fluent Inc. November 27, 2001
12-1 i
CONTENTS
13 Modeling Surface Chemistry
13-1
14 Modeling Evaporating Liquid Spray
14-1
15 Using the VOF Model
15-1
16 Modeling Cavitation
16-1
17 Using the Mixture and Eulerian Multiphase Models
17-1
18 Using the Eulerian Multiphase Model for Granular Flow 18-1
ii
19 Modeling Solidification
19-1
20 Postprocessing
20-1
21 Turbo Postprocessing
21-1
22 Parallel Processing
22-1
c Fluent Inc. November 27, 2001
Tutorial 11. Modeling Species Transport and Gaseous Combustion Introduction: This tutorial examines chemical species mixing and combustion of a gaseous fuel. A cylindrical combustor burning methane (CH4 ) in air is studied using the finite-rate chemistry model in FLUENT. In this tutorial you will learn how to: • Enable physical models, select material properties, and define boundary conditions for a turbulent flow with chemical species mixing and reaction • Initiate and solve the combustion simulation using the segregated solver • Compare the results computed with constant and variable specific heat • Examine the reacting flow results using graphics • Predict thermal and prompt NOx production • Use custom field functions to compute NO parts per million Prerequisites: This tutorial assumes that you have performed Tutorial 1 and are familiar with the FLUENT interface. It also assumes that you have developed a basic familiarity with the solution of turbulent flows using FLUENT. You may find it helpful to read about chemical reaction modeling in the User’s Guide. Otherwise, no previous experience with chemical reaction or combustion modeling is assumed. Problem Description: The cylindrical combustor considered in this tutorial is shown in Figure 11.1. The flame considered is a turbulent diffusion flame. A small nozzle in the center of the combustor
c Fluent Inc. November 27, 2001
11-1
Modeling Species Transport and Gaseous Combustion
Wall: 300K
0.005m
Air, 0.5 m/s, 300K
Methane, 80 m/s, 300K
0.225 m
introduces methane at 80 m/s. Ambient air enters the combustor coaxially at 0.5 m/s. The overall equivalence ratio is approximately 0.76 (about 28% excess air). The high-speed methane jet initially expands with little interference from the outer wall, and entrains and mixes with the low-speed air. The Reynolds number based on the methane jet diameter is approximately 5.7 × 103 .
L
C 1.8 m
Figure 11.1: Combustion of Methane Gas in a Turbulent Diffusion Flame Furnace
Background: In this tutorial, you will use the generalized finite-rate chemistry model to analyze the methane-air combustion system. The combustion will be modeled using a global one-step reaction mechanism, assuming complete conversion of the fuel to CO2 and H2 O. The reaction equation is CH4 + 2O2 → CO2 + 2H2 O
(11.1)
This reaction will be defined in terms of stoichiometric coefficients, formation enthalpies, and parameters that control the reaction rate. The reaction rate will be determined assuming that turbulent mixing is the rate-limiting process, with the turbulence-chemistry interaction modeled using the eddy-dissipation model. 11-2
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
Preparation 1. Copy the file gascomb/gascomb.msh from the FLUENT documentation CD to your working directory (as described in Tutorial 1). 2. Start the 2D version of FLUENT.
Step 1: Grid 1. Read the grid file gascomb.msh. File −→ Read −→Case... After reading the grid file, FLUENT will report that 1615 quadrilateral fluid cells have been read, along with a number of boundary faces with different zone identifiers. 2. Check the grid. Grid −→Check The grid check lists the minimum and maximum x and y values from the grid, and reports on a number of other grid features that are checked. Any errors in the grid would be reported at this time. For instance, the cell volumes must never be negative. Note that the domain extents are reported in units of meters, the default unit of length in FLUENT. Since this grid was created in units of millimeters, the Scale Grid panel will be used to scale the grid into meters. 3. Scale the grid. Grid −→Scale... (a) Under Units Conversion, select mm from the drop-down list to complete the phrase Grid Was Created In mm. (b) Click on Scale and confirm that the maximum x and y values are 1.8 and 0.225 meters, respectively, as indicated in Figure 11.1.
c Fluent Inc. November 27, 2001
11-3
Modeling Species Transport and Gaseous Combustion
Note: Because the default SI units will be used in this tutorial, there is no need to change any units in this problem. 4. Display the grid. Display −→Grid...
Grid
Feb 05, 2001 FLUENT 6.0 (2d, segregated, lam)
Figure 11.2: The Quadrilateral Grid for the Combustor Model
Extra: You can use the right mouse button to check which zone number corresponds to each boundary. If you click the right mouse button on one of the boundaries in the graphics window, its zone number, name, and type will be printed in the FLUENTconsole window. This feature is especially useful when you have several zones of the same type and you want to distinguish between them quickly.
11-4
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
Step 2: Models 1. Define the domain as axisymmetric, and keep the default (segregated) solver. Define −→ Models −→Solver...
c Fluent Inc. November 27, 2001
11-5
Modeling Species Transport and Gaseous Combustion
2. Enable the k- turbulence model. Define −→ Models −→Viscous...
The panel will expand to provide further options. Click OK to accept the default Standard model and parameters.
11-6
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
3. Enable heat transfer by activating the energy equation. Define −→ Models −→Energy...
c Fluent Inc. November 27, 2001
11-7
Modeling Species Transport and Gaseous Combustion
4. Enable chemical species transport and reaction. Define −→ Models −→Species...
(a) Select Species Transport under Model. (b) Select Volumetric under Reactions. (c) Choose methane-air in the Mixture Material drop-down list. The Mixture Material list contains the set of chemical mixtures that exist in the FLUENT database. By selecting one of the pre-defined mixtures, you are accessing a complete description of the reacting system. The chemical species in the system and their physical and thermodynamic properties are defined by your selection of the mixture material. You can alter the mixture material selection or modify the mixture material properties using the Materials panel (see Step 3: Materials).
11-8
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
(d) Select Eddy-Dissipation under Turbulence-Chemistry Interaction. The eddy-dissipation model computes the rate of reaction under the assumption that chemical kinetics are fast compared to the rate at which reactants are mixed by turbulent fluctuations (eddies). (e) Click OK. After you click OK in the Species Model panel, a warning about the symmetry zone will appear in the console window: Warning: It appears that symmetry zone 5 should actually be an axis (it has faces with zero area projections). Unless you change the zone type from symmetry to axis, you may not be able to continue the solution without encountering floating point errors.
In this axisymmetric model, the centerline should be treated using the axis boundary condition instead of symmetry. You will change the symmetry zone to an axis boundary in Step 4: Boundary Conditions. The console window will also list the properties that are required for the models you have enabled. You will see an Information dialog box, reminding you to confirm the property values that have been extracted from the database.
(f) Click OK to continue.
c Fluent Inc. November 27, 2001
11-9
Modeling Species Transport and Gaseous Combustion
Step 3: Materials Define −→Materials...
The Materials panel shows the mixture material, methane-air, that was enabled in the Species Model panel. The properties for this mixture material have been copied from the FLUENT database and can be modified by you. Here, you will modify the default setting for the mixture by enabling the gas law. By default, the mixture material uses constant properties: you will retain this constant property assumption for now, allowing only the mixture density to vary with temperature and composition. The influence 11-10
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
of variable property inputs on the combustion prediction will be examined in a later part of this tutorial. 1. Retain incompressible-ideal-gas in the Density drop-down list. 2. Click the Edit... button to the right of Mixture Species. This opens the Species panel.
You can add or remove species from the mixture material using this panel. Here, the species that make up the methane-air mixture are predefined and require no modification. 3. Click Cancel to close the panel without making any changes. 4. In the Materials panel, click the Edit... button to the right of the Reaction drop-down list. This will open the Reactions panel.
c Fluent Inc. November 27, 2001
11-11
Modeling Species Transport and Gaseous Combustion
The eddy-dissipation reaction model ignores chemical kinetics (the Arrhenius rate) and uses only the Mixing Rate parameters in the Reactions panel. The Arrhenius Rate section of the panel is therefore inactive. (The Rate Exponent and Arrhenius Rate entries are included in the database and are employed when the alternate finite-
11-12
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
rate/eddy-dissipation model is used.) See the User’s Guide for details. 5. Accept the default settings for the Mixing Rate constants by clicking the OK button. 6. Use the scroll bar to review the remaining properties. Click on the Change/Create button to accept the material property settings and then Close the panel.
As noted above, the initial calculation will be performed assuming that all properties except density are constant. Using constant transport proper-
c Fluent Inc. November 27, 2001
11-13
Modeling Species Transport and Gaseous Combustion
ties (viscosity, thermal conductivity, and mass diffusion coefficients) is acceptable here because the flow is fully turbulent. The molecular transport properties will play a minor role compared to turbulent transport. The assumption of constant specific heat, in contrast, has a strong effect on the combustion solution, and you will change this property definition in Step 6: Solution Using Non-Constant Heat Capacity.
11-14
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
Step 4: Boundary Conditions 1. Convert the symmetry zone to the axis type. The symmetry zone must be converted to an axis to prevent numerical difficulties where the radius goes to zero. Define −→Boundary Conditions...
(a) Select symmetry-5 in the Zone list and then select axis in the Type list.
c Fluent Inc. November 27, 2001
11-15
Modeling Species Transport and Gaseous Combustion
You will be prompted to accept the change of boundary type:
(b) Click Yes to confirm the change.
(c) In the resulting Axis panel, click OK to accept the default axis zone name. 2. Set the boundary conditions for the air inlet, velocity-inlet-8. Hint: Redisplay the grid without the fluid zone. This will show the boundaries. Use the right mouse button to probe the air inlet. The console window and the Boundary Conditions panel will show that the air inlet is labeled velocity-inlet-8.
11-16
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
(a) Rename the boundary air-inlet in the Zone Name text entry box. (b) Set the boundary conditions at the air inlet as shown in the panel.
c Fluent Inc. November 27, 2001
11-17
Modeling Species Transport and Gaseous Combustion
3. Set the fuel inlet boundary conditions for velocity-inlet-6.
(a) Rename this zone fuel-inlet and assign inlet conditions as shown in the panel.
11-18
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
4. Set the following conditions for the exit boundary, pressure-outlet-9:
Note: The Backflow values in this panel are utilized only when backflow occurs at the pressure outlet. Reasonable values should always be assigned, since backflow may occur during intermediate iterations and could affect the solution stability.
c Fluent Inc. November 27, 2001
11-19
Modeling Species Transport and Gaseous Combustion
5. Set the boundary conditions for the outer wall, wall-7. Hint: Use the mouse-probe method described above for the air inlet to determine which zone corresponds to the outer wall. The outer wall zone will be selected in the Boundary Conditions panel once the outer wall boundary is probed.
11-20
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
(a) Rename this boundary outer-wall in the Zone Name text entry box. (b) Set the thermal condition to Temperature and keep the default temperature of 300 K. (c) Retain the default settings in the Momentum and Species sections of the panel.
c Fluent Inc. November 27, 2001
11-21
Modeling Species Transport and Gaseous Combustion
6. Set the boundary conditions for wall-2, which represents the small fuel inlet nozzle.
(a) Rename this boundary nozzle in the Zone Name text entry box. (b) Accept the default thermal condition of Heat Flux with a value of zero (adiabatic wall). (c) Retain the default settings in the Momentum and Species sections of the panel.
11-22
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
Step 5: Initial Solution Using Constant Heat Capacity 1. Initialize the field variables. Solve −→ Initialize −→Initialize...
(a) Select all-zones in the Compute From drop-down list. (b) Adjust the Initial Values for Temperature to 2000 and ch4 Mass Fraction to 0.2. (c) Click Init to initialize the variables, and then close the panel. Initializing the flow using a high temperature and non-zero fuel content will allow the combustion reaction to begin. The initial condition acts as a numerical “spark” to ignite the methaneair mixture. This initialization is especially critical when you include finite-rate kinetics in the overall reaction rate.
c Fluent Inc. November 27, 2001
11-23
Modeling Species Transport and Gaseous Combustion
2. Set the under-relaxation factors. The default under-relaxation parameters in FLUENT are set to high values. For a combustion model it may be necessary to reduce the under-relaxation to stabilize the solution. Some experimentation is typically necessary to establish the optimal under-relaxation. For this tutorial it is sufficient to reduce the species under-relaxation to 0.9. Solve −→ Controls −→Solution...
(a) Use the slider bar next to the Under-Relaxation Factors list to locate each species and set its under-relaxation factor to 0.9.
11-24
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
3. Turn on residual plotting during the calculation. Solve −→ Monitors −→Residual...
(a) Under Options, select Plot. (b) Click OK.
c Fluent Inc. November 27, 2001
11-25
Modeling Species Transport and Gaseous Combustion
4. Save the case file (gascomb1.cas). File −→ Write −→Case... (a) Keep the Write Binary Files button on to produce a smaller, unformatted binary file. (b) Enter the file name gascomb1.cas in the Case File text entry box. (c) Click OK to proceed with the file writing. 5. Start the calculation by requesting 500 iterations. Solve −→Iterate...
The solution converges in about 300 iterations. 6. Save the case and data files (gascomb1.cas and gascomb1.dat). File −→ Write −→Case & Data... Note: FLUENT will ask you to confirm that the previous case file is to be overwritten.
11-26
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
7. Review the current state of the solution by viewing contours of temperature (Figure 11.3). Display −→Contours...
(a) Select Temperature... and Static Temperature in the Contours Of drop-down list. (b) Click Display. The temperature contours are shown in Figure 11.3. The peak temperature, predicted using a constant heat capacity of 1000 J/kg-K, is over 2900 K. This overprediction of the flame temperature can be remedied by a more realistic model for the temperature and composition dependence of the heat capacity, as illustrated in the next step of the tutorial.
c Fluent Inc. November 27, 2001
11-27
Modeling Species Transport and Gaseous Combustion
2.94e+03 2.67e+03 2.41e+03 2.14e+03 1.88e+03 1.62e+03 1.35e+03 1.09e+03 8.27e+02 5.64e+02 3.00e+02
Contours of Static Temperature (k)
Jun 05, 2001 FLUENT 6.0 (axi, segregated, spe5, ske)
Figure 11.3: Temperature Contours: Constant cp
11-28
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
Step 6: Solution Using Non-Constant Heat Capacity As noted above, the strong temperature and composition dependence of the specific heat will have a significant impact on the predicted flame temperature. In this step you will use the temperature-varying property information in the FLUENT database to recompute the solution. 1. Enable composition dependence of the specific heat. Define −→Materials...
c Fluent Inc. November 27, 2001
11-29
Modeling Species Transport and Gaseous Combustion
(a) In the drop-down list next to Cp, select mixing-law as the specific heat method. (b) Click on the Change/Create button to render the mixture specific heat based on a local mass-fraction-weighted average of all the species. 2. Enable temperature dependence of the specific heat for each species.
11-30
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
(a) In the Material Type drop-down list, select fluid. The fluid material type gives you access to each species in the mixture. (b) Select carbon-dioxide (co2) under Fluid Materials. (c) In the drop-down list for Cp, select piecewise-polynomial. This will open the Piecewise Polynomial Profile panel.
i. Click OK to accept the default coefficients describing the temperature variation of cp for carbon dioxide. The default coefficients describe the polynomial cp (T ) and are extracted from the FLUENT property database. ii. Click on Change/Create in the Materials panel to accept the change in properties for CO2 . (d) Repeat steps (b) and (c) above for the remaining species (CH4 , N2 , O2 , and H2 O). Remember to click on Change/ Create to accept the change for each species.
c Fluent Inc. November 27, 2001
11-31
Modeling Species Transport and Gaseous Combustion
3. Request 500 more iterations. Solve −→Iterate... Note: The residuals will jump significantly as the solution adjusts to the new specific heat representation. The solution converges after about 250 additional iterations. 4. Save the new case and data files (gascomb2.cas and gascomb2.dat). File −→ Write −→Case & Data...
11-32
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
Step 7: Postprocessing Review the solution by examining graphical displays of the results and performing surface integrations at the combustor exit. 1. View contours of temperature (Figure 11.4). Display −→Contours... (a) Select Temperature... and Static Temperature in the Contours Of drop-down list. (b) Click Display. The temperature contours are shown in Figure 11.4. The peak temperature has dropped to about 2200 K as a result of the temperatureand composition-dependent specific heat. 2.23e+03 2.04e+03 1.85e+03 1.65e+03 1.46e+03 1.27e+03 1.07e+03 8.79e+02 6.86e+02 4.93e+02 3.00e+02
Contours of Static Temperature (k)
Jun 05, 2001 FLUENT 6.0 (axi, segregated, spe5, ske)
Figure 11.4: Temperature Contours: Variable cp
c Fluent Inc. November 27, 2001
11-33
Modeling Species Transport and Gaseous Combustion
2. Plot contours of specific heat (Figure 11.5). Contours of the mixture specific heat will show how it varies through the domain. Display −→Contours... (a) Select Properties... and Specific Heat (Cp) in the Contours Of drop-down list. (b) Click Display. The contours are shown in Figure 11.5. The mixture specific heat is largest where the CH4 is concentrated, near the fuel inlet, and where the temperature and combustion product concentrations are large. The increase in heat capacity, relative to the constant value used before, substantially lowers the peak flame temperature. 2.80e+03 2.62e+03 2.44e+03 2.26e+03 2.08e+03 1.90e+03 1.72e+03 1.55e+03 1.37e+03 1.19e+03 1.01e+03
Contours of Specific Heat (Cp) (j/kg-k)
Jun 05, 2001 FLUENT 6.0 (axi, segregated, spe5, ske)
Figure 11.5: Contours of Specific Heat
11-34
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
3. Display velocity vectors (Figure 11.6). Display −→Vectors...
(a) Click the Vector Options... button. This opens the Vector Options panel.
c Fluent Inc. November 27, 2001
11-35
Modeling Species Transport and Gaseous Combustion
(b) Select the Fixed Length option and click Apply. The fixed length option is useful when the vector magnitude varies dramatically. With fixed length vectors, the velocity magnitude is described only by color instead of by both vector length and color. (c) In the Vectors panel, reset the Scale to 0.01 and click Display. The velocity vectors are shown in Figure 11.6.
11-36
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
8.24e+01 7.42e+01 6.60e+01 5.78e+01 4.96e+01 4.14e+01 3.32e+01 2.50e+01 1.68e+01 8.57e+00 3.66e-01
Velocity Vectors Colored By Velocity Magnitude (m/s)
Jun 05, 2001 FLUENT 6.0 (axi, segregated, spe5, ske)
Figure 11.6: Velocity Vectors: Variable cp
c Fluent Inc. November 27, 2001
11-37
Modeling Species Transport and Gaseous Combustion
4. Plot contours of stream function (Figure 11.7). Display −→Contours...
(a) Select Velocity... and Stream Function in the Contours Of dropdown list. (b) Click Display. The stream function contours are shown in Figure 11.7. The entrainment of air into the high-velocity methane jet is clearly visible in the streamline display.
11-38
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
1.55e-02 1.39e-02 1.24e-02 1.08e-02 9.27e-03 7.73e-03 6.18e-03 4.64e-03 3.09e-03 1.55e-03 0.00e+00
Contours of Stream Function (kg/s)
Jun 05, 2001 FLUENT 6.0 (axi, segregated, spe5, ske)
Figure 11.7: Stream Function Contours: Variable cp
c Fluent Inc. November 27, 2001
11-39
Modeling Species Transport and Gaseous Combustion
5. Plot contours of mass fraction for each species. Display −→Contours... (a) Select Species... and Mass fraction of ch4 in the Contours Of drop-down list. (b) Turn on the Filled button under Options. (c) Click Display. The CH4 mass fraction contours are shown in Figure 11.8. (d) Repeat for the remaining species. The mass fraction contours for O2 , CO2 , and H2 O are shown in Figures 11.9, 11.10, and 11.11. 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 0.00e+00
Contours of Mass fraction of ch4
Jun 05, 2001 FLUENT 6.0 (axi, segregated, spe5, ske)
Figure 11.8: CH4 Mass Fraction
11-40
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
2.30e-01 2.07e-01 1.84e-01 1.61e-01 1.38e-01 1.15e-01 9.20e-02 6.90e-02 4.60e-02 2.30e-02 0.00e+00
Contours of Mass fraction of o2
Jun 05, 2001 FLUENT 6.0 (axi, segregated, spe5, ske)
Figure 11.9: O2 Mass Fraction
1.46e-01 1.31e-01 1.17e-01 1.02e-01 8.76e-02 7.30e-02 5.84e-02 4.38e-02 2.92e-02 1.46e-02 0.00e+00
Contours of Mass fraction of co2
Jun 05, 2001 FLUENT 6.0 (axi, segregated, spe5, ske)
Figure 11.10: CO2 Mass Fraction
c Fluent Inc. November 27, 2001
11-41
Modeling Species Transport and Gaseous Combustion
1.20e-01 1.08e-01 9.56e-02 8.37e-02 7.17e-02 5.98e-02 4.78e-02 3.59e-02 2.39e-02 1.20e-02 0.00e+00
Contours of Mass fraction of h2o
Jun 05, 2001 FLUENT 6.0 (axi, segregated, spe5, ske)
Figure 11.11: H2 O Mass Fraction
11-42
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
6. Determine the average exit temperature and velocity. Report −→Surface Integrals...
(a) Select Mass-Weighted Average in the Report Type drop-down list. (b) Select Temperature... and Static Temperature in the Field Variable drop-down list. The mass-averaged temperature will be computed as R
~ T ρ~v · dA T = R ~ ρ~v · dA
(11.2)
(c) Select pressure-outlet-9 as the surface over which to perform the integration. (d) Click Compute. The mass-weighted average exit temperature is about 1775 K.
c Fluent Inc. November 27, 2001
11-43
Modeling Species Transport and Gaseous Combustion
(e) Select Area-Weighted Average as the Report Type and Velocity Magnitude as the Field Variable. The area-weighted velocity-magnitude average will be computed as v¯ =
1 A
Z
v dA
(11.3)
(f) Click Compute. The area-averaged exit velocity is about 3.10 m/s.
11-44
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
Step 8: NOx Prediction In this section you will extend the FLUENT model to include the prediction of NOx . You will first calculate the formation of both thermal and prompt NOx , then calculate each separately to determine the contribution of each mechanism. 1. Enable the NOx model. Define −→ Models −→ Pollutants −→NOx...
(a) Under Models, enable Thermal NO and Prompt NO. (b) Select Temperature in the PDF Mode drop-down list under Turbulence Interaction to enable the turbulence-chemistry interaction. If turbulence interaction is not enabled, you will be computing NOx formation without considering the important influence of turbulent fluctuations on the time-averaged reaction rates.
c Fluent Inc. November 27, 2001
11-45
Modeling Species Transport and Gaseous Combustion
(c) Select Partial-equilibrium in the [O] Model drop down list under Thermal NO Parameters. The partial-equilibrium model is used to predict the O radical concentration required for thermal NOx prediction. (d) Set the Equivalence Ratio to 0.76 under Prompt NO Parameters, and keep the default Fuel Species and Fuel Carbon Number. The equivalence ratio defines the fuel-air ratio (relative to stoichiometric conditions) and is used in the calculation of prompt NOx formation. The Fuel Carbon Number is the number of carbon atoms per molecule of fuel and is used in the prompt NOx prediction. The Fuel Species designation is also used in the prompt NOx model. (e) Click OK to accept these changes.
11-46
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
2. Enable the calculation of only the NO species, and set the underrelaxation factor for this equation. Solve −→ Controls −→Solution...
(a) In the Equations list, deselect all variables except the NO species. (b) Increase the NO under-relaxation factor to 1.0. You will predict NOx formation in a “postprocessing” mode, with the flow field, temperature, and hydrocarbon combustion species concentrations fixed. Thus, only the NO equation is computed. Prediction of NO in this mode is justified on the grounds that the NO concentrations are very low and have negligible impact on the hydrocarbon combustion prediction.
c Fluent Inc. November 27, 2001
11-47
Modeling Species Transport and Gaseous Combustion
3. Reduce the convergence criterion for the NO species equation. Solve −→ Monitors −→Residual...
(a) Set the Convergence Criterion to 1e-6 and click OK. 4. Request 50 more iterations. Solve −→Iterate... The solution converges in about 10 iterations. 5. Save the new case and data files (gascomb3.cas and gascomb3.dat).
11-48
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
6. Review the solution by displaying contours of NO mass fraction (Figure 11.12). Display −→Contours... (a) Select NOx... and Mass fraction of NO in the Contours Of drop-down list. (b) Deselect Filled under Options and click Display. The NO mass fraction contours are shown in Figure 11.12. The peak concentration of NO is located in a region of high temperature where oxygen and nitrogen are available. 3.49e-03 3.14e-03 2.79e-03 2.44e-03 2.09e-03 1.74e-03 1.39e-03 1.05e-03 6.97e-04 3.49e-04 0.00e+00
Contours of Mass fraction of no
Jun 05, 2001 FLUENT 6.0 (axi, segregated, spe5, ske)
Figure 11.12: Contours of NO Mass Fraction: Prompt and Thermal NOx
c Fluent Inc. November 27, 2001
11-49
Modeling Species Transport and Gaseous Combustion
7. Calculate the average exit NO mass fraction. Report −→Surface Integrals...
(a) Select Mass-Weighted Average in the Report Type drop-down list and NOx... and Mass fraction of NO in the Field Variable drop-down list. (b) Select pressure-outlet-9 as the surface over which to perform the integration. (c) Click Compute. The mass-weighted average exit NO mass fraction is about 0.00309.
11-50
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
8. Disable the prompt NOx mechanism and solve for thermal NOx only. Define −→ Models −→ Pollutants −→NOx... (a) Turn off Prompt NO under Models to disable the prompt NOx mechanism, and click OK. (b) Request 50 iterations. Solve −→Iterate... The solution converges in about 10 iterations. (c) Review the thermal NOx solution by viewing contours of NO mass fraction (Figure 11.13). Display −→Contours... i. Check that NOx... and Mass fraction of NO are selected in the Contours Of drop-down list. ii. Click Display. The NO mass fraction contours are shown in Figure 11.13. The concentration of NO is slightly lower without the prompt NOx mechanism. (d) Compute the average exit NO mass fraction with only thermal NOx formation. Report −→Surface Integrals... Hint: Follow the same procedure you used earlier for the calculation with both thermal and prompt NOx formation. The mass-weighted average exit NO mass fraction, with thermal but no prompt NOx formation, is about 0.00305.
c Fluent Inc. November 27, 2001
11-51
Modeling Species Transport and Gaseous Combustion
3.46e-03 3.11e-03 2.77e-03 2.42e-03 2.08e-03 1.73e-03 1.38e-03 1.04e-03 6.92e-04 3.46e-04 0.00e+00
Contours of Mass fraction of no
Jun 05, 2001 FLUENT 6.0 (axi, segregated, spe5, ske)
Figure 11.13: Contours of NO Mass Fraction: Thermal NOx Formation
11-52
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
9. Solve for prompt NOx production only. Define −→ Models −→ Pollutants −→NOx... (a) Turn off Thermal NO and turn on Prompt NO under Models, and click OK. (b) Request 50 iterations. The solution converges in about 10 iterations. Solve −→Iterate... (c) Review the prompt NOx solution by viewing contours of NO mass fraction (Figure 11.14). Display −→Contours... The NO mass fraction contours are shown in Figure 11.14. The prompt NOx mechanism is most significant in fuel-rich flames. In this case the flame is lean and prompt NO production is low. 6.10e-05 5.49e-05 4.88e-05 4.27e-05 3.66e-05 3.05e-05 2.44e-05 1.83e-05 1.22e-05 6.10e-06 7.08e-29
Contours of Mass fraction of no
Jun 05, 2001 FLUENT 6.0 (axi, segregated, spe5, ske)
Figure 11.14: Contours of NO Mass Fraction: Prompt NOx Formation
c Fluent Inc. November 27, 2001
11-53
Modeling Species Transport and Gaseous Combustion
(d) Compute the average exit NO mass fraction with only prompt NOx formation. Report −→Surface Integrals... Hint: Follow the same procedure you used earlier for the calculation with both thermal and prompt NOx formation. The mass-weighted average exit NO mass fraction, with only prompt NOx formation, is about 0.000044. Note: The individual thermal and prompt NO mass fractions do not add up to the levels predicted with the two models combined. This is because reversible reactions are involved. NO produced in one reaction can be destroyed in another reaction.
11-54
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
10. Use a custom field function to compute NO parts per million (ppm). Define −→Custom Field Functions... NO ppm is computed from the following equation: NO ppm =
NO mole fraction × 106 1 − H2 O mole fraction
(11.4)
where
NO mole fraction =
NO mass fraction × mixture MW 30
(11.5)
and the mixture molecular weight is 1 mixture MW = X mass fraction i
(11.6)
MW
where MW is the molecular weight of each species. First you will create a function for Equation 11.6. Then you will substitute Equation 11.5 into Equation 11.4 and create a function for Equation 11.4.
c Fluent Inc. November 27, 2001
11-55
Modeling Species Transport and Gaseous Combustion
(a) Create a custom field function for the mixture molecular weight.
i. Click on the 1 calculator button, then on /, and then on (. ii. Select Species... and Mass fraction of ch4 in the Field Functions drop-down list. Click Select to add this variable to the field function Definition. iii. Click on / and then click on 1 and 6 to enter 16 (the molecular weight of methane). iv. Continue in this fashion to complete the definition of the mixture molecular weight field function. v. Enter bulk-mw in the New Function Name text entry box. vi. Click Define to add the new field function to the variable list.
11-56
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
(b) Create a field function for NO ppm.
i. Select NOx... and Mass fraction of NO in the Field Functions drop-down list. Click Select to add this variable to the field function Definition. ii. Click the × button to introduce the multiplication sign. iii. Select Custom Field Functions... and bulk-mw in the Field Functions drop-down list. Click Select to add this variable to the field function Definition. iv. Click on / and then click on 3 and 0 to enter 30 (the molecular weight of NO). v. Click the × button and then click on 1 and 0 to enter 10. vi. Click on y^x and then on 6. vii. Complete the definition of NO ppm as shown in the panel above. viii. Enter no-ppm in the New Function Name text entry box. ix. Click Define to add the new field function to the variable list.
c Fluent Inc. November 27, 2001
11-57
Modeling Species Transport and Gaseous Combustion
11. Plot contours of NO ppm (Figure 11.15). Display −→Contours... (a) Select Custom Field Functions... and no-ppm in the Contours Of drop-down list. (b) Click Display. The NO ppm contours are shown in Figure 11.15. The contours closely resemble the mass fraction contours (Figure 11.14), as expected. 6.80e+01 6.12e+01 5.44e+01 4.76e+01 4.08e+01 3.40e+01 2.72e+01 2.04e+01 1.36e+01 6.80e+00 6.80e-23
Contours of no-ppm
Jun 05, 2001 FLUENT 6.0 (axi, segregated, spe5, ske)
Figure 11.15: Contours of NO ppm: Prompt NOx Formation
11-58
c Fluent Inc. November 27, 2001
Modeling Species Transport and Gaseous Combustion
Summary: In this tutorial you used FLUENT to model the transport, mixing, and reaction of chemical species. The reaction system was defined by using and modifying a mixture-material entry in the FLUENT database. The procedures used here for simulation of hydrocarbon combustion can be applied to other reacting flow systems. This exercise illustrated the important role of the mixture heat capacity in the prediction of flame temperature. The combustion modeling results are summarized in the following table. (Note that some of the values in the table were not explicitly calculated during the tutorial.)
Constant cp Variable cp
Peak Temp. (K) 2935 2231
Exit Temp. (K) 2150 1775
Exit Velocity (m/s) 3.75 3.10
The use of a constant cp results in a significant overprediction of the peak temperature. The average exit temperature and velocity are also overpredicted. While the variable cp solution produces dramatic improvements in the predicted results, further improvements are possible by considering additional models and features available in FLUENT, as discussed below. The NOx production in this case was dominated by the thermal NO mechanism. This mechanism is very sensitive to temperature. Every effort should be made to ensure that the temperature solution is not overpredicted, since this will lead to unrealistically high predicted levels of NO. Further Improvements: Further improvements can be expected by including the effects of intermediate species and radiation, both of which will result in lower predicted combustion temperatures. The single-step reaction process used in this tutorial cannot account for the moderating effects of intermediate reaction products,
c Fluent Inc. November 27, 2001
11-59
Modeling Species Transport and Gaseous Combustion
such as CO and H2 . Multiple-step reactions can be used to address these species. If a multi-step Magnussen model is used, considerably more computational effort is required to solve for the additional species. Where applicable, the non-premixed combustion model can be used to account for intermediate species at a reduced computational cost. See the User’s Guide for more details on the non-premixed combustion model. Radiation heat transfer tends to make the temperature distribution more uniform, thereby lowering the peak temperature. In addition, radiation heat transfer to the wall can be very significant (especially here, with the wall temperature set at 300 K). The large influence of radiation can be anticipated by computing the Boltzmann number for the flow: Bo =
(ρUcp )inlet convection ∼ 3 radiation σTAF
where σ is the Boltzmann constant (5.729×10−8 W/m2 -K4 ) and TAF is the adiabatic flame temperature. For a quick estimate, assume ρ = 1 kg/m3 , U = 0.5 m/s, and cp = 1000 J/kg-K (the majority of the inflow is air). Assume TAF = 2000 K. The resulting Boltzmann number is Bo = 1.09, which shows that radiation is just about as important as convection for this problem. See the User’s Guide and Tutorial 5 for details on radiation modeling.
11-60
c Fluent Inc. November 27, 2001
Tutorial 12. Using the Non-Premixed Combustion Model
Introduction: A pulverized coal combustion simulation involves modeling a continuous gas phase flow field and its interaction with a discrete phase of coal particles. The coal particles, traveling through the gas, will devolatilize and undergo char combustion, creating a source of fuel for reaction in the gas phase. Reaction can be modeled using either the species transport model or the non-premixed combustion model. In this tutorial you will model a simplified coal combustion furnace using the non-premixed combustion model for the reaction chemistry. In this tutorial you will learn how to: • Prepare a PDF table for a pulverized coal fuel using the prePDF preprocessor • Define FLUENT inputs for non-premixed combustion chemistry modeling • Define a discrete second phase of coal particles • Solve a simulation involving reacting discrete phase coal particles The non-premixed combustion model uses a modeling approach that solves transport equations for one or two conserved scalars, the mixture fractions. Multiple chemical species, including radicals and intermediate species, may be included in the problem definition and their concentrations will be derived from the predicted mixture fraction distribution. Property data for the species are accessed through a chemical database and turbulence-chemistry interaction is modeled using a Beta or double-delta probability density function (PDF). See the User’s Guide for more detail on the non-premixed combustion modeling approach.
c Fluent Inc. November 27, 2001
12-1
Using the Non-Premixed Combustion Model
Prerequisites: This tutorial assumes that you are familiar with the menu structure in FLUENT, and that you have solved Tutorial 1 or its equivalent. Some steps in the setup and solution procedure will not be shown explicitly. Problem Description: The coal combustion system considered in this tutorial is a simple 10 m by 1 m two-dimensional duct depicted in Figure 12.1. Only half of the domain width is modeled because of symmetry. The inlet of the 2D duct is split into two streams. A high-speed stream near the center of the duct enters at 50 m/s and spans 0.125 m. The other stream enters at 15 m/s and spans 0.375 m. Both streams are air at 1500 K. Coal particles enter the furnace near the center of the high-speed stream with a mass flow rate of 0.1 kg/s (total flow rate in the furnace is 0.2 kg/s). The duct wall has a constant temperature of 1200 K. The Reynolds number based on the inlet dimension and the average inlet velocity is about 100,000. Thus, the flow is turbulent. Details regarding the coal composition and size distribution are included in Step 5: Models: Continuous (Gas) Phase and Step 8: Materials: Discrete Phase.
12-2
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
T = 1200 K w
Air: 15 m/s, 1500 K
0.5 m Coal Injection: 0.1 kg/s 0.125 m
Air: 50 m/s, 1500 K Symmetry Plane 10 m
Figure 12.1: 2D Furnace with Pulverized Coal Combustion
Preparation for prePDF 1. Start prePDF. When you use the non-premixed combustion model, you prepare a PDF file with the preprocessor, prePDF. The PDF file contains information that relates species concentrations and temperatures to the mixture fraction values, and is used by FLUENT to obtain these scalars during the solution procedure.
c Fluent Inc. November 27, 2001
12-3
Using the Non-Premixed Combustion Model
Step 1: Define the Preliminary Adiabatic System in prePDF 1. Define the prePDF model type. You can define either a single fuel stream, or a fuel stream plus a secondary stream. Enabling a secondary stream allows you to keep track of two mixture fractions. For coal combustion, this would allow you to track volatile matter (the secondary stream) separately from the char (fuel stream). In this tutorial, we will not follow this approach. Instead, we will model coal using a single mixture fraction. Setup −→Case...
