PDF
Free Surface Mixer
Introduction
This example of turbulent flow in a partially baffled mixer shows how to set up The Rotating Machinery, Turbulent Flow interfaces from the Mixer Module with free surface and stationary free surface features. The mixed fluid is water, and the flow is modeled using the k-ε turbulence model. Both frozen-rotor and time-dependent simulations are performed and compared. The mixer geometry used in this model corresponds to the one used by J.-P. Torré and others (Ref. 1).
Model Definition
The mixer is a glass-lined, under-baffled stirred vessel. Figure 1 shows the model geometry. It includes a three-bladed impeller and two beavertail baffles supported at the top of the vessel. The tank bottom is curved, allowing the three-bladed impeller to be placed close to the bottom. The cylindrical part of the tank has a diameter of 450 mm, and the initial water level is 700 mm. The two contoured baffles hang from the top of the mixer, and their lower part is 256 mm above the bottom of the vessel.
Figure 1: Geometry of the mixer with two rods and a three-bladed impeller.
The fluid contained in the mixer, water, is mixed using an impeller with a rotational velocity of 100 rpm. The flow in the mixer is modeled using the k-ε turbulence model.
The model is solved in two steps. First, a Frozen Rotor study is used to reach a good initial solution for the time-dependent study without having to solve the transient startup of the problem. In order to converge this step, a parametric sweep is used to first solve the model with a lower Reynolds number by using a higher value of the dynamic viscosity, and then computed again with the actual dynamic viscosity of the fluid. Then, a Time Dependent study is solved for a period of 1.8 seconds. This corresponds to 3 revolutions of the impeller.
Free surface
The top boundary corresponds to the two-phase interface separating the modeled water from the external air. In the transient case, this is modeled using the free surface feature and a deforming domain. Assuming that the dynamic viscosity and density of the air are negligible compared to the corresponding values for the water, so that the velocity and viscous stresses of the air do not affect the flow in the vessel, the following condition is applied for the normal stress:
Here pext = 0 Pa is the pressure outside the free surface domain, and σ is the water/air surface tension coefficient. The kinematic free surface condition sets the mesh to follow the motion of the fluid in the normal direction to the surface:
The free surface feature is not available in the frozen rotor study since the deformation of the mesh cannot be tracked. In this case, the Stationary Free Surface feature can be used to approximate the deformation of the free surface from the pressure distribution on the boundary. This boundary condition applies a slip condition together with an external pressure. After computing the frozen rotor simulation, a Stationary Free Surface study step can be used to evaluate the free surface deformation ηFS from the pressure obtained in the frozen rotor study using a linearized free surface condition:
Here x = x0 represents the position of the undisturbed surface.
Results and Discussion
The resulting velocity and free surface deformation in the mixer for the frozen-rotor and time-dependent studies are shown in Figure 2 and Figure 3, respectively. The turbulent viscosities are depicted in Figure 4 and Figure 5. It can be observed that the velocity field and turbulent viscosity obtained in the frozen-rotor simulation agree well with the time-dependent results. The stationary free surface feature is also able to provide a good prediction of the vortex induced deformation that develops on the free surface. However, the time-dependent study also provides the transient evolution of the free surface deformation and its instabilities.
Figure 2: Velocity field and free surface position for the frozen rotor study.
Figure 3: Velocity field and free surface position at t = 1.8 s.
Figure 4: Turbulent viscosity for the frozen rotor case.
Figure 5: Turbulent viscosity at t = 1.8 s.
Figure 6 and Figure 7 show the velocity distribution in one vertical and five horizontal cross sections. The larger velocities are observed near the rotating blades, which induce a flow toward the walls. Upon reaching the wall, vertical high speed streaks form along the outer walls, and the fluid velocity decreases toward the top of the vessel. A swirl flow pattern can be observed at the upper part of the tank, resulting in a small central vortex adjacent to the free surface.
Figure 6: Velocity field in the middle xz-plane at t = 1.8 s.
Figure 7: Velocity field in 5 xy-planes.
Notes About the COMSOL Implementation
This model has a large number of degrees of freedom and requires an iterative solver for optimal performance. The Algebraic Multigrid Solver suggested per default is optimal for the Time Dependent study. A Geometric Multigrid Solver should be used in the frozen rotor study step since the Algebraic Multigrid Solver is not suited for the Stationary Free Surface feature.