(a) Under Heat transfer options, keep the default setting of Adiabatic. The coal combustor studied in this tutorial is a non-adiabatic system, with heat transfer at the combustor wall and heat 12-4
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
transfer to the coal particles from the gas. Therefore, a nonadiabatic combustion system must be considered in prePDF. Because non-adiabatic calculations are more time-consuming than those for adiabatic systems, you will start the prePDF setup by considering the results of an adiabatic system. By computing the PDF/equilibrium chemistry results for the adiabatic system, you will determine appropriate system parameters that will make the non-adiabatic calculation more efficient. Specifically, the adiabatic calculation will provide information on the peak (adiabatic) flame temperature, the stoichiometric mixture fraction, and the importance of individual components to the chemical system. This process of beginning with an adiabatic system calculation should be followed in all PDF calculations that ultimately require a non-adiabatic model. (b) Under Chemistry models, keep the default setting of Equilibrium Chemistry. In most PDF-based simulations, the Equilibrium Chemistry option is recommended. The Stoichiometric Reaction (mixed is burned) option requires less computation but is generally less accurate. The Laminar Flamelets option offers the ability to include aerodynamic strain induced non-equilibrium effects, such as super-equilibrium radical concentration and sub-equilibrium temperatures. This can be important for NOx prediction, but is excluded here. (c) Keep the default setting of the PDF models. The Beta PDF integration is always recommended because it is more accurate than the Delta PDF approach. (d) Under Empirically Defined Streams, enable the Fuel stream option. This will allow you to define the fuel stream using the empirical input option. The empirical input option allows you to define the composition in terms of atom fractions of H, C, N, and O, along with the lower heating value and heat capacity
c Fluent Inc. November 27, 2001
12-5
Using the Non-Premixed Combustion Model
of the fuel. This is a useful option when the ultimate analysis and heating value of the coal are known. (e) Click Apply and close the panel.
12-6
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
2. Define the chemical species in the system. The choice of which species to include depends on the fuel type and combustion system. Guidelines on this selection are provided in the FLUENT User’s Guide. Here, you will assume that the equilibrium system consists of 13 species: C, C(s), CH4 , CO, CO2 , H, H2 , H2 O, N, N2 , O, O2 , and OH. C, H, O, and N are included because the fuel stream will be defined in terms of these atom fractions, using the “empirical” input method. !
You should include both C and C(S) in the system when the empirical input option is used.
Setup −→ Species −→Define...
(a) Set the Maximum # of Species to 13. Use the up and down arrows to set the maximum number of species, or enter the number in the text field followed by . (b) Select the top species in the Defined Species list (initially labeled UNDEFINED).
c Fluent Inc. November 27, 2001
12-7
Using the Non-Premixed Combustion Model
(c) In the Database Species drop-down list, use the slider bar to scroll the list, and select C. The Defined Species list now shows C as the first entry. (d) Select the next species in the Defined Species list (or increment the Species # counter to 2). (e) In the Database Species drop-down list, use the slider bar to scroll the list, and select the next species (C(S)). (f) Repeat steps (d) and (e) until all 13 species are defined. (g) Click Apply and then close the panel. Note: In other combustion systems, you might want to include additional chemical species, but you should not add slow chemical species like NOx . 3. Determine the fuel composition inputs. The fuel considered here is known, from proximate analysis, to consist of 28% volatiles, 64% char, and 8% ash. You will use this information, along with the ultimate analysis given below, to define the coal composition in prePDF. The fuel stream composition (char and volatiles) is derived as follows. Begin by converting the proximate data to a dry-ash-free basis: Proximate Analysis Volatiles Char (C(s)) Ash
Wt % (dry) 28 64 8
Wt % (DAF) 30.4 69.6 -
The ultimate analysis, for the dry-ash-free coal, is known to be: Element C H O N S 12-8
Wt % (DAF) 89.3 5.0 3.4 1.5 0.8
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
For modeling simplicity, the sulfur content of the coal can be combined into the nitrogen mass fraction, to yield: Element C H O N S
Wt % (DAF) 89.3 5.0 3.4 2.3 -
We can combine the proximate and ultimate analysis data to yield the following elemental composition of the volatile stream: Element C H O N Total
Wt % 89.3 5.0 3.4 2.3
Moles 7.44 5 0.21 0.16 12.81
Mole Fraction 0.581 0.390 0.016 0.013
You will enter the mole fractions in the final column, above, in order to define the fuel composition. prePDF will use this information, along with the coal heating value, to define the species present in the fuel. The lower heating value of coal (DAF) is known to be: • LCVcoal,DAF = 35.3 MJ/kg The specific heat and density of the coal are known to be 1000 J/kgK and 1 kg/m3 respectively.
c Fluent Inc. November 27, 2001
12-9
Using the Non-Premixed Combustion Model
4. Enter the fuel and oxidizer compositions. Setup −→ Species −→Composition... (a) Enable the input of the oxidizer stream composition. The oxidizer (air) consists of 21% O2 and 79% N2 by volume.
i. Under Stream, select Oxidiser. ii. Under Specify Composition In, retain the default selection of Mole Fractions. iii. Select O2 in the Defined Species list and enter 0.21 in the Species Fraction field. 12-10
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
iv. Select N2 in the Defined Species list and enter 0.79 in the Species Fraction field. (b) Enable the input of the fuel stream composition. Note: Because the empirical input option is enabled for the fuel stream, you will be prompted to enter atom mole fractions for C, H, O, and N, along with the heating value and heat capacity of the coal.
i. Under Stream, select Fuel. ii. Under Specify Composition In, retain the default selection of Mole Fractions.
c Fluent Inc. November 27, 2001
12-11
Using the Non-Premixed Combustion Model
iii. Select C in the Defined Species list and enter 0.581 in the Atom Fraction field. iv. Select H in the Defined Species list and enter 0.390 in the Atom Fraction field. v. Select N in the Defined Species list and enter 0.016 in the Atom Fraction field. vi. Select O in the Defined Species list and enter 0.013 in the Atom Fraction field. vii. Enter 3.53e7 J/kg for the Lower Caloric Value and 1000 J/kg-K for the Specific Heat. viii. Click Apply and close the panel. 5. Define the density of the solid carbon. Here, a value of 1300 kg/m3 is assumed. Setup −→ Species −→Density...
(a) Select C(S) in the Defined Species list. (b) Set the Density to 1300. (c) Click Apply and close the panel.
12-12
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
Note: prePDF will use this information during computation of the mixture density for the fuel. You should enter the density of solid char. This input will differ from the coal density defined in FLUENT, which is the apparent density of the ashcontaining coal particles. 6. Define the system operating conditions. The system pressure and inlet stream temperatures are required for the equilibrium chemistry calculation. The fuel stream inlet temperature for coal combustion should be the temperature at the onset of devolatilization. The oxidizer inlet temperature should correspond to the air inlet temperature. In this tutorial, the coal devolatilization temperature will be set to 400 K and the air inlet temperature is 1500 K. The system pressure is one atmosphere. Setup −→Operating Conditions...
c Fluent Inc. November 27, 2001
12-13
Using the Non-Premixed Combustion Model
(a) Enter 400 K and 1500 K as the Fuel and Oxidiser inlet temperatures. (b) Click Apply and close the panel.
12-14
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
Step 2: Compute and Review the Adiabatic System prePDF Look-Up Tables 1. Accept the default PDF solution parameters. Setup −→Solution Parameters...
The look-up table calculation performed by prePDF will result in a table of values for species mole fractions and temperature at a set of discrete mixture fraction values. You control the number and distribution of these discrete points using the Solution Parameters panel. You can also set the Fuel Rich Flamability Limit in this panel. The Fuel Rich Flamability Limit allows you to perform a “partial equilibrium” calculation, suspending equilibrium calculations when the mixture fraction exceeds the specified rich limit. This increases the efficiency of the PDF calculation, allowing you to bypass the complex equilibrium calculations in the fuel-rich region, and is more physically realistic than the assumption of full equilibrium. For empirically defined streams, the rich limit is always 1.0 and cannot be altered.
c Fluent Inc. November 27, 2001
12-15
Using the Non-Premixed Combustion Model
(a) Keep the default setting for Automatic Distribution. This feature allows you to improve the prePDF prediction by optimizing the distribution of the discrete mixture fraction values, clustering them around the peak temperature value. If you choose not to use the Automatic Distribution, you should set the distribution center point on the rich side of the stoichiometric scale mixture fraction. (b) Click Apply and close the panel. 2. Save your inputs (coal ad.inp). File −→ Write −→Input... 3. Calculate the adiabatic system chemistry. Calculate −→PDF Table During the calculation, prePDF first retrieves thermodynamic data from the database. Then the time-averaged values of temperature, composition, and density at the discrete mixture-fraction/mixturefraction-variance points (21 points as defined in the Solution Parameters panel) are calculated. The result will be a set of tables containing time-averaged values of species mole fractions, density, and temperature at each discrete value of these two parameters. prePDF reports the progress of the look-up table construction in the console window. When the calculations are complete, prePDF will warn you that equilibrium calculations have been performed for the fuel inlet. You can simply acknowledge this warning, as the equilibrium conditions predicted do not impact your modeling inputs unless the fuel stream is representing a gaseous fuel inlet.
12-16
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
4. Save the adiabatic PDF file (coal ad.pdf). File −→ Write −→PDF... (a) Under File Type, select Write Formatted File. When you write a PDF file, prePDF will save a binary file by default. If you are planning to use the PDF file on the same machine, you can save the file using the default Write Binary File option. However, if you are planning to use the PDF file on a different machine, you should save an ASCII (formatted) file from prePDF. Note that ASCII files take up more disk space than binary files. (b) Under Solver, select FLUENT 6. (c) Enter coal ad.pdf as the Pdf File name. (d) Click OK to write the file. 5. Examine the temperature/mixture-fraction relationship in the adiabatic system. The results of the adiabatic calculation provide insight into the system description that will be used for the non-adiabatic calculation. Display −→PDF Table...
(a) Select TEMPERATURE from the Plot Variable list and then click Display to generate the table (Figure 12.2).
c Fluent Inc. November 27, 2001
12-17
Using the Non-Premixed Combustion Model
The temperature display shows how the time-averaged system temperature varies with the mean mixture fraction and its variance. The temperature/mixture-fraction relationship shows that the peak flame temperature is about 2750 K at fuel stoichiometric mixture fractions of approximately 0.1. The relatively high flame temperature is a result of the high pre-heat in the combustion air. Note: The adiabatic flame temperature predicted by the adiabatic system calculation will be used to select the maximum temperature in the non-adiabatic system calculation.
2.8E+03
2.4E+03 T E M P E R A T U R E
2.0E+03
2.50E-01 2.00E-01
1.6E+03 1.50E-01 SCALED-F-VARIANCE
K
1.00E-01
1.2E+03 5.00E-02
7.6E+02
0.00E+00 0.00E+00
2.00E-01
4.00E-01
6.00E-01
8.00E-01
1.00E+00
F-MEAN
PDF TABLE - CHEMICAL EQUILIBRIUM MEAN FLAME TEMPERATURE
prePDF V4.00
Fluent Inc.
Figure 12.2: Time-Averaged Temperature: Adiabatic prePDF Calculation
12-18
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
Step 3: Create and Compute the Non-Adiabatic prePDF System Creating a non-adiabatic PDF system description requires that you do the following: • Redefine the system as non-adiabatic. • Set the peak system temperature (based on the adiabatic result of 2750 K). After these modifications, you will recompute the system chemistry and save a non-adiabatic PDF file for use in FLUENT.
c Fluent Inc. November 27, 2001
12-19
Using the Non-Premixed Combustion Model
1. Define the prePDF model type as non-adiabatic. Setup −→Case...
(a) Select Non-Adiabatic under Heat transfer options and click Apply.
12-20
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
2. Set the system temperature limits. Minimum and maximum temperatures in the system are required when the PDF calculation is non-adiabatic. The minimum temperature should be a few degrees lower than the lowest boundary condition temperature (e.g., the inlet temperature or wall temperature). In coal combustion systems, the minimum system temperature should also be set below the temperature at which the volatiles begin to evolve from the coal. Here, the vaporization temperature at which devolatilization begins will be set to 400 K. Thus, the minimum system temperature is set to 298 K (the default). The maximum temperature should be at least 100 K higher than the peak flame temperature found in the preliminary adiabatic calculation. Here, the maximum temperature will be taken as 3000 K, well above the peak adiabatic system temperature of 2750 K. Setup −→Operating Conditions...
c Fluent Inc. November 27, 2001
12-21
Using the Non-Premixed Combustion Model
(a) Enter 298 for Min. Temperature and 3000 for Max. Temperature. (b) Click Apply and close the panel. 3. Save the non-adiabatic system inputs (coal.inp). File −→ Write −→Input... 4. Compute the non-adiabatic PDF look-up tables. Calculate −→PDF Table The non-adiabatic prePDF calculation requires much more computation than the adiabatic calculation. prePDF begins by accessing the thermodynamic data from the database. Next, the enthalpy 12-22
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
field is initialized and the enthalpy grid adjusted to account for inlet conditions and solution parameters. Time-averaged values of temperature, composition, and density at the discrete mixturefraction/mixture-fraction-variance/enthalpy points (21 points, as defined in the Solution Parameters panel) are then calculated. The result will be a set of tables containing time-averaged values of species mole fractions, density, and temperature at each discrete value of these three parameters. When the calculations are complete, prePDF will warn you that equilibrium calculations have been performed for the fuel inlet. As noted above, you can simply acknowledge this warning, which has no impact on your inputs when you are modeling coal or liquid fuels.
5. Write the PDF output file (coal.pdf). File −→ Write −→PDF... (a) Under File Type, select Write Formatted File. (b) Select FLUENT 6 under Solver. (c) Enter coal.pdf as the Pdf File name. (d) Click OK to write the file.
c Fluent Inc. November 27, 2001
12-23
Using the Non-Premixed Combustion Model
6. Review one slice of the 3D look-up table prepared by prePDF. Display −→Nonadiabatic Table...
(a) Select TEMPERATURE from the Plot Variable drop-down list and click Display (Figure 12.3). Note: Review of the 3D look-up tables is accomplished on a sliceby-slice basis. By default, the slice selected is that corresponding to the adiabatic enthalpy values. This display should look very similar to the look-up table created during the adiabatic calculation. You can select other slices of constant enthalpy for display, as well.
12-24
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
2.8E+03
2.4E+03 T E M P E R A T U R E
2.0E+03
2.50E-01 2.00E-01
1.6E+03 1.50E-01 SCALED-F-VARIANCE
K
1.00E-01
1.2E+03 5.00E-02
7.6E+02
0.00E+00 0.00E+00
2.00E-01
4.00E-01
6.00E-01
8.00E-01
1.00E+00
F-MEAN
MEAN ENTHALPY SLICE NUMBER 23
prePDF V4.00
MEAN FLAME TEMPERATURE FROM 3D-PDF-TABLE
Fluent Inc.
Figure 12.3: Non-Adiabatic Temperature Look-Up Table on the Slice Corresponding to Adiabatic Enthalpy
c Fluent Inc. November 27, 2001
12-25
Using the Non-Premixed Combustion Model
7. Examine the species/mixture-fraction relationship in the non-adiabatic system. Display −→Nonadiabatic Table...
(a) Select SPECIES from the Plot Variable drop-down list. The Species Selection panel will open automatically. (b) In the Species Selection panel, select C(S) in the Species dropdown list and click OK.
(c) Click Display in the Nonadiabatic-Table panel to generate the table (Figure 12.4). 8. Follow the steps above to plot the instantaneous mole fractions for CO (Figure 12.5).
12-26
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
7.6E-01
6.1E-01 M O L E F R A C T I O N
4.6E-01
2.50E-01 2.00E-01
3.1E-01 1.50E-01 SCALED-F-VARIANCE 1.00E-01
1.5E-01 5.00E-02
0.0E+00
0.00E+00 0.00E+00
2.00E-01
4.00E-01
6.00E-01
8.00E-01
1.00E+00
F-MEAN
MEAN ENTHALPY SLICE NUMBER 23 SPECIES C(S)
prePDF V4.00
FROM 3D-PDF-TABLE
Fluent Inc.
Figure 12.4: Time-Averaged C(S) Mole Fractions: prePDF Calculation
Non-Adiabatic
3.1E-01
2.4E-01 M O L E F R A C T I O N
1.8E-01
2.50E-01 2.00E-01
1.2E-01 1.50E-01 SCALED-F-VARIANCE 1.00E-01
6.1E-02 5.00E-02
0.0E+00
0.00E+00 0.00E+00
2.00E-01
4.00E-01
6.00E-01
8.00E-01
1.00E+00
F-MEAN
MEAN ENTHALPY SLICE NUMBER 23 SPECIES CO
FROM 3D-PDF-TABLE
prePDF V4.00
Fluent Inc.
Figure 12.5: Time-Averaged CO Mole Fractions: Non-Adiabatic prePDF Calculation
c Fluent Inc. November 27, 2001
12-27
Using the Non-Premixed Combustion Model
9. Exit from prePDF. File −→Exit
Preparation for FLUENT Calculation With the PDF file creation completed, you are ready to use the nonpremixed combustion model in FLUENT to predict the combusting flow in the coal furnace. 1. Copy the file coal/coal.msh from the FLUENT documentation CD to your working directory (as described in Tutorial 1). The mesh file coal.msh is a quadrilateral mesh describing the system geometry shown in Figure 12.1. 2. Start the 2D version of FLUENT.
12-28
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
Step 4: Grid 1. Read the 2D mesh file, coal.msh. File −→ Read −→Case... The FLUENT console window reports that the mesh contains 1357 quadrilateral cells. 2. Check the grid. Grid −→Check The grid check should not report any errors or negative volumes. 3. Display the grid (Figure 12.6). Display −→Grid... Due to the grid resolution and the size of the domain, you may find it more useful to display just the outline, or to zoom in on various portions of the grid display. Note: You can use the mouse probe button (right button, by default) to find out the boundary zone labels. As annotated in Figure 12.7, the upstream boundary contains two velocity inlets (for the low-speed and high-speed air streams), the downstream boundary is a pressure outlet, the top boundary is a wall, and the bottom boundary is a symmetry plane.
c Fluent Inc. November 27, 2001
12-29
Using the Non-Premixed Combustion Model
Grid
Aug 28, 2001 FLUENT 6.0 (2d, segregated, lam)
Figure 12.6: 2D Coal Furnace Mesh Outline Display
wall-7
velocity-inlet-2
velocity-inlet-8
symmetry-5
Grid
Aug 28, 2001 FLUENT 6.0 (2d, segregated, lam)
Figure 12.7: Mesh Display with Annotated Boundary Types
12-30
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
Step 5: Models: Continuous (Gas) Phase 1. Accept the default segregated solver. The non-premixed combustion model is available only with the segregated solver. Define −→ Models −→Solver...
c Fluent Inc. November 27, 2001
12-31
Using the Non-Premixed Combustion Model
2. Turn on the standard k- turbulence model. Define −→ Models −→Viscous...
Note: As indicated in the problem description, the Reynolds number of the flow is about 105 . Thus, the flow is turbulent and the high-Re k- model is suitable.
12-32
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
3. Turn on the non-premixed combustion model. Define −→ Models −→Species... (a) Select Non-Premixed Combustion under Model. The panel will expand to show the related inputs.
When you click OK, FLUENT will open the Select File dialog box, requesting input of the PDF file to be used in the simulation. (b) In the Select File dialog box, select and read the non-adiabatic PDF file (coal.pdf). FLUENT reports in the console window that it is reading the nonadiabatic PDF file containing 13 species. It also reports that a new material, called pdf-mixture, has been created. This mixture contains the 13 species that you defined in prePDF and their thermodynamic properties. FLUENT will present an Information dialog box telling you that available material properties have changed. You will be setting properties later, so you can simply click OK in the dialog box to acknowledge this information. Note: FLUENT will automatically activate solution of the energy equation when it reads the non-adiabatic PDF file, so you do not need to visit the Energy panel to enable heat transfer.
c Fluent Inc. November 27, 2001
12-33
Using the Non-Premixed Combustion Model
4. Turn on radiation by selecting the P1 radiation model. Define −→ Models −→Radiation...
The P-1 model is one of the radiation models that can account for the exchange of radiation between gas and particulates. After you click OK, FLUENT will present an Information dialog box telling you that available material properties have changed. You will be setting properties later, so you can simply click OK in the dialog box to acknowledge this information.
12-34
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
Step 6: Models: Discrete Phase The flow of pulverized coal particles will be modeled by FLUENT using the discrete phase model. This model predicts the trajectories of individual coal particles, each representing a continuous stream (or mass flow) of coal. Heat, momentum, and mass transfer between the coal and the gas will be included by alternately computing the discrete phase trajectories and the gas phase continuum equations. 1. Enable the discrete phase coupling to the continuous phase flow prediction. Define −→ Models −→Discrete Phase... (a) Under Interaction, turn on the Interaction with Continuous Phase option. This option enables coupling, in which the discrete phase trajectories (along with heat and mass transfer to the particles) are allowed to impact the gas phase equations. If you leave this option turned off, you can track particles but they will have no impact on the continuous phase flow.
c Fluent Inc. November 27, 2001
12-35
Using the Non-Premixed Combustion Model
(b) Set the coupling parameter, the Number of Continuous Phase Iterations per DPM Iteration, to 20. You should use higher values of this parameter in problems that include a high particle mass loading or a larger grid size. Less frequent trajectory updates can be beneficial in such problems, in order to converge the gas phase equations more com12-36
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
pletely prior to repeating the trajectory calculation. (c) Under Tracking Parameters, set the Max. Number of Steps to 10000. The limit on the number of trajectory time steps is used to abort trajectories of particles that are trapped in the domain (e.g., in a recirculation). (d) Retain the default Length Scale of 0.01 m. The Length Scale controls the time step size used for integration of the discrete phase trajectories. The value of 0.01 m used here implies that roughly 1000 time steps will be used to compute trajectories along the 10 m length of the domain. (e) Under Options, turn on Particle Radiation Interaction.
c Fluent Inc. November 27, 2001
12-37
Using the Non-Premixed Combustion Model
2. Create the discrete phase coal injections. The flow of the pulverized coal is defined by the initial conditions that describe the coal as it enters the gas. FLUENT will use these initial conditions as the starting point for its time integration of the particle equations of motion (the trajectory calculations). Here, the total mass flow rate of coal (in the half-width of the duct) is 0.1 kg/s (per unit meter depth). The particles will be assumed to obey a Rosin-Rammler size distribution between 70 and 200 micron diameter. Other initial conditions (velocity, temperature, position) are detailed below along with the appropriate input procedures. Define −→ Injections...
(a) Click the Create button in the Injections panel. This will open the Set Injection Properties panel where you will define the initial conditions defining the flow of coal particles.
12-38
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
In the Set Injection Properties panel you will define the initial conditions of the flow of coal particles. The particle stream will be defined as a group of 10 distinct initial conditions, all identical except for diameter, which will obey the RosinRammler size distribution law. (b) Select group in the Injection Type drop-down list.
c Fluent Inc. November 27, 2001
12-39
Using the Non-Premixed Combustion Model
(c) Set the Number of Particle Streams to 10. These inputs tell FLUENT to represent the range of specified initial conditions by 10 discrete particle streams, each with its own set of discrete initial conditions. Here, this will result in 10 discrete particle diameters, as the diameter will be varied within the injection group. (d) Select Combusting under Particle Type. By selecting Combusting you are activating the submodels for coal devolatilization and char burnout. Similarly, selecting Droplet would enable the submodels for droplet evaporation and boiling. (e) Select coal-mv in the Material drop-down list. The Material list contains the combusting particle materials in the FLUENT database. You can select an appropriate coal from this list and then review or modify its properties in the Materials panel (see Step 8: Materials: Discrete Phase). (f) Select rosin-rammler in the Diameter Distribution drop-down list. The coal particles have a nonuniform size distribution with diameters ranging from 70 µm to 200 µm. The size distribution fits the Rosin-Rammler equation, with a mean diameter of 134 µm and a spread parameter of 4.52. (g) Select o2 (the default) in the Oxidizing Species drop-down list.
12-40
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
(h) Specify the range of initial conditions under Point Properties starting with the following inputs for First Point: • X-Position: 0.001 m • Y-Position: 0.03124 m • X-Velocity: 10 m/s • Y-Velocity: 5 m/s • Temperature = 300 K • Total Flow Rate: 0.1 kg/s • Min. Diameter: 70e-6 m • Max. Diameter: 200e-6 m • Mean Diameter: 134e-6 m • Spread Parameter: 4.52 (i) Under Last Point, specify identical inputs for position, velocity, and temperature. (j) Define the turbulent dispersion. i. Click on Turbulent Dispersion. The panel will change to show the related inputs.
c Fluent Inc. November 27, 2001
12-41
Using the Non-Premixed Combustion Model
ii. Under Stochastic Tracking, turn on Stochastic Model. Stochastic tracks model the effect of turbulence in the gas phase on the particle trajectories. Including stochastic tracking is important in coal combustion simulations, to simulate realistic particle dispersion. iii. Set the Number of Tries to 10.
12-42
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
Note: The new injection (named injection-0, by default) now appears in the Injections panel.
This panel can be used to copy and delete injection definitions. You can also select an existing injection and list the initial conditions of particle streams defined by that injection in the console window. The listing for the injection-0 group will show 10 particle streams, each with a unique diameter between the specified minimum and maximum value, obtained from the Rosin-Rammler distribution, and a unique mass flow rate.
c Fluent Inc. November 27, 2001
12-43
Using the Non-Premixed Combustion Model
Step 7: Materials: Continuous Phase All thermodynamic data including density, specific heat, and formation enthalpies are extracted from the prePDF chemical database when the non-premixed combustion model is used. These properties are transferred to FLUENT as the pdf-mixture material, for which only transport properties, such as viscosity and thermal conductivity, need to be defined. Define −→Materials...
12-44
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
1. Set Thermal Conductivity to 0.025 (constant). 2. Set Viscosity to 2e-5 (constant). 3. Select wsggm-cell-based in the drop-down list for the Absorption Coefficient. This specifies a composition-dependent absorption coefficient, using the weighted-sum-of-gray-gases model. See the User’s Guide for details. 4. Click the Change/Create button. Note: You can click on the View... button next to Mixture Species to view the species included in the pdf-mixture material. These are the species included during the system chemistry setup in prePDF. Note that the Density and Cp laws cannot be altered: these properties are stored in the non-premixed combustion look-up tables. prePDF uses the gas law to compute the mixture density and a mass-weighted mixing law to compute the mixture cp . Although it is possible for you to alter the properties of the individual species, you should not do so when the non-premixed combustion model is used. This would create an inconsistency with the look-up table created in prePDF.
c Fluent Inc. November 27, 2001
12-45
Using the Non-Premixed Combustion Model
Step 8: Materials: Discrete Phase Define −→Materials...
1. Select combusting-particle from the Material Type list. The combusting-particle material type appears because you have activated combusting particles using the Set Injection Properties panel. Other discrete phase material types (droplets, inert particles) will appear in this list if you have created injections of those types. 2. Keep the current selection (coal-mv) in the Combusting Particle Materials list.
12-46
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
This is the combusting particle material type that you selected from the list of database options in the Set Injection Properties panel. Additional combusting particle materials can be copied from the property database, if desired. You can click the Database... button in order to view the combusting-particle materials that are available. Here, you will simply modify the property settings for the selected material, coal-mv. 3. Set the following constant property values for the coal-mv material: Density Cp Thermal Conductivity Latent Heat Vaporization Temperature Volatile Component Fraction (%) Binary Diffusivity Particle Emissivity Particle Scattering Factor Swelling Coefficient Burnout Stoichiometric Ratio Combustible Fraction (%)
1300 kg/m3 1000 J/kg-K 0.0454 w/m-k 0 400 K 28 5e-4 m2/s 0.9 0.6 2 2.67 64
FLUENT uses these inputs as follows: • Density impacts the particle inertia and body forces (when the gravitational acceleration is non-zero). • Cp determines the heat required to change the particle temperature. • Latent Heat is the heat required to vaporize the volatiles. This can usually be set to zero when the non-premixed combustion model is used for coal combustion. If the volatile composition has been selected in order to preserve the heating value of the fuel, the latent heat has been effectively included. (You would, however, use a non-zero latent heat if water content had been included in the volatile definition as vapor phase H2 O.)
c Fluent Inc. November 27, 2001
12-47
Using the Non-Premixed Combustion Model
• Vaporization Temperature is the temperature at which the coal devolatilization begins. It should be set equal to the fuel inlet temperature used in prePDF. • Volatile Component Fraction determines the mass of each coal particle that is devolatilized. • Binary Diffusivity is the diffusivity of oxidant to the particle surface and is used in the diffusion-limited char burnout rate. • Particle Emissivity is the emissivity of the particles. It is used to compute radiation heat transfer to the particles. • Particle Scattering Factor is the scattering factor due to particles. • Swelling Coefficient determines the change in diameter during coal devolatilization. A swelling coefficient of 2 implies that the particle size will double as the volatile fraction is released. • Burnout Stoichiometric Ratio is used in the calculation of the diffusion-controlled burnout rate. Otherwise, this parameter has no impact when the non-premixed combustion model is used. When finite-rate chemistry is used instead, the stoichiometric ratio defines the mass of oxidant required per mass of char. The default value represents oxidation of C(s) to CO2 . • Combustible Fraction is the mass fraction of char in the coal particle. It determines the mass of each coal particle that is consumed by the char burnout submodel. !
12-48
The settings for the Vaporization Temperature, Combustible Fraction, and Volatile Component Fraction inputs should all be consistent with your prePDF inputs. (See Step 1: Define the Preliminary Adiabatic System in prePDF.)
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
4. Select the Single Rate Devolatilization Model for Devolatilization Model. (a) Select the single-rate option in the Devolatilization Model dropdown list. This opens the Single Rate Devolatilization Model panel.
(b) Accept the default devolatilization model parameters. 5. Select kinetics/diffusion-limited for the Combustion Model. (a) Select the kinetic/diffusion-limited option in the Combustion Model drop-down list. This opens the Kinetics/Diffusion Limited Combustion Model panel.
(b) Accept the default values. 6. Click Change/Create and then close the Materials panel.
c Fluent Inc. November 27, 2001
12-49
Using the Non-Premixed Combustion Model
Step 9: Boundary Conditions Define −→Boundary Conditions... Hint: You can click your mouse probe button (the right button, by default) on the desired boundary zone in the graphics display window. FLUENT will then select that zone in the Boundary Conditions panel. 1. Set the following conditions for the velocity-inlet-2 zone (the lowspeed inlet boundary). Note: Turbulence parameters are defined here based on intensity and hydraulic diameter. The relatively large turbulence intensity of 10% may be typical for combustion air flows. The hydraulic diameter has been set to twice the height of the 2D inlet stream. For the non-premixed combustion calculation, you need to define the inlet Mean Mixture Fraction and Mixture Fraction Variance. For coal combustion, all fuel comes from the discrete phase and thus the gas phase inlets have zero mixture fraction. Therefore, you can accept the zero default settings.
12-50
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
c Fluent Inc. November 27, 2001
12-51
Using the Non-Premixed Combustion Model
2. Set the following conditions for the velocity-inlet-8 zone (the highspeed inlet boundary).
12-52
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
3. Set the following conditions for the pressure-outlet-6 zone (the exit boundary).
The exit gauge pressure of zero simply defines the system pressure at the exit to be the operating pressure. The backflow conditions for scalars (temperature, mixture fraction, turbulence parameters) will be used only if flow is entrained into the domain through the exit. It is a good idea to use reasonable values in case flow reversal occurs at the exit at some point during the solution process.
c Fluent Inc. November 27, 2001
12-53
Using the Non-Premixed Combustion Model
4. Set conditions for the wall-7 zone (the furnace wall). The furnace wall will be treated as an isothermal boundary with a temperature of 1200 K.
(a) Under Thermal Conditions, select Temperature. (b) Enter 1200 in the Temperature field. Note: The default boundary condition for particles that hit the wall is reflect, as shown under DPM. Alternate treatments can be selected, using the BC Type list, for particles that hit the wall.
12-54
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
Step 10: Solution 1. Set the P1 under-relaxation factor to 1. Solve −→ Controls −→Solution... 2. Initialize the flow field using conditions at velocity-inlet-2. Solve −→ Initialize −→Initialize...
(a) Select velocity-inlet-2 in the Compute From list. (b) Click the Init button to initialize the flow field, and then close the panel. !
The Apply button does not initialize the flow field data. You must use the Init button. (Apply simply allows you to store your initialization parameters for later use.)
Note: Here, with very high pre-heat of the oxidizer stream, you can start the combustion calculation from the inlet-based initialization. In general, you may need to start your coal combustion calculations by patching a high-temperature region and
c Fluent Inc. November 27, 2001
12-55
Using the Non-Premixed Combustion Model
performing a discrete phase trajectory calculation. This provides the initial volatile and char release required to initiate combustion. The Solve/Initialize/Patch... menu item and the solve/dpm-update text command can be used to perform this initialization. 3. Enable the display of residuals during the solution process. Solve −→ Monitors −→Residual... 4. Save the case file (coal.cas). File −→ Write −→Case... 5. Begin the calculation by requesting 400 iterations. Solve −→Iterate...
Note: The default convergence criteria will be met in about 170 iterations. 6. Save the converged flow data (coal.dat). File −→ Write −→Data...
12-56
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
Step 11: Postprocessing 1. Display the predicted temperature field (Figure 12.8). Display −→Contours...
The peak temperature in the system is about 2260 K. Hint: Use the Views panel (Display/Views...) to mirror the display about the symmetry plane.
c Fluent Inc. November 27, 2001
12-57
Using the Non-Premixed Combustion Model
2.26e+03 2.16e+03 2.05e+03 1.94e+03 1.84e+03 1.73e+03 1.63e+03 1.52e+03 1.41e+03 1.31e+03 1.20e+03
Contours of Static Temperature (k)
Sep 10, 2001 FLUENT 6.0 (2d, segregated, pdf13, ske)
Figure 12.8: Temperature Contours
12-58
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
2. Display the Mean Mixture Fraction distribution (Figure 12.9). Display −→Contours...
The mixture-fraction distribution shows where the char and volatiles released from the coal exist in the gas phase.
c Fluent Inc. November 27, 2001
12-59
Using the Non-Premixed Combustion Model
3.72e-02 3.35e-02 2.98e-02 2.61e-02 2.23e-02 1.86e-02 1.49e-02 1.12e-02 7.45e-03 3.72e-03 0.00e+00
Contours of Mean Mixture Fraction
Sep 10, 2001 FLUENT 6.0 (2d, segregated, pdf13, ske)
Figure 12.9: Mixture-Fraction Distribution
12-60
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
3. Display the devolatilization rate (Figure 12.10). Display −→Contours...
(a) Select Discrete Phase Model... and DPM Evaporation/Devolatilization in the drop-down lists under Contours Of. 4. Display the char burnout rate (Figure 12.11) by selecting DPM Burnout from the lower drop-down list. Note: The display of devolatilization rate shows that volatiles are released after the coal travels about one eighth of the furnace length. (The onset of devolatilization occurs when the coal temperature reaches the specified value of 400 K.) The char burnout occurs following complete devolatilization. Figure 12.11 shows that burnout is complete at about three-quarters of the furnace.
c Fluent Inc. November 27, 2001
12-61
Using the Non-Premixed Combustion Model
2.95e-03 2.66e-03 2.36e-03 2.07e-03 1.77e-03 1.48e-03 1.18e-03 8.86e-04 5.90e-04 2.95e-04 0.00e+00
Contours of DPM Evaporation/Devolatilization (kg/s)
Sep 10, 2001 FLUENT 6.0 (2d, segregated, pdf13, ske)
Figure 12.10: Devolatilization Rate
4.42e-04 3.97e-04 3.53e-04 3.09e-04 2.65e-04 2.21e-04 1.77e-04 1.32e-04 8.83e-05 4.42e-05 0.00e+00
Contours of DPM Burnout (kg/s)
Sep 10, 2001 FLUENT 6.0 (2d, segregated, pdf13, ske)
Figure 12.11: Char Burnout Rate
12-62
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
5. Display the particle trajectory of one particle stream (Figure 12.12). Display −→Particle Tracks...
(a) Select injection-0 in the Release From Injections list. (b) Select Particle Residence Time in the Color By drop-down list. (c) Turn on Track Single Particle Stream and set the Stream ID to 5. (d) Click Display.
c Fluent Inc. November 27, 2001
12-63
Using the Non-Premixed Combustion Model
3.63e-01 3.27e-01 2.90e-01 2.54e-01 2.18e-01 1.81e-01 1.45e-01 1.09e-01 7.26e-02 3.63e-02 0.00e+00
Particle Traces Colored by Particle Residence Time (s)
Sep 10, 2001 FLUENT 6.0 (2d, segregated, pdf13, ske)
Figure 12.12: Trajectories of Particle Stream 5 Colored by Particle Residence Time
12-64
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
6. Display the oxygen distribution (Figure 12.13). Display −→Contours...
Note: Although transport equations are solved only for the mixture fraction and its variance, you can still display the predicted chemical species concentrations. These are predicted by the PDF equilibrium chemistry model. 7. Select other species and display their mass fraction distributions (e.g., Figures 12.14–12.16).
c Fluent Inc. November 27, 2001
12-65
Using the Non-Premixed Combustion Model
2.33e-01 2.22e-01 2.11e-01 2.00e-01 1.89e-01 1.78e-01 1.67e-01 1.56e-01 1.45e-01 1.34e-01 1.23e-01
Contours of Mass fraction of o2
Sep 10, 2001 FLUENT 6.0 (2d, segregated, pdf13, ske)
Figure 12.13: O2 Distribution 1.19e-01 1.07e-01 9.54e-02 8.35e-02 7.15e-02 5.96e-02 4.77e-02 3.58e-02 2.38e-02 1.19e-02 0.00e+00
Contours of Mass fraction of co2
Sep 10, 2001 FLUENT 6.0 (2d, segregated, pdf13, ske)
Figure 12.14: CO2 Distribution
12-66
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
1.60e-02 1.44e-02 1.28e-02 1.12e-02 9.62e-03 8.02e-03 6.42e-03 4.81e-03 3.21e-03 1.60e-03 0.00e+00
Contours of Mass fraction of h2o
Sep 10, 2001 FLUENT 6.0 (2d, segregated, pdf13, ske)
Figure 12.15: H2 O Distribution 6.99e-03 6.29e-03 5.59e-03 4.89e-03 4.19e-03 3.49e-03 2.79e-03 2.10e-03 1.40e-03 6.99e-04 0.00e+00
Contours of Mass fraction of co
Sep 10, 2001 FLUENT 6.0 (2d, segregated, pdf13, ske)
Figure 12.16: CO Distribution
c Fluent Inc. November 27, 2001
12-67
Using the Non-Premixed Combustion Model
Step 12: Energy Balances and Particle Reporting FLUENT can provide many useful reports, including overall energy accounting and detailed information regarding heat and mass transfer from the discrete phase. Here, you will examine these reports. 1. Compute the fluxes of heat through the domain boundaries. Report −→Fluxes...