Reference
1. J.-P. Torré and others, “An Experimental and Computational Study of the Vortex Shape in a Partially Baffled Agitated Vessel,” Chem. Eng. Sci., vol. 62, no. 7, pp. 1915–1926, 2007.
Application Library path: Mixer_Module/Tutorials/free_surface_mixer
Modeling Instructions
From the File menu, choose New.
New
In the New window, click  Model Wizard.
Model Wizard
1
In the Model Wizard window, click  3D.
2
In the Select Physics tree, select Fluid Flow > Single-Phase Flow > Rotating Machinery, Fluid Flow > Turbulent Flow > Turbulent Flow, k-ε.
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select Preset Studies for Selected Physics Interfaces > Frozen Rotor with Stationary Free Surface.
6
Click  Done.
Geometry 1
Load the model geometry from a geometry sequence file. It imports the mixer geometry and uses virtual operations to simplify the geometry for efficient meshing. It also contains selections that are used throughout the model setup and results processing.
1
In the Geometry toolbar, click Insert Sequence and choose Insert Sequence.
2
Browse to the model’s Application Libraries folder and double-click the file free_surface_mixer_geom_sequence.mph.
3
In the Geometry toolbar, click  Build All.
4
Click the  Zoom Extents button in the Graphics toolbar.
Global Definitions
Parameters 1
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
viscFact
1
1
Viscosity factor
Step 1 (step1)
1
In the Home toolbar, click  Functions and choose Global > Step.
2
In the Settings window for Step, locate the Parameters section.
3
In the Location text field, type 0.5.
4
Click to expand the Smoothing section. From the Number of continuous derivatives list, choose 1.
5
Click  Plot.
Moving Mesh
Rotating Domain 1
1
In the Model Builder window, under Component 1 (comp1) > Moving Mesh click Rotating Domain 1.
2
Select Domain 3 only.
3
In the Settings window for Rotating Domain, locate the Rotation section.
4
In the f text field, type 100[rpm].
5
Locate the Axis section. Specify the urot vector as
0
X
0
Y
1
Z
Component 1 (comp1)
Deforming Domain 1
1
In the Moving Mesh toolbar, click  Deforming Domain.
2
Select Domain 2 only.
Turbulent Flow, k-ε (spf)
1
In the Model Builder window, under Component 1 (comp1) click Turbulent Flow, k-ε (spf).
2
In the Settings window for Turbulent Flow, k-ε, locate the Physical Model section.
3
Select the Include gravity checkbox.
Wall 2
1
In the Physics toolbar, click  Boundaries and choose Wall.
2
Select Boundary 32 only.
3
In the Settings window for Wall, click to expand the Wall Movement section.
4
From the Translational velocity list, choose Zero (Fixed wall).
The Translational velocity is set to Zero (Fixed Wall) to ensure that the wall is not moving. If Automatic from frame is selected, the wall will rotate due to the angular velocity of the Rotating Domain.
Stationary Free Surface 1
1
In the Physics toolbar, click  Boundaries and choose Stationary Free Surface.
2
In the Settings window for Stationary Free Surface, locate the Boundary Selection section.
3
From the Selection list, choose Free Surface.
Free Surface 1
1
In the Physics toolbar, click  Boundaries and choose Free Surface.
2
In the Settings window for Free Surface, locate the Boundary Selection section.
3
From the Selection list, choose Free Surface.
The Stationary Free Surface will be used in the Frozen Rotor study, while Free Surface will override it in the Time Dependent study.
Add Material
1
In the Materials toolbar, click  Add Material to open the Add Material window.
2
Go to the Add Material window.
3
In the tree, select Built-in > Water, liquid.
4
Right-click and choose Add to Component 1 (comp1).
5
In the Materials toolbar, click  Add Material to close the Add Material window.
Materials
Water, liquid (mat1)
1
In the Settings window for Material, locate the Material Contents section.
2
In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Dynamic viscosity
mu
eta(T)*viscFact
Pa·s
Basic
Mesh 1
1
In the Model Builder window, under Component 1 (comp1) click Mesh 1.
2
In the Settings window for Mesh, locate the Physics-Controlled Mesh section.
3
In the table, clear the Use checkbox for Geometric Analysis, Detail Size.
4
Right-click Component 1 (comp1) > Mesh 1 and choose Edit Physics-Induced Sequence.
Size
1
In the Model Builder window, under Component 1 (comp1) > Mesh 1 click Size.
2
In the Settings window for Size, locate the Element Size section.