(a) Select Total Heat Transfer Rate under Options. (b) Under Boundaries, select the pressure-outlet-6, velocity-inlet-2, velocity-inlet-8, and wall-7 zones. (c) Click Compute. Note: Positive flux reports indicate heat addition to the domain. Negative values indicate heat leaving the domain. In reacting flows, the heat report uses total enthalpy (sensible heat plus
12-68
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
heat of formation of the chemical species). Here, the net “imbalance” of total enthalpy (about 14 KW) represents the total enthalpy addition from the discrete phase. 2. Compute the volume sources of heat transferred between the gas and discrete particle phase. Report −→Volume Integrals...
(a) Select Sum under Options. (b) Select Discrete Phase Model... and DPM Enthalpy Source in the drop-down lists under Field Variable. (c) Select fluid-1 under Cell Zones. (d) Click Compute. The total enthalpy transfer to the discrete phase from the gas is about -13.2 KW, as expected based on the boundary flux report above. This represents the total enthalpy addition from the discrete phase to the gas during the devolatilization and char combustion processes.
c Fluent Inc. November 27, 2001
12-69
Using the Non-Premixed Combustion Model
3. Obtain a summary report on the particle trajectories. The discrete phase model summary report provides detailed information about the particle residence time, heat and mass transfer between the continuous and discrete phases, and (for combusting particles) char conversion and volatile yield. Display −→Particle Tracks... (a) Select Summary under Report Type. (b) Select injection-0. (c) Click Track. FLUENT will report the summary in the console window. (You can write the report to a file by selecting File under Report to. (d) Review the summary printed in the console window:
12-70
c Fluent Inc. November 27, 2001
Using the Non-Premixed Combustion Model
DPM Iteration .... number tracked = 100, escaped = 0, aborted = 0, trapped = 0, evaporated = 0, incomp Fate
Number
---Incomplete
-----100
Elapsed Time (s) Inj Min Max Avg Std Dev ---------- ---------- ---------- ---------- ------2.398e-01 4.653e-01 3.096e-01 4.818e-02 inj
(*)- Mass Transfer Summary -(*) Fate ---Incomplete
Mass Flow (kg/s) Initial Final Change ---------- ---------- ---------1.000e-01 8.005e-03 -9.200e-02 (*)- Energy Transfer Summary -(*)
Fate ---Incomplete
Heat Content (W) Initial Final Change ---------- ---------- ----------3.712e+03 9.532e+03 1.324e+04 (*)- Combusting Particles -(*)
Fate ---Incomplete
Volatile Content (kg/s) Initial Final %Conv ---------- ---------- ------2.800e-02 0.000e+00 100.00
Char Content (kg/s) Initial Final %Con ---------- ---------- -----6.400e-02 5.351e-06 99.9
Done.
The report shows that the average residence time of the coal particles is about 0.33 seconds. Volatiles are completely released within the domain and the char conversion is 100% . Extra: You can obtain a detailed report of the particle position, velocity, diameter, and temperature along the trajectories of individual particles. This type of detailed track reporting can be useful if you are trying to understand unusual or important details in the discrete model behavior. To generate the report, visit the Particle Tracks panel. Select Step By Step under Report Type, and File under Report to. Enable the Track Single Particle Stream option, and set the Stream ID to the desired particle stream. Clicking Track will bring
c Fluent Inc. November 27, 2001
12-71
Using the Non-Premixed Combustion Model
up the Select File dialog box, where you will enter the name of the file to be written. This file can then be viewed with a text editor.
Summary: Coal combustion modeling involves the prediction of volatile evolution and char burnout from the pulverized coal along with simulation of the combustion chemistry occuring in the gas phase. In this tutorial you learned how to use the non-premixed combustion model to represent the gas phase combustion chemistry. In this approach the fuel composition was defined in prePDF and the fuel was assumed to react according to the equilibrium system data. This equilibrium chemistry model can be applied to other turbulent, diffusion-reaction systems. Note that you can also model coal combustion using the finite-rate chemistry model. You also learned how to set up and solve a problem involving a discrete phase of combusting particles. You created discrete phase injections, activated coupling to the gas phase, and defined the discrete phase material properties. These procedures can be used to set up other simulations involving reacting or inert particles.
12-72
c Fluent Inc. November 27, 2001
Tutorial 13. Chemistry
Modeling Surface
Introduction: In chemically reacting laminar flows, such as those encountered in chemical vapor deposition (CVD) applications, accurate modeling of time-dependent hydrodynamics, heat and mass transfer, and chemical reactions (including wall surface reactions) is important. Tutorials 11 and 12 deal with reacting flows with applications in gaseous fuel and coal combustion. In this tutorial, surface reactions are considered. In this tutorial, you will learn how to: • Enable physical models, select material properties, and define boundary conditions for a chemically reacting laminar flow involving wall surface reactions. • Read a user-defined function into FLUENT and use the file to define a parabolic velocity profile • Set temperature-dependent thermal conductivity in solids • Calculate the deposition solution using the segregated solver • Examine the flow results using graphics • Compare results for a single-step surface deposition reaction and a three-reaction mechanism Prerequisites: This tutorial assumes that you are familiar with the FLUENT user interface, and that you have solved Tutorial 1. Some steps in the setup and solution procedure will not be shown explicitly. Before beginning, you should read Sections 13.1 and 13.2 in the User’s Guide. Section 13.1 deals with species transport and chemically reacting flows. In particular, you should be familiar with
c Fluent Inc. November 27, 2001
13-1
Modeling Surface Chemistry
the Arrhenius rate equation as this equation is used for both the gas phase and surface reactions modeled in this tutorial. Section 13.2 describes wall surface reaction modeling and chemical vapor deposition (CVD). Problem Description: The laminar horizontal CVD reactor shown in Figure 13.1 will be modeled. Top wall – cooled 2 INLET
Quartz 2
OUTLET 3.5
Susceptor Quartz
.5 5
10
15
.5
(All dimensions in centimeters.)
Figure 13.1: An Outline of the Reactor Configuration The inlet gas is a mixture of silane SiH4 (g) and hydrogen H2 (g) at a temperature of 300 K. It enters the reactor through the inlet at the left end and flows for 5 cm between quartz walls that are separated by 2 cm. The gas mixture then flows over the heated substrate and silicon Si(s) is deposited on the heated susceptor as governed by the following gas phase and surface reactions: Reaction 1 (gas): Reaction 2 (surface): Reaction 3 (surface):
SiH4 (g) → SiH2 (g) + H2 (g) SiH4 (g) → Si(s) + 2H2 (g) SiH2 (g) → Si(s) + H2 (g)
As mentioned earlier, the inlet gas is a mixture of silane and hydrogen. In the inlet mixture the mass fraction of SiH4 is 0.0157 and the remainder is H2 . The inlet velocity is parabolic with zero velocity at the wall and an average velocity of 17.5 cm/sec, and the Reynolds number is approximately 60. The top wall is cooled to 300 K, and the susceptor is heated to a uniform temperature of 1300 K. 13-2
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
This tutorial has been divided into two parts. In the first case to be analyzed, a single-step surface deposition reaction is simulated and deposition of silicon from silane is examined. This involves deposition on a heated substrate, and only Reaction 2 is modeled. The deposition reaction is diffusion controlled: any silane that diffuses to solid surfaces will react and deposit silicon. The lower quartz walls are treated as thermally conducting walls. The exterior edges of the quartz walls are modeled as insulated (that is, zero-heat-flux) walls. Heat will be transferred into these quartz walls from the edges in contact with the heated susceptor, and the heat conducted from the susceptor is eventually transferred to the gas mixture through the interior faces of the lower quartz walls. The second part deals with the complete three-reaction mechanism. The mass diffusivity of SiH2 is determined from kinetic theory.
c Fluent Inc. November 27, 2001
13-3
Modeling Surface Chemistry
Preparation 1. Copy the files cvd/cvd.msh and cvd/inlet.c from the FLUENT documentation CD to your working directory (as described in Tutorial 1). A user-defined function will be used to define the parabolic inlet velocity. This function has already been written (inlet.c). You will only need to compile it within FLUENT. 2. Start the 2D version of FLUENT.
Step 1: Grid 1. Read in the mesh file cvd.msh. File −→ Read −→Case... As FLUENT reads the grid file, it will report that several wall zones are being separated. In the original grid, a single wall zone was used as the external boundary of the quartz regions and the internal boundary between the quartz and the fluid. FLUENT splits up the initial wall zone, placing the internal and external boundaries in separate zones. Note: If a wall zone has a fluid or solid region on each side, it is called a “two-sided wall”. When you read a grid with this type of wall zone into FLUENT a “shadow” zone is automatically created so that each side of the wall is a distinct wall zone. In this tutorial, FLUENT gives a message in the console window to inform you that it is creating a shadow wall (wall-24:005shadow). This is coupled to wall-24:005.
13-4
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
2. Check the grid. Grid −→Check Note: The grid check lists the minimum and maximum x and y values from the grid, and reports on a number of other grid features that are checked. Any errors in the grid would be reported at this time. For instance, the cell volumes must never be negative. Note that the domain extents are reported in units of meters, the default unit of length in FLUENT. Since this grid was created in units of centimeters, the Scale Grid panel will be used to scale the grid into meters. 3. Scale the grid. Grid −→Scale...
(a) In the Units Conversion drop-down list, select cm to complete the phrase Grid Was Created In cm (centimeters). (b) Click on Scale to scale the grid. The final Domain Extents should appear as in the panel above. Note: Because the default SI units will be used in this tutorial, there is no need to change any units.
c Fluent Inc. November 27, 2001
13-5
Modeling Surface Chemistry
4. Display the grid (Figure 13.2). Display −→Grid...
Extra: You can use the right mouse button to check which zone number corresponds to each boundary. If you click the right mouse button on one of the boundaries in the graphics window, its name and type will be printed in the FLUENT console window. This feature is especially useful when you have several zones of the same type and you want to distinguish between them quickly.
13-6
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
Grid
Jun 06, 2001 FLUENT 6.0 (2d, segregated, lam)
Figure 13.2: Grid Display
c Fluent Inc. November 27, 2001
13-7
Modeling Surface Chemistry
Step 2: Models In this problem, the energy equation and the species conservation equations will be solved, along with the momentum and continuity equations. 1. Keep the default solver settings. Define −→ Models −→Solver...
2. Enable heat transfer by activating the energy equation. Define −→ Models −→Energy...
13-8
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
3. Enable chemical species transport and reaction. Define −→ Models −→Species...
(a) Under Model, select Species Transport. This will expand the Species Model panel. (b) Under Reactions, select Volumetric. The panel will expand further. (c) Under Reactions, select Wall Surface. The panel will expand again.
c Fluent Inc. November 27, 2001
13-9
Modeling Surface Chemistry
(d) Under Wall Surface Reaction Options, select Heat of Surface Reactions and Mass Deposition Source. Turning on the Heat of Surface Reactions option enables modeling of heat release due to surface reactions. Mass Deposition Source is selected because there is a certain loss of mass due to the surface deposition reaction, i.e., Si(s) is being deposited out. If you were to do an overall mass balance without taking this fact into account, you would end up with a slight imbalance. (e) Keep the Diffusion Energy Source option turned on. Note: This includes the effect of enthalpy transport due to species diffusion in the energy equation, which contributes to the energy balance, especially for the case of Lewis numbers far from unity. (f) In the Mixture Material drop-down list, select silane-hydrogen (near the bottom). FLUENT will report the Number of Volumetric Species to be 2, and the Number of Surface Species to be 1. Note: In the first part of this tutorial, a one-step reaction is considered. Later, a three-step reaction will be considered. (g) Click OK. The console window will list the properties that are required for the models that you have enabled. You will see an Information dialog box, reminding you to confirm the property values that have been extracted from the database.
13-10
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
(h) Click OK in the Information dialog box to continue.
Step 3: Materials Define −→Materials...
The Materials panel shows the mixture material, silane-hydrogen, that was enabled in the Species Model panel. The properties for this mixture material are stored in the FLUENT database and can be modified by you.
c Fluent Inc. November 27, 2001
13-11
Modeling Surface Chemistry
Here, you will modify the default settings for the mixture by selecting the mixing-law model for cp . Density will be computed using the incompressible ideal-gas law, assuming an operating pressure of one atmosphere (1.0132 × 105 Pa, the default). Viscosity and thermal conductivity are predefined as polynomial functions of temperature, given by the following equations: µ = 3.17 × 10−6 + 2.04 × 10−8 T − 3.52 × 10−12 T 2
(13.1)
k = 3.8 × 10−2 + 5.41 × 10−4 T − 2.51 × 10−7 T 2 + 8.57 × 10−11 T 3 (13.2) These properties are those of pure H2 and can be used here because of the low concentration of SiH4 . 1. Define the material properties for the silane-hydrogen mixture. (a) Under Properties, click the Edit... button to the right of Mixture Species. This will open the Species panel.
13-12
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
In general, you can add or remove species from the mixture material. Here, the species that make up the silane-hydrogen mixture are predefined and require no modification. (b) Click Cancel to close the panel without making any changes. (c) In the Materials panel, select mixing-law in the Cp drop-down list. This instructs FLUENT to compute the mixture’s specific heat capacity as a mass fraction average of the pure species heat capacities. (The properties of these individual species will be reviewed in a later step.) (d) Click Change/Create. This will accept the material property settings for the mixture. (e) Under Properties, click the Edit... button to the right of Reaction. This will open the Reactions panel.
c Fluent Inc. November 27, 2001
13-13
Modeling Surface Chemistry
The panel shows that the Total Number of Reactions is 1, the Number of Reactants is 1, and the Number of Products is 2. The stoichiometric coefficients for the reaction are also shown, along with the values of Pre-exponential Factor Ak , Activation Energy Ek and Temperature Exponent βk used in the Arrhenius Rate equation. (f) Click Cancel to close the panel without making any changes.
13-14
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
2. Review the properties of the constituent species in the mixture.
(a) In the Materials panel, select fluid in the Material Type dropdown list. (b) In the Fluid Materials drop-down list, select silane (sih4) or hydrogen (h2) to view its individual properties.
c Fluent Inc. November 27, 2001
13-15
Modeling Surface Chemistry
3. Define the material properties for the quartz wall. The lower quartz wall is a conducting wall, with its thermal conductivity defined as a second-order polynomial given by k = 1.692 − 0.00193T + 3.196 × 10−6 T 2
(13.3)
(a) In the Material Type drop-down list, select solid. (b) Enter quartz in the Name text entry box. (c) Delete the name al in the Chemical Formula text entry box.
13-16
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
(d) Under Properties, select polynomial in the Thermal Conductivity drop-down list. This will open the Polynomial Profile panel.
(e) Increase the number of Coefficients to 3. This will activate the coefficient text entry fields. (f) Input the values for Coefficients 1, 2, 3, as shown in the panel above. (g) Click OK. (h) Answer No when FLUENT asks if it is OK to overwrite aluminum. FLUENT will create the new material, quartz, leaving aluminum unchanged. Note: The values of Density and Cp for quartz are left as the default values, since these values will not be used in any calculations. (i) In the Materials panel, click Change/Create and Close the panel. This will accept the material property settings for the solid material.
c Fluent Inc. November 27, 2001
13-17
Modeling Surface Chemistry
Step 4: Boundary Conditions Define −→Boundary Conditions... 1. Keep the default settings for fluid-1. The material for the fluid zone was set to silane-hydrogen when silane-hydrogen was selected as the mixture material in the Species Model panel. You cannot change the material in the Fluid panel when you are modeling species transport or reactions. 2. Set the conditions for solid-2.
(a) In the Material Name drop-down list, select quartz.
13-18
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
3. Set the boundary conditions for the top wall of the domain (wall10).
(a) Change the Zone Name from wall-10 to top-wall. (b) Under Thermal Conditions, select Temperature and keep the default setting of 300 K.
c Fluent Inc. November 27, 2001
13-19
Modeling Surface Chemistry
4. Set the boundary conditions for the top of the susceptor (wall-20).
(a) Change the Zone Name from wall-20 to susceptor. (b) Under Thermal Conditions, select Temperature. (c) Set the Temperature to 1300 K. (d) Click the Species tab to view the conditions for species transport and reactions.
13-20
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
(e) Turn on the Surface Reactions option.
c Fluent Inc. November 27, 2001
13-21
Modeling Surface Chemistry
5. Set the boundary conditions for the side of the susceptor (wall24:003). (a) Change the Zone Name from wall-24:003 to susceptor-side. (b) Under Thermal Conditions, select Temperature. (c) Set the Temperature to 1300 K. (d) In the Species section of the panel, turn on the Surface Reactions option. 6. Set the boundary conditions for the outer wall of the quartz region (wall-24).
(a) Change the Zone Name from wall-24 to outer-quartz-wall. (b) Keep the default setting of 0 for Heat Flux. (c) In the Material Name drop-down list, select quartz.
13-22
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
7. Set the conditions for the boundary between the quartz and fluid regions (wall-24:005).
(a) Change the Zone Name from wall-24:005 to quartz-fluidboundary. (b) Under Thermal Conditions, keep the default setting of Coupled. (c) In the Material Name drop-down list, select quartz. 8. Set the boundary conditions for wall-24:005-shadow. The boundary conditions are already set for wall-24:005-shadow, because it is coupled to wall-24:005 (renamed quartz-fluid-boundary).
c Fluent Inc. November 27, 2001
13-23
Modeling Surface Chemistry
It just needs to be given a more meaningful name. (a) Change the Zone Name from wall-24:005-shadow to quartz-fluid-boundary-shadow. 9. Define the conditions for the flow inlet (velocity-inlet-4). The u velocity at the inlet is defined as a parabolic profile in the y direction. The fully developed parabolic velocity profile for a twodimensional parallel plate duct is described by the following equation: u 3 = 1− Um 2 where u Um y a
= = = =
2 !
y a
(13.4)
local velocity in the x direction (m/s) mean velocity (m/s) y coordinate measured from the center of the duct (m) half-height of the duct (m)
In this case, Um is given as 0.175 m/s and a is 0.01 m. To use the polynomial fit for the u velocity, it is necessary to transform the y coordinate to the FLUENT global coordinate system, and to substitute the actual values of a and Um in Equation 13.4. Since the centerline of the duct is located at yFL = 0.03, the following relationship exists: y = yFL − 0.03
(13.5)
Substituting these values of y, a, and Um into the definition of a fully developed velocity profile, the polynomial equation required for FLUENT is obtained: 2 u = −2.1 + 157.5yFL − 2625yFL
(13.6)
A user-defined function (inlet.c) has been written to define the polynomial equation (Equation 13.6) required for the parabolic velocity profile. 13-24
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
Note: See the separate UDF Manual for details about user-defined functions. (a) Read in the user-defined function. Define −→ User-Defined −→ Functions −→Interpreted...
i. Enter inlet.c as the Source File Name. ii. Click Compile. The user-defined function has already been defined, but it needs to be compiled within FLUENT before it can be used in the solver. iii. Close the Interpreted UDFs panel.
c Fluent Inc. November 27, 2001
13-25
Modeling Surface Chemistry
(b) Set the boundary conditions for velocity-inlet-4.
i. In the Velocity Specification Method drop-down list, select Components. ii. Select udf inlet uv parabolic (the user-defined function) in the X-Velocity drop-down list. iii. Keep the default temperature of 300 K. iv. Under Species Mass Fractions, enter 0.0157 for sih4.
13-26
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
10. For the flow outlet (pressure-outlet-11), keep the default value of zero for the Species Mass Fraction.
c Fluent Inc. November 27, 2001
13-27
Modeling Surface Chemistry
Step 5: Solution for Single-Reaction Case 1. Initialize the flow field using the boundary conditions set at velocityinlet-4. Solve −→ Initialize −→Initialize...
(a) Select velocity-inlet-4 in the Compute From drop-down list. (b) Click Init, and Close the panel.
13-28
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
2. Turn on residual plotting during the calculation. Solve −→ Monitors −→Residual...
(a) Select Plot under Options, and click OK. 3. Save the case file (cvd.cas). File −→ Write −→Case...
c Fluent Inc. November 27, 2001
13-29
Modeling Surface Chemistry
4. Start the calculation by requesting 100 iterations. Solve −→Iterate...
The solution converges in about 30 iterations. During the first few iterations, the console window will report reversed flow on pressure-outlet 11. This is normal, and is related to the iterative process and the value of the pressure field during that iteration. Eventually, you will have all the flow leaving the domain. 5. Save the case and data files (cvd1.cas and cvd1.dat). File −→ Write −→Case & Data...
13-30
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
Step 6: Postprocessing for Single-Reaction Case 1. Display velocity vectors (Figure 13.3). Display −→Vectors...
(a) Click Display.
c Fluent Inc. November 27, 2001
13-31
Modeling Surface Chemistry
6.33e-01 5.70e-01 5.07e-01 4.44e-01 3.81e-01 3.18e-01 2.55e-01 1.93e-01 1.30e-01 6.67e-02 3.72e-03
Velocity Vectors Colored By Velocity Magnitude (m/s)
Jun 06, 2001 FLUENT 6.0 (2d, segregated, spe2, lam)
Figure 13.3: Velocity Vectors for the One-Reaction Case
The magnitude of the velocity increases as the gas flows over the heated substrate. Since the density of the gas decreases with increasing temperature, the velocity increases so as to conserve the mass flow rate. A small recirculation zone is also seen downstream of the susceptor.
13-32
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
2. Display contours of temperature (Figure 13.4). Display −→Contours...
(a) Select Temperature... and Static Temperature in the Contours Of drop-down list. (b) Click Display.
c Fluent Inc. November 27, 2001
13-33
Modeling Surface Chemistry
1.30e+03 1.20e+03 1.10e+03 1.00e+03 9.00e+02 8.00e+02 7.00e+02 6.00e+02 5.00e+02 4.00e+02 3.00e+02
Contours of Static Temperature (k)
Jun 06, 2001 FLUENT 6.0 (2d, segregated, spe2, lam)
Figure 13.4: Temperature Contours for the One-Reaction Case
The temperature contours show that the heat conduction into the quartz wall heats the gas mixture upstream of the susceptor.
13-34
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
3. Display contours of silane mass fraction (Figure 13.5). Display −→Contours... (a) Select Species... and Mass fraction of sih4 in the Contours Of drop-down list. (b) Click Display. 1.57e-02 1.41e-02 1.26e-02 1.10e-02 9.43e-03 7.86e-03 6.29e-03 4.72e-03 3.16e-03 1.59e-03 2.07e-05
Contours of Mass fraction of sih4
Jun 06, 2001 FLUENT 6.0 (2d, segregated, spe2, lam)
Figure 13.5: Contours of SiH4 Mass Fraction for the One-Reaction Case Figure 13.5 shows that the mass fraction gradient is large where the deposition reaction begins. The mass fraction of SiH4 near the susceptor is very small since the reaction is very fast and diffusioncontrolled. The mass fraction gradient of SiH4 above the susceptor drives the diffusion of SiH4 from above the susceptor to the surface where the reaction occurs.
c Fluent Inc. November 27, 2001
13-35
Modeling Surface Chemistry
4. Plot the surface deposition rate of Si on the susceptor (Figure 13.6). Plot −→XY Plot...
(a) Select Species... and Surface Deposition Rate of si in the Y Axis Function drop-down list. (b) Under Options, deselect Node Values. The source/sink terms due to the surface reaction are deposited in the cell adjacent to the wall cells, so it is necessary to plot the cell values and not the node values. (c) In the Surfaces list, select susceptor. (d) Click Plot.
13-36
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
susceptor 4.50e-05
4.00e-05
3.50e-05
3.00e-05
Surface Deposition Rate of si
2.50e-05
2.00e-05
1.50e-05
1.00e-05 0.05
0.06
0.07
0.08
0.09
0.1
0.11
0.12
0.13
0.14
0.15
Position (m)
Surface Deposition Rate of si
Jun 06, 2001 FLUENT 6.0 (2d, segregated, spe2, lam)
Figure 13.6: Surface Deposition Rate of Si The peak of the surface deposition rate occurs at the beginning of the susceptor (where the concentration of SiH4 is highest). The increase in deposition rate at the right-hand side of the susceptor is related to the backward-facing step in this problem.
c Fluent Inc. November 27, 2001
13-37
Modeling Surface Chemistry
(e) Write the deposition rate data to a file. You can read this file into FLUENT at a later time to recreate this plot. You will do this later in the tutorial to compare the deposition rates for the one-reaction and three-reaction cases. i. In the Solution XY Plot panel, select Write to File under Options. The Plot button will become the Write... button. ii. Click on the Write... button. This will open the Select File dialog box. iii. In the XY File text entry box, enter one reac.xy and click OK.
13-38
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
Step 7: Solution for Three-Step Reaction Case The single-step surface reaction will now be replaced by the following three-step reaction mechanism: SiH4 (g) → SiH2 (g) + H2 (g) SiH4 (g) → Si(s) + 2H2 (g) SiH2 (g) → Si(s) + H2 (g) The first reaction is a gas phase reaction which breaks SiH4 into SiH2 . The surface deposition of Si(s) takes place in the two separate surface reactions listed above. The reaction rates (as defined in Jasinski and Childs [1]) are as follows: Reaction (k) 1 2 3
Phase g s s
Ak 2.115×1015 3.340×10−1 1.000×1015
Ek 2.590 ×108 7.815 ×107 1.000 ×102
0
νj 0 ,k 1.0 1.0 1.0
βk 0.0 0.5 0.0
Since the current model has SiH2 added to the gas mixture, the mass diffusivity of SiH2 in hydrogen needs to be determined. Kinetic theory will be used to model this process. 1. Copy the material for the three-reaction mechanism from the materials database, and modify its properties. Define −→Materials... (a) Click on Database... to open the Database Materials panel.
c Fluent Inc. November 27, 2001
13-39
Modeling Surface Chemistry
(b) In the Mixture Materials list, select silane-hydrogen-3-step. The properties of this mixture will be displayed. (c) Click the View... button to the right of Mixture Species to view the selected species. (d) Click the View... button to the right of Reaction to view the defined reactions. The different reactions can be viewed by changing the Reaction ID in the top left corner of the Reactions panel. (e) In the Database Materials panel, click Copy and then Close the panel. 13-40
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
The properties will be down-loaded from the database into your FLUENT case. Your own copy of the mixture’s properties will now be displayed in the Materials panel, where you can modify them.
(f) In the Materials panel, select mixing-law in the Cp drop-down list. (g) In the Mass Diffusivity drop-down list, select kinetic-theory . Hint: You will need to scroll down to see Mass Diffusivity. (h) Click Change/Create, and Close the Materials panel.
c Fluent Inc. November 27, 2001
13-41
Modeling Surface Chemistry
2. Select the three-step reaction for the species transport calculation. Define −→ Models −→Species...
(a) In the Mixture Material drop-down list, select silane-hydrogen3-step. (b) Under Wall Surface Reaction Options, turn off the Heat of Surface Reactions and Mass Deposition Source. Turning off these effects temporarily makes the solution process more stable at the start of the calculation. (c) Click OK to accept the updated model.
13-42
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
!
When you changed the mixture material by adding species, the order of the species changed. When this occurs, all boundary conditions, solver parameters, and solution data for species will be reset to the default values. You must redefine species boundary conditions and solution parameters for the newly defined problem.
3. Review the boundary conditions for the flow inlet (velocity-inlet-4). Define −→Boundary Conditions... Check to see that these are the same as those set in Step 4: Boundary Conditions, Part 9. 4. Re-initialize the flow field. Solve −→ Initialize −→Initialize... !
Since the order of the species has been changed, the original data file now has incorrect data for the species. It is therefore recommended that you re-initialize the flow field by reselecting the conditions at velocity-inlet-4 as the initial conditions. (a) Select velocity-inlet-4 in the Compute From drop-down list. (b) Click Init, and then Close the panel.
5. Save the case file (cvd2.cas). File −→ Write −→Case... 6. Request 20 iterations. Solve −→Iterate... 7. Add the effects of surface reactions and the deposition source in the continuity equation. Define −→ Models −→Species... (a) Under Wall Surface Reaction Options, turn on the Heat of Surface Reactions and Mass Deposition Source options. 8. Request another 20 iterations. Solve −→Iterate... The solution converges in a total of about 30 iterations.
c Fluent Inc. November 27, 2001
13-43
Modeling Surface Chemistry
9. Save the case and data files (cvd3.cas and cvd3.dat). File −→ Write −→Case & Data...
Step 8: Postprocessing for Three-Step Reaction Case 1. Display velocity vectors (Figure 13.7). Display −→Vectors... The flow pattern looks very similar to that observed in Figure 13.3, for the single-step reaction. 6.33e-01 5.70e-01 5.07e-01 4.44e-01 3.81e-01 3.18e-01 2.55e-01 1.92e-01 1.30e-01 6.67e-02 3.78e-03
Velocity Vectors Colored By Velocity Magnitude (m/s)
Jun 06, 2001 FLUENT 6.0 (2d, segregated, spe3, lam)
Figure 13.7: Velocity Vectors for the Three-Step Reaction
13-44
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
2. Display contours of temperature (Figure 13.8). Display −→Contours... The temperature contours look very similar to those shown in Figure 13.4, for the single-step reaction. 1.30e+03 1.20e+03 1.10e+03 1.00e+03 9.00e+02 8.00e+02 7.00e+02 6.00e+02 5.00e+02 4.00e+02 3.00e+02
Contours of Static Temperature (k)
Jun 06, 2001 FLUENT 6.0 (2d, segregated, spe3, lam)
Figure 13.8: Temperature Contours for the Three-Step Reaction
3. Display contours of SiH4 mass fraction (Figure 13.9) and SiH2 mass fraction (Figure 13.10). Display −→Contours... The primary effect of changing the reaction mechanism is the distribution of species mass fraction.
c Fluent Inc. November 27, 2001
13-45
Modeling Surface Chemistry
1.57e-02 1.41e-02 1.26e-02 1.10e-02 9.42e-03 7.85e-03 6.28e-03 4.71e-03 3.14e-03 1.57e-03 2.64e-11
Contours of Mass fraction of sih4
Jun 06, 2001 FLUENT 6.0 (2d, segregated, spe3, lam)
Figure 13.9: Contours of SiH4 Mass Fraction for the Three-Step Reaction 4.63e-03 4.17e-03 3.70e-03 3.24e-03 2.78e-03 2.31e-03 1.85e-03 1.39e-03 9.26e-04 4.63e-04 0.00e+00
Contours of Mass fraction of sih2
Jun 06, 2001 FLUENT 6.0 (2d, segregated, spe3, lam)
Figure 13.10: Contours of SiH2 Mass Fraction for the Three-Step Reaction
13-46
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
4. Plot the surface deposition rate of Si on the susceptor for the threereaction case and compare the results for the two reaction mechanisms. Plot −→XY Plot... (a) Plot the surface mass flux of Si on the susceptor for the threereaction case (Figure 13.11). i. In the Solution XY Plot panel, select Species... and Surface Deposition Rate of si in the Y Axis Function drop-down lists. ii. Check that Node Values is turned off and susceptor is selected in the Surfaces list. iii. Click on the Curves... button. This will open the Curves - Solution XY Plot panel.
iv. In the Curves - Solution XY Plot panel, select x in the Symbol drop-down list. v. Change the Size of the Marker Style to 0.5. vi. Click Apply, and Close the panel.
c Fluent Inc. November 27, 2001
13-47
Modeling Surface Chemistry
vii. In the Solution XY Plot panel under Options, deselect Write to File. The Write... button will become the Plot button again. viii. Click Plot. susceptor 4.00e-05
3.50e-05
3.00e-05
Surface Deposition Rate of si
2.50e-05
2.00e-05
1.50e-05
1.00e-05 0.05
0.06
0.07
0.08
0.09
0.1
0.11
0.12
0.13
0.14
0.15
Position (m)
Surface Deposition Rate of si
Jun 06, 2001 FLUENT 6.0 (2d, segregated, spe3, lam)
Figure 13.11: Surface Deposition Rate of Si for the Three-Step Reaction
13-48
c Fluent Inc. November 27, 2001
Modeling Surface Chemistry
(b) Compare the results for the two reaction mechanisms, using a single XY plot of Si surface deposition rate. i. In the Solution XY Plot panel, click the Load File... button. This will open the Select File dialog box. ii. In the Select File dialog box, select one reac.xy (the XY plot created for the one-step reaction) in the Files list. iii. Click OK. iv. In the Solution XY Plot panel, click Plot. The surface deposition rates for the one-reaction and the three-reaction cases can now be easily compared in Figure 13.12. susceptor susceptor 4.50e-05
4.00e-05
3.50e-05
3.00e-05
Surface Deposition Rate of si
2.50e-05
2.00e-05
1.50e-05
1.00e-05 0.05
0.06
0.07
0.08
0.09
0.1
0.11
0.12
0.13
0.14
0.15
Position (m)
Surface Deposition Rate of si
Jun 06, 2001 FLUENT 6.0 (2d, segregated, spe3, lam)
Figure 13.12: Composite Plot of Surface Deposition Rate of Si
c Fluent Inc. November 27, 2001
13-49
Modeling Surface Chemistry
Summary: In chemically reacting laminar flows, accurate modeling of time-dependent hydrodynamics, heat and mass transfer, and chemical reactions (including wall surface reactions) is important. In this tutorial, you first simulated a single-step surface deposition reaction and examined the deposition of silicon from silane onto a susceptor. The lower quartz walls were modeled as thermally conducting walls using a second-order polynomial distribution to define the thermal conductivity. The velocity profile at the inlet was defined as parabolic, using a user-defined function. The single-step surface reaction was then replaced with a threestep reaction, and kinetic theory was used to determine the mass diffusivity of SiH2 in hydrogen. The surface deposition rate was compared for the one-step reaction and three-step reaction cases. References: 1. Jasinski, T.J. and Childs, E.P., “Numerical Modeling Tools for Chemical Vapor Deposition”, NASA Report CR-4480, TM1504, Creare Inc., December 1992.
13-50
c Fluent Inc. November 27, 2001
Tutorial 14. Modeling Evaporating Liquid Spray
Introduction: In this tutorial, FLUENT’s air-blast atomizer model is used to predict the droplet behavior of an evaporating methanol spray. The air flow is modeled first as a steady-state problem without droplets. To predict the behavior of individual droplets in the atomizer, several other discrete-phase models, including collision and breakup, are used in an unsteady calculation. In this tutorial you will learn how to: • Create periodic zones • Define a discrete-phase spray injection for an air-blast atomizer • Calculate a transient solution using the second-order implicit unsteady formulation Prerequisites: This tutorial assumes that you are familiar with the menu structure in FLUENT and that you have solved or read Tutorial 1. Some steps in the setup and solution procedure will not be shown explicitly. Problem Description: The geometry to be considered in this tutorial is shown in Figure 14.1. Methanol is cooled to −10◦ C before being introduced into an air-blast atomizer. The atomizer contains an inner air stream surrounded by a swirling annular stream. (The species include the components of air as well as water vapor, so the model can be expanded to include combustion, if desired.) To make use of the periodicity of the problem, only a 30-degree section of the atomizer will be modeled.
c Fluent Inc. November 27, 2001
14-1
Modeling Evaporating Liquid Spray
inner air stream swirling annular stream
Z
Y
X
Figure 14.1: Problem Specification
Preparation 1. Copy the file spray/sector.msh from the FLUENT documentation CD to your working directory (as described in Tutorial 1). 2. Start the 3D version of FLUENT.