3
Click the Custom button.
4
Locate the Element Size Parameters section. In the Maximum element size text field, type 0.02.
5
In the Minimum element size text field, type 0.008.
6
In the Maximum element growth rate text field, type 1.12.
Size 1
1
In the Model Builder window, click Size 1.
2
In the Settings window for Size, locate the Element Size section.
3
From the Predefined list, choose Fine.
4
Click the Custom button.
5
Locate the Element Size Parameters section.
6
Select the Maximum element size checkbox. In the associated text field, type 0.02.
7
Select the Minimum element size checkbox. In the associated text field, type 0.004.
8
Select the Maximum element growth rate checkbox. In the associated text field, type 1.12.
9
Select the Curvature factor checkbox.
10
Select the Resolution of narrow regions checkbox.
Free Tetrahedral 1
1
In the Model Builder window, click Free Tetrahedral 1.
2
In the Settings window for Free Tetrahedral, locate the Domain Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domains 1 and 3 only.
5
Click the  Wireframe Rendering button in the Graphics toolbar to be able to locate the entities inside the vessel.
Size 1
1
Right-click Free Tetrahedral 1 and choose Size.
2
In the Settings window for Size, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Boundary.
4
Click  Paste Selection.
5
In the Paste Selection dialog, type 8, 20, 30, 31, 32 in the Selection text field.
6
Click OK.
7
In the Settings window for Size, locate the Element Size section.
8
From the Predefined list, choose Extra fine.
9
Click the Custom button.
10
Locate the Element Size Parameters section.
11
Select the Maximum element size checkbox. In the associated text field, type 0.013.
12
Select the Curvature factor checkbox. In the associated text field, type 0.35.
Size 2
1
Right-click Free Tetrahedral 1 and choose Size.
2
In the Settings window for Size, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Boundary.
4
Click  Paste Selection.
5
In the Paste Selection dialog, type 34, 38, 68 in the Selection text field.
6
Click OK.
7
In the Settings window for Size, locate the Element Size section.
8
From the Predefined list, choose Extremely fine.
Free Tetrahedral 1
Right-click Free Tetrahedral 1 and choose Build Selected.
Swept 1
1
In the Mesh toolbar, click  Swept.
2
In the Settings window for Swept, locate the Domain Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domain 4 only.
Distribution 1
1
Right-click Swept 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
From the Distribution type list, choose Predefined.
4
In the Number of elements text field, type 16.
5
In the Element ratio text field, type 1.6.
Swept 2
In the Mesh toolbar, click  Swept.
Distribution 1
1
Right-click Swept 2 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
From the Distribution type list, choose Predefined.
4
In the Number of elements text field, type 12.
5
In the Element ratio text field, type 2.
Boundary Layer Properties 1
1
In the Model Builder window, expand the Boundary Layers 1 node, then click Boundary Layer Properties 1.
2
In the Settings window for Boundary Layer Properties, locate the Layers section.
3
In the Number of layers text field, type 6.
4
In the Thickness adjustment factor text field, type 2.
5
Click  Build All.
6
Click the  Wireframe Rendering button in the Graphics toolbar to go back to the default view.
Build manual multigrid levels for optimal performance. Start by referencing the initial mesh, then scale it. To prevent elements from becoming too small, set a minimum element size manually for the new meshes.
Mesh 2
In the Mesh toolbar, click Add Mesh and choose Add Mesh.
Reference 1
1
In the Mesh toolbar, click  Modify and choose Reference.
2
In the Settings window for Reference, locate the Reference section.
3
From the Mesh list, choose Mesh 1.
Scale 1
1
In the Mesh toolbar, click  More Attributes and choose Scale.
2
In the Settings window for Scale, locate the Scale section.
3
In the Element size scale text field, type 2.
Reference 1
In the Model Builder window, right-click Reference 1 and choose Expand.
Size
1
In the Model Builder window, under Component 1 (comp1) > Meshes > Mesh 2 click Size.
2
In the Settings window for Size, locate the Element Size Parameters section.
3
In the Minimum element size text field, type 0.009*2.
Size 1
1
In the Model Builder window, click Size 1.
2
In the Settings window for Size, locate the Element Size Parameters section.
3
In the Minimum element size text field, type 0.004*2.
4
Click  Build All.
Mesh 3
In the Mesh toolbar, click Add Mesh and choose Add Mesh.
Reference 1
1
In the Mesh toolbar, click  Modify and choose Reference.