14-2
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
Step 1: Grid 1. Read in the mesh file sector.msh. File −→ Read −→Case... 2. Check the grid. Grid −→Check FLUENT will perform various checks on the mesh and will report the progress in the console window. Pay particular attention to the reported minimum volume. Make sure this is a positive number. 3. Display the grid. Display −→Grid...
(a) Under Options, select Faces. (b) Under Surfaces, select only atomizer-wall, central air, and swirling air. (c) Click the Colors... button.
c Fluent Inc. November 27, 2001
14-3
Modeling Evaporating Liquid Spray
(d) In the Grid Colors panel, select Color By ID. This will assign a different color to each zone in the domain, rather than to each type of zone. (e) In the Grid Display panel, click Display. The graphics display will be updated to show the grid. You will now change the display again to zoom in on an isometric view of the atomizer section. 4. Change the display to an isometric view. Display −→Views...
14-4
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
(a) Select isometric in the Views list and click Restore. (b) Zoom in with your mouse to obtain the view shown in Figure 14.2.
Z
Y
X
Grid
Apr 19, 2001 FLUENT 6.0 (3d, segregated, lam)
Figure 14.2: Air-Blast Atomizer Mesh Display
c Fluent Inc. November 27, 2001
14-5
Modeling Evaporating Liquid Spray
5. Using the text interface, change zones periodic-a and periodic-b from wall zones to periodic zones. (a) In the console window, type the commands shown in boxes in the dialog below.
> grid /grid> modify-zones /grid/modify-zones> list-zones id name type ---- ---------------- ----------------1 fluid fluid 2 atomizer-wall wall 3 central_air mass-flow-inlet 4 co-flow-air velocity-inlet 5 outlet pressure-outlet 6 swirling_air velocity-inlet 7 periodic-a wall 8 periodic-b wall 9 outer-wall wall 11 default-interior interior
material -----------------air aluminum
aluminum aluminum aluminum
kind ---cell face face face face face face face face face
/grid/modify-zones> make-periodic Periodic zone [()] 7 Shadow zone [()] 8 Rotational periodic? (if no, translational) [yes] yes Create periodic zones? [yes] yes all 1923 faces matched for zones 7 and 8. zone 8 deleted created periodic zones.
14-6
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
6. Reorder the grid. To speed up the solution procedure, the mesh should be reordered, which will substantially reduce the bandwidth. Grid −→ Reorder −→Domain FLUENT will report its progress in the console window: >> Reordering domain using Reverse Cuthill-McKee method: zones, cells, faces, done. Bandwidth reduction = 3286/102 = 32.22 Done.
c Fluent Inc. November 27, 2001
14-7
Modeling Evaporating Liquid Spray
Step 2: Models 1. Keep the default solver settings. Define −→ Models −→Solver...
2. Enable heat transfer by activating the energy equation. Define −→ Models −→Energy...
14-8
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
3. Enable the realizable k- turbulence model. Define −→ Models −→Viscous...
The realizable k- model gives a more accurate prediction of the spreading rate of both planar and round jets than the standard k- model.
c Fluent Inc. November 27, 2001
14-9
Modeling Evaporating Liquid Spray
4. Enable chemical species transport and reaction. Define −→ Models −→Species...
(a) Select Species Transport under Model. (b) Choose methyl-alcohol-air in the Mixture Material drop-down list. The Mixture Material list contains the set of chemical mixtures that exist in the FLUENT database. By selecting one of the pre-defined mixtures, you are accessing a complete description of the reacting system. The chemical species in the system and their physical and thermodynamic properties are defined by your selection of the mixture material. You can alter the mixture material selection or modify the mixture material properties using the Materials panel (see Step 6: Solution: Unsteady Flow).
14-10
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
!
When you click OK, the console window will list the properties that are required for the models you have enabled. You will see an Information dialog box, reminding you to confirm the property values that have been extracted from the database.
(c) Click OK in the Information dialog box to continue.
c Fluent Inc. November 27, 2001
14-11
Modeling Evaporating Liquid Spray
Step 3: Boundary Conditions Define −→Boundary Conditions... 1. Set the following conditions for the inner air stream (central air).
14-12
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
2. Set the following conditions for the air stream surrounding the atomizer (co-flow-air).
c Fluent Inc. November 27, 2001
14-13
Modeling Evaporating Liquid Spray
3. Set the following conditions for the exit boundary (outlet).
14-14
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
4. Set the following conditions for the swirling annular stream (swirling air).
c Fluent Inc. November 27, 2001
14-15
Modeling Evaporating Liquid Spray
5. Set the following conditions for the outer wall of the atomizer (outer-wall).
14-16
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
Step 4: Initial Solution Without Droplets The airflow will first be solved and analyzed without droplets. 1. Initialize the flow field. Solve −→ Initialize −→Initialize...
(a) Select co-flow-air in the Compute From drop-down list. (b) Click Init to initialize the variables, and then close the panel.
c Fluent Inc. November 27, 2001
14-17
Modeling Evaporating Liquid Spray
2. Keep the default under-relaxation factors. Solve −→ Controls −→Solution...
14-18
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
3. Turn on residual plotting during the calculation. Solve −→ Monitors −→Residual...
(a) Under Options, select Plot. (b) Click OK.
c Fluent Inc. November 27, 2001
14-19
Modeling Evaporating Liquid Spray
4. Save the case file (spray1.cas). File −→ Write −→Case... 5. Start the calculation by requesting 200 iterations. Solve −→Iterate... The solution will converge after about 175 iterations. 6. Save the case and data files (spray1.cas and spray1.dat). File −→ Write −→Case & Data... Note: FLUENT will ask you to confirm that the previous case file is to be overwritten. 7. Create a clip plane to examine the flow field at the midpoint of the atomizer section. Surface −→Iso-Surface...
14-20
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
(a) Select Grid... and Angular Coordinate in the Surface of Constant lists. (b) Click on Compute to update the minimum and maximum values. (c) Enter 15 in the Iso-Values field. (d) Enter angle=15 for the New Surface Name. (e) Click on Create to create the isosurface. 8. Review the current state of the solution by examining contours of velocity magnitude (Figure 14.3). Display −→Contours...
c Fluent Inc. November 27, 2001
14-21
Modeling Evaporating Liquid Spray
(a) Select Velocity... and Velocity Magnitude in the Contours Of drop-down list. (b) Under Options, select Filled and Draw Grid. This will open the Grid Display panel.
(c) Keep the current grid display settings and close the Grid Display panel. (d) In the Contours panel, select angle=15 in the Surfaces list. (e) Click Display. (f) Use your mouse to obtain the view shown in Figure 14.3.
14-22
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
8.53e+01 7.68e+01 6.82e+01 5.97e+01 5.12e+01 4.27e+01 3.41e+01 2.56e+01 1.71e+01 8.53e+00
Z
Y
0.00e+00 X
Contours of Velocity Magnitude (m/s)
Jul 03, 2001 FLUENT 6.0 (3d, segregated, spe5, rke)
Figure 14.3: Velocity Magnitude at Mid-Point of Atomizer Section
c Fluent Inc. November 27, 2001
14-23
Modeling Evaporating Liquid Spray
9. Display path lines of the air in the swirling annular stream (Figure 14.4). Display −→Path Lines...
(a) In the Release From Surfaces list, select swirling air. You will need to scroll down to access this item. (b) Increase the Skip value to 5. (c) Under Options, select Draw Grid. This will open the Grid Display panel. (d) Keep the current grid display settings and close the Grid Display panel. (e) Click Display in the Path Lines panel. (f) Use your mouse to obtain the view shown in Figure 14.4.
14-24
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
3.00e+01 2.70e+01 2.40e+01 2.10e+01 1.80e+01 1.50e+01 1.20e+01 9.00e+00 6.00e+00 3.00e+00
Z
Y
0.00e+00 X
Path Lines Colored by Particle Id
Jul 03, 2001 FLUENT 6.0 (3d, segregated, spe5, rke)
Figure 14.4: Path Lines of Air in the Swirling Annular Stream
c Fluent Inc. November 27, 2001
14-25
Modeling Evaporating Liquid Spray
Step 5: Enable Time Dependence and Create a Spray Injection In this step you will define a transient flow and create a discrete phase spray injection. 1. Enable a time-dependent flow calculation. Define −→ Models −→Solver...
(a) Under Time, select Unsteady. (b) Under Unsteady Formulation, select 2nd-Order Implicit.
14-26
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
2. Define the discrete phase modeling parameters. Define −→ Models −→Discrete Phase...
c Fluent Inc. November 27, 2001
14-27
Modeling Evaporating Liquid Spray
(a) Define the interphase interaction. i. Under Interaction, turn on Interaction with Continuous Phase. This will include the effects of the discrete phase trajectories on the continuous phase. ii. Under Number of Continuous Phase Iterations per DPM Iteration, enter a value of 1000. This option controls the iterative solution of the discrete phase within each gas-phase time step. Higher values are more desirable for sprays. (b) Specify the Tracking Parameters. i. Deselect the Specify Length Scale option. ii. Keep the default value of Step Length Factor. (c) Set the Unsteady Options. i. Under Spray Models, select Droplet Collision and Droplet Breakup. ii. Under Breakup Model, keep the default selection of TAB. iii. Under Constants, enter a value of 0.05 for y0. This parameter is the dimensionless droplet distortion at t = 0. (d) Under Drag Parameters, select dynamic-drag in the Drag Law drop-down list. The dynamic-drag law is available only when the Droplet Breakup model is used.
14-28
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
3. Create the spray injection. In this step, you will define the characteristics of the atomizer. Define −→Injections...
(a) Click the Create button at the top of the panel. This will open the Set Injection Properties panel.
c Fluent Inc. November 27, 2001
14-29
Modeling Evaporating Liquid Spray
(b) In the Injection Type drop-down list, select air-blast-atomizer. (c) Increase the Number Of Particle Streams to 60. This option controls how many parcels of droplets are introduced into the domain at every time step. (d) Under Particle Type, select Droplet. (e) In the Material drop-down list, select methyl-alcohol-liquid. (f) Set the point properties for the injection. 14-30
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
i. Set the X-Position, Y-Position, and Z-Position of the injection to 0, 0, and 0.0015. ii. Set the X-Axis, Y-Axis, and Z-Axis of the injection to 0, 0, and 1. iii. Set the Temperature to 263 K. iv. Set the Flow Rate to 1.7e-4 kg/s. This is the methanol flow rate for a 30-degree section of the atomizer. The actual atomizer flow rate is 12 times this value. v. Keep the default Start Time of 0 s and set the Stop Time to 100 s. For this problem, the injection should begin at t = 0 and not stop until long after the time period of interest. A large value for the stop time (e.g., 100 s) will ensure that the injection will essentially never stop. vi. Set the Injector Inner Diam. to 0.0035 m, and the Injector Outer Diam. to 0.0045 m. vii. Set the Spray Half Angle to -45 deg. The spray angle is the angle between the liquid sheet trajectory and the injector centerline. In this case, the value is negative because the sheet is initially converging toward the centerline. viii. Set the Relative Velocity to 82.6 m/s. The relative velocity is the expected relative velocity between the atomizing air and the liquid sheet. ix. Keep the default Azimuthal Start Angle of 0 deg and set the Azimuthal Stop Angle to 30 deg. This will restrict the injection to the 30-degree section of the atomizer that is being modeled.
c Fluent Inc. November 27, 2001
14-31
Modeling Evaporating Liquid Spray
(g) Define the turbulent dispersion. i. Click the Turbulent Dispersion tab. The lower half of the panel will change to show options for the turbulent dispersion model. ii. Under Stochastic Tracking, turn on the Stochastic Model and Random Eddy Lifetime options. These models will account for the turbulent dispersion of the droplets. 4. Set the droplet material properties. Because the secondary atomization models (breakup and coalescence) are used, the droplet properties must be set. Define −→Materials...
14-32
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
(a) In the Material Type drop-down list, select droplet-particle. (b) Under Properties, enter a value of 0.0056 kg/m-s for Viscosity. (c) Under Properties, scroll down and enter a value of 0.0222 N/m for Droplet Surface Tension. (d) Click Change/Create to accept the change in properties for the methanol droplet material.
c Fluent Inc. November 27, 2001
14-33
Modeling Evaporating Liquid Spray
Step 6: Solution: Unsteady Flow 1. Set the initial condition for the discrete phase. Resetting the discrete phase model sources will make sure that the interphase coupling is initialized. Solve −→ Initialize −→Reset DPM Sources 2. Set the time step parameters. The selection of the time step is critical for accurate time-dependent flow predictions. Solve −→Iterate...
14-34
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
(a) Set the Time Step Size to 5e-05 s. (b) Click Apply. 3. Save the transient solution case file (spray2.cas). File −→ Write −→Case... 4. Calculate a solution for one time step. Solve −→Iterate... It is a good idea to do one time step initially so you can check the position of the atomizer droplets before they are significantly dispersed. (a) Set the Number of Time Steps to 1. (b) Click Iterate. !
You will notice that FLUENT will perform 20 iterations for the first time step. Since this is the specified Max Iterations per Time Step, the solution is not yet completely converged. For a real problem, it is important that you allow the solution to converge at each time step, so you may need to increase the Max Iterations per Time Step. The default of 20 is used in this tutorial to speed up the calculation.
5. Save the new case and data files (spray2.cas and spray2.dat). File −→ Write −→Case & Data... 6. Display the trajectories of the droplets in the spray injection (Figure 14.5). This will allow you to review the location of the atomizer droplets after just one time step. They should therefore still be near their initial injection positions. Display −→Particle Tracks...
c Fluent Inc. November 27, 2001
14-35
Modeling Evaporating Liquid Spray
(a) In the Style drop-down list, select point. (b) Click the Style Attributes... button. This will open the Path Style Attributes panel.
14-36
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
(c) Set the Marker Size to 0.25 and click OK. (d) In the Particle Tracks panel, select Draw Grid under Options. This will open the Grid Display panel.
c Fluent Inc. November 27, 2001
14-37
Modeling Evaporating Liquid Spray
(e) Keep the current display settings and close the panel. (f) In the Particle Tracks panel, select Particle Variables... and Particle Diameter in the Color By drop-down list. This will display the location of the droplets colored by their diameters. (g) In the Release From Injections list, select injection-0. (h) Click Display. (i) Use your mouse to obtain the view shown in Figure 14.4. 1.35e-04 1.22e-04 1.10e-04 9.79e-05 8.57e-05 7.35e-05 6.13e-05 4.91e-05 3.69e-05 2.46e-05
Z
Y
1.24e-05 X
Particle Traces Colored by Particle Diameter (m) (Time=5.0000e-05) Jul 11, 2001 FLUENT 6.0 (3d, segregated, spe5, rke, unsteady)
Figure 14.5: Particle Tracks for the Spray Injection After 1 Time Step The air-blast atomizer model assumes that a cylindrical liquid sheet exits the atomizer, which then disintegrates into ligaments and droplets. Appropriately, the model determines that the droplets should be input into the domain in a ring. The radius of this disk is determined from the inner and outer radii of the injector. Note that the maximum diameter of the droplets is about 10−4 m, or 0.1 mm. This is slightly smaller than the film height, which makes sense. Recall that the inner diameter 14-38
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
and outer diameter of the injector are 3.5 mm and 4.5 mm, respectively. The film height is then 12 (4.5 − 3.5) = 0.5 mm. The range in the droplet sizes is due to the fact that the airblast atomizer automatically uses a droplet distribution. Also note that the droplets are placed a slight distance away from the injector. Once the droplets are injected into the domain, they can collide/coalesce with other droplets as determined by the secondary models (breakup and collision). However, once a droplet has been introduced into the domain, the air-blast atomizer model no longer affects the droplet. 7. Request 10 more time steps. Solve −→Iterate... 8. Save the new case and data files (spray3.cas and spray3.dat).
c Fluent Inc. November 27, 2001
14-39
Modeling Evaporating Liquid Spray
Step 7: Postprocessing 1. Display the particle trajectories again, to see how the droplets have dispersed. Display −→Particle Tracks... (a) Click Display in the Particle Tracks panel. (b) Use your mouse to obtain the view shown in Figure 14.6. 2.78e-04 2.52e-04 2.25e-04 1.98e-04 1.72e-04 1.45e-04 1.18e-04 9.18e-05 6.52e-05 3.85e-05
Z
Y
1.19e-05 X
Particle Traces Colored by Particle Diameter (m) (Time=5.5000e-04) Jul 11, 2001 FLUENT 6.0 (3d, segregated, spe5, rke, unsteady)
Figure 14.6: Particle Tracks for the Spray Injection After 11 Time Steps
14-40
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
2. Create an isosurface of the methanol mass fraction. Surface −→Iso-Surface...
(a) Select Species... and Mass fraction of ch3oh in the Surface of Constant lists. (b) Click on Compute to update the minimum and maximum values. (c) Enter 0.001339 in the Iso-Values field. (d) Enter methanol-mf=0.001339 for the New Surface Name. (e) Click on Create to create the isosurface.
c Fluent Inc. November 27, 2001
14-41
Modeling Evaporating Liquid Spray
3. Display the isosurface you just created (methanol-mf=0.001339). Display −→Grid...
(a) Select methanol-mf=0.001339 in the Surfaces list. (b) Click the Colors... button.
14-42
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
(c) In the Grid Colors panel, select Color By Type. (d) Scroll down and select surface in the Types list and dark red in the Colors list. This will ensure that the isosurface is displayed in red, which contrasts better with the rest of the grid. (e) In the Grid Display panel, click Display. The graphics display will be updated to show the isosurface.
c Fluent Inc. November 27, 2001
14-43
Modeling Evaporating Liquid Spray
4. Modify the view to include the entire atomizer. Display −→Views...
(a) Increase the number of Periodic Repeats to 11. (b) Click Apply in the Views panel. (c) In the Grid Display panel, click Display. The graphics display will be updated to show the entire atomizer. (d) Use your mouse to obtain the view shown in Figure 14.7.
14-44
c Fluent Inc. November 27, 2001
Modeling Evaporating Liquid Spray
Z
Y
X
Grid (Time=5.5000e-04)
Jul 16, 2001 FLUENT 6.0 (3d, segregated, spe5, rke, unsteady)
Figure 14.7: Full Atomizer Display with Surface of Constant Methanol Mass Fraction
Summary: In this tutorial, you defined a discrete-phase spray injection for an air-blast atomizer and calculated a transient solution using the second-order implicit unsteady formulation. You viewed the location of methanol droplet particles after they had exited the atomizer and examined an isosurface of the methanol mass fraction.
c Fluent Inc. November 27, 2001
14-45
Modeling Evaporating Liquid Spray
14-46
c Fluent Inc. November 27, 2001
Tutorial 15.
Using the VOF Model
Introduction: This tutorial illustrates the setup and solution of the two-dimensional turbulent fluid flow in a partially filled spinning bowl. In this tutorial you will learn how to: • Set up and solve a transient free-surface problem using the segregated solver • Model the effect of gravity • Copy a material from the property database • Patch initial conditions in a subset of the domain • Define a custom field function • Mirror and rotate the view in the graphics window • Examine the fluid flow and the free-surface shape using velocity vectors and volume fraction contours Prerequisites: This tutorial requires a basic familiarity with FLUENT. You may also find it helpful to read about VOF multiphase flow modeling in the FLUENT User’s Guide. Otherwise, no previous experience with multiphase modeling is required. Problem Description: The information relevant to this problem is shown in Figure 15.1. A large bowl, 1 m in radius, is one-third filled with water and is open to the atmosphere. The bowl spins with an angular velocity of 3 rad/sec. Based on the rotating water, the Reynolds number is about 106 , so the flow is modeled as turbulent.
c Fluent Inc. November 27, 2001
15-1
Using the VOF Model
2 m
1m
Bowl: Ω = Air:
ρ =
µ = Water: ρ = µ =
3 rad/s 1.225 kg/m3 -5
1.7894 x 10 kg/m-s 998.2 kg/m 3 -3
1 x 10 kg/m-s
Figure 15.1: Water and Air in a Spinning Bowl
Preparation 1. Copy the file vof/bowl.msh from the FLUENT documentation CD to your working directory (as described in Tutorial 1). The mesh file bowl.msh is a quadrilateral mesh describing the system geometry shown in Figure 15.1. 2. Start the 2D version of FLUENT.
15-2
c Fluent Inc. November 27, 2001
Using the VOF Model
Step 1: Grid 1. Read the 2D grid file, bowl.msh. File −→ Read −→Case... 2. Display the grid (Figure 15.2). Display −→Grid...
As shown in Figure 15.2, half of the bowl is modeled, with a symmetry boundary at the centerline. The bowl is shown lying on its side, with the region to be modeled extending from the centerline to the outer wall. When you begin to display data graphically, you will need to rotate the view and mirror it across the centerline to obtain a more realistic view of the model. This step will be performed later in the tutorial.
c Fluent Inc. November 27, 2001
15-3
Using the VOF Model
Grid
Jun 12, 2001 FLUENT 6.0 (2d, segregated, lam)
Figure 15.2: Grid Display
15-4
c Fluent Inc. November 27, 2001
Using the VOF Model
Step 2: Models 1. Specify a transient model with axisymmetric swirl. Define −→ Models −→Solver...
(a) Retain the default Segregated solver. The segregated solver must be used for multiphase calculations. (b) Under Space, select Axisymmetric Swirl. (c) Under Time, select Unsteady.
c Fluent Inc. November 27, 2001
15-5
Using the VOF Model
2. Turn on the VOF model. Define −→ Models −→Multiphase...
(a) Select Volume of Fluid as the Model. The panel will expand to show inputs for the VOF model. (b) Under VOF Parameters, select Geo-Reconstruct (the default) as the VOF Scheme. This is the most accurate interface-tracking scheme, and is recommended for most transient VOF calculations. When you click OK, FLUENT will report that one of the zone types will need to be changed before proceeding with the calcu15-6
c Fluent Inc. November 27, 2001
Using the VOF Model
lation. You will take care of this step when you input boundary conditions for the problem. 3. Turn on the standard k- turbulence model. Define −→ Models −→Viscous...
(a) Select k-epsilon as the Model, and retain the default setting of Standard under k-epsilon Model.
c Fluent Inc. November 27, 2001
15-7
Using the VOF Model
Step 3: Materials 1. Copy water from the materials database so that it can be used for the secondary phase. Define −→Materials... (a) Click on the Database... button to open the Database Materials panel.
15-8
c Fluent Inc. November 27, 2001
Using the VOF Model
(b) In the Fluid Materials list (near the bottom), select waterliquid. (c) Click on Copy and close the Database Materials and Materials panels.
Step 4: Phases Here, water is defined as the secondary phase mainly for convenience in setting up the problem. When you define the initial solution, you will be patching an initial swirl velocity in the bottom third of the bowl, where the water is. It is more convenient to patch a water volume fraction of 1 there than to patch an air volume fraction of 1 in the rest of the domain. Also, the default volume fraction at the pressure inlet is 0, which is the correct value if water is the secondary phase. In general, you can specify the primary and secondary phases whichever way you prefer. It is a good idea, especially in more complicated problems, to consider how your choice will affect the ease of problem setup. 1. Define the air and water phases within the bowl. Define −→Phases...
c Fluent Inc. November 27, 2001
15-9
Using the VOF Model
(a) Specify air as the primary phase. i. Select phase-1 and click the Set... button.
ii. In the Primary Phase panel, enter air for the Name. iii. Keep the default selection of air for the Phase Material. (b) Specify water as the secondary phase. i. Select phase-2 and click the Set... button.
ii. In the Secondary Phase panel, enter water for the Name. iii. Select water-liquid from the Phase Material drop-down list.
15-10
c Fluent Inc. November 27, 2001
Using the VOF Model
Step 5: Operating Conditions 1. Set the gravitational acceleration. Define −→Operating Conditions...
(a) Turn on Gravity. The panel will expand to show additional inputs. (b) Set the Gravitational Acceleration in the X direction to 9.81 m/s2 . Since the centerline of the bowl is the x axis, gravity points in the positive x direction. 2. Set the operating density. (a) Under Variable-Density Parameters, turn on the Specified Operating Density option and accept the Operating Density of 1.225. It is a good idea to set the operating density to be the density of the lighter phase. This excludes the buildup of hydrostatic pressure within the lighter phase, improving the round-off accuracy for the momentum balance.
c Fluent Inc. November 27, 2001
15-11
Using the VOF Model
Note: The Reference Pressure Location (0,0) is situated in a region where the fluid will always be 100% of one of the phases (air), a condition that is essential for smooth and rapid convergence. If it were not, you would need to change it to a more appropriate location.
Step 6: Boundary Conditions Define −→Boundary Conditions... 1. Change the bowl centerline from a symmetry boundary to an axis boundary. For axisymmetric models, the axis of symmetry must be an axis zone. (a) Select symmetry-2 in the Zone list in the Boundary Conditions panel. (b) In the Type list, choose axis. You will have to scroll to the top of the list. (c) Click Yes in the Question dialog box that appears.
(d) Click OK in the Axis panel to accept the default Zone Name.
15-12
c Fluent Inc. November 27, 2001
Using the VOF Model
2. Set the conditions at the top of the bowl (the pressure inlet). For the VOF model, you will specify conditions for the mixture (i.e., conditions that apply to all phases) and also conditions that are specific to the secondary phase. There are no conditions to be specified for the primary phase. (a) Set the conditions for the mixture. i. In the Boundary Conditions panel, keep the default selection of mixture in the Phase drop-down list and click Set....
ii. Set the Turb. Kinetic Energy to 2.25e-2 and the Turb. Dissipation Rate to 7.92e-3. Since there is initially no flow passing through the pressure inlet, you need to specify k and explicitly rather than using one of the other turbulence specification methods. All of the other methods require you to specify the turbulence intensity, which is 0 in this case. The values for k and are computed as follows: c Fluent Inc. November 27, 2001
15-13
Using the VOF Model
k = (Iwwall )2
=
0.093/4 k3/2 `
where the turbulence intensity I is 0.05 (close to zero), wwall is 3 m/s, and ` is 0.07 (obtained by multiplying 0.07 by the maximum radius of the bowl, which is 1). See the User’s Guide for details about the specification of turbulence boundary conditions at flow inlets and exits. (b) Check the volume fraction of the secondary phase. i. In the Boundary Conditions panel, select water from the Phase drop-down list and click Set....
ii. Retain the default Volume Fraction of 0. A water volume fraction of 0 indicates that only air is present at the pressure inlet.
15-14
c Fluent Inc. November 27, 2001
Using the VOF Model
3. Set the conditions for the spinning bowl (the wall boundary). For a wall boundary, all conditions are specified for the mixture. There are no conditions to be specified for the individual phases. (a) In the Boundary Conditions panel, select mixture in the Phase drop-down list and click Set....
c Fluent Inc. November 27, 2001
15-15
Using the VOF Model
(b) Select Moving Wall under Wall Motion. The panel will expand to show inputs for the wall motion. (c) Under Motion, choose Rotational and then set the rotational Speed (Ω) to 3 rad/s.
15-16
c Fluent Inc. November 27, 2001
Using the VOF Model
Step 7: Solution In simple flows, the under-relaxation factors can usually be increased at the start of the calculation. This is particularly true when the VOF model is used, where high under-relaxation on all variables can greatly improve the performance of the solver. 1. Set the solution parameters. Solve −→ Controls −→Solution...
(a) Set all Under-Relaxation factors to 1. !
Be sure to use the scroll bar to access the under-relaxation factors that are initially out of view.
c Fluent Inc. November 27, 2001
15-17
Using the VOF Model
(b) Under Discretization, choose the Body Force Weighted scheme in the drop-down list next to Pressure. The body-force-weighted pressure discretization scheme is recommended when you solve a VOF problem involving gravity. (c) Also under Discretization, select PISO as the Pressure-Velocity Coupling method. PISO is recommended for transient flow calculations. 2. Enable the display of residuals during the solution process. Solve −→ Monitors −→Residual...
(a) Under Options, select Plot. (b) Click the OK button.
15-18
c Fluent Inc. November 27, 2001
Using the VOF Model
3. Enable the plotting of the axial velocity of water near the outer edge of the bowl during the calculation. For transient calculations, it is often useful to monitor the value of a particular variable to see how it changes over time. Here you will first specify the point at which you want to track the velocity, and then define the monitoring parameters. (a) Define a point surface near the outer edge of the bowl. Surface −→Point...
i. Set the x0 and y0 coordinates to 0.75 and 0.65. ii. Enter point for the New Surface Name. iii. Click Create.
c Fluent Inc. November 27, 2001
15-19
Using the VOF Model
(b) Define the monitoring parameters. Solve −→ Monitors −→Surface...
i. Increase the Surface Monitors value to 1. ii. Turn on the Plot and Write options for monitor-1. Note: When the Write option is selected in the Surface Monitors panel, the velocity history will be written to a file. If you do not select the Write option, the history information will be lost when you exit FLUENT. iii. In the drop-down list under Every, choose Time Step. iv. Click on Define... to specify the surface monitor parameters in the Define Surface Monitor panel.
15-20
c Fluent Inc. November 27, 2001
Using the VOF Model
v. Select Vertex Average from the Report Type drop-down list. This is the recommended choice when you are monitoring the value at a single point using a point surface. vi. Select Flow Time in the X Axis drop-down list. vii. Select Velocity... and Axial Velocity in the Report Of dropdown lists. viii. Select point in the Surfaces list. ix. Enter axial-velocity.out for the File Name. x. Click OK in the Define Surface Monitor panel and then in the Surface Monitors panel.
c Fluent Inc. November 27, 2001
15-21
Using the VOF Model
4. Initialize the solution. Solve −→ Initialize −→Initialize...
(a) Select pressure-inlet-4 in the Compute From drop-down list. All initial values will be set to zero, except for the turbulence quantities. (b) Click Init and close the panel.
15-22
c Fluent Inc. November 27, 2001
Using the VOF Model
5. Patch the initial distribution of water (i.e., water volume fraction of 1.0) and a swirl velocity of 3 rad/s in the bottom third of the bowl (where the water is). In order to patch a value in just a portion of the domain, you will need to define a cell “register” for that region. You will use the same tool that is used to mark a region of cells for adaption. Also, you will need to define a custom function for the swirl velocity. (a) Define a register for the bottom third of the domain. Adapt −→Region...
i. Set the (Xminimum,Yminimum) coordinate to (0.66,0), and the (Xmaximum,Ymaximum) coordinate to (1,1). ii. Click the Mark button. This creates a register containing the cells in this region.
c Fluent Inc. November 27, 2001
15-23
Using the VOF Model
(b) Check the register to be sure it is correct. Adapt −→Manage...
i. Select the register (hexahedron-r0) in the Registers list and click Display. The graphics display will show the bottom third of the bowl in red.
15-24
c Fluent Inc. November 27, 2001
Using the VOF Model
(c) Define a custom field function for the swirl velocity w = 3r. Define −→Custom Field Functions...
i. Click the 3 button on the calculator pad. The 3 will appear in the Definition field. If you make a mistake, click the DEL button to delete the last item you added to the function definition. ii. Click the X button on the calculator pad. iii. In the Field Functions drop-down list, select Grid... and Radial Coordinate. iv. Click the Select button. radial-coordinate will appear in the Definition. v. Enter a New Function Name of swirl-init. vi. Click Define. Note: If you wish to check the function definition, click on the Manage... button and select swirl-init.
c Fluent Inc. November 27, 2001
15-25
Using the VOF Model
(d) Patch the water volume fraction in the bottom third of the bowl. Solve −→ Initialize −→Patch...
i. Choose water Volume Fraction in the Variable list. ii. Select hexahedron-r0 in the Registers To Patch list. iii. Set the Value to 1. iv. Click Patch. This sets the water volume fraction to 1 in the lower third of the bowl. That is, you have defined the lower third of the bowl to be filled with water.
15-26
c Fluent Inc. November 27, 2001
Using the VOF Model
(e) Patch the swirl velocity in the bottom third of the bowl.
i. Choose Swirl Velocity in the Variable list. ii. Enable the Use Field Function option and select swirl-init in the Field Function list. iii. Click Patch. It’s a good idea to check your patch by displaying contours of the patched fields.
c Fluent Inc. November 27, 2001
15-27
Using the VOF Model
(f) Display contours of swirl velocity. Display −→Contours...
i. Select Velocity... and Swirl Velocity in the Contours Of lists. ii. Enable the Filled option and turn off the Node Values option. Since the values you patched are cell values, you should view the cell values, rather than the node values, to check that the patch has been performed correctly. (FLUENT computes the node values by averaging the cell values.) iii. Click Display. To make the view more realistic, you will need to rotate the display and mirror it across the centerline.
15-28
c Fluent Inc. November 27, 2001
Using the VOF Model
(g) Rotate the view and mirror it across the centerline. Display −→Views...
i. Select axis-2 in the Mirror Planes list and click Apply. ii. Use your middle and left mouse buttons to zoom and translate the view so that the entire bowl is visible in the graphics display. iii. Click on the Camera... button to open the Camera Parameters panel.
c Fluent Inc. November 27, 2001
15-29
Using the VOF Model
iv. Using your left mouse button, rotate the dial clockwise until the bowl appears upright in the graphics window (90◦ ). v. Close the Camera Parameters panel. vi. In the Views panel, click on the Save button under Actions to save the mirrored, upright view, and then close the panel. When you do this, view-0 will be added to the list of Views. The upright view of the bowl in Figure 15.3 correctly shows that w = 3r in the region of the bowl that is filled with water. 2.35e+00 2.12e+00 1.88e+00 1.65e+00 1.41e+00 1.18e+00 9.41e-01 7.06e-01 4.70e-01 2.35e-01 0.00e+00
Contours of Swirl Velocity (m/s) (Time=0.0000e+00) Jun 12, 2001 FLUENT 6.0 (axi, swirl, segregated, vof, ske, unsteady)
Figure 15.3: Contours of Initial Swirl Velocity
15-30
c Fluent Inc. November 27, 2001
Using the VOF Model
(h) Display contours of water volume fraction.
i. Select Phases... and Volume fraction of water in the Contours Of lists. ii. Set the number of contour Levels to 2 and click Display. There are only two possible values for the volume fraction at this point: 0 or 1. Figure 15.4 correctly shows that the bottom third of the bowl contains water.
c Fluent Inc. November 27, 2001
15-31
Using the VOF Model
1.00e+00
0.00e+00
Contours of Volume fraction of water (Time=0.0000e+00) Jun 12, 2001 FLUENT 6.0 (axi, swirl, segregated, vof, ske, unsteady)
Figure 15.4: Contours of Initial Water Volume Fraction
15-32
c Fluent Inc. November 27, 2001
Using the VOF Model
6. Set the time-step parameters for the calculation. Solve −→Iterate... (a) Set the Time Step Size to 0.002 seconds. (b) Click Apply. This will save the time step size to the case file (the next time a case file is saved). 7. Request saving of data files every 100 time steps. File −→ Write −→Autosave...