2
In the Settings window for Reference, locate the Reference section.
3
From the Mesh list, choose Mesh 2.
Scale 1
1
In the Mesh toolbar, click  More Attributes and choose Scale.
2
In the Settings window for Scale, locate the Scale section.
3
In the Element size scale text field, type 2.
Reference 1
In the Model Builder window, right-click Reference 1 and choose Expand.
Size 1
1
In the Settings window for Size, locate the Element Size Parameters section.
2
In the Minimum element size text field, type 0.004*4.
Size
1
In the Model Builder window, click Size.
2
In the Settings window for Size, locate the Element Size Parameters section.
3
In the Minimum element size text field, type 0.009*4.
4
Click  Build All.
Disable Deforming Domain in the frozen rotor study.
Study 1
Step 1: Frozen Rotor
1
In the Model Builder window, under Study 1 click Step 1: Frozen Rotor.
2
In the Settings window for Frozen Rotor, locate the Physics and Variables Selection section.
3
Select the Modify model configuration for study step checkbox.
4
In the tree, select Component 1 (comp1) > Moving Mesh, Controls spatial frame > Deforming Domain 1.
5
Click  Disable.
6
Click to expand the Mesh Selection section. In the table, enter the following settings:
Component
Mesh
Geometry 1
Mesh 1
7
Click to expand the Study Extensions section. Select the Auxiliary sweep checkbox.
8
Click  Add.
9
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
viscFact (Viscosity factor)
50 1
 
10
From the Run continuation for list, choose No parameter.
11
From the Reuse solution from previous step list, choose Yes.
12
Click the  Show More Options button in the Model Builder toolbar.
13
In the Show More Options dialog, in the tree, select the checkbox for the node Study > Multigrid Level.
14
Click OK.
15
Right-click Study 1 > Step 1: Frozen Rotor and choose Multigrid Level.
16
In the Settings window for Multigrid Level, locate the Mesh Selection section.
17
In the table, enter the following settings:
Component
Mesh
Geometry 1
Mesh 2
18
In the Model Builder window, right-click Step 1: Frozen Rotor and choose Multigrid Level.
Step 2: Stationary Free Surface
1
In the Settings window for Stationary Free Surface, locate the Physics and Variables Selection section.
2
Select the Modify model configuration for study step checkbox.
3
In the tree, select Component 1 (comp1) > Moving Mesh, Controls spatial frame > Deforming Domain 1.
4
Right-click and choose Disable.
5
Click to expand the Mesh Selection section. In the table, enter the following settings:
Component
Mesh
Geometry 1
Mesh 1
Solution 1 (sol1)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 1 (sol1) node.
3
In the Model Builder window, expand the Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 1 > Segregated 1 node.
4
In the Model Builder window, expand the Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 1 > AMG, fluid flow variables (spf_spatial1) node, then click Multigrid 1.
5
In the Settings window for Multigrid, locate the General section.
6
From the Hierarchy generation method list, choose Manual.
7
In the Study toolbar, click  Compute.
Results
Velocity (spf)
Before working with plots, disable the automatic update of plots. Due to the size of the datasets created, it is more convenient to generate plots actively.
1
In the Model Builder window, click Results.
2
In the Settings window for Results, locate the Update of Results section.
3
Select the Only plot when requested checkbox.
4
In the Model Builder window, click Velocity (spf).
5
In the Settings window for 3D Plot Group, locate the Plot Settings section.
6
Clear the Plot dataset edges checkbox.
Multislice 1
1
In the Model Builder window, expand the Velocity (spf) node.
2
Right-click Multislice 1 and choose Delete.
Surface 1
1
Right-click Velocity (spf) and choose Surface.
2
In the Settings window for Surface, locate the Coloring and Style section.
3
From the Color table list, choose WaveLight.
Selection 1
1
Right-click Surface 1 and choose Selection.
2
In the Settings window for Selection, locate the Selection section.
3
From the Selection list, choose Free Surface.
Deformation 1
1
In the Model Builder window, right-click Surface 1 and choose Deformation.
2
In the Settings window for Deformation, locate the Expression section.
3
In the x-component text field, type 0.
4
In the y-component text field, type 0.
5
In the z-component text field, type spf.etaFS.
6
Locate the Scale section. Select the Scale factor checkbox.
Arrow Volume 1
1
In the Model Builder window, right-click Velocity (spf) and choose Arrow Volume.