(a) Set the Autosave Case File Frequency to 0 and the Autosave Data File Frequency to 100. (b) Enter the Filename bowl and then click OK. FLUENT will append the time step value to the file name prefix (bowl). The standard .dat extension will also be appended. This will yield file names of the form bowl100.dat, where 100 is the time step number. 8. Save the initial case and data files (bowl.cas and bowl.dat). File −→ Write −→Case & Data... 9. Request 1000 time steps. Solve −→Iterate...
c Fluent Inc. November 27, 2001
15-33
Using the VOF Model
Since the time step is 0.002 seconds, you will be calculating up to t= 2 seconds. FLUENT will automatically save a data file after every 0.2 seconds, so you will have 10 data files for postprocessing. Figure 15.5 shows the time history for the axial velocity. The velocity is clearly oscillating, and the oscillations appear to be decaying over time (as the peaks become smaller). This periodic oscillation has a cycle of 1 second. The switch from a positive to a negative axial velocity indicates that the water is sloshing up and down the sides of the bowl in an attempt to reach an equilibrium position. The fact that the amplitude is decaying suggests that equilibrium will be reached at some point. The periodic behavior in evidence will therefore be present only during the initial startup phase of the bowl rotation. 0.3000
0.2000
0.1000
Average of Surface Vertex Values (m/s)
0.0000
-0.1000
-0.2000
-0.3000 0.0000 0.2000 0.4000 0.6000 0.8000 1.0000 1.2000 1.4000 1.6000 1.8000 2.0000
Flow Time
Convergence history of Axial Velocity on point (Time=2.0000e+00) Jun 13, 2001 FLUENT 6.0 (axi, swirl, segregated, vof, ske, unsteady)
Figure 15.5: Time History of Axial Velocity
15-34
c Fluent Inc. November 27, 2001
Using the VOF Model
Step 8: Postprocessing As indicated by changes in axial velocity in Figure 15.5, the flow field is oscillating periodically. In this step, you will examine the flow field at several different times. (Recall that FLUENT saved 10 data files for you during the calculation.) 1. Read in the data file of interest. File −→ Read −→Data... 2. Display filled contours of water volume fraction. Display −→Contours... Hint: Follow the instructions in substep 5h of Step 7: Solution (on page 15-31), but turn Node Values back on. Figures 15.6–15.9 show that the water level decreases from t = 0.4 to t = 0.6, then increases from t = 0.6 to t = 1. At t = 1, the water level in the center of the bowl has risen above the initial level, so you can expect the cycle to repeat as the water level begins to decrease again in an attempt to return to equilibrium. (You can read in the data files between t = 1 and t = 2 to confirm that this is in fact what happens. Since the time history of axial velocity (Figure 15.5) shows that the velocity oscillation is decaying over time, you can expect that if you were to continue the calculation, the water level would eventually reach some point where the gravitational and centrifugal forces balance and the water level reaches a new equilibrium point. Extra: Try continuing the calculation to determine how long it takes for the axial velocity oscillations in Figure 15.5 to disappear.
c Fluent Inc. November 27, 2001
15-35
Using the VOF Model
1.00e+00
0.00e+00
Contours of Volume fraction of water (Time=4.0000e-01) Jun 12, 2001 FLUENT 6.0 (axi, swirl, segregated, vof, ske, unsteady)
Figure 15.6: Shape of the Free Surface at t = 0.4 1.00e+00
0.00e+00
Contours of Volume fraction of water (Time=6.0000e-01) Jun 12, 2001 FLUENT 6.0 (axi, swirl, segregated, vof, ske, unsteady)
Figure 15.7: Shape of the Free Surface at t = 0.6
15-36
c Fluent Inc. November 27, 2001
Using the VOF Model
1.00e+00
0.00e+00
Contours of Volume fraction of water (Time=8.0000e-01) Jun 12, 2001 FLUENT 6.0 (axi, swirl, segregated, vof, ske, unsteady)
Figure 15.8: Shape of the Free Surface at t = 0.8 1.00e+00
0.00e+00
Contours of Volume fraction of water (Time=9.9999e-01) Jun 12, 2001 FLUENT 6.0 (axi, swirl, segregated, vof, ske, unsteady)
Figure 15.9: Shape of the Free Surface at t = 1
c Fluent Inc. November 27, 2001
15-37
Using the VOF Model
3. Plot contours of stream function. (a) Select Stream Function (in the Velocity... category) in the Contours Of drop-down list. (b) Turn off the Filled option and increase the number of contour Levels to 30. (c) Click on Display. In Figures 15.10–15.13, you can see a recirculation region that falls and rises as the water level changes. To get a better sense of these recirculating patterns, you will next look at velocity vectors.
15-38
c Fluent Inc. November 27, 2001
Using the VOF Model
2.58e+01 2.41e+01 2.24e+01 2.06e+01 1.89e+01 1.72e+01 1.55e+01 1.38e+01 1.20e+01 1.03e+01 8.60e+00 6.88e+00 5.16e+00 3.44e+00 1.72e+00 0.00e+00
Contours of Stream Function (kg/s) (Time=4.0000e-01) Jun 12, 2001 FLUENT 6.0 (axi, swirl, segregated, vof, ske, unsteady)
Figure 15.10: Contours of Stream Function at t = 0.4 2.65e+01 2.47e+01 2.29e+01 2.12e+01 1.94e+01 1.76e+01 1.59e+01 1.41e+01 1.24e+01 1.06e+01 8.82e+00 7.06e+00 5.29e+00 3.53e+00 1.76e+00 0.00e+00
Contours of Stream Function (kg/s) (Time=6.0000e-01) Jun 12, 2001 FLUENT 6.0 (axi, swirl, segregated, vof, ske, unsteady)
Figure 15.11: Contours of Stream Function at t = 0.6
c Fluent Inc. November 27, 2001
15-39
Using the VOF Model
4.73e+01 4.41e+01 4.10e+01 3.78e+01 3.47e+01 3.15e+01 2.84e+01 2.52e+01 2.21e+01 1.89e+01 1.58e+01 1.26e+01 9.46e+00 6.31e+00 3.15e+00 0.00e+00
Contours of Stream Function (kg/s) (Time=8.0000e-01) Jun 12, 2001 FLUENT 6.0 (axi, swirl, segregated, vof, ske, unsteady)
Figure 15.12: Contours of Stream Function at t = 0.8 8.84e+00 8.25e+00 7.66e+00 7.07e+00 6.48e+00 5.89e+00 5.30e+00 4.71e+00 4.13e+00 3.54e+00 2.95e+00 2.36e+00 1.77e+00 1.18e+00 5.89e-01 0.00e+00
Contours of Stream Function (kg/s) (Time=9.9999e-01) Jun 12, 2001 FLUENT 6.0 (axi, swirl, segregated, vof, ske, unsteady)
Figure 15.13: Contours of Stream Function at t = 1
15-40
c Fluent Inc. November 27, 2001
Using the VOF Model
4. Plot velocity vectors in the bowl. Display −→Vectors...
(a) In the Style drop-down list, select arrow. This will make the velocity direction easier to see. (b) Increase the Scale factor to 6 and increase the Skip value to 1. (c) Click on Vector Options... to open the Vector Options panel.
c Fluent Inc. November 27, 2001
15-41
Using the VOF Model
i. Turn off the Z Component. This allows you to examine the non-swirling components only. ii. Click Apply and close the panel. (d) Click on Display. Figures 15.14–15.17 show the changes in water and air flow patterns between t = 0.4 and t = 1. In Figure 15.14, you can see that the flow in the middle of the bowl is being pulled down by gravitational forces, and pushed out and up along the sides of the bowl by centrifugal forces. This causes the water level to decrease in the center of the bowl, as shown in the volume fraction contour plots, and also results in the formation of a recirculation region in the air above the water surface. In Figure 15.15, the flow has reversed direction, and is slowly rising up in the middle of the bowl and being pulled down along the sides of the bowl. This reversal occurs because the earlier flow pattern caused the water to overshoot the equilibrium position. The gravity and centrifugal forces now act to compensate for this overshoot.
15-42
c Fluent Inc. November 27, 2001
Using the VOF Model
1.92e+00 1.79e+00 1.66e+00 1.54e+00 1.41e+00 1.28e+00 1.16e+00 1.03e+00 9.00e-01 7.73e-01 6.46e-01 5.18e-01 3.91e-01 2.63e-01 1.36e-01 8.63e-03
Velocity Vectors Colored By Velocity Magnitude (m/s) (Time=4.0000e-01) Jun 12, 2001 FLUENT 6.0 (axi, swirl, segregated, vof, ske, unsteady)
Figure 15.14: Velocity Vectors for the Air and Water at t = 0.4 1.94e+00 1.81e+00 1.68e+00 1.55e+00 1.42e+00 1.30e+00 1.17e+00 1.04e+00 9.07e-01 7.77e-01 6.48e-01 5.18e-01 3.89e-01 2.59e-01 1.30e-01 4.88e-04
Velocity Vectors Colored By Velocity Magnitude (m/s) (Time=6.0000e-01) Jun 12, 2001 FLUENT 6.0 (axi, swirl, segregated, vof, ske, unsteady)
Figure 15.15: Velocity Vectors for the Air and Water at t = 0.6
c Fluent Inc. November 27, 2001
15-43
Using the VOF Model
2.13e+00 1.99e+00 1.85e+00 1.71e+00 1.57e+00 1.42e+00 1.28e+00 1.14e+00 9.98e-01 8.56e-01 7.15e-01 5.73e-01 4.31e-01 2.89e-01 1.47e-01 5.04e-03
Velocity Vectors Colored By Velocity Magnitude (m/s) (Time=8.0000e-01) Jun 12, 2001 FLUENT 6.0 (axi, swirl, segregated, vof, ske, unsteady)
Figure 15.16: Velocity Vectors for the Air and Water at t = 0.8 2.12e+00 1.98e+00 1.84e+00 1.70e+00 1.56e+00 1.41e+00 1.27e+00 1.13e+00 9.91e-01 8.50e-01 7.09e-01 5.68e-01 4.27e-01 2.85e-01 1.44e-01 3.06e-03
Velocity Vectors Colored By Velocity Magnitude (m/s) (Time=9.9999e-01) Jun 12, 2001 FLUENT 6.0 (axi, swirl, segregated, vof, ske, unsteady)
Figure 15.17: Velocity Vectors for the Air and Water at t = 1
15-44
c Fluent Inc. November 27, 2001
Using the VOF Model
In Figure 15.16 you can see that the flow is rising up more quickly in the middle of the bowl, and in Figure 15.17 you can see that the flow is still moving upward, but more slowly. These patterns correspond to the volume fraction plots at these times. As the upward motion in the center of the bowl decreases, you can expect the flow to reverse as the water again seeks to reach a state of equilibrium. Summary: In this tutorial, you have learned how to use the VOF free surface model to solve a problem involving a spinning bowl of water. The time-dependent VOF formulation is used in this problem to track the shape of the free surface and the flow field inside the spinning bowl. You observed the changing pattern of the water and air in the bowl by displaying volume fraction contours, stream function contours, and velocity vectors at t = 0.4, t = 0.6, t = 0.8, and t = 1 second.
c Fluent Inc. November 27, 2001
15-45
Tutorial 16.
Modeling Cavitation
Introduction: This tutorial examines the flow of water around a torpedo. Cavitation occurs in many applications as a result of flow acceleration over a body surface. Vapor production is localized at the wall where the pressure is below the vaporization pressure pv , so grid refinement and the use of non-equilibrium wall functions improve the accuracy of the simulation. The case is taken from a paper by Kunz et al. [1]. Using FLUENT’s multiphase modeling capability, you will be able to predict the inception of cavitation near the nose of the torpedo. In this tutorial you will learn how to: • Set boundary conditions for external flow • Use the mixture model with cavitation effects • Calculate a solution using the segregated solver • Use a pressure coefficient monitor to check solution convergence Prerequisites: This tutorial assumes that you are familiar with the menu structure in FLUENT and that you have solved or read Tutorial 1. Some steps in the setup and solution procedure will not be shown explicitly. Problem Description: The problem considers the cavitation caused by the flow of water around a torpedo at an incidence angle of zero and a free-stream velocity of 1 m/s (U∞ = 1 m/s). The torpedo diameter is 0.136 m. The geometry of the torpedo is shown in Figure 16.1.
c Fluent Inc. November 27, 2001
16-1
Modeling Cavitation
D = 0.136 m U = 1 m/s
Figure 16.1: Problem Specification
Preparation 1. Copy the file cav/cav.msh from the FLUENT documentation CD to your working directory (as described in Tutorial 1). 2. Start the 2D version of FLUENT.
16-2
c Fluent Inc. November 27, 2001
Modeling Cavitation
Step 1: Grid 1. Read the grid file (cav.msh). File −→ Read −→Case... As FLUENT reads the grid file, it will report its progress in the console window. 2. Check the grid. Grid −→Check FLUENT will perform various checks on the mesh and will report the progress in the console window. Pay particular attention to the reported minimum volume. Make sure this is a positive number. 3. Display the grid. Display −→Grid...
c Fluent Inc. November 27, 2001
16-3
Modeling Cavitation
(a) Display the grid using the default settings (Figure 16.2). As shown in Figure 16.2, half of the torpedo is modeled, with an axis boundary at the centerline. Especially when you begin to display data graphically, you may want to mirror the view across the centerline to obtain a more realistic view of the model. This step will be performed later in the tutorial. (b) Use the middle mouse button to zoom in on the image so you can see the mesh near the torpedo (Figures 16.3 and 16.4).
Grid
Jun 18, 2001 FLUENT 6.0 (axi, segregated, mixture, ske)
Figure 16.2: The Grid Around the Torpedo This mesh is quadrilateral. The gradients normal to the torpedo wall are much greater than those tangent to the torpedo, except near the tip and at the transition between the nose and the main body. Consequently, the cells nearest the surface have very high aspect ratios.
16-4
c Fluent Inc. November 27, 2001
Modeling Cavitation
Grid
Jun 18, 2001 FLUENT 6.0 (axi, segregated, mixture, ske)
Figure 16.3: The Grid After Zooming In on the Torpedo
Grid
Jun 18, 2001 FLUENT 6.0 (axi, segregated, mixture, ske)
Figure 16.4: The Grid After Zooming In Further on the Torpedo
c Fluent Inc. November 27, 2001
16-5
Modeling Cavitation
Step 2: Models 1. Specify a steady-state axisymmetric model. Define −→ Models −→Solver... The segregated solver must be used for multiphase calculations.
(a) Under Space, select Axisymmetric. (b) Keep the default settings for everything else. Note: A computationally-intensive unsteady calculation is necessary to accurately simulate the irregular cyclic process of bubble formation, growth, filling by water jet re-entry, and breakoff. In this tutorial, you will perform a steady-state calculation to simulate just the formation of the first bubble near the nose of the torpedo.
16-6
c Fluent Inc. November 27, 2001
Modeling Cavitation
2. Enable the multiphase mixture model with cavitation effects. Define −→ Models −→Multiphase... (a) Select Mixture as the Model. The panel will expand. (b) Under Mixture Parameters, turn off Slip Velocity. Since there is no significant difference in velocities for the different phases, there is no need to solve for the slip velocity equation. (c) Select Cavitation under Interphase Mass Transfer. The panel will expand again to show the cavitation inputs.
c Fluent Inc. November 27, 2001
16-7
Modeling Cavitation
(d) Enter 101175 for the Vaporization Pressure. The vaporization pressure depends on the operating pressure, the free-stream velocity, the density of the liquid, and a nondimensional parameter known as the cavitation number. The value above is taken from the literature. (e) Set the Bubble Number Density to 9e6. The Bubble Number Density is the number of bubbles of vapor per unit volume, and is assumed constant. The value of 9×106 is taken from the literature. 3. Turn on the standard k- turbulence model with non-equilibrium wall functions. Define −→ Models −→Viscous... (a) Select k-epsilon as the Model.
16-8
c Fluent Inc. November 27, 2001
Modeling Cavitation
(b) Keep the default selection of Standard under k-epsilon Model. The standard k- model has been found to be quite effective in accurately resolving the near-wall region when non-equilibrium wall functions are used. (c) Select Non-Equilibrium Wall Functions under Near-Wall Treatment.
c Fluent Inc. November 27, 2001
16-9
Modeling Cavitation
Step 3: Materials 1. Copy liquid water and water vapor from the materials database so that they can be used for the primary and secondary phases. Define −→Materials... (a) Click the Database... button in the Materials panel. The Database Materials panel will open.
16-10
c Fluent Inc. November 27, 2001
Modeling Cavitation
(b) In the list of Fluid Materials, select water-liquid (h2o). (c) Click Copy to copy the information for liquid water to your model. (d) In the list of Fluid Materials, select water-vapor (h2o). (e) Click Copy to copy the information for water vapor to your model. (f) Close the Database Materials panel and the Materials panel.
c Fluent Inc. November 27, 2001
16-11
Modeling Cavitation
Step 4: Phases 1. Define the liquid water and water vapor phases that flow around the torpedo. Define −→Phases...
(a) Specify liquid water as the primary phase. i. Select phase-1 and click the Set... button.
ii. In the Primary Phase panel, enter water for the Name. iii. Select water-liquid from the Phase Material drop-down list.
16-12
c Fluent Inc. November 27, 2001
Modeling Cavitation
(b) Specify water vapor as the secondary phase. i. Select phase-2 and click the Set... button.
ii. In the Secondary Phase panel, enter water-vapor for the Name. iii. Select water-vapor from the Phase Material drop-down list.
c Fluent Inc. November 27, 2001
16-13
Modeling Cavitation
Step 5: Boundary Conditions For this problem, you need to set the boundary conditions for two boundaries: the velocity inlet and the pressure outlet. The velocity inlet comprises the circular arc grid boundary, and the pressure outlet is the downstream boundary, opposite the velocity inlet. 1. Set the conditions for the velocity inlet (velocity-inlet-5). For the multiphase mixture model, you will specify conditions for the mixture (i.e., conditions that apply to all phases) and also conditions that are specific to the primary and secondary phases. In this tutorial, boundary conditions are needed for the mixture and secondary phase only. (a) Set the conditions for the mixture. Define −→Boundary Conditions... i. In the Boundary Conditions panel, keep the default selection of mixture in the Phase drop-down list and click Set.... ii. In the Velocity Specification Method drop-down list, select Components. iii. In the Reference Frame drop-down list, keep the default selection of Absolute. iv. Under Axial-Velocity (m/s), input 1. v. In the Turbulence Specification Method drop-down list, select Intensity and Viscosity Ratio. vi. Set Turbulence Intensity to 0.5% and Turbulence Viscosity Ratio to 5. For external flows, you should choose a viscosity ratio between 1 and 10.
16-14
c Fluent Inc. November 27, 2001
Modeling Cavitation
(b) Check the volume fraction of the secondary phase. i. In the Boundary Conditions panel, select water-vapor from the Phase drop-down list and click Set....
ii. Retain the default Volume Fraction of 0.
c Fluent Inc. November 27, 2001
16-15
Modeling Cavitation
2. Set the boundary conditions for the pressure outlet (pressure-outlet4). The turbulence conditions you input at the pressure outlet will be used only if flow enters the domain through this boundary. You can set them equal to the inlet values, as no flow reversal is expected at the pressure outlet. In general, however, it is important to set reasonable values for these downstream scalar values, in case flow reversal occurs at some point during the calculation. (a) Set the conditions for the mixture. i. In the Boundary Conditions panel, select mixture in the Phase drop-down list and click Set....
ii. Select Intensity and Viscosity Ratio for the Turbulence Specification Method. iii. Set the Turbulence Intensity to 0.5%. iv. Set the Turbulent Viscosity Ratio to 5. (b) Check the volume fraction of the secondary phase. i. In the Boundary Conditions panel, select water-vapor from the Phase drop-down list and click Set.... ii. Retain the default Volume Fraction of 0.
16-16
c Fluent Inc. November 27, 2001
Modeling Cavitation
Step 6: Solution 1. Set the solution parameters. Solve −→ Controls −→Solution...
(a) Under Under-Relaxation Factors, set the under-relaxation factor for Momentum to 0.1. (b) Scroll down and set the Vaporization Mass under-relaxation factor to 0.001. The source term created by “evaporation” greatly affects the numerics of the pressure correction. In order to prevent divergence, you need to use a small under-relaxation factor for this source term.
c Fluent Inc. November 27, 2001
16-17
Modeling Cavitation
(c) Set the under-relaxation factor for Volume Fraction to 0.1. (d) Under Discretization, select PRESTO! in the Pressure dropdown list and Second Order Upwind in the Momentum dropdown list. 2. Enable the plotting of residuals during the calculation. Solve −→ Monitors −→Residual...
(a) Change the convergence criterion for continuity to 1e-5 for improved accuracy. (b) Select Plot under Options, and click on OK.
16-18
c Fluent Inc. November 27, 2001
Modeling Cavitation
3. Initialize the solution. Solve −→ Initialize −→Initialize...
(a) Select velocity-inlet-5 in the Compute From drop-down list. (b) Click Init to initialize the solution. 4. Set the reference values for the torpedo. To monitor the convergence of the calculation, you will enable the plotting of the area-weighted average of the pressure coefficient on the outer boundary of the torpedo. Reference values must be set correctly in order for the pressure coefficient calculated by FLUENT to be realistic. FLUENT uses the reference density to calculate the pressure coefficient. For the first few iterations, when the solution is fluctuating, the pressure coefficient will behave erratically. This can cause the scale of the y axis for the plot to be set too wide, making variations in the value of the coefficient less evident. To avoid this problem, you will have FLUENT perform a small number of iterations, and then you will adjust the pressure coefficient monitor scale.
c Fluent Inc. November 27, 2001
16-19
Modeling Cavitation
Report −→Reference Values...
(a) In the Compute From drop-down list, select velocity-inlet-5. The panel will update to reflect the new values.
16-20
c Fluent Inc. November 27, 2001
Modeling Cavitation
5. Set up a monitor for the pressure coefficient. Solve −→ Monitors −→Surface... Plotting the pressure coefficient will help you monitor the convergence of the solution.
(a) Increase the number of Surface Monitors to 1. (b) Enable the Plot and Write options for monitor-1. (c) Click on Define... to the right of monitor-1. This will open the Define Surface Monitor panel.
c Fluent Inc. November 27, 2001
16-21
Modeling Cavitation
(d) In the Report Of drop-down lists, select Pressure... and Pressure Coefficient. (e) In the Report Type drop-down list, select Area-Weighted Average. (f) Set the Plot Window to 1. (g) In the Surfaces list, select wall-1. (h) Click OK in the Define Surface Monitor panel and then in the Surface Monitors panel.
16-22
c Fluent Inc. November 27, 2001
Modeling Cavitation
6. Save the case file (cav.cas). File −→ Write −→Case... 7. Start the calculation by requesting 50 iterations. Solve −→Iterate... 8. Change the plot scale for the pressure coefficient. Solve −→ Monitors −→Surface... (a) Click on Define... to the right of monitor-1. This will open the Define Surface Monitor panel.
i. Click the Axes... button. The Axes - Surface Monitor Plot panel will open.
c Fluent Inc. November 27, 2001
16-23
Modeling Cavitation
ii. In the Axes - Surface Monitor Plot panel, select Y as the Axis. iii. Under Number Format, set Precision to 4. iv. Deselect Auto Range. v. Enter a new Range of -0.04 to 0. vi. Click Apply and close the Axes - Surface Monitor Plot panel. (b) Continue the calculation by requesting 1100 additional iterations. Solve −→Iterate... FLUENT will ask you to confirm that it is OK to append data to the pressure coefficient monitor file. (c) Click Yes to continue. The pressure coefficient has not converged yet, as shown in Figure 16.5, but an inspection of the pressure contours and 16-24
c Fluent Inc. November 27, 2001
Modeling Cavitation
the pressure coefficient values on the surface of the torpedo in the next step show good correlation with existing experimental data [1].
0.0000 -0.0050 -0.0100 -0.0150
Area Weighted Average
-0.0200 -0.0250 -0.0300 -0.0350 -0.0400 0
200
400
600
800
1000
1200
Iteration
Convergence history of Pressure Coefficient on wall-1
Jun 19, 2001 FLUENT 6.0 (axi, segregated, mixture, ske)
Figure 16.5: Pressure Coefficient History (d) Save the data file (cav.dat). File −→ Write −→Data...
c Fluent Inc. November 27, 2001
16-25
Modeling Cavitation
Step 7: Postprocessing 1. Plot the pressure around the torpedo. Display −→Contours...
(a) Select Pressure... and Static Pressure in the drop-down lists under Contours Of. (b) Select Filled under Options. (c) Click Display. Note the low-pressure region near the nose of the torpedo in Figure 16.6. This is where cavitation is expected to occur. To make the view more realistic, you will need to mirror it across the centerline.
16-26
c Fluent Inc. November 27, 2001
Modeling Cavitation
5.33e+02 4.59e+02 3.84e+02 3.09e+02 2.34e+02 1.60e+02 8.49e+01 1.02e+01 -6.46e+01 -1.39e+02 -2.14e+02
Contours of Static Pressure (pascal)
Jun 19, 2001 FLUENT 6.0 (axi, segregated, mixture, ske)
Figure 16.6: Contours of Static Pressure 2. Mirror the display across the centerline. Display −→Views...
c Fluent Inc. November 27, 2001
16-27
Modeling Cavitation
(a) Select axis-2 in the Mirror Planes list and click Apply. (b) Use your middle and left mouse buttons to zoom and translate the view so that the entire torpedo is visible in the graphics display (Figure 16.7). 5.33e+02 4.59e+02 3.84e+02 3.09e+02 2.34e+02 1.60e+02 8.49e+01 1.02e+01 -6.46e+01 -1.39e+02 -2.14e+02
Contours of Static Pressure (pascal)
Jun 28, 2001 FLUENT 6.0 (axi, segregated, mixture, ske)
Figure 16.7: Mirrored View of Contours of Static Pressure 3. Plot the volume fraction of water vapor. Display −→Contours... (a) Select Phases... and Volume fraction of water-vapor in the dropdown lists under Contours Of. (b) Click Display. Note that the low-pressure region near the nose of the torpedo (Figure 16.7) coincides with the highest volume fraction of water vapor in Figure 16.8.
16-28
c Fluent Inc. November 27, 2001
Modeling Cavitation
7.33e-01 6.59e-01 5.86e-01 5.13e-01 4.40e-01 3.66e-01 2.93e-01 2.20e-01 1.47e-01 7.33e-02 0.00e+00
Contours of Volume fraction of water-vapor
Jun 28, 2001 FLUENT 6.0 (axi, segregated, mixture, ske)
Figure 16.8: Contours of Water Vapor Volume Fraction
c Fluent Inc. November 27, 2001
16-29
Modeling Cavitation
4. Plot the variation of the pressure coefficient on the surface of the torpedo. You used the area-weighted average of the pressure coefficient on wall-1 to monitor the solution convergence. Now you will plot the pressure coefficient distribution on wall-1 at the last iteration performed. Plot −→XY Plot...
(a) Under Y Axis Function, select Pressure... and Pressure Coefficient. (b) Under Surfaces, select wall-1. (c) Click Plot.
16-30
c Fluent Inc. November 27, 2001
Modeling Cavitation
wall-1 1.20e+00 1.00e+00 8.00e-01 6.00e-01 4.00e-01
Pressure Coefficient
2.00e-01 0.00e+00 -2.00e-01 -4.00e-01 -6.00e-01 -0.1
0
0.1
0.2
0.3
0.4
0.5
0.6
0.7
Position (m)
Pressure Coefficient
Jun 19, 2001 FLUENT 6.0 (axi, segregated, mixture, ske)
Figure 16.9: Pressure Coefficient Distribution on the Torpedo
c Fluent Inc. November 27, 2001
16-31
Modeling Cavitation
Summary: This tutorial demonstrated how to set up a cavitating flow around a torpedo, using FLUENT’s multiphase mixture model with cavitation effects. You learned how to set the boundary conditions for an external flow, check grid validity by plotting y + , and how to use surface monitors to monitor the solution convergence. A steady-state solution was calculated to simulate the formation of a vapor bubble close to the nose of the torpedo. Even within this first approximation, good correlation is found between the calculated pressure coefficient distribution on the surface of the torpedo and that shown in published data [1]. A more computationallyintensive unsteady calculation is necessary to accurately simulate the irregular cyclic process of bubble formation, growth, filling by water jet re-entry, and breakoff. References: 1. Kunz, R.F., Boger, B.A., Chyczewski, T.S., Stineberg, D.R., Gibeling, H.J., and Govindan T.R.,“Multiphase CFD of Natural Ventilated Cavitation about Submerged Bodies”, in ASME paper FEDSM99-7364, Proceedings of 3rd ASME/JSME Joint Fluids Engineering Conference, 1999.
16-32
c Fluent Inc. November 27, 2001
Tutorial 17. Using the Mixture and Eulerian Multiphase Models
Introduction: This tutorial examines the flow of water and air in a tee junction. First you will solve the problem using the less computationally-intensive mixture model, and then you will turn to the more accurate Eulerian model. Finally, you will compare the results obtained with the two approaches. In this tutorial you will learn how to: • Use the mixture model with slip velocities • Set boundary conditions for internal flow • Calculate a solution using the segregated solver • Use the Eulerian model • Compare the results obtained with the two approaches Prerequisites: This tutorial assumes that you are familiar with the menu structure in FLUENT and that you have solved or read Tutorial 1. Some steps in the setup and solution procedure will not be shown explicitly. Problem Description: This problem considers an air-water mixture flowing upwards in a duct and then splitting in a tee-junction. The ducts are 25 mm in width, the inlet section of the duct is 125 mm long, and the top and the side ducts are 250 mm long. The geometry and data for the problem are shown in Figure 17.1.
c Fluent Inc. November 27, 2001
17-1
Using the Mixture and Eulerian Multiphase Models
velocity inlet water: v = - 0.31 m/s air: v = - 0.45 m/s
pressure outlet
velocity inlet water: ρ=1000 kg/m3 µ=9e-4 kg/m-s v=1.53 m/s
air: ρ=1.2 kg/m3 µ=2e-5 kg/m-s v=1.6 m/s vol frac=0.02 bubble diam=1 mm
Figure 17.1: Problem Specification
17-2
c Fluent Inc. November 27, 2001
Using the Mixture and Eulerian Multiphase Models
Preparation 1. Copy the file tee/tee.msh from the FLUENT documentation CD to your working directory (as described in Tutorial 1). 2. Start the 2D version of FLUENT.
c Fluent Inc. November 27, 2001
17-3
Using the Mixture and Eulerian Multiphase Models
Step 1: Grid 1. Read the grid file (tee.msh). File −→ Read −→Case... As FLUENT reads the grid file, it will report its progress in the console window. 2. Check the grid. Grid −→Check FLUENT will perform various checks on the mesh and will report the progress in the console window. Pay particular attention to the reported minimum volume. Make sure this is a positive number. 3. Display the grid. Display −→Grid...
(a) Display the grid using the default settings (Figure 17.2). 17-4
c Fluent Inc. November 27, 2001
Using the Mixture and Eulerian Multiphase Models
Grid
Jul 24, 2001 FLUENT 6.0 (2d, segregated, lam)
Figure 17.2: The Grid in the Tee Junction Extra: You can use the right mouse button to check which zone number corresponds to each boundary. If you click the right mouse button on one of the boundaries in the graphics window, its zone number, name, and type will be printed in the FLUENT console window. This feature is especially useful when you have several zones of the same type and you want to distinguish between them quickly.
c Fluent Inc. November 27, 2001
17-5
Using the Mixture and Eulerian Multiphase Models
Step 2: Models 1. Keep the default settings for the 2D segregated steady-state solver. Define −→ Models −→Solver... The segregated solver must be used for multiphase calculations.
2. Enable the multiphase mixture model with slip velocities. Define −→ Models −→Multiphase... (a) Select Mixture as the Model. The panel will expand to show the inputs for the mixture model. (b) Under Mixture Parameters, keep the Slip Velocity turned on. Since there will be significant difference in velocities for the different phases, you need to solve the slip velocity equation.
17-6
c Fluent Inc. November 27, 2001
Using the Mixture and Eulerian Multiphase Models
(c) Under Body Force Formulation, select Implicit Body Force. This treatment improves solution convergence by accounting for the partial equilibrium of the pressure gradient and body forces in the momentum equations. It is used when body forces are large in comparison to viscous and convective forces, namely in VOF and mixture problems.
c Fluent Inc. November 27, 2001
17-7
Using the Mixture and Eulerian Multiphase Models
3. Turn on the standard k- turbulence model with standard wall functions. Define −→ Models −→Viscous...
(a) Select k-epsilon as the Model. (b) Under k-epsilon Model, keep the default selection of Standard. The standard k- model has been found to be quite effective in accurately resolving mixture problems when standard wall functions are used. (c) Keep the default selection of Standard Wall Functions under Near-Wall Treatment. This problem does not require a particularly fine grid, and standard wall functions will be used.
17-8
c Fluent Inc. November 27, 2001
Using the Mixture and Eulerian Multiphase Models
4. Set the gravitational acceleration. Define −→Operating Conditions... (a) Turn on Gravity. The panel will expand to show additional inputs.
(b) Set the Gravitational Acceleration in the Y direction to -9.81 m/s2 .
c Fluent Inc. November 27, 2001
17-9
Using the Mixture and Eulerian Multiphase Models
Step 3: Materials 1. Copy liquid water from the materials database so that it can be used for the primary phase. Define −→Materials... (a) Click the Database... button in the Materials panel. The Database Materials panel will open.
17-10
c Fluent Inc. November 27, 2001
Using the Mixture and Eulerian Multiphase Models
(b) In the list of Fluid Materials, select water-liquid (h2o). (c) Click Copy to copy the information for liquid water to your model. (d) Close the Database Materials panel and the Materials panel.
c Fluent Inc. November 27, 2001
17-11
Using the Mixture and Eulerian Multiphase Models
Step 4: Phases 1. Define the liquid water and air phases that flow in the tee junction. Define −→Phases...
(a) Specify liquid water as the primary phase. i. Select phase-1 and click the Set... button.
ii. In the Primary Phase panel, enter water for the Name. iii. Select water-liquid from the Phase Material drop-down list.
17-12
c Fluent Inc. November 27, 2001
Using the Mixture and Eulerian Multiphase Models
(b) Specify air as the secondary phase. i. Select phase-2 and click the Set... button.
ii. In the Secondary Phase panel, enter air for the Name. iii. Select air from the Phase Material drop-down list. iv. Set the Diameter to 0.001 m.
c Fluent Inc. November 27, 2001
17-13
Using the Mixture and Eulerian Multiphase Models
2. Check the slip velocity formulation to be used. (a) Click the Interaction... button in the Phases panel.
(b) In the Phase Interaction panel, keep the default selection of manninen-et-al in the Slip Velocity drop-down list.
17-14
c Fluent Inc. November 27, 2001
Using the Mixture and Eulerian Multiphase Models
Step 5: Boundary Conditions For this problem, you need to set the boundary conditions for three boundaries: the upper and lower velocity inlets and the pressure outlet. Define −→Boundary Conditions... 1. Set the conditions for the lower velocity inlet (velocity-inlet-4). For the multiphase mixture model, you will specify conditions at a velocity inlet for the mixture (i.e., conditions that apply to all phases) and also conditions that are specific to the primary and secondary phases. (a) Set the conditions at velocity-inlet-4 for the mixture. i. In the Boundary Conditions panel, keep the default selection of mixture in the Phase drop-down list and click Set....
ii. In the Turbulence Specification Method drop-down list, select Intensity and Length Scale. iii. Set Turbulence Intensity to 10% and Turbulence Length Scale to 0.025 m.
c Fluent Inc. November 27, 2001
17-15
Using the Mixture and Eulerian Multiphase Models
(b) Set the conditions for the primary phase. i. In the Boundary Conditions panel, select water from the Phase drop-down list and click Set....
ii. Keep the default Velocity Specification Method and Reference Frame. iii. Set the Velocity Magnitude to 1.53.
17-16
c Fluent Inc. November 27, 2001
Using the Mixture and Eulerian Multiphase Models
(c) Set the conditions for the secondary phase. i. In the Boundary Conditions panel, select air from the Phase drop-down list and click Set....
ii. Keep the default Velocity Specification Method and Reference Frame. iii. Set the Velocity Magnitude to 1.6. iv. Set the Volume Fraction to 0.02.
c Fluent Inc. November 27, 2001
17-17
Using the Mixture and Eulerian Multiphase Models
2. Set the conditions for the upper velocity inlet (velocity-inlet-5). (a) Set the conditions at velocity-inlet-5 for the mixture. i. In the Boundary Conditions panel, select mixture in the Phase drop-down list and click Set....
ii. In the Turbulence Specification Method drop-down list, select Intensity and Length Scale. iii. Set Turbulence Intensity to 10% and Turbulence Length Scale to 0.025 m.
17-18
c Fluent Inc. November 27, 2001
Using the Mixture and Eulerian Multiphase Models
(b) Set the conditions for the primary phase. i. In the Boundary Conditions panel, select water from the Phase drop-down list and click Set....
ii. Keep the default Velocity Specification Method and Reference Frame. iii. Set the Velocity Magnitude to -0.31. In this problem, outflow characteristics at the upper velocity inlet are assumed to be known, and therefore imposed as a boundary condition.
c Fluent Inc. November 27, 2001
17-19
Using the Mixture and Eulerian Multiphase Models
(c) Set the conditions for the secondary phase. i. In the Boundary Conditions panel, select air from the Phase drop-down list and click Set....
ii. Keep the default Velocity Specification Method and Reference Frame. iii. Set the Velocity Magnitude to -0.45. iv. Set the Volume Fraction to 0.02.
17-20
c Fluent Inc. November 27, 2001
Using the Mixture and Eulerian Multiphase Models
3. Set the boundary conditions for the pressure outlet (pressure-outlet3). For the multiphase mixture model, you will specify conditions at a pressure outlet for the mixture and for the secondary phase. There are no conditions to be set for the primary phase. The turbulence conditions you input at the pressure outlet will be used only if flow enters the domain through this boundary. You can set them equal to the inlet values, as no flow reversal is expected at the pressure outlet. In general, however, it is important to set reasonable values for these downstream scalar values, in case flow reversal occurs at some point during the calculation. (a) Set the conditions at pressure-outlet-3 for the mixture. i. In the Boundary Conditions panel, select mixture in the Phase drop-down list and click Set....
ii. In the Turbulence Specification Method drop-down list, select Intensity and Length Scale. iii. Set the Backflow Turbulence Intensity to 10%. iv. Set the Backflow Turbulence Length Scale to 0.025.
c Fluent Inc. November 27, 2001
17-21
Using the Mixture and Eulerian Multiphase Models
(b) Set the conditions for the secondary phase. i. In the Boundary Conditions panel, select air from the Phase drop-down list and click Set.... ii. Set the Backflow Volume Fraction to 0.02.
17-22
c Fluent Inc. November 27, 2001
Using the Mixture and Eulerian Multiphase Models
Step 6: Solution Using the Mixture Model 1. Set the solution parameters. Solve −→ Controls −→Solution...
(a) Keep all default Under-Relaxation Factors. (b) Under Discretization, select PRESTO! in the Pressure dropdown list. 2. Enable the plotting of residuals during the calculation. Solve −→ Monitors −→Residual...
c Fluent Inc. November 27, 2001
17-23
Using the Mixture and Eulerian Multiphase Models
3. Initialize the solution. Solve −→ Initialize −→Initialize...
4. Save the case file (tee.cas). File −→ Write −→Case... 5. Start the calculation by requesting 1000 iterations. Solve −→Iterate... The solution will converge in approximately 600 iterations. 6. Save the case and data files (tee.cas and tee.dat). File −→ Write −→Case & Data...
17-24
c Fluent Inc. November 27, 2001
Using the Mixture and Eulerian Multiphase Models
Step 7: Postprocessing for the Mixture Solution 1. Display the pressure field in the tee. Display −→Contours...
(a) Select Pressure... and Static Pressure in the Contours Of dropdown lists. (b) Select Filled under Options. (c) Click Display.
c Fluent Inc. November 27, 2001
17-25
Using the Mixture and Eulerian Multiphase Models
2.34e+03 1.95e+03 1.55e+03 1.16e+03 7.70e+02 3.77e+02 -1.54e+01 -4.08e+02 -8.01e+02 -1.19e+03 -1.59e+03
Contours of Static Pressure (pascal)
Aug 17, 2001 FLUENT 6.0 (2d, segregated, mixture, ske)
Figure 17.3: Contours of Static Pressure
17-26
c Fluent Inc. November 27, 2001
Using the Mixture and Eulerian Multiphase Models
2. Display contours of velocity magnitude (Figure 17.4). Display −→Contours... (a) Select Velocity... and Velocity Magnitude in the Contours Of drop-down lists. (b) Click Display. 2.22e+00 2.00e+00 1.78e+00 1.56e+00 1.33e+00 1.11e+00 8.89e-01 6.67e-01 4.45e-01 2.22e-01 0.00e+00
Contours of Velocity Magnitude (m/s)
Aug 17, 2001 FLUENT 6.0 (2d, segregated, mixture, ske)
Figure 17.4: Contours of Velocity Magnitude 3. Display the volume fraction of air. Display −→Contours... (a) Select Phases... and Volume fraction of air in the Contours Of drop-down lists. (b) Click Display. In Figure 17.5, note the small bubble of air that separates at the sharp edge of the horizontal arm of the tee junction, and the small layer of air that floats in the same area above the water, marching towards the pressure outlet.
c Fluent Inc. November 27, 2001
17-27
Using the Mixture and Eulerian Multiphase Models
9.34e-01 8.41e-01 7.47e-01 6.54e-01 5.60e-01 4.67e-01 3.74e-01 2.80e-01 1.87e-01 9.34e-02 0.00e+00
Contours of Volume fraction of air
Aug 17, 2001 FLUENT 6.0 (2d, segregated, mixture, ske)
Figure 17.5: Contours of Air Volume Fraction
17-28
c Fluent Inc. November 27, 2001
Using the Mixture and Eulerian Multiphase Models
Step 8: Setup and Solution for the Eulerian Model You will use the solution obtained with the mixture model as an initial condition for the calculation with the Eulerian model. 1. Turn on the Eulerian model. Define −→ Models −→Multiphase...
(a) Under Models, select Eulerian.
c Fluent Inc. November 27, 2001
17-29
Using the Mixture and Eulerian Multiphase Models
2. Specify the drag law to be used for computing the interphase momentum transfer. Define −→Phases... (a) Click the Interaction... button in the Phases panel.
(b) In the Phase Interaction panel, keep the default selection of schiller-naumann in the Drag Coefficient drop-down list. Note: For this problem there are no parameters to be set for the individual phases, other than those that you specified when you set up the phases for the mixture model calculation. If you use the Eulerian model for a flow involving a granular secondary phase, there are additional parameters that you need to set. There are also other options in the Phase Interaction panel that may be relevant for other applications. See the User’s Guide for complete details on setting up an Eulerian multiphase calculation.
17-30
c Fluent Inc. November 27, 2001
Using the Mixture and Eulerian Multiphase Models
3. Select the multiphase turbulence model. Define −→ Models −→Viscous...
(a) Under k-epsilon Multiphase Model, keep the default selection of Mixture. The mixture turbulence model 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. See section 20.4.7 of the User’s Guide for more information on turbulence models for the Eulerian multiphase model.
c Fluent Inc. November 27, 2001
17-31
Using the Mixture and Eulerian Multiphase Models
4. Continue the solution by requesting 1000 additional iterations. Solve −→Iterate... The solution will converge after about 300 additional iterations. 5. Save the case and data files (tee2.cas and tee2.dat). File −→ Write −→Case & Data...
17-32
c Fluent Inc. November 27, 2001
Using the Mixture and Eulerian Multiphase Models
Step 9: Postprocessing for the Eulerian Model 1. Display the pressure field in the tee. Display −→Contours... 2.54e+03 2.14e+03 1.75e+03 1.35e+03 9.55e+02 5.59e+02 1.63e+02 -2.33e+02 -6.29e+02 -1.02e+03 -1.42e+03
Contours of Static Pressure (pascal)
Aug 17, 2001 FLUENT 6.0 (2d, segregated, eulerian, ske)
Figure 17.6: Contours of Static Pressure
2. Display contours of velocity magnitude for the water (Figure 17.7). Display −→Contours... (a) In the Contours Of drop-down lists, select Velocity... and water Velocity Magnitude. Because the Eulerian model solves individual momentum equations for each phase, you have the choice of which phase to plot solution data for. (b) Click Display. 3. Display the volume fraction of air. Display −→Contours...
c Fluent Inc. November 27, 2001
17-33
Using the Mixture and Eulerian Multiphase Models
2.25e+00 2.03e+00 1.80e+00 1.58e+00 1.36e+00 1.13e+00 9.09e-01 6.85e-01 4.62e-01 2.38e-01 1.43e-02
Contours of water Velocity Magnitude (m/s)
Aug 17, 2001 FLUENT 6.0 (2d, segregated, eulerian, ske)
Figure 17.7: Contours of Water Velocity Magnitude
9.41e-01 8.47e-01 7.53e-01 6.58e-01 5.64e-01 4.70e-01 3.76e-01 2.82e-01 1.88e-01 9.41e-02 0.00e+00
Contours of Volume fraction of air
Aug 17, 2001 FLUENT 6.0 (2d, segregated, eulerian, ske)
Figure 17.8: Contours of Air Volume Fraction
17-34
c Fluent Inc. November 27, 2001
Using the Mixture and Eulerian Multiphase Models
Note that the air bubble at the tee junction in Figure 17.8 is slightly different from the one that you observed in the solution obtained with the mixture model (Figure 17.5). The Eulerian model generally offers better accuracy than the mixture model, as it solves separate sets of equations for each individual phase, rather than modeling slip velocity between phases. See Sections 20.3 and 20.4 of the User’s Guide for more information about the mixture and Eulerian models. Summary: This tutorial demonstrated how to set up and solve a multiphase problem using the mixture model and the Eulerian model. You learned how to set boundary conditions for the mixture and both phases. The solution obtained with the mixture model was used as a starting point for the calculation with the Eulerian model. After completing calculations with both models, you compared the results obtained with the two approaches.
c Fluent Inc. November 27, 2001
17-35
Tutorial 18. Using the Eulerian Multiphase Model for Granular Flow
Introduction: Mixing tanks are used to maintain solid particles or droplets of heavy fluids in suspension. Mixing may be required to enhance reaction during chemical processing or to prevent sedimentation. In this tutorial, you will use the Eulerian multiphase model to solve the particle suspension problem. The Eulerian multiphase model solves momentum equations for each of the phases, which are allowed to mix in any proportion. In this tutorial you will learn how to: • Use the granular Eulerian multiphase model • Specify fixed velocities with a user-defined function (UDF) to simulate an impeller • Set boundary conditions for internal flow • Calculate a solution using the segregated solver • Solve a time-accurate transient problem Prerequisites: This tutorial assumes that you are familiar with the menu structure in FLUENT and that you have solved or read Tutorial 1. Some steps in the setup and solution procedure will not be shown explicitly. Problem Description: The problem involves the transient startup of an impeller-driven mixing tank. The primary phase is water, while the secondary phase consists of sand particles with a 111 micron diameter. The sand is initially settled at the bottom of the tank, to a level just above the impeller. A schematic of the mixing tank
c Fluent Inc. November 29, 2001
18-1
Using the Eulerian Multiphase Model for Granular Flow
and the initial sand position is shown in Figure 18.1. The domain is modeled as 2D axisymmetric. The fixed-values option will be used to simulate the impeller. Experimental data are used to represent the time-averaged velocity and turbulence values at the impeller location. This approach avoids the need to model the impeller itself. These experimental data are provided in a user-defined function. .4446 m
.016 m water .4446 m
impeller settled .1728 m sand bed .116 m
.0864 m
Figure 18.1: Problem Specification
18-2
c Fluent Inc. November 29, 2001
Using the Eulerian Multiphase Model for Granular Flow
Preparation 1. Copy the files mixtank/mixtank.msh and mixtank/fix.c from the FLUENT documentation CD to your working directory (as described in Tutorial 1). 2. Start the 2D version of FLUENT.
Step 1: Grid 1. Read the grid file (mixtank.msh). File −→ Read −→Case... As FLUENT reads the grid file, it will report its progress in the console window. 2. Check the grid. Grid −→Check FLUENT will perform various checks on the mesh and will report the progress in the console window. Pay particular attention to the reported minimum volume. Make sure this is a positive number. 3. Display the grid. Display −→Grid... (a) Display the grid using the default settings (Figure 18.2). Extra: You can use the right mouse button to check which zone number corresponds to each boundary. If you click the right mouse button on one of the boundaries in the graphics window, its zone number, name, and type will be printed in the FLUENT console window. This feature is especially useful when you have several zones of the same type and you want to distinguish between them quickly.
c Fluent Inc. November 29, 2001
18-3
Using the Eulerian Multiphase Model for Granular Flow
Y Z
X
Grid (Time=2.1000e+01)
Jul 30, 2001 FLUENT 6.0 (axi, segregated, eulerian, ske, unsteady)
Figure 18.2: Grid Display 4. Manipulate the grid display to show the full tank upright. Display −→Views...
18-4
c Fluent Inc. November 29, 2001
Using the Eulerian Multiphase Model for Granular Flow
(a) Under Mirror Planes
, select axis.
(b) Click Apply. The grid display will be updated to show both sides of the tank. (c) Click Auto Scale . This option is used to scale and center the current display without changing its orientation (Figure 18.3).
Y Z
X
Grid (Time=2.1000e+01)
Jul 30, 2001 FLUENT 6.0 (axi, segregated, eulerian, ske, unsteady)
Figure 18.3: Grid Display with Both Sides of the Tank
c Fluent Inc. November 29, 2001
18-5
Using the Eulerian Multiphase Model for Granular Flow
(d) Click on Camera... to display the tank in an upright position. This will open the Camera Parameters
panel.
(e) Click with the left mouse button on the indicator of the dial and drag it in the counter-clockwise direction till the upright view is displayed (Figure 18.4). (f) Click Apply and close the Camera Parameters and Views panels. Note: When experimenting with different view manipulation techniques, you may accidentally “lose” your geometry in the display. You can easily return to the default (front) view by clicking on the Default button in the Views panel.
18-6
c Fluent Inc. November 29, 2001
Using the Eulerian Multiphase Model for Granular Flow
X Y
Z
Grid (Time=2.1000e+01)
Jul 30, 2001 FLUENT 6.0 (axi, segregated, eulerian, ske, unsteady)
Figure 18.4: Grid Display of the Upright Tank
c Fluent Inc. November 29, 2001
18-7
Using the Eulerian Multiphase Model for Granular Flow
Step 2: Models 1. Specify a transient, axisymmetric model. Define −→ Models
−→Solver...
(a) Retain the default Segregated
solver.
The segregated solver must be used for multiphase calculations. (b) Under Space , select Axisymmetric. (c) Under Time, select Unsteady .
18-8
c Fluent Inc. November 29, 2001
Using the Eulerian Multiphase Model for Granular Flow
2. Enable the Eulerian multiphase model. Define −→ Models
−→Multiphase...
(a) Select Eulerian as the Model . The panel will expand to show the inputs for the Eulerian model.
(b) Keep the default settings for the Eulerian model.
c Fluent Inc. November 29, 2001
18-9
Using the Eulerian Multiphase Model for Granular Flow
3. Turn on the k- turbulence model with standard wall functions. Define −→ Models
−→Viscous...
(a) Select k-epsilon (2 eqn)
as the Model .
(b) Keep the default selection of Standard Wall Functions Near-Wall Treatment.
under
This problem does not require a particularly fine grid, and standard wall functions will be used. (c) Under k-epsilon Multiphase Model
, select the Dispersed model.
The dispersed turbulence model is applicable in this case because there is clearly one primary continuous phase and the material density ratio of the phases is about 2.5. Furthermore,
18-10
c Fluent Inc. November 29, 2001
Using the Eulerian Multiphase Model for Granular Flow
the Stokes number is much less than 1. Therefore, the particle’s kinetic energy will not depart significantly from that of the liquid. 4. Set the gravitational acceleration. Define −→Operating Conditions... (a) Turn on Gravity . The panel will expand to show additional inputs.
(b) Set the Gravitational Acceleration
c Fluent Inc. November 29, 2001
in the X direction to -9.81 m/s2 .
18-11
Using the Eulerian Multiphase Model for Granular Flow
Step 3: Materials In this step, you will add liquid water to the list of fluid materials by copying it from the materials database, and create a new material called sand. Define −→Materials... 1. Copy liquid water from the materials database so that it can be used for the primary phase. (a) Click the Database... button in the Materials panel. The Database Materials
18-12
panel will open.
c Fluent Inc. November 29, 2001
Using the Eulerian Multiphase Model for Granular Flow
(b) In the list of Fluid Materials , select water-liquid (h2o
).
(c) Click Copy to copy the information for liquid water to your model. (d) Close the Database Materials
panel.
2. Create a new material called sand .
c Fluent Inc. November 29, 2001
18-13
Using the Eulerian Multiphase Model for Granular Flow
(a) Type the name sand in the Name text-entry box. (b) Under Properties , enter 2500 kg/m3 as the Density . (c) Remove the entry for Chemical Formula so the field is blank. (d) Click on Change/Create
and close the Materials panel.
When you click Change/Create , a question dialog box will appear, asking you if water-liquid should be overwritten. Click No to retain water-liquid and add the new material, sand , to the list. The Materials panel will be updated to show the new material name in the Fluid Materials list.
18-14
c Fluent Inc. November 29, 2001
Using the Eulerian Multiphase Model for Granular Flow
Step 4: Phases 1. Define the primary (water) and secondary (sand) phases. Define −→Phases...
(a) Specify water as the primary phase. i. Select phase-1 and click the Set... button.
ii. In the Primary Phase iii. Select water-liquid
c Fluent Inc. November 29, 2001
panel, enter water for the Name.
from the Phase Material
drop-down list.
18-15
Using the Eulerian Multiphase Model for Granular Flow
(b) Specify sand as the secondary phase. i. Select phase-2 and click the Set... button.
ii. In the Secondary Phase
panel, enter sand for the Name.
iii. Select sand from the Phase Material
drop-down list.
iv. Turn on the Granular option. v. Define the properties of the sand phase. A. Enter 0.000111 as the Diameter. B. Select syamlal-obrien from the Granular Viscosity down list.
drop-
C. Select lun-et-al from the Granular Bulk Viscosity down list.
drop-
D. Enter 0.6 as the Packing Limit .
18-16
c Fluent Inc. November 29, 2001
Using the Eulerian Multiphase Model for Granular Flow
(c) Specify the drag law to be used for computing the interphase momentum transfer. i. Click the Interaction...
button in the Phases panel.
ii. In the Phase Interaction panel, select gidaspow Coefficient drop-down list.
c Fluent Inc. November 29, 2001
in the Drag
18-17
Using the Eulerian Multiphase Model for Granular Flow
Step 5: Boundary Conditions For this problem, there are no conditions to be specified on the outer boundaries. Within the domain, there are three fluid zones, representing the impeller region, the region where the sand is initially located, and the rest of the tank. There are no conditions to be specified in the latter two zones, so you will need to set conditions only in the zone representing the impeller. As mentioned earlier, a UDF is used to specify the fixed velocities that simulate the impeller. The values of the time-averaged impeller velocity components and turbulence quantities are based on experimental measurement. The variation of these values may be expressed as a function of radius, and imposed as polynomials according to: variable = A1 + A2 r + A3 r 2 + A4 r 3 + ... The order of polynomial to be used depends on the behavior of the function being fitted. For this tutorial, the polynomial coefficients shown in Table 18.1 are provided in the UDF fix.c. Table 18.1: Impeller Profile Specifications Variable u velocity v velocity kinetic energy dissipation Variable u velocity v velocity kinetic energy dissipation
A1 -7.1357e-2 3.1131e-2 2.2723e-2 -6.5819e-2 A4 4.5578e+4 -2.0051e+4 9.4615e+3 1.1643e+5
A2 54.304 -10.313 6.7989 88.845
A3 -3.1345e+3 9.5558e+2 -424.18 -5.3731e+3
A5 -1.9664e+5 1.1856e+5 -7.7251e+4 -9.1202e+5
A6 – – 1.8410e+5 1.9567e+6
See the separate UDF Manual for details about setting up a UDF using the DEFINE PROFILE macro. Note that, while this macro is usually used to specify a profile condition on a boundary face zone, it is used in fix.c
18-18
c Fluent Inc. November 29, 2001
Using the Eulerian Multiphase Model for Granular Flow
to specify the condition in a fluid cell zone. The arguments of the macro have been changed accordingly. 1. Compile the UDF, fix.c, using the Interpreted UDFs panel. Define −→ User-Defined −→ Functions
−→Interpreted...
(a) Enter fix.c under Source File Name . !
Make sure that the C source code for your UDF and your mesh file reside in your working directory. If your source code is not in your working directory, then when you compile the UDF you must enter the file’s complete path in the Interpreted UDFs panel, instead of just the filename.
(b) Keep the default Stack Size setting of 10000. (c) Turn on the Display Assembly Listing option. Turning on the Display Assembly Listing option will cause a listing of the assembly language code to appear in your console window when the function compiles. (d) Click Compile to compile your UDF. Note: The name and contents of your UDF will be stored in your case file when you write the case file.
c Fluent Inc. November 29, 2001
18-19
Using the Eulerian Multiphase Model for Granular Flow
2. Set the conditions for the fluid zone representing the impeller (fixzone ). You will specify the conditions for the water and the sand separately. There are no conditions to be specified for the mixture (i.e., conditions that apply to all phases); the default conditions for the mixture are acceptable. Define −→Boundary Conditions... (a) Set the conditions on fix-zone for the water. All of the conditions for the water will come from the UDF. i. In the Boundary Conditions panel, select water from the Phase drop-down list and click Set... .
ii. Turn on the Fixed Values option. The panel will expand to show the related inputs. iii. Select udf fixed u from the drop-down list to the right of Axial Velocity . iv. Select udf fixed v for Radial Velocity .
18-20
c Fluent Inc. November 29, 2001
Using the Eulerian Multiphase Model for Granular Flow
v. Select udf fixed ke for Turbulence Kinetic Energy
.
vi. Select udf fixed diss for Turbulence Dissipation Rate
.
(b) Set the conditions on fix-zone for the sand. All of the conditions for the sand will come from the UDF. i. In the Boundary Conditions panel, select sand from the Phase drop-down list and click Set... .
ii. Turn on the Fixed Values option. The panel will expand to show the related inputs. iii. Select udf fixed u for Axial Velocity . iv. Select udf fixed v for Radial Velocity .
c Fluent Inc. November 29, 2001
18-21
Using the Eulerian Multiphase Model for Granular Flow
Step 6: Solution 1. Set the solution parameters. Solve −→ Controls
−→Solution...
(a) For the Under-Relaxation Factors , set Pressure to 0.5, Momentum to 0.2, and Turbulent Viscosity to 0.8. (b) Under Discretization , keep the default settings. 2. Enable the plotting of residuals during the calculation. Solve −→ Monitors
−→Residual...
3. Initialize the solution using the default initial values. Solve −→ Initialize −→Initialize... 18-22
c Fluent Inc. November 29, 2001
Using the Eulerian Multiphase Model for Granular Flow
4. Patch the initial sand bed configuration.
(a) In the Variable list, select sand Volume Fraction (b) Select initial-sand in the Zones To Patch
.
list.
(c) Set the Value to 0.56. (d) Click Patch . 5. Set the time stepping parameters. Solve −→Iterate... (a) Set the Time Step Size to 0.005. (b) Under Iteration , set the Max Iterations per Time Step
to 40.
(c) Click Apply.
c Fluent Inc. November 29, 2001
18-23
Using the Eulerian Multiphase Model for Granular Flow
6. Save the initial case and data files (mixtank.cas and mixtank.dat). File −→ Write −→Case & Data... The problem statement is now complete. As a precaution, you should review the impeller velocity fixes and sand bed patch after running the calculation for a single time step. Since you are using a UDF for the velocity profiles, you need to perform one time step in order for the profiles to be calculated and available for viewing. 7. Run the calculation for 0.005 seconds. Solve −→Iterate... (a) Set the Number of Time Steps
to 1.
(b) Click Iterate.
18-24
c Fluent Inc. November 29, 2001
Using the Eulerian Multiphase Model for Granular Flow
8. Check the initial velocities and sand volume fraction. In order to display the initial velocities in the fluid zone where you have fixed their values (fix-zone) , you will need to create a zone surface for it. (a) Create a zone surface for fix-zone . Surface −→Zone...
i. In the Zone list, select fix-zone . ii. Under New Surface Name , retain the default name. The default name is the same as the zone name. FLUENT will automatically assign the default name to the new surface when it is created. iii. Click on Create and close the panel. The new surface will be added to the Surfaces list in the Zone Surface panel.
c Fluent Inc. November 29, 2001
18-25
Using the Eulerian Multiphase Model for Granular Flow
(b) Display the initial impeller velocities for water. Display −→Vectors...
i. Select water Velocity
in the Vectors Of
drop-down list.
ii. Select Velocity... and water Velocity Magnitude By drop-down lists.
in the Color
iii. In the Surfaces list, select fix-zone . iv. In the Style drop-down list, select arrow . v. Click Display. FLUENT will display the water velocity vector fixes at the impeller location, as shown in Figure 18.5.
18-26
c Fluent Inc. November 29, 2001
Using the Eulerian Multiphase Model for Granular Flow
8.08e-01 7.27e-01 6.46e-01 5.65e-01 4.85e-01 4.04e-01 3.23e-01 2.42e-01 1.62e-01 8.08e-02 8.41e-06
water-velocity Colored By water Velocity Magnitude (m/s) (Time=5.0000e-03) Nov 19, 2001 FLUENT 6.0 (axi, segregated, eulerian, ske, unsteady)
Figure 18.5: Initial Impeller Velocities for Water
c Fluent Inc. November 29, 2001
18-27
Using the Eulerian Multiphase Model for Granular Flow
(c) Display the initial impeller velocities for sand. Display −→Vectors... i. Select sand Velocity
in the Vectors Of
drop-down list.
ii. Select Velocity... and sand Velocity Magnitude By drop-down lists.
in the Color
iii. Click Display. FLUENT will display the sand velocity vector fixes at the impeller location, as shown in Figure 18.6. 8.01e-01 7.21e-01 6.41e-01 5.61e-01 4.80e-01 4.00e-01 3.20e-01 2.40e-01 1.60e-01 8.01e-02 0.00e+00
sand-velocity Colored By sand Velocity Magnitude (m/s) (Time=5.0000e-03) Nov 19, 2001 FLUENT 6.0 (axi, segregated, eulerian, ske, unsteady)
Figure 18.6: Initial Impeller Velocities for Sand
18-28
c Fluent Inc. November 29, 2001
Using the Eulerian Multiphase Model for Granular Flow
(d) Display contours of sand volume fraction. Display −→Contours...
i. Select Phases... and Volume fraction of sand tours Of drop-down lists.
in the Con-
ii. Select Filled under Options . iii. Click Display. FLUENT will display the initial location of the settled sand bed, shown in Figure 18.7.
c Fluent Inc. November 29, 2001
18-29
Using the Eulerian Multiphase Model for Granular Flow
5.62e-01 5.06e-01 4.50e-01 3.94e-01 3.37e-01 2.81e-01 2.25e-01 1.69e-01 1.12e-01 5.62e-02 0.00e+00
Contours of Volume fraction of sand (Time=5.0000e-03) Nov 19, 2001 FLUENT 6.0 (axi, segregated, eulerian, ske, unsteady)
Figure 18.7: Initial Settled Sand Bed
18-30
c Fluent Inc. November 29, 2001
Using the Eulerian Multiphase Model for Granular Flow
9. Run the calculation for 1 second. Solve −→Iterate... (a) Set the Number of Time Steps
to 199.
(b) Click Iterate. After 200 time steps have been computed (a total of 1 second of operation), you will review the results before continuing. 10. Save the case and data files (mixtank1.cas and mixtank1.dat). File −→ Write −→Case & Data... 11. Examine the results of the calculation after 1 second. (a) Display the velocity vectors in the whole tank for the water. Display −→Vectors... !
Remember to deselect fix-zone in the Surfaces list.
Figure 18.8 shows the water velocity vectors after 1 second of operation. The circulation is confined to the region near the impeller, and has not yet had time to develop in the upper portions of the tank. (b) Display the velocity vectors for the sand. Display −→Vectors... Figure 18.9 shows the sand velocity vectors after 1 second of operation. The circulation of sand around the impeller is significant, but note that no sand vectors are plotted in the upper part of the tank, where the sand is not yet present.
c Fluent Inc. November 29, 2001
18-31
Using the Eulerian Multiphase Model for Granular Flow
8.11e-01 7.30e-01 6.49e-01 5.68e-01 4.87e-01 4.06e-01 3.25e-01 2.44e-01 1.62e-01 8.14e-02 2.31e-04
water-velocity Colored By water Velocity Magnitude (m/s) (Time=1.0000e+00) Nov 19, 2001 FLUENT 6.0 (axi, segregated, eulerian, ske, unsteady)
Figure 18.8: Water Velocity Vectors after 1 Second
8.17e-01 7.35e-01 6.53e-01 5.72e-01 4.90e-01 4.08e-01 3.27e-01 2.45e-01 1.63e-01 8.17e-02 0.00e+00
sand-velocity Colored By sand Velocity Magnitude (m/s) (Time=1.0000e+00) Nov 19, 2001 FLUENT 6.0 (axi, segregated, eulerian, ske, unsteady)
Figure 18.9: Sand Velocity Vectors after 1 Second
18-32
c Fluent Inc. November 29, 2001
Using the Eulerian Multiphase Model for Granular Flow
(c) Display contours of sand volume fraction. Display −→Contours... Notice that the action of the impeller draws clear fluid from above the originally settled bed and mixes it into the sand. To compensate, the sand bed is lifted up slightly. The maximum sand volume fraction has increased as a result of settling underneath the impeller and near the outer radius of the tank. 5.47e-01 4.93e-01 4.38e-01 3.83e-01 3.28e-01 2.74e-01 2.19e-01 1.64e-01 1.09e-01 5.47e-02 0.00e+00
Contours of Volume fraction of sand (Time=1.0000e+00) Nov 19, 2001 FLUENT 6.0 (axi, segregated, eulerian, ske, unsteady)
Figure 18.10: Contours of Sand Volume Fraction after 1 Second 12. Continue the calculation for another 19 seconds. Solve −→Iterate... (a) Set the Time Step Size to 0.01. The initial calculation was performed with a very small time step size to stabilize the solution. After the initial calculation, you can usually increase the time step to speed up the calculation. (b) Set the Number of Time Steps
to 1900.
(c) Click Iterate.
c Fluent Inc. November 29, 2001
18-33
Using the Eulerian Multiphase Model for Granular Flow
The transient calculation will continue to 20 seconds. 13. Save the case and data files (mixtank20.cas and mixtank20.dat). File −→ Write −→Case & Data...
18-34
c Fluent Inc. November 29, 2001
Using the Eulerian Multiphase Model for Granular Flow
Step 7: Postprocessing You will now examine the progress of the sand and water in the mixing tank after a total of 20 seconds.The mixing tank has nearly, but not quite, reached a steady flow solution. 1. Display the velocity vectors for the water. Display −→Vectors... Figure 18.11 shows the water velocity vectors after 20 seconds of operation. The circulation of water is now very strong in the lower portion of the tank, though modest near the top. 8.31e-01 7.48e-01 6.65e-01 5.82e-01 4.99e-01 4.16e-01 3.33e-01 2.50e-01 1.67e-01 8.44e-02 1.41e-03
water-velocity Colored By water Velocity Magnitude (m/s) (Time=2.0000e+01) Nov 19, 2001 FLUENT 6.0 (axi, segregated, eulerian, ske, unsteady)
Figure 18.11: Water Velocity Vectors after 20 Seconds
c Fluent Inc. November 29, 2001
18-35
Using the Eulerian Multiphase Model for Granular Flow
2. Display the velocity vectors for the sand. Display −→Vectors... Figure 18.12 shows the sand velocity vectors after 20 seconds of operation. The sand has now been suspended much higher within the mixing tank, but does not reach the upper region of the tank. The water velocity in that region is not sufficient to overcome the gravity force on the sand particles. 8.34e-01 7.51e-01 6.67e-01 5.84e-01 5.01e-01 4.17e-01 3.34e-01 2.50e-01 1.67e-01 8.34e-02 0.00e+00
sand-velocity Colored By sand Velocity Magnitude (m/s) (Time=2.0000e+01) Nov 19, 2001 FLUENT 6.0 (axi, segregated, eulerian, ske, unsteady)
Figure 18.12: Sand Velocity Vectors after 20 Seconds
18-36
c Fluent Inc. November 29, 2001
Using the Eulerian Multiphase Model for Granular Flow
3. Display contours of sand volume fraction. Display −→Contours... Figure 18.13 shows the contours of sand volume fraction after 20 seconds of operation. 3.23e-01 2.91e-01 2.59e-01 2.26e-01 1.94e-01 1.62e-01 1.29e-01 9.70e-02 6.47e-02 3.23e-02 0.00e+00
Contours of Volume fraction of sand (Time=2.0000e+01) Nov 19, 2001 FLUENT 6.0 (axi, segregated, eulerian, ske, unsteady)
Figure 18.13: Contours of Sand Volume Fraction after 20 Seconds
c Fluent Inc. November 29, 2001
18-37
Using the Eulerian Multiphase Model for Granular Flow
4. Display filled contours of static pressure in the mixing tank. (a) Select Pressure... and Relative Static Pressure Of drop-down lists.
in the Contours
(b) Click Display. Figure 18.14 shows the pressure distribution after 20 seconds of operation. Notice that the pressure field represents the hydrostatic pressure except for some slight deviations due to the flow of the impeller near the bottom of the tank. 1.50e+02 1.63e+01 -1.18e+02 -2.52e+02 -3.86e+02 -5.20e+02 -6.55e+02 -7.89e+02 -9.23e+02 -1.06e+03 -1.19e+03
Contours of Static Pressure (pascal) (Time=2.0000e+01) Nov 19, 2001 FLUENT 6.0 (axi, segregated, eulerian, ske, unsteady)
Figure 18.14: Contours of Pressure after 20 Seconds
Summary: This tutorial demonstrated how to set up and solve a granular multiphase problem using the Eulerian multiphase model. The problem involved particle suspension in a mixing tank and postprocessing showed the near-steady-state behavior of the sand in the mixing tank.
18-38
c Fluent Inc. November 29, 2001
Tutorial 19.
Modeling Solidification
Introduction: This tutorial illustrates how to set up and solve a problem involving solidification. In this tutorial, you will learn how to: • Define a solidification problem • Define pull velocities for simulation of continuous casting • Define a surface tension gradient for Marangoni convection • Solve a solidification problem Prerequisites: This tutorial assumes that you are familiar with the menu structure in FLUENT, and that you have solved Tutorial 1. Some steps in the setup and solution procedure will not be shown explicitly. Problem Description: This tutorial demonstrates the setup and solution procedure for a fluid flow and heat transfer problem involving solidification, namely the Czochralski growth process. The geometry considered is a 2D axisymmetric bowl (shown in Figure 19.1), containing a liquid metal. The bottom and sides of the bowl are heated above the liquidus temperature, as is the free surface of the liquid. The liquid is solidified by heat loss from the crystal and the solid is pulled out of the domain at a rate of 0.001 m/s and a temperature of 500 K. There is a steady injection of liquid at the bottom of the bowl with a velocity of 1.01×10−3 and a temperature of 1300 K. Material properties are listed in Figure 19.1. Starting with an existing 2D mesh, the details regarding the setup and solution procedure for the solidification problem are presented. The steady conduction solution for this problem is computed as an initial condition. Then, the fluid flow is turned on to investigate the effect of natural and Marangoni convection in an unsteady fashion.
c Fluent Inc. November 27, 2001
19-1
Modeling Solidification
T = 1400 K
g
Free Surface 2
h = 100 W/m K Tenv= 1500 K
T = 1300 K
0.05 m 0.1 m T = 500 K u = 0.001 m/s T = 500 K u = 0.00101 m/s 0.03 m Ω = 1 rad/s
T = 1300 K
Mushy Region
Crystal
0.1 m
ρ µ
k cp
∂σ/∂T Tsolidus Tliquidus
L Amush
3
= 8000 − 0.1*T kg/m = 5.53 x 10-3 kg/m-s = 30 W/m-K = 680 J/kg-K = −3.6 x 10-4 N/m-K = 1100 K = 1200 K 5 = 1 x 10 J/kg = 1 x 104 kg/m3 -s
Figure 19.1: Solidification in Czochralski model
19-2
c Fluent Inc. November 27, 2001
Modeling Solidification
Preparation 1. Copy the file solid/solid.msh from the FLUENT documentation CD to your working directory (as described in Tutorial 1). 2. Start the 2D version of FLUENT.
Step 1: Grid 1. Read the mesh file solid.msh. File −→ Read −→Case... As this mesh is read by FLUENT, messages appear in the console window reporting the progress of the reading. 2. Check the grid. Grid −→Check FLUENT performs various checks on the mesh and reports the progress in the console window. Pay particular attention to the minimum volume. Make sure this is a positive number. 3. Display the grid (Figure 19.2). Display −→ Grid...
c Fluent Inc. November 27, 2001
19-3
Modeling Solidification
Grid
Jun 19, 2001 FLUENT 6.0 (2d, segregated, lam)
Figure 19.2: Graphics Display of Grid
19-4
c Fluent Inc. November 27, 2001
Modeling Solidification
Step 2: Models 1. Enable the modeling of axisymmetric swirl. Define −→ Models −→Solver...
(a) Under Space, select Axisymmetric Swirl. (b) Keep the default settings for everything else.
c Fluent Inc. November 27, 2001
19-5
Modeling Solidification
2. Define the solidification model. Define −→ Models −→Solidification & Melting... (a) Under Model, turn on Solidification/Melting. The panel will expand to show the related inputs.
(b) Under Parameters, keep the default value for the Mushy Zone Constant. The default value of 100000 is acceptable for most cases. (c) Turn on Include Pull Velocities. The panel will expand to show an additional input. Including the pull velocities accounts for the movement of the solidified material as it is continuously withdrawn from the domain in the continuous casting process. Note: It is possible to have FLUENT compute the pull velocities during the calculation, but this approach is computationally expensive, and is recommended only if the pull velocities are strongly dependent on the location of the liquid-solid interface. In this tutorial, you will patch values for the pull velocities instead of having FLUENT compute them. See the User’s Guide for more information.
19-6
c Fluent Inc. November 27, 2001
Modeling Solidification
Note: When you click OK in the Solidification/Melting panel, FLUENT will present an Information dialog box telling you that available material properties have changed for the solidification model. You will be setting properties later, so you can simply click OK in the dialog box to acknowledge this information. Note: FLUENT will automatically enable the energy calculation when you enable the solidification model, so you need not visit the Energy panel. 3. Add the effect of gravity on the model. Define −→Operating Conditions...
(a) Turn on Gravity. The panel will expand to show additional inputs. (b) Set the Gravitational Acceleration in the X direction to -9.81 m/s2 .
c Fluent Inc. November 27, 2001
19-7
Modeling Solidification
Step 3: Materials In this step, you will create a new material and specify its properties, including the melting heat, solidus temperature, and liquidus temperature. Define −→Materials...
1. In the Name field, enter liquid-metal. 2. Specify the density as a function of temperature. As shown in Figure 19.1, the density of the material is defined by a polynomial function: ρ = 8000 − 0.1T .
19-8
c Fluent Inc. November 27, 2001
Modeling Solidification
(a) Select Polynomial in the Density drop-down list. The Polynomial Profile will open.
(b) Increase the value of Coefficients to 2. (c) Enter 8000 for coefficient 1 and -0.1 for coefficient 2. When you click OK in the Polynomial Profile panel, a question dialog box will appear, asking you if air should be overwritten. Click No to retain air and add the new material, liquid-metal, to the list. The Materials panel will be updated to show the new material name in the Fluid Materials list. You will need to select liquid-metal in the Fluid Materials drop-down list to set the other material properties. 3. Set the specific heat, Cp, to 680 J/kg-K. 4. Set the Thermal Conductivity to 30 W/m-K. 5. Set the Viscosity to 0.00553 kg/m-s. 6. Set the Melting Heat to 100000 J/kg. 7. Set the Solidus Temperature to 1100 K. 8. Set the Liquidus Temperature to 1200 K. 9. Click on Change/Create and close the Materials panel.
c Fluent Inc. November 27, 2001
19-9
Modeling Solidification
Step 4: Boundary Conditions Define −→Boundary Conditions... 1. Set the boundary conditions for the fluid.
(a) Select liquid-metal in the Material Name drop-down list. 2. Set the boundary conditions for the velocity inlet.
19-10
c Fluent Inc. November 27, 2001
Modeling Solidification
(a) Set the Velocity Magnitude to 0.00101 m/s. (b) Set the Temperature to 1300 K. 3. Set boundary conditions for the outlet. Here, the solid is pulled out with a specified velocity, so a velocity inlet is used with the velocities pointing outwards.
(a) In the Velocity Specification Method drop-down list, select Components. The panel will change to show related inputs. (b) Set the Axial-Velocity to 0.001 m/s. (c) Set the Swirl Angular Velocity to 1 rad/s. (d) Set the Temperature to 500 K.
c Fluent Inc. November 27, 2001
19-11
Modeling Solidification
4. Set the boundary conditions for the bottom wall.
(a) Select Temperature under Thermal Conditions. (b) Set the Temperature to 1300 K.
19-12
c Fluent Inc. November 27, 2001
Modeling Solidification
5. Set the boundary conditions for the free surface. The specified shear and Marangoni stress boundary conditions are useful in modeling situations in which the shear stress (rather than the motion of the fluid) is known. A free surface condition is an example of such a situation. In this case, the conduction is Marangoni stress driven and the shear stress is dependent on the surface tension, which is a function of temperature.
(a) Specify the thermal conditions. i. Select Convection under Thermal Conditions. The panel will change to show related inputs. ii. Set the Heat Transfer Coefficient to 100 W/m2 -K. iii. Set the Free Stream Temperature to 1500 K. (b) Specify the shear conditions. i. Click the Momentum tab. The wall motion and shear condition will be displayed.
c Fluent Inc. November 27, 2001
19-13
Modeling Solidification
ii. Under Shear Condition, select Marangoni Stress. The Marangoni Stress condition allows you to specify the gradient of the surface tension with respect to temperature at a wall boundary. iii. Set the Surface Tension Gradient to -0.00036 N/m-K. 6. Set the boundary conditions for the side wall. (a) Select Temperature under Thermal Conditions. (b) Set the Temperature to 1400 K. 7. Set the boundary conditions for the solid wall. (a) Specify the thermal conditions. i. Select Temperature under Thermal Conditions. ii. Set the Temperature to 500 K. (b) Specify the wall motion. i. Click the Momentum tab.
19-14
c Fluent Inc. November 27, 2001
Modeling Solidification
ii. Under Wall Motion, select Moving Wall. The panel will expand to show additional parameters. iii. Under Motion, select Rotational. The panel changes to show the rotational speed. iv. Under Speed, set the rotational velocity to 1.0 rad/s.
c Fluent Inc. November 27, 2001
19-15
Modeling Solidification
Step 5: Solution: Steady Conduction In this step, you will disable the calculation of the flow and swirl velocity equations, and calculate the conduction only. This steady-state solution will be used as the initial condition for the time-dependent fluid flow and heat transfer calculation. 1. Set the solution parameters. In this step, you will specify the discretization schemes to be used, and temporarily turn off the calculation of the flow and swirl velocity equations. Solve −→ Controls −→Solution...
19-16
c Fluent Inc. November 27, 2001
Modeling Solidification
(a) In the Equations list, deselect Flow and Swirl Velocity. (b) Keep the default values for all Under-Relaxation Factors. (c) Under Discretization, select PRESTO! for Pressure, SIMPLE for Pressure-Velocity Coupling, and First Order Upwind for Momentum and Swirl Velocity. 2. Initialize the solution. Solve −→ Initialize −→Initialize...
(a) Check that the value for Initial Temperature is set to 300 K. Since you are solving only the steady conduction problem, the initial values for the pressure and velocities will not be used. (b) Click on Init and Close the panel.
c Fluent Inc. November 27, 2001
19-17
Modeling Solidification
3. Define a custom field function for the swirl pull velocity. You will use this field function to patch a variable value for the swirl pull velocity in the next step. The swirl pull velocity is equal to Ωr, where Ω is the angular velocity and r is the radial coordinate. Since Ω = 1 rad/s, you can simplify the equation to simply r. In this example, the value of Ω is included for demonstration purposes. Define −→Custom Field Functions...
(a) In the Field Functions drop-down lists, select Grid... and Radial Coordinate. (b) Click the Select button. radial-coordinate will appear in the Definition field. If you make a mistake, click the DEL button on the calculator pad to delete the last item you added to the function definition. (c) Click the X button on the calculator pad. (d) Click on 1. (e) Enter omegar as the New Function Name.
19-18
c Fluent Inc. November 27, 2001
Modeling Solidification
(f) Click Define and close the panel. If you wish to check the function definition, click on Manage... and select omegar. 4. Patch the pull velocities. As noted earlier, you will patch values for the pull velocities, rather than having FLUENT compute them. Since the radial pull velocity is zero, you will patch just the axial and swirl pull velocities. Solve −→ Initialize −→Patch...
(a) Specify the value of the axial pull velocity. i. In the Variable list, select Axial Pull Velocity. ii. Select fluid in the Zones To Patch list. iii. Set the Value to 0.001 m/s. iv. Click Patch.
c Fluent Inc. November 27, 2001
19-19
Modeling Solidification
(b) Specify the value of the swirl pull velocity.
i. In the Variable list, select Swirl Pull Velocity. ii. Enable the Use Field Function option. iii. Select omegar in the Field Function list. iv. Click Patch.
19-20
c Fluent Inc. November 27, 2001
Modeling Solidification
5. Enable the plotting of residuals during the calculation. Solve −→ Monitors −→Residual...
(a) Under Options, select Plot. (b) Click OK. 6. Save the initial case and data files (solid0.cas and solid0.dat). File −→ Write −→Case & Data...
c Fluent Inc. November 27, 2001
19-21
Modeling Solidification
7. Start the calculation by requesting 20 iterations. Solve −→Iterate... 8. Display filled contours of temperature (Figure 19.3). Display −→Contours...
(a) Under Options, select Filled. (b) Select Temperature... and Static Temperature in the Contours Of drop-down lists. (c) Click Display.
19-22
c Fluent Inc. November 27, 2001
Modeling Solidification
1.40e+03 1.31e+03 1.22e+03 1.13e+03 1.04e+03 9.50e+02 8.60e+02 7.70e+02 6.80e+02 5.90e+02 5.00e+02
Contours of Static Temperature (k)
Jun 20, 2001 FLUENT 6.0 (axi, swirl, segregated, lam)
Figure 19.3: Contours of Temperature for Steady Conduction Solution
The thickness of the mushy zone can be determined from the contours of temperature. The mushy zone is the region where the temperature is between the liquidus temperature and solidus temperature. 9. Save the case and data files for the steady conduction solution (solid.cas and solid.dat). File −→ Write −→Case & Data...
c Fluent Inc. November 27, 2001
19-23
Modeling Solidification
Step 6: Solution: Unsteady Flow and Heat Transfer In this step, you will turn on time dependence and include the flow and swirl velocity equations in the calculation. You will then solve the unsteady problem using the steady conduction solution as the initial condition. 1. Enable a time-dependent solution. Define −→ Models −→Solver...
(a) Under Time, select Unsteady. (b) Under Unsteady Formulation, retain 1st-Order Implicit.
19-24
c Fluent Inc. November 27, 2001
Modeling Solidification
2. Enable the solution of the flow and swirl velocity equations. Solve −→ Controls −→Solution... (a) Select Flow and Swirl Velocity in the Equations list and keep the selection of Energy. Now all three items in the Equations list will be selected. (b) Keep the default values for all Under-Relaxation Factors. (c) Under Discretization, retain the settings for all parameters. 3. Save the initial case and data files (solid01.cas and solid01.dat). File −→ Write −→Case & Data... 4. Run the calculation for 2 time steps. Solve −→Iterate...
c Fluent Inc. November 27, 2001
19-25
Modeling Solidification
(a) Under Time, set the Time Step Size to 0.1 seconds. (b) Set the Number of Time Steps to 2. (c) Under Iteration, retain the default value of 20 for Max Iterations per Time Step. (d) Click Iterate. 5. Examine the results of the calculation after 0.2 seconds. (a) Display filled contours of temperature (Figure 19.4). Display −→Contours... i. Select Temperature... and Static Temperature in the Contours Of drop-down lists. ii. Click Display. 1.40e+03 1.31e+03 1.22e+03 1.13e+03 1.04e+03 9.50e+02 8.60e+02 7.70e+02 6.80e+02 5.90e+02 5.00e+02
Contours of Static Temperature (k) (Time=2.0000e-01) Jul 06, 2001 FLUENT 6.0 (axi, swirl, segregated, lam, unsteady)
Figure 19.4: Contours of Temperature at t = 0.2 s The temperature contours show the gradient in temperature from the hot walls on the left to the cooler zone on the right.
19-26
c Fluent Inc. November 27, 2001
Modeling Solidification
(b) Display contours of stream function (Figure 19.5). i. Under Options, deselect Filled. ii. Select Velocity... and Stream Function in the Contours Of drop-down lists. iii. Click Display. 2.12e-02 1.91e-02 1.69e-02 1.48e-02 1.27e-02 1.06e-02 8.47e-03 6.36e-03 4.24e-03 2.12e-03 0.00e+00
Contours of Stream Function (kg/s) (Time=2.0000e-01) Nov 19, 2001 FLUENT 6.0 (axi, swirl, segregated, lam, unsteady)
Figure 19.5: Contours of Stream Function at t = 0.2 s As shown in Figure 19.5, the liquid is beginning to circulate in a large eddy, driven by natural convection and Marangoni convection on the free surface. (c) Display contours of liquid fraction (Figure 19.6). i. Select Solidification/Melting... and Liquid Fraction in the Contours Of drop-down lists. ii. Click Display. The liquid fraction contours show the current position of the melt front. Note that in Figure 19.6, the mushy zone divides the liquid and solid regions roughly in half.
c Fluent Inc. November 27, 2001
19-27
Modeling Solidification
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 0.00e+00
Contours of Liquid Fraction (Time=2.0000e-01)
Aug 07, 2001 FLUENT 6.0 (axi, swirl, segregated, lam, unsteady)
Figure 19.6: Contours of Liquid Fraction at t = 0.2 s
19-28
c Fluent Inc. November 27, 2001
Modeling Solidification
6. Continue the calculation for 48 additional time steps. Solve −→Iterate... After a total of 50 time steps have been completed, the elapsed time will be 5 seconds. 7. Examine the results of the calculation after 5 seconds. (a) Display filled contours of temperature (Figure 19.7). 1.40e+03 1.31e+03 1.22e+03 1.13e+03 1.04e+03 9.50e+02 8.60e+02 7.70e+02 6.80e+02 5.90e+02 5.00e+02
Contours of Static Temperature (k) (Time=5.0000e+00) Aug 07, 2001 FLUENT 6.0 (axi, swirl, segregated, lam, unsteady)
Figure 19.7: Contours of Temperature at t = 5 s As shown in Figure 19.7, the temperature contours are fairly uniform through the melt front and solid material. The distortion of the temperature field due to the recirculating liquid is also clearly evident. In a continuous casting process, it is important to pull out the solidified material at the proper time. If the material is pulled out too soon, it will not have solidified; that is, it will still be in a mushy state. If it is pulled out too late, it solidifies in the casting pool and cannot be pulled out in the required shape. The optimal rate of pull can be determined from the contours of liquidus temperature and solidus temperature.
c Fluent Inc. November 27, 2001
19-29
Modeling Solidification
(b) Display contours of stream function (Figure 19.8). Display −→Contours... 1.33e-01 1.20e-01 1.07e-01 9.32e-02 7.99e-02 6.66e-02 5.33e-02 4.00e-02 2.66e-02 1.33e-02 0.00e+00
Contours of Stream Function (kg/s) (Time=5.0000e+00) Nov 19, 2001 FLUENT 6.0 (axi, swirl, segregated, lam, unsteady)
Figure 19.8: Contours of Stream Function at t = 5 s Note that the flow has developed more fully now, as compared with Figure 19.5 after 0.2 seconds. The main eddy, driven by natural convection and Marangoni stress, dominates the flow. To examine the position of the melt front and the extent of the mushy zone, you will plot the contours of liquid fraction. (c) Display contours of liquid fraction (Figure 19.9). The introduction of liquid material at the left of the domain is balanced by the pulling of the solidified material from the right. After 5 seconds, the equilibrium position of the melt front is beginning to be established. 8. Save the case and data files for the solution at 5 seconds (solid5.cas and solid5.dat). File −→ Write −→Case & Data...
19-30
c Fluent Inc. November 27, 2001
Modeling Solidification
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 0.00e+00
Contours of Liquid Fraction (Time=5.0000e+00)
Nov 19, 2001 FLUENT 6.0 (axi, swirl, segregated, lam, unsteady)
Figure 19.9: Contours of Liquid Fraction at t = 5 s
c Fluent Inc. November 27, 2001
19-31
Modeling Solidification
Summary: In this tutorial, you studied the setup and solution for a fluid flow problem involving solidification for the Czochralski growth process. The solidification model in FLUENT can be used to model the continuous casting process where a solid material is continuously pulled out from the casting domain. In this tutorial, you patched a constant value and a custom field function for the pull velocities instead of computing them. For cases where the pull velocity is not changing over the domain, this approach is used as it is computationally less expensive than having FLUENT compute the pull velocities during the calculation. For more information about the solidification/melting model, see the User’s Guide.
19-32
c Fluent Inc. November 27, 2001
Tutorial 20.
Postprocessing
Introduction: In this tutorial, the postprocessing capabilities of FLUENT are demonstrated for a 3D laminar flow involving conjugate heat transfer. The flow is over a rectangular heat-generating electronics chip which is mounted on a flat circuit board. The heat transfer involves the coupling of conduction in the chip and conduction and convection in the surrounding fluid. The physics of conjugate heat transfer such as this is common in many engineering applications, including the design and cooling of electronic components. In this example, you will read the case and data files (without doing the calculation) and perform a number of postprocessing exercises. In the process, you will learn how to: • Create surfaces for the display of 3D data • Display velocity vectors • Display filled contours of temperature on several surfaces • Mirror a display about a symmetry plane • Add lights to the display at multiple locations • Use the Scene Description and Animate panels to animate the graphics display • Use the Sweep Surface panel to display results on successive slices of the domain • Display pathlines • Plot quantitative results • Overlay and “explode” a display • Annotate your display
c Fluent Inc. November 27, 2001
20-1
Postprocessing
Prerequisites: This tutorial assumes that you are familiar with the menu structure in FLUENT, and that you have solved Tutorial 1. Problem Description: The problem to be considered is shown schematically in Figure 20.1. The configuration consists of a series of sideby-side electronic chips, or modules, mounted on a circuit board. Air flow, confined between the circuit board and an upper wall, cools the modules. To take advantage of the symmetry present in the problem, the model will extend from the middle of one module to the plane of symmetry between it and the next module. As shown in the figure, each half-module is assumed to generate 2.0 Watts and to have a bulk conductivity of 1.0 W/m2 -K. The circuit board conductivity is assumed to be one order of magnitude lower: 0.1 W/m2 -K. The air flow enters the system at 298 K with a velocity of 1 m/s. The Reynolds number of the flow, based on the module height, is about 600. The flow is therefore treated as laminar. Symmetry Planes Top Wall Externally Cooled Bottom Wall Externally Cooled Air Flow 1.0 m/s 298 K
Electronic Module (one half) k = 1.0 W/m2-K Q = 2.0 Watts Circuit Board k = 0.1 W/m2-K
Figure 20.1: Problem Specification
20-2
c Fluent Inc. November 27, 2001
Postprocessing
Preparation 1. Copy the files chip/chip.cas and chip/chip.dat from the FLUENT documentation CD to your working directory (as described in Tutorial 1). 2. Start the 3D version of FLUENT.
Step 1: Reading the Case and Data Files 1. Read in the case and data files (chip.cas and chip.dat). File −→ Read −→Case & Data... Once you select chip.cas, chip.dat will be read automatically.
c Fluent Inc. November 27, 2001
20-3
Postprocessing
Step 2: Grid Display 1. Display the grid. Display −→Grid...
(a) Under Options, select Edges. (b) In the Surfaces list, select board-top and chip. (c) Click Display. Note: You may want to scroll through the Surfaces list to be sure that no other surfaces are selected. You can also deselect all surfaces by clicking on the far-right button at the top of the Surfaces list, and then select the desired surfaces for display.
20-4
c Fluent Inc. November 27, 2001
Postprocessing
2. Use your left mouse button to rotate the view, and your middle mouse button to zoom the view until you obtain an enlarged isometric display of the circuit board in the region of the chip, as shown in Figure 20.2.
Y
X Z
Grid
Jul 05, 2001 FLUENT 6.0 (3d, segregated, lam)
Figure 20.2: Graphics Display of the Chip and Board Surfaces
Extra: You can use the right mouse button to check which zone number corresponds to each boundary. If you click the right mouse button on one of the boundaries displayed in the graphics window, its zone number, name, and type will be printed in the console window. This feature is especially useful when you have several zones of the same type and you want to distinguish between them quickly.
c Fluent Inc. November 27, 2001
20-5
Postprocessing
3. Create a filled surface display. (a) In the Grid Display panel under Options, deselect Edges and select Faces. (b) Click Display. The surfaces run together with no shading to separate the chip from the board. 4. Add shading effects by enabling lights. Display −→Options...
(a) Under Lighting Attributes, enable the Lights On. (b) Click Apply. Shading will be added to the surface grid display (Figure 20.3).
20-6
c Fluent Inc. November 27, 2001
Postprocessing
Y
X Z
Grid
Jul 05, 2001 FLUENT 6.0 (3d, segregated, lam)
Figure 20.3: Graphics Display of the Chip and Board Surfaces with Default Lighting
c Fluent Inc. November 27, 2001
20-7
Postprocessing
(c) In the Display Options panel, click on the Lights... button. This will open the Lights panel.
Note: When you turn lights on, the default settings are for light 0 (indicated by the Light ID), corresponding to a white light at the position (1, 1, 1), as indicated by the unit vectors under Direction.
20-8
c Fluent Inc. November 27, 2001
Postprocessing
(d) Add a light at (-1,1,1). i. Increase the Light ID to 1 and enable the Light On option. ii. Set X, Y, and Z to -1, 1, and 1. iii. Click Apply. (e) Repeat this procedure to add a second light (Light ID=2) at (-1,1,-1). The result is a more softly shaded display (Figure 20.4).
Y
X Z
Grid
Jul 05, 2001 FLUENT 6.0 (3d, segregated, lam)
Figure 20.4: Graphics Display of the Chip and Board Surfaces with Additional Lighting
c Fluent Inc. November 27, 2001
20-9
Postprocessing
Extra: You can use your left mouse button to rotate the ball in the Active Lights window in the Lights panel, as shown below. By doing so, you can gain a perspective view on the relative locations of the lights that are currently active, and see the shading effect on the ball at the center.
You can also change the color of one or more of the lights by typing the name of a color in the Color field or moving the Red, Green, and Blue sliders.
20-10
c Fluent Inc. November 27, 2001
Postprocessing
Step 3: Isosurface Creation To display results in a 3D model, you will need surfaces on which the data can be displayed. FLUENT creates surfaces for all boundary zones automatically. In the case file that you have read, several of these surfaces have been renamed. Examples are board-sym and board-ends, which correspond to the side and end faces of the circuit board. In general, you may want to define additional surfaces for the purpose of viewing your results, such as a plane in Cartesian space, for example. In this exercise, you will create a horizontal plane cutting through the middle of the module. This surface will have a y value of 0.25 inches, and will be used in a later step for displaying the temperature and velocity fields. 1. Create a surface of constant y coordinate. Surface −→Iso-Surface...
c Fluent Inc. November 27, 2001
20-11
Postprocessing
(a) In the Surface of Constant drop-down lists, select Grid... and Y-Coordinate. (b) Click Compute. The Min and Max fields will display the y extents of the domain. (c) Enter 0.25 under Iso-Values. (d) Enter y=0.25in under New Surface Name. (e) Click Create, and Close the panel.
20-12
c Fluent Inc. November 27, 2001
Postprocessing
Step 4: Contours 1. Plot filled contours of temperature on the symmetry plane (Figure 20.5). Display −→Contours...
(a) Under Options, select Filled. (b) Select Temperature... and Static Temperature in the Contours Of drop-down lists. (c) In the Surfaces list, select board-sym, chip-sym, and fluid-sym. (d) Click Display. The temperature contour will be displayed. (e) Rotate and zoom the display using the left and middle mouse buttons, respectively, to obtain the view shown in Figure 20.5.
c Fluent Inc. November 27, 2001
20-13
Postprocessing
4.09e+02 3.98e+02 3.87e+02 3.76e+02 3.64e+02 3.53e+02 3.42e+02 3.31e+02 3.20e+02 3.09e+02 2.98e+02
Y ZX
Contours of Static Temperature (k)
Jun 06, 2001 FLUENT 6.0 (3d, segregated, lam)
Figure 20.5: Filled Contours of Temperature on the Symmetry Surfaces
Hint: If you can and
the display disappears from the screen at any time, or if are having difficulty manipulating it with the mouse, you open the Views panel from the Display pull-down menu use the Default button to reset the view.
Note the peak temperatures in the chip where the heat is generated, along with the higher temperatures in the wake where the flow is recirculating.
20-14
c Fluent Inc. November 27, 2001
Postprocessing
2. Plot filled contours of temperature on the horizontal plane at y=0.25 in (Figure 20.6). (a) In the Contours panel under Surfaces, deselect the symmetry planes and select y=0.25in. (b) Click Display. (c) Zoom the display using your middle mouse button to obtain the view shown in Figure 20.6. 4.09e+02 3.98e+02 3.87e+02 3.76e+02 3.64e+02 3.53e+02 3.42e+02 3.31e+02 3.20e+02 3.09e+02 2.98e+02
Y X Z
Contours of Static Temperature (k)
Jun 06, 2001 FLUENT 6.0 (3d, segregated, lam)
Figure 20.6: Filled Contours of Temperature on the y = 0.25 in. Surface In the contour display (Figure 20.6), the high temperatures in the wake of the module are clearly visible. You may want to display other quantities using the Contours panel, such as velocity magnitude or pressure).
c Fluent Inc. November 27, 2001
20-15
Postprocessing
Step 5: Velocity Vectors Velocity vectors provide an excellent visualization of the flow around the module, depicting details of the wake structure. 1. Display velocity vectors on the symmetry plane through the module centerline (Figure 20.7). Display −→Vectors...
(a) In the Surfaces list, select fluid-sym. (b) Set the Scale Factor to 1.9. (c) Click Display.
20-16
c Fluent Inc. November 27, 2001
Postprocessing
(d) Rotate and zoom the display to observe the vortex near the stagnation point and in the wake of the module (Figure 20.7). 1.41e+00 1.27e+00 1.13e+00 9.89e-01 8.50e-01 7.11e-01 5.72e-01 4.33e-01 2.94e-01 1.54e-01
Y X
1.53e-02
Z
Velocity Vectors Colored By Velocity Magnitude (m/s)
Jun 06, 2001 FLUENT 6.0 (3d, segregated, lam)
Figure 20.7: Velocity Vectors in the Module Symmetry Plane
Note: The vectors in Figure 20.7 are shown without arrowheads. You can modify the arrow style in the Vectors panel by selecting a different option from the Style drop-down list. Extra: If you want to decrease the number of vectors displayed, you can increase the Skip factor to a non-zero value.
c Fluent Inc. November 27, 2001
20-17
Postprocessing
2. Plot velocity vectors in the horizontal plane intersecting the module (Figure 20.9). After plotting the vectors, you will enhance your view by mirroring the display about the module centerline and by adding the display of the module surfaces. Display −→Vectors...
(a) Deselect all surfaces by clicking the unshaded icon to the right of Surfaces. (b) In the Surfaces list, select y=0.25in. (c) Set the Scale to 3.8. 20-18
c Fluent Inc. November 27, 2001
Postprocessing
(d) Under Options, select Draw Grid. This will open the Grid Display panel.
(e) Under Options, check that Faces is selected. (f) In the Surfaces list, select board-top and chip. (g) Click Colors.... This will open the Grid Colors panel.
c Fluent Inc. November 27, 2001
20-19
Postprocessing
(h) In the Types list, select wall. (i) In the Colors list, select light blue, and then Close the panel. (j) In the Grid Display panel, click Display and then Close the panel. (k) Use your mouse to obtain the view shown in Figure 20.8. (l) In the Vectors panel, click Display. (m) Rotate the display with your mouse to obtain the view shown in Figure 20.9.
20-20
c Fluent Inc. November 27, 2001
Postprocessing
Y X Z
Grid
Jun 06, 2001 FLUENT 6.0 (3d, segregated, lam)
Figure 20.8: Filled Surface Display for the Chip and Board Top
1.41e+00 1.27e+00 1.13e+00 9.89e-01 8.50e-01 7.11e-01 5.72e-01 4.33e-01 2.94e-01 1.54e-01 1.53e-02
Y
X Z
Velocity Vectors Colored By Velocity Magnitude (m/s)
Jun 06, 2001 FLUENT 6.0 (3d, segregated, lam)
Figure 20.9: Velocity Vectors and Chip and Board Top Surfaces
c Fluent Inc. November 27, 2001
20-21
Postprocessing
3. Mirror the view about the chip symmetry plane (Figure 20.10). Display −→Views...
(a) In the Mirror Planes list, select symmetry-18. Note: This zone is the centerline plane of the module, and its selection will create a mirror of the entire display about the centerline plane. (b) Click Apply. The display will be updated in your graphics window (Figure 20.10). Extra: You may want to experiment with different views and/or scale factors for the velocities to examine different regions (upstream and downstream of the chip, for example).
20-22
c Fluent Inc. November 27, 2001
Postprocessing
1.41e+00 1.27e+00 1.13e+00 9.89e-01 8.50e-01 7.11e-01 5.72e-01 4.33e-01 2.94e-01 1.54e-01 1.53e-02
YX Z
Velocity Vectors Colored By Velocity Magnitude (m/s)
Jun 06, 2001 FLUENT 6.0 (3d, segregated, lam)
Figure 20.10: Velocity Vectors and Chip and Board Top Surfaces after Mirroring
c Fluent Inc. November 27, 2001
20-23
Postprocessing
Step 6: Animation The surface temperature distribution on the module and on the circuit board can be displayed by selecting these boundaries for display of temperature contours. You can then view the display dynamically, using the animation feature. While effective animation is best conducted on “highend” graphics workstations, you can follow the procedures below on any workstation. If your graphics display speed is slow, the animation playback will take some time and will appear choppy, with the redrawing very obvious. On fast graphics workstations, the animation will appear smooth and continuous and will provide an excellent visualization of the display from a variety of spatial orientations. On many machines, you can improve the smoothness of the animation by turning on the Double Buffering option in the Display Options panel. 1. Display filled contours of surface temperature on the board-top and chip, excluding the symmetry surfaces (Figure 20.11). Display −→Contours...
20-24
c Fluent Inc. November 27, 2001
Postprocessing
(a) Under Options, select Filled. (b) Select Temperature... and Static Temperature in the Contours Of drop-down lists. (c) Deselect all surfaces by clicking the unshaded icon to the right of Surfaces. (d) In the Surfaces list, select board-top and chip. (e) Click Display. (f) Zoom the display as needed to obtain the view shown in Figure 20.11. The temperature display (Figure 20.11) shows the high temperatures on the downstream portions of the module and the relatively localized heating of the circuit board around the module.
c Fluent Inc. November 27, 2001
20-25
Postprocessing
4.09e+02 3.98e+02 3.87e+02 3.76e+02 3.64e+02 3.53e+02 3.42e+02 3.31e+02 3.20e+02 3.09e+02 2.98e+02
YX Z
Contours of Static Temperature (k)
Jun 06, 2001 FLUENT 6.0 (3d, segregated, lam)
Figure 20.11: Filled Temperature Contours on the Chip and Board Top Surfaces
20-26
c Fluent Inc. November 27, 2001
Postprocessing
2. Animate the surface temperature display by changing the point of view. Display −→Animate...
You will use the current display (Figure 20.11) as the starting view for the animation (Frame = 1). (a) Under Key Frames, click Add. This will store the current display as Key-1. (b) Zoom the view to focus on the module region. (c) Under Key Frames, change the Frame number to 10. (d) Click Add. This will store the new display as Key-10.
c Fluent Inc. November 27, 2001
20-27
Postprocessing
The zoomed view will be the tenth keyframe of the animation, with intermediate displays (2 through 9) to be filled in during the animation. (e) Rotate the view and un-zoom the display so that the downstream side of the module is in the foreground, as shown in Figure 20.12. (f) Change the Frame number to 20. (g) Click Add. This will store the new display as Key-20. 3. To animate the view, click on the “play” arrow button (second from the right in the row of playback buttons) in the Playback section of the Animate panel. Extra: You can change the Playback mode if you want to “auto repeat” or “auto reverse” the animation. When you are in either of these Playback modes, you can click on the “stop” button (square) to stop the continuous animation.
20-28
c Fluent Inc. November 27, 2001
Postprocessing
4.09e+02 3.98e+02 3.87e+02 3.76e+02 3.64e+02 3.53e+02 3.42e+02 3.31e+02 3.20e+02 3.09e+02 2.98e+02 Z
Y X
Contours of Static Temperature (k)
Jun 06, 2001 FLUENT 6.0 (3d, segregated, lam)
Figure 20.12: Filled Temperature Contours on the Chip and Board Top Surfaces
c Fluent Inc. November 27, 2001
20-29
Postprocessing
Step 7: Displaying Pathlines Pathlines are the lines traveled by neutrally buoyant particles in equilibrium with the fluid motion. Pathlines are an excellent tool for visualization of complex three-dimensional flows. In this example, you will use pathlines to examine the flow around and in the wake of the module. 1. Create a rake from which the pathlines will emanate. Surface −→Line/Rake...
20-30
c Fluent Inc. November 27, 2001
Postprocessing
(a) In the Type drop-down list, select Rake. A rake surface consists of a specified number of points equally spaced between two specified endpoints. A line surface (the other option in the Type list) is a line that includes the specified endpoints and extends through the domain; data points on a line surface will not be equally spaced. (b) Keep the default of 10 for the Number of Points along the rake. This will generate 10 pathlines. (c) Under End Points, enter the coordinates of the line, using a starting coordinate of (1.0, 0.105, 0.07) and an ending coordinate of (1.0, 0.25, 0.07), as shown in the panel above. This will define a vertical line in front of the module, about halfway between the centerline and edge. (d) Enter pathline-rake for the New Surface Name. You will refer to the rake by this name when you plot the pathlines. (e) Click Create, and Close the panel.
c Fluent Inc. November 27, 2001
20-31
Postprocessing
2. Draw the pathlines (Figure 20.13). Display −→Path Lines...
(a) In the Release From Surfaces list, select pathline-rake. (b) Set the Step Size to 0.001 inch and the number of Steps to 6000. Note: A simple rule of thumb to follow when you are setting these two parameters is that if you want the particles to advance through a domain of length L, the Step Size times the number of Steps should be approximately equal to L. (c) Under Options, select Draw Grid. This will open the Grid Display panel. (d) In the Surfaces list, select board-top and chip. These surfaces should already be selected from the earlier exercise where the grid was displayed with velocity vectors, Step 5: Velocity Vectors. 20-32
c Fluent Inc. November 27, 2001
Postprocessing
(e) Under Options, check that Faces is selected, and then Close the panel. (f) In the Path Lines panel, click Display. The pathlines will be drawn on the surface. (g) Rotate the display so that the flow field in front and in the wake of the chip is visible, as shown in Figure 20.13. 3.00e+01 2.70e+01 2.40e+01 2.10e+01 1.80e+01 1.50e+01 1.20e+01 9.00e+00 6.00e+00 3.00e+00 0.00e+00
Y
X Z
Path Lines Colored by Particle Id
Jun 06, 2001 FLUENT 6.0 (3d, segregated, lam)
Figure 20.13: Pathlines Shown on a Display of the Chip and Board Surfaces.
c Fluent Inc. November 27, 2001
20-33
Postprocessing
Step 8: Overlaying Velocity Vectors on the Pathline Display The overlay capability, provided in the Scene Description panel, allows you to display multiple results on a single plot. You can exercise this capability by adding a velocity vector display to the pathlines just plotted. 1. Enable the overlays feature. Display −→Scene...
(a) Under Scene Composition, select Overlays. (b) Click Apply.
20-34
c Fluent Inc. November 27, 2001
Postprocessing
2. Add a plot of vectors on the chip centerline plane. Display −→Vectors...
(a) Under Options, deselect Draw Grid. (b) Deselect all surfaces by clicking the unshaded icon to the right of Surfaces. (c) In the Surfaces list, select fluid-sym. (d) Set the Scale to 3.8. Because the grid surfaces are already displayed and overlaying is active, there is no need to redisplay the grid surfaces.
c Fluent Inc. November 27, 2001
20-35
Postprocessing
(e) Click Display. (f) Use your mouse to obtain the view that is shown in Figure 20.14.
1.41e+00 1.27e+00 1.13e+00 9.89e-01 8.50e-01 7.11e-01 5.72e-01 4.33e-01 2.94e-01 1.54e-01 1.53e-02
Y
X Z
Velocity Vectors Colored By Velocity Magnitude (m/s)
Jun 06, 2001 FLUENT 6.0 (3d, segregated, lam)
Figure 20.14: Overlay of Velocity Vectors and Pathlines Display
Note: The final display (Figure 20.14) does not require mirroring about the symmetry plane because the vectors obscure the mirrored image. You may turn off the mirroring option in the Views panel at any stage during this exercise.
20-36
c Fluent Inc. November 27, 2001
Postprocessing
Step 9: Exploded Views The Scene Description panel stores each display that you request and allows you to manipulate the displayed items individually. This capability can be used to generate “exploded” views, in which results are translated or rotated out of the physical domain for enhanced display. Below, you can experiment with this capability by displaying “side-by-side” velocity vectors and temperature contours on a streamwise plane in the module wake. 1. Delete the velocity vectors and pathlines from the current display. Display −→Scene...
(a) In the Names list, select the velocity vectors and pathlines. (b) Click Delete Geometry. (c) Click Apply. The Scene Description panel should then contain only the two grid surfaces (board-top and chip).
c Fluent Inc. November 27, 2001
20-37
Postprocessing
2. Create a plotting surface at x=3 inches (named x=3.0in), just downstream of the trailing edge of the module. Surface −→Iso-Surface...
Hint: If you forget how to create an isosurface, see Step 3: Isosurface Creation.
20-38
c Fluent Inc. November 27, 2001
Postprocessing
3. Add the display of filled temperature contours on the x=3.0in surface. Display −→Contours...
(a) Under Options, deselect Draw Grid. (b) Deselect all surfaces by clicking on the unshaded icon to the right of Surfaces. (c) In the Surfaces list, select x=3.0in. (d) Click Display, and Close the panel. The filled temperature contours will be displayed on the x=3.0 in. surface.
c Fluent Inc. November 27, 2001
20-39
Postprocessing
4. Add the velocity vectors on the x=3.0in plotting surface. Display −→Vectors...
(a) Under Options, deselect Draw Grid. (b) Deselect all surfaces by clicking on the unshaded icon to the right of Surfaces. (c) In the Surfaces list, select x=3.0in. (d) Increase the Skip to 2. (e) Change the Scale to 1.9. (f) Click Display.
20-40
c Fluent Inc. November 27, 2001
Postprocessing
The display will show the vectors superimposed on the contours of temperature at x=3.0 in. 5. Create the exploded view (Figure 20.15) by translating the contour display, placing it above the vectors. Display −→Scene... (a) In the Scene Description panel, select contour-6-temperature in the Names list. (b) Click Transform.... This will open the Transformations panel.
(c) Under Translate, enter 1 inch for Y. (d) Click Apply, and Close the Transformations panel. The exploded view allows you to see the contours and vectors as distinct displays in the final scene (Figure 20.15). 6. Turn off the Overlays. (a) In the Scene Description panel, deselect the Overlays option. (b) Click Apply, and Close the panel.
c Fluent Inc. November 27, 2001
20-41
Postprocessing
1.41e+00 1.27e+00 1.13e+00 9.89e-01 8.50e-01 7.11e-01 5.72e-01 4.33e-01 2.94e-01 1.54e-01
Y X
1.53e-02
Z
Velocity Vectors Colored By Velocity Magnitude (m/s)
Jun 12, 2001 FLUENT 6.0 (3d, segregated, lam)
Figure 20.15: Exploded Scene Display of Temperature and Velocity
20-42
c Fluent Inc. November 27, 2001
Postprocessing
Step 10: Animating the Display of Results in Successive Streamwise Planes Often, you may want to march through the flow domain, displaying a particular variable on successive slices of the domain. While this task could be accomplished manually, plotting each plane in turn, or using the Scene Description and Animate panels, here you will use the Sweep Surface panel to facilitate the process. To illustrate the display of results on successive slices of the domain, you will plot contours of velocity magnitude on planes of constant x coordinate. 1. Delete the vectors and temperature contours from the display. Display −→Scene... (a) In the Scene Description panel, select contour-6-temperature and vv-6-velocity-magnitude in the Names list. (b) Click Delete Geometry. (c) Click Apply, and Close the panel. The panel and display window will be updated to contain only the grid surfaces. 2. Use your mouse to un-zoom the view in the graphics window so that the entire board surface is visible. 3. Generate contours of velocity magnitude and sweep them through the domain along the x axis. Display −→Sweep Surface...
c Fluent Inc. November 27, 2001
20-43
Postprocessing
(a) Keep the default Sweep Axis (the x axis). (b) Under Animation, set the Initial Value to 0 m and the Final Value to 0.1651 m. !
The units for the initial and final values are in meters, regardless of the length units being used in the model. Here, the initial and final values are set to the Min Value and Max Value, to generate an animation through the entire domain.
(c) Set the number of Frames to 20. (d) Select Contours under Display Type. This will open the Contours panel.
20-44
c Fluent Inc. November 27, 2001
Postprocessing
i. In the Contours panel, select Velocity... and Velocity Magnitude in the Contours Of drop-down lists. ii. In the Contours panel, click OK. (e) Click on Animate in the Sweep Surface panel. You will see the velocity contour plot displayed at 20 successive streamwise planes. FLUENT automatically interpolates the contoured data on the streamwise planes between the specified end points. Especially on high-end graphics workstations, this can be an effective way to study how a flow variable changes throughout the domain.
c Fluent Inc. November 27, 2001
20-45
Postprocessing
Step 11: XY Plots XY plotting can be used to display quantitative results of your CFD simulations. Here, you will complete your review of the module cooling simulation by plotting the temperature distribution along the top centerline of the module. 1. Define the line along which to plot results. Surface −→Line/Rake...
(a) In the Type drop-down list, select Line. (b) Under End Points, enter the coordinates of the line, using a starting coordinate of (2.0, 0.4, 0.01) and an ending coordinate of (2.75, 0.4, 0.01), as shown in the panel above. These coordinates define the top centerline of the module. (c) Enter top-center-line as the New Surface Name. 20-46
c Fluent Inc. November 27, 2001
Postprocessing
(d) Click Create. 2. Plot the temperature distribution along the top centerline of the module (Figure 20.16). Plot −→XY Plot...
(a) Select Temperature... and Static Temperature in the Y Axis Function drop-down lists. (b) In the Surfaces list, select top-center-line. (c) Keep the default Plot Direction of X. This will plot temperature vs. the x coordinate along the selected line (top-center-line). (d) Click Axes... to modify the axis range. This will open the Axes - Solution XY Plot panel .
c Fluent Inc. November 27, 2001
20-47
Postprocessing
(e) Under Axis, select X. (f) Under Options, deselect Auto Range. (g) Set the Range using a Minimum of 2.0 and a Maximum of 2.75. (h) Click Apply, and Close the panel. (i) In the Solution XY Plot panel, click Plot. The temperature distribution (Figure 20.16) shows the temperature increase across the module surface as the thermal boundary layer develops in the cooling air flow.
20-48
c Fluent Inc. November 27, 2001
Postprocessing
top-center-line 4.02e+02
4.00e+02
3.98e+02
3.96e+02
Static Temperature (k)
3.94e+02
3.92e+02
3.90e+02
3.88e+02 2
Y Z
X
Static Temperature
2.1
2.2
2.3
2.4
2.5
2.6
2.7
2.8
Position (in)
Jun 06, 2001 FLUENT 6.0 (3d, segregated, lam)
Figure 20.16: Temperature Along the Top Centerline of the Module
c Fluent Inc. November 27, 2001
20-49
Postprocessing
Step 12: Annotation You can annotate your display with the text of your choice. Display −→Annotate...
1. In the Annotation Text field, enter the text describing your plot (e.g., Temperature Along the Top Centerline). 2. Click Add. A Working dialog box will appear telling you to select the desired location of the text using the mouse-probe button, which is, by default, the right button. 3. Click your right mouse button in the graphics display window where you want the text to appear, and you will see the text displayed at the desired location (Figure 20.17).
20-50
c Fluent Inc. November 27, 2001
Postprocessing
top-center-line
Temperature Along the Top Centerline 4.02e+02
4.00e+02
3.98e+02
3.96e+02
Static Temperature (k)
3.94e+02
3.92e+02
3.90e+02
3.88e+02 2
Y Z
X
Static Temperature
2.1
2.2
2.3
2.4
2.5
2.6
2.7
2.8
Position (in)
Jun 06, 2001 FLUENT 6.0 (3d, segregated, lam)
Figure 20.17: Temperature Along the Top Centerline of the Module
Extra: If you want to move the text to a new location on the screen, click Delete Text in the Annotate panel, and click Add once again, defining a new position with your mouse. Note: Depending on the size of your graphics window and the hardcopy file format you choose, the font size of the annotation text you see on the screen may be different from the font size in a hardcopy file of that graphics window. The annotation text font size is absolute, while the rest of the items in the graphics window are scaled to the proportions of the hardcopy.
c Fluent Inc. November 27, 2001
20-51
Postprocessing
Step 13: Saving Hardcopy Files You can save hardcopy files of the graphics display in many different formats, including PostScript, encapsulated PostScript, TIFF, PICT, and window dumps. Here, the procedure for saving a color PostScript file is shown. File −→Hardcopy...
1. Under Format, select PostScript. 2. Under Coloring, select Color. 3. Click Save.... This will open the Select File dialog box. 4. In the Select File dialog box, enter a name for the hardcopy file. Summary: This tutorial has demonstrated the use of many of the extensive postprocessing features available in FLUENT. For more information on these and related features, see the “Graphics and Visualization” and “Alphanumeric Reporting” chapters in the User’s Guide. 20-52
c Fluent Inc. November 27, 2001
Tutorial 21.
Turbo Postprocessing
Introduction: This tutorial demonstrates the turbomachinery postprocessing capabilities of FLUENT. In this example, you will read the case and data files (without doing the calculation) and perform a number of turbomachinery-specific postprocessing exercises. In the process, you will learn how to: • Define the topology of a turbomachinery model • Create surfaces for the display of 3D data • Revolve 3D geometry to display a 360-degree image • Report turbomachinery quantities • Display averaged contours for turbomachinery • Display 2D contours for turbomachinery • Display averaged XY plots for turbomachinery Prerequisites: This tutorial assumes that you are familiar with the menu structure in FLUENT, and that you have solved Tutorial 1. Some steps will not be shown explicitly. Problem Description: The problem to be considered is shown schematically in Figure 21.1. The flow of air through a centrifugal compressor is simulated. The model consists of a single 3D sector of the compressor, to take advantage of the circumferential periodicity in the problem. FLUENT’s postprocessing capabilities readily allow you to display realistic full 360-degree images of the solution obtained.
c Fluent Inc. November 27, 2001
21-1
Turbo Postprocessing
inlet
shroud side
hub side
outlet
Figure 21.1: Problem Specification
21-2
c Fluent Inc. November 27, 2001
Turbo Postprocessing
Preparation 1. Copy the files turbo/turbo.cas and turbo/turbo.dat from the FLUENT documentation CD to your working directory (as described in Tutorial 1). 2. Start the 3D version of FLUENT.
Step 1: Reading the Case and Data Files 1. Read in the case and data files (turbo.cas and turbo.dat). File −→ Read −→Case & Data... Once you select turbo.cas, turbo.dat will be read automatically.
c Fluent Inc. November 27, 2001
21-3
Turbo Postprocessing
Step 2: Grid Display Display −→Grid...
1. Under Options, select Edges. 2. Under Edge Type, select Outline. 3. Deselect all surfaces, and then click on Outline at the bottom of the panel. 4. Click Display. 5. Use your left mouse button to rotate the view, and your middle mouse button to zoom the view until you obtain an isometric display of the compressor duct, as shown in Figure 21.2.
21-4
c Fluent Inc. November 27, 2001
Turbo Postprocessing
Y X
Z
Grid
Jul 31, 2001 FLUENT 6.0 (3d, coupled imp, rke)
Figure 21.2: Graphics Display of the Edges of the Compressor Mesh
Extra: You can use the right mouse button to check which zone number corresponds to each boundary. If you click the right mouse button on one of the boundaries displayed in the graphics window, its zone number, name, and type will be printed in the console window. This feature is especially useful when you have several zones of the same type and you want to distinguish between them quickly.
c Fluent Inc. November 27, 2001
21-5
Turbo Postprocessing
Step 3: Defining the Turbomachinery Topology In order to establish the turbomachinery-specific coordinate system used in subsequent postprocessing functions, FLUENT requires you to define the topology of the flow domain. Specifically, you will select boundary zones that comprise the hub, shroud, inlet, outlet, and periodics. Note that boundaries may consist of more than one zone. See Section 25.9.1 of the User’s Guide for more information. The topology setup that you define will be saved to the case file when you save the current model. Thus, if you read this case back into FLUENT, you do not need to set up the topology again. Define −→Turbo Topology...
1. Specify the surfaces representing the hub. (a) Under Boundaries, keep the default selection of Hub. (b) In the Surfaces list, select the surfaces that represent the hub (wall-diffuser-hub, wall-hub, and wall-inlet-hub.) 21-6
c Fluent Inc. November 27, 2001
Turbo Postprocessing
2. Specify the surfaces representing the casing. (a) Under Boundaries, select Casing. (b) In the Surfaces list, select wall-diffuser-shroud, wall-inlet-shroud, and wall-shroud. 3. Specify the surfaces representing the periodic boundaries. (a) Under Boundaries, select Theta Periodic. (b) In the Surfaces list, select periodic.33, periodic.34, and periodic.35. Note: While Theta Periodic represents periodic boundary zones on the circumferential boundaries of the flow passage, Theta Min and Theta Max are wall surfaces at the minimum and maximum θ position on a circumferential boundary. There are no such wall surfaces in this problem. 4. Specify the surface representing the Inlet (inlet). 5. Specify the surface representing the Outlet (outlet). 6. Specify the surface representing the Blade (wall-blade). 7. Click Apply to set all of the turbomachinery boundaries. FLUENT will inform you that the turbomachinery postprocessing functions have been activated, and the Turbo menu will appear in FLUENT’s menu bar at the top of the console window. Note: You can display the selected surfaces by clicking on Display at the bottom of the panel. This is useful as a graphical check to ensure that all relevant surfaces have been selected.
c Fluent Inc. November 27, 2001
21-7
Turbo Postprocessing
Step 4: Isosurface Creation To display results in a 3D model, you will need surfaces on which the data can be displayed. FLUENT creates surfaces for all boundary zones automatically. In a general application, you may want to define additional surfaces for the purpose of viewing results. FLUENT’s turbo postprocessing capabilities allow you to define more complex surfaces, specific to the application and the particular topology that you defined. In this step, you will create surfaces of iso-meridional (marching along the streamwise direction) and spanwise (distance between the hub and the shroud) coordinates in the compressor. Surface −→Iso-Surface... 1. Create surfaces of constant meridional coordinate.
(a) In the Surface of Constant drop-down lists, select Grid... and Meridional Coordinate. (b) Enter 0.2 under Iso-Values. (c) Enter meridional-0.2 under New Surface Name. 21-8
c Fluent Inc. November 27, 2001
Turbo Postprocessing
(d) Click Create. Note: The iso-values you enter for these turbo-specific surfaces are expressed as a percentage of the entire domain (i.e., you just defined a surface of meridional coordinate equal to 20% of the path along the duct). (e) Repeat the steps above to define surfaces of meridional coordinates equal to 0.4, 0.6, and 0.8. 2. Create surfaces of constant spanwise coordinate.
(a) In the Surface of Constant drop-down lists, select Grid... and Spanwise Coordinate (b) Enter 0.25 under Iso-Values. (c) Enter spanwise-0.25 under New Surface Name. (d) Click Create. (e) Repeat the steps above to define surfaces of spanwise coordinates equal to 0.5 and 0.75.
c Fluent Inc. November 27, 2001
21-9
Turbo Postprocessing
Step 5: Contours 1. Plot filled contours of pressure on the meridional isosurfaces (Figure 21.3). Display −→Contours...
(a) Under Options, select Filled. (b) Select Pressure... and Static Pressure in the Contours Of dropdown lists. (c) In the Surfaces list, select inlet, meridional-0.2, meridional-0.4, meridional-0.6, meridional-0.8, and outlet. (d) Under Options, select Draw Grid, and keep the current settings in the Grid Display panel.
21-10
c Fluent Inc. November 27, 2001
Turbo Postprocessing
(e) Click Display in the Contours panel. (f) Rotate and zoom the display using the left and middle mouse buttons, respectively, to obtain the view shown in Figure 21.3. 1.84e+00 1.73e+00 1.62e+00 1.50e+00 1.39e+00 1.28e+00 1.17e+00 1.06e+00 9.44e-01 8.32e-01 7.20e-01 X
Y Z
Contours of Static Pressure (atm)
Jul 27, 2001 FLUENT 6.0 (3d, coupled imp, rke)
Figure 21.3: Filled Contours of Pressure on the Meridional Isosurfaces
In Figure 21.3, you can observe the buildup of static pressure along the duct.
c Fluent Inc. November 27, 2001
21-11
Turbo Postprocessing
2. Plot filled contours of Mach number (Figure 21.4). (a) Select Velocity... and Mach Number in the Contours Of dropdown lists. (b) Click Display. 1.04e+00 9.35e-01 8.35e-01 7.34e-01 6.34e-01 5.33e-01 4.33e-01 3.32e-01 2.32e-01 1.31e-01 3.05e-02 X
Y Z
Contours of Mach Number
Jul 27, 2001 FLUENT 6.0 (3d, coupled imp, rke)
Figure 21.4: Filled Contours of Mach Number on the Meridional Isosurfaces In Figure 21.4, you can observe locations at which the flow becomes slightly supersonic, about halfway through the duct.
21-12
c Fluent Inc. November 27, 2001
Turbo Postprocessing
3. Plot filled contours of Mach number on the spanwise isosurfaces (Figure 21.5). (a) In the Surfaces list, deselect all surfaces, and then select spanwise0.25, spanwise-0.5, and spanwise-0.75. (b) Click Display. 1.04e+00 9.35e-01 8.35e-01 7.34e-01 6.34e-01 5.33e-01 4.33e-01 3.32e-01 2.32e-01 1.31e-01 3.05e-02
X
Y Z
Contours of Mach Number
Jul 27, 2001 FLUENT 6.0 (3d, coupled imp, rke)
Figure 21.5: Filled Contours of Mach Number on the Spanwise Isosurfaces The display in Figure 21.5 allows you to further study the variation of the Mach number inside the duct. You may want to explore using different combinations of surfaces to display the same or additional variables.
c Fluent Inc. November 27, 2001
21-13
Turbo Postprocessing
4. Display a 360-degree image of the Mach number contours on the 0.5 spanwise isosurface (Figure 21.6). (a) Redisplay the contours, just on the 0.5 spanwise isosurface. i. In the Surfaces list, deselect spanwise-0.25 and spanwise0.75. ii. Click Display. (b) Display the full 360-degree geometry. Display −→Views...
i. Set Periodic Repeats to 20. ii. Click Apply. The display will be updated to show the entire geometry. Note: This step demonstrates a typical view-manipulation task. See Tutorial 20 for further examples of postprocessing features.
21-14
c Fluent Inc. November 27, 2001
Turbo Postprocessing
1.04e+00 9.35e-01 8.35e-01 7.34e-01 6.34e-01 5.33e-01 4.33e-01 3.32e-01 2.32e-01 1.31e-01 3.05e-02 X
Y Z
Contours of Mach Number
Jul 27, 2001 FLUENT 6.0 (3d, coupled imp, rke)
Figure 21.6: Filled Contours of Mach Number on the 0.5 Spanwise Iso Surface
c Fluent Inc. November 27, 2001
21-15
Turbo Postprocessing
Step 6: Reporting Turbo Quantities The turbomachinery report gives you some tabulated information specific to the application and the defined topology. See Section 25.9.2 of the User’s Guide for details. Turbo −→Report... 1. Under Averages, keep the default of Mass-Weighted. 2. Click Compute.
21-16
c Fluent Inc. November 27, 2001
Turbo Postprocessing
c Fluent Inc. November 27, 2001
21-17
Turbo Postprocessing
Step 7: Averaged Contours Turbo averaged contours are generated as projections of the values of a variable averaged in the circumferential direction and visualized on an rz plane. 1. Turn off the periodic repeats. Display −→Views... (a) In the Views panel, enter 0 in the Periodic Repeats field. (b) Click Apply. 2. Display filled contours of averaged static pressure (Figure 21.7). Turbo −→Averaged Contours...
(a) In the Contours Of drop-down lists, select Pressure... and Static Pressure. (b) Click Display.
21-18
c Fluent Inc. November 27, 2001
Turbo Postprocessing
1.80e+00 1.72e+00 1.63e+00 1.54e+00 1.45e+00 1.36e+00 1.28e+00 1.19e+00 1.10e+00 1.01e+00 9.24e-01
Y Z
X
Averaged Turbo Contour - pressure (atm) (atm)
Aug 13, 2001 FLUENT 6.0 (3d, coupled imp, rke)
Figure 21.7: Filled Contours of Averaged Static Pressure
c Fluent Inc. November 27, 2001
21-19
Turbo Postprocessing
Step 8: 2D Contours In postprocessing a turbomachinery solution, it is often desirable to display contours on constant pitchwise, spanwise, or meridional coordinates, and then project these contours onto a plane. This permits easier evaluation of the contours, especially for surfaces that are highly threedimensional. FLUENT allows you to display contours in this fashion using the Turbo 2D Contours panel. 1. Display 2D contours of Mach number. Turbo −→2D Contours...
(a) Under Surface of Constant, keep the default selection of Pitchwise Value. (b) In the Contours Of drop-down lists, select Velocity... and Mach Number. (c) Under Fractional Distance, enter 0.25. (d) Under Projection Direction, select Radial. 21-20
c Fluent Inc. November 27, 2001
Turbo Postprocessing
(e) Click Display. (f) Use your mouse to obtain the view shown in Figure 21.8. 8.30e-01 7.63e-01 6.95e-01 6.28e-01 5.61e-01 4.94e-01 4.26e-01 3.59e-01 2.92e-01 2.25e-01 1.57e-01
Y XZ
2D Turbo Contour - mach-number
Jul 27, 2001 FLUENT 6.0 (3d, coupled imp, rke)
Figure 21.8: 2D Contours of Mach Number on Surface of Pitchwise Value 0.25.
c Fluent Inc. November 27, 2001
21-21
Turbo Postprocessing
Step 9: Averaged XY Plots In addition to displaying data on different combinations of complex 3D and flattened surfaces, FLUENT’s turbo postprocessing capabilities allow you to display XY plots of averaged variables, relevant to the specific topology of a turbomachinery problem. In particular, you will be able to plot circumferentially-averaged values of variables as a function of either the spanwise coordinate or the meridional coordinate. 1. Plot temperature as a function of the meridional coordinate. Turbo −→Averaged XY Plot...
(a) In the Y Axis Function drop-down lists, select Temperature... and Static Temperature. (b) In the X Axis Function drop-down list, select Meridional Distance. (c) Under Fractional Distance, enter 0.9. (d) Click Plot.
21-22
c Fluent Inc. November 27, 2001
Turbo Postprocessing
3.60e+02 3.50e+02 3.40e+02 3.30e+02
temperature (k)
3.20e+02 3.10e+02 3.00e+02 2.90e+02 2.80e+02 0
Y
0.1
0.2
0.3
0.4
0.5
0.6
0.7
0.8
0.9
1
Meridional Distance
X Z Averaged XY - temperature (k)
Jul 27, 2001 FLUENT 6.0 (3d, coupled imp, rke)
Figure 21.9: Averaged XY Plot of Static Temperature on Spanwise Surface of 0.9 Isovalue
Summary: This tutorial has demonstrated the use of some of the turbomachinery-specific postprocessing features of FLUENT. These features can be accessed once you have defined the topology of the problem. More extensive general-purpose postprocessing features are demonstrated in Tutorial 20. See also the “Graphics and Visualization” and “Alphanumeric Reporting” chapters in the User’s Guide.
c Fluent Inc. November 27, 2001
21-23
Tutorial 22.
Parallel Processing
Introduction: This tutorial illustrates the setup and solution of a simple 2D problem using FLUENT’s parallel processing capabilities. In order to be run in parallel, the mesh must be divided into smaller, evenly sized partitions. Each FLUENT process, called a compute node, will solve on a single partition, and information will be passed back and forth across all partition interfaces. FLUENT’s solver allows parallel processing on a dedicated parallel machine, or a network of heterogeneous workstations running UNIX, or a network of workstations running Windows. The tutorial assumes that both FLUENT and network communication software have been correctly installed (see the separate installation instructions and related information for details). The case chosen is the mixing elbow problem you solved in Tutorial 1. In this tutorial you will learn how to: • Start the parallel version of FLUENT • Partition a grid for parallel processing • Use a parallel network of workstations • Check the performance of the parallel solver Prerequisites: This tutorial assumes that you are familiar with the menu structure in FLUENT, and that you have solved Tutorial 1. Problem Description: The problem to be considered is shown schematically in Figure 22.1. A cold fluid at 26◦ C enters through the large pipe and mixes with a warmer fluid at 40◦ C in the elbow. The pipe dimensions are in inches, and the fluid properties and boundary conditions are given in SI units. The Reynolds number at the main inlet is 2.03 × 105 , so that a turbulent model will be necessary.
c Fluent Inc. November 27, 2001
22-1
Parallel Processing
Density:
ρ = 1000 kg/m 3
Viscosity:
-4 µ = 8 x 10 Pa-s
Conductivity:
k = 0.677 W/m-K
32 ″
Specific Heat: C = 4216 J/kg-K p
39.9
3°
3°
U x = 0.2 m/s T = 26 °C I = 5%
39.9
16 ″
16 ″ 12 ″ 32 ″
4″ U y = 1 m/s T = 40 °C I = 5%
Figure 22.1: Problem Specification
22-2
c Fluent Inc. November 27, 2001
Parallel Processing
Preparation 1. Copy the file parallel/elbow3.cas from the FLUENT documentation CD to your working directory (as described in Tutorial 1). You can partition the grid before or after you set up the problem (by defining models, boundary conditions, etc.). It is best to partition after the problem is set up, since partitioning has some model dependencies (e.g., sliding-mesh and shell-conduction encapsulation). Because you already set up this problem in Tutorial 1, you can save the effort of redefining the models and boundary conditions.
Step 1: Starting the Parallel Version of FLUENT Since the procedure for starting the parallel version of FLUENT is dependent upon the type of machine(s) you are using, four versions of this step are provided here. Follow the procedure for the machine configuration that is appropriate for you. • Step 1A: Multiprocessor UNIX Machine • Step 1B: Multiprocessor Windows Machine • Step 1C: Network of UNIX Workstations • Step 1D: Network of Windows Workstations
c Fluent Inc. November 27, 2001
22-3
Parallel Processing
Step 1A: Multiprocessor UNIX Machine 1. At the command prompt, type fluent. !
Do not specify any argument (e.g., 2d).
2. Specify the 2D parallel version. File −→Run...
(a) Under Versions, turn on Parallel. (b) Under Options, specify 2 as the number of Processes. (c) Under Options, keep the Default selection in the Communicator drop-down list. (d) Click Run. 22-4
c Fluent Inc. November 27, 2001
Parallel Processing
Note: It is also possible to start the multiprocessor parallel version of FLUENT from the command line instead of using the Select Solver panel. See Chapter 28 of the User’s Guide for details.
Step 1B: Multiprocessor Windows Machine 1. At the DOS command prompt, type fluent 2d -t2 to start the 2D parallel version with two processes.
c Fluent Inc. November 27, 2001
22-5
Parallel Processing
Step 1C: Network of UNIX Workstations 1. At the command prompt, type fluent. !
Do not specify any argument (e.g., 2d).
2. Specify the 2D network parallel version. File −→Run...
(a) Under Versions, turn on Parallel. (b) Under Options, keep the default value of 1 as the number of Processes. You will spawn processes to other machines in the next step.
22-6
c Fluent Inc. November 27, 2001
Parallel Processing
(c) Under Options, select Socket in the Communicator drop-down list. (d) Click Run. Note: It is also possible to start the network parallel version from the command line instead of using the Select Solver panel. See Chapter 28 of the User’s Guide for details. 3. Spawn one additional computational node. Parallel −→ Network −→Configure...
(a) Specify the machine on which you want to spawn the process. i. Under Host Entry, specify the machine name in the Hostname field. ii. Enter your user ID in the Username field.
c Fluent Inc. November 27, 2001
22-7
Parallel Processing
iii. Click Add. The machine will be added to the Available Hosts list. Note: It is possible to create a list of available machines and add them to the hosts database, rather than adding machines manually. See Chapter 28 of the User’s Guide for details. (b) Select the newly added host in the Available Hosts list. Note: If you do not have access to another machine, you can spawn the second node on your own machine by selecting it from the Available Hosts list, although you will incur a performance penalty on a single processor machine. (c) Under Spawn Count, keep the default value of 1. This will give you the desired total number of 2 computational nodes. (d) Click Spawn. FLUENT will inform you in a Working dialog box that it is spawning the new node. When it is done, the new node will appear in the Spawned Compute Nodes list, as shown below.
22-8
c Fluent Inc. November 27, 2001
Parallel Processing
Hint: If you accidentally spawn an undesired computational node, you can remove it by selecting it from the Spawned Compute Nodes list and clicking on Kill. 4. Check the network connectivity information. Although FLUENT displays a message confirming the connection to each new compute node and summarizing the host and node processes defined, you may find it useful to review the same information at some time during your session, especially if more compute nodes are spawned to several different machines. Parallel −→Show Connectivity...
c Fluent Inc. November 27, 2001
22-9
Parallel Processing
(a) Specify the number of the Compute Node of interest (0). For information about all defined compute nodes, you will select node 0, since this is the node from which all other nodes are spawned. (b) Click Print. -------------------------------------------------------------------ID Comm. Hostname O.S. PID Mach ID HW ID Name -------------------------------------------------------------------n1 net dori hpux 11681 1 7 Fluent Node host net bilbo hpux 12697 0 3 Fluent Host n0* net bilbo hpux 12698 0 -1 Fluent Node
ID is the sequential denomination of each compute node (the host process is always host), Hostname is the name of the machine hosting the compute node (or the host process), O.S is the architecture, PID is the process ID number, Mach ID is the compute node ID, and HW ID is an identifier specific to the communicator used.
22-10
c Fluent Inc. November 27, 2001
Parallel Processing
Step 1D: Network of Windows Workstations The procedure below is for using the RSHD communicator software that is included with FLUENT. You can use a different communicator if one is available on your system. See the User’s Guide for more information. 1. At the DOS command prompt, type fluent 2d -pnet -t1 to start the 2D network parallel version with one process. You will spawn a second compute node in the next step. 2. Spawn an additional compute node, following the procedure described in Step 1C, substep 3, for a network of UNIX machines. 3. Check the network connectivity, following substep 4 of Step 1C.
c Fluent Inc. November 27, 2001
22-11
Parallel Processing
Step 2: Reading and Partitioning the Grid When you use the parallel solver, you need to subdivide (or partition) the grid into groups of cells that can be solved on separate processors. If you read an unpartitioned grid into the parallel solver, FLUENT will automatically partition it, using the default partition settings. You can then check the partitions, to see if you need to modify the settings and repartition the grid. 1. Inspect the automatic partitioning settings. Parallel −→Auto Partition...
If the Case File option is turned on (the default setting), and there exists a valid partition section in the case file (i.e., one where the number of partitions in the case file divides evenly into the number of compute nodes), then that partition information will be used rather than repartitioning the mesh. You need to turn off the Case File option only if you want to change other parameters in the Auto Partition Grid panel. (a) Keep all defaults in the Auto Partition Grid panel. When you keep the Case File option turned on, FLUENT will automatically select a partitioning method for you. This is the preferred initial approach for most problems. In the next step you will inspect the partitions created and be able to change them, if you so choose.
22-12
c Fluent Inc. November 27, 2001
Parallel Processing
2. Read the case file parallel.cas. File −→ Read −→Case... 3. Display the grid (Figure 22.2). Display −→Grid...
Grid
Jul 03, 2001 FLUENT 6.0 (2d, segregated, ske)
Figure 22.2: Triangular Grid for the Mixing Elbow
c Fluent Inc. November 27, 2001
22-13
Parallel Processing
4. Check the partition information. Parallel −→Partition...
(a) Click Print Active Partitions. FLUENT will print the active partition statistics to the console window. Note: FLUENT distinguishes between two cell partition schemes within a parallel problem: the active cell partition, and the stored cell partition. Here, both are set to the cell partition that was created upon reading the case file. If you re-partition the grid using the Partition Grid panel, the new partition will be referred to as the stored cell partition. To make it the active cell partition, you need to click on the Use Stored Partitions button in the Partition Grid panel. The active cell partition is used for the current calculation, while the stored cell partition (the last partition performed) is used when you save a case file. This distinction is made mainly to allow you to partition a case on one machine or network of machines and solve 22-14
c Fluent Inc. November 27, 2001
Parallel Processing
it on a different one. See Chapter 28 of the User’s Guide for more information. >> 2 Active Partitions: P Cells I-Cells Cell Ratio 0 612 10 0.016 1 612 13 0.021
Faces I-Faces Face Ratio Neigh 985 13 0.013 1010 13 0.013
----------------------------------------------------------------Collective Partition Statistics: Minimum Maximum Total ----------------------------------------------------------------Cell count 612 612 1224 Mean cell count deviation 0.0% 0.0% Partition boundary cell count 10 13 23 Partition boundary cell count ratio 1.6% 2.1% 1.9% Face count Mean face count deviation Partition boundary face count Partition boundary face count ratio
985 -1.3% 13 1.3%
1010 1.3% 13 1.3%
1982 13 0.7%
Partition neighbor count 1 1 ----------------------------------------------------------------Partition Method Principal Axes Original Partition Count 2 Done.
(b) Review the partition statistics. An optimal partition should produce an equal number of cells in each partition for load balancing, a minimum number of partition interfaces to reduce interpartition communication bandwidth, and a minimum number of partition neighbors to reduce the startup time for communication. Here, you will be looking for relatively small values of mean cell and face count deviation and total partition boundary cell and face count ratio.
c Fluent Inc. November 27, 2001
22-15
Parallel Processing
5. Examine the partitions graphically. (a) Initialize the solution. Even though you are not going to start a solution at this point, you have to perform a solution initialization in order to use the Contours panel to inspect the partition you just created. Solve −→ Initialize −→Initialize... (b) Display the cell partitions (Figure 22.3). Display −→Contours...
i. In the Contours Of drop-down lists, select Cell Info... and Active Cell Partition. ii. Under Options, select Filled. iii. Set the number of Levels to 2, the number of compute nodes. 22-16
c Fluent Inc. November 27, 2001
Parallel Processing
iv. Click Display. 1.00e+00
0.00e+00
Contours of Cell Partition
Jul 03, 2001 FLUENT 6.0 (2d, segregated, ske)
Figure 22.3: Cell Partitions As shown in Figure 22.3, the cell partitions are acceptable for this problem. The position of the interface reveals that the criteria mentioned above will be matched. If you were unsatisfied with the partitions, you could use the Partition Grid panel to repartition the grid. See the User’s Guide for details about the procedure and options for manually partitioning a grid. Recall that, if you wish to use the modified partitions for a calculation, you will need to make the Stored Cell Partition the Active Cell Partition by either clicking on the Use Stored Partitions button in the Partition Grid panel or saving the case file and reading it back into FLUENT. 6. Save the case file with the partitioned mesh (elbow4.cas). File −→ Write −→Case...
c Fluent Inc. November 27, 2001
22-17
Parallel Processing
Step 3: Solution 1. Initialize the flow field using the boundary conditions set at velocityinlet-5. Solve −→ Initialize −→Initialize...
(a) Choose velocity-inlet-5 from the Compute From list. (b) Click on Init and Close the panel. 2. Enable the plotting of residuals during the calculation. Solve −→ Monitors −→Residual... 3. Start the calculation by requesting 100 iterations. Solve −→Iterate... The solution will converge in approximately 72 iterations. 4. Save the data file (elbow4.dat). File −→ Write −→Data...
22-18
c Fluent Inc. November 27, 2001
Parallel Processing
Step 4: Checking Parallel Performance Generally, you will use the parallel solver for large, computationallyintensive problems, and you will want to check the parallel performance to determine if any optimization is required. See Chapter 28 of the User’s Guide for details. Although the example in this tutorial is a simple 2D case, here you will check the parallel performance as an exercise. Parallel −→ Timer −→Usage Performance Timer for 71 iterations on 2 compute nodes Average wall-clock time per iteration: 0.021 sec Global reductions per iteration: 80 ops Global reductions time per iteration: 0.000 sec (0.0%) Message count per iteration: 199 messages Data transfer per iteration: 0.009 MB LE solves per iteration: 6 solves LE wall-clock time per iteration: 0.005 sec (23.7%) LE global solves per iteration: 2 solves LE global wall-clock time per iteration: 0.000 sec (0.8%) AMG cycles per iteration: 9 cycles Relaxation sweeps per iteration: 276 sweeps Relaxation exchanges per iteration: 61 exchanges Total wall-clock time: Total CPU time:
1.463 sec 2.900 sec
The most accurate way to evaluate parallel performance is by running the same parallel problem on 1 CPU and on n CPUs, and comparing the Total wall-clock time (elapsed time for the iterations) in both cases. Ideally you would want to have the Total wall-clock time with n CPUs be 1/n times the Total wall-clock time with 1 CPU. In practice, this improvement will be reduced by the performance of the communication subsystem of your hardware, and the overhead of the parallel process itself. As a rough estimate of parallel performance, you can compare the Total wall-clock time with the CPU time. In this case the CPU time was approximately 1.98 times the Total wall-clock time.
c Fluent Inc. November 27, 2001
22-19
Parallel Processing
For a parallel process run on two compute nodes, this reveals very good parallel performance, even though the advantage over a serial calculation is small, as expected for this simple 2D problem.
Step 5: Postprocessing See Tutorial 1 for complete postprocessing exercises for this example. Here, two plots are generated so that you can confirm that the results you obtained with the parallel solver are the same as those you obtained with the serial solver. 1. Display an XY plot of temperature across the exit (Figure 22.4). Plot −→ XY Plot...
(a) Select Temperature... and Static Temperature in the Y Axis Function drop-down lists. 22-20
c Fluent Inc. November 27, 2001
Parallel Processing
(b) Select pressure-outlet-7 in the Surfaces list. (c) Click on Plot. pressure-outle 3.15e+02
3.10e+02
3.05e+02
Static Temperature (k)
3.00e+02
2.95e+02
2.90e+02 48
50
52
54
56
58
60
62
64
Position (in)
Static Temperature
Jul 03, 2001 FLUENT 6.0 (2d, segregated, ske)
Figure 22.4: Temperature Distribution at the Outlet
c Fluent Inc. November 27, 2001
22-21
Parallel Processing
2. Display filled contours of the custom field function dynam-head (Figure 22.5). Display −→ Contours...
(a) Select Custom Field Functions... in the drop-down list under Contours Of. The function you created in Tutorial 1, dynam-head, will be shown in the lower drop-down list. (b) Change the number of Levels back to 20. (c) Click on Display, and then Close the panel.
22-22
c Fluent Inc. November 27, 2001
Parallel Processing
7.60e+02 6.84e+02 6.08e+02 5.32e+02 4.56e+02 3.80e+02 3.04e+02 2.28e+02 1.52e+02 7.60e+01 0.00e+00
Contours of dynam-head
Jul 03, 2001 FLUENT 6.0 (2d, segregated, ske)
Figure 22.5: Contours of the Custom Field Function, Dynamic Head
Summary: In this tutorial you learned how to solve a simple 2D problem using FLUENT’s parallel solver. Here the automatic grid partitioning performed by FLUENT when you read the mesh into the parallel version was found to be acceptable. You also learned how to check the performance of the parallel solver to determine if optimizations are required. See the User’s Guide for additional details about using the parallel solver.
c Fluent Inc. November 27, 2001
22-23