2
In the Settings window for Arrow Volume, locate the Arrow Positioning section.
3
Find the x grid points subsection. In the Points text field, type 30.
4
Find the y grid points subsection. In the Points text field, type 30.
5
Find the z grid points subsection. In the Points text field, type 3.
6
Locate the Coloring and Style section.
7
Select the Scale factor checkbox. In the associated text field, type 0.07.
Color Expression 1
1
Right-click Arrow Volume 1 and choose Color Expression.
2
In the Settings window for Color Expression, locate the Coloring and Style section.
3
From the Color table list, choose RainbowLight.
Surface 2
1
In the Model Builder window, right-click Velocity (spf) and choose Surface.
2
In the Settings window for Surface, locate the Coloring and Style section.
3
From the Coloring list, choose Uniform.
4
From the Color list, choose Gray.
5
Click to expand the Title section. From the Title type list, choose None.
Selection 1
1
Right-click Surface 2 and choose Selection.
2
In the Settings window for Selection, locate the Selection section.
3
From the Selection list, choose Walls.
4
In the list, choose 1 and 3.
5
Click  Remove from Selection.
6
Select Boundaries 2, 8–29, and 32–69 only.
7
In the Velocity (spf) toolbar, click  Plot.
Next, create a plot for the turbulent viscosity.
Turbulent Viscosity
1
In the Results toolbar, click  3D Plot Group.
2
In the Settings window for 3D Plot Group, type Turbulent Viscosity in the Label text field.
3
Locate the Plot Settings section. Clear the Plot dataset edges checkbox.
Multislice 1
1
In the Turbulent Viscosity toolbar, click  More Plots and choose Multislice.
2
In the Settings window for Multislice, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Turbulent Flow, k-ε > Turbulence variables > spf.muT - Turbulent dynamic viscosity - Pa·s.
3
Locate the Multiplane Data section. Find the x-planes subsection. In the Planes text field, type 0.
4
Find the z-planes subsection. In the Planes text field, type 3.
5
Locate the Coloring and Style section. From the Color table list, choose ConopiformisZero.
Surface 1
1
In the Model Builder window, right-click Turbulent Viscosity and choose Surface.
2
In the Settings window for Surface, locate the Coloring and Style section.
3
From the Coloring list, choose Uniform.
4
From the Color list, choose Gray.
5
Locate the Title section. From the Title type list, choose None.
Selection 1
1
Right-click Surface 1 and choose Selection.
2
In the Settings window for Selection, locate the Selection section.
3
From the Selection list, choose Walls.
4
In the list, choose 1 and 3.
5
Click  Remove from Selection.
6
Select Boundaries 2, 8–29, and 32–69 only.
7
In the Turbulent Viscosity toolbar, click  Plot.
Velocity xy
1
In the Results toolbar, click  3D Plot Group.
2
In the Settings window for 3D Plot Group, type Velocity xy in the Label text field.
3
Locate the Plot Settings section. Clear the Plot dataset edges checkbox.
Slice 1
1
Right-click Velocity xy and choose Slice.
2
In the Settings window for Slice, locate the Plane Data section.
3
From the Plane list, choose xy-planes.
4
In the Velocity xy toolbar, click  Plot.
Add Study
1
In the Home toolbar, click  Add Study to open the Add Study window.
2
Go to the Add Study window.
3
Find the Studies subsection. In the Select Study tree, select General Studies > Time Dependent.
4
Right-click and choose Add Study.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Study 2
Step 1: Time Dependent
1
In the Settings window for Time Dependent, locate the Study Settings section.
2
In the Output times text field, type range(0,0.05,1.8).
3
Click to expand the Values of Dependent Variables section. Find the Initial values of variables solved for subsection. From the Settings list, choose User controlled.
4
From the Method list, choose Solution.
5
From the Study list, choose Study 1, Stationary Free Surface.
6
From the Selection list, choose Last.
7
Click to expand the Mesh Selection section. In the table, enter the following settings:
Component
Mesh
Geometry 1
Mesh 1
8
In the Model Builder window, click Study 2.
9
In the Settings window for Study, locate the Study Settings section.
10
Clear the Generate default plots checkbox  because you can duplicate the previous plots and only need top update the dataset.
11
In the Study toolbar, click  Get Initial Value.
First, group the plots to make the results section clearer and easier to follow. Then, duplicate the group and assign the correct dataset. This way, during the time-dependent study, you can view the results while they are being computed.
Results
Pressure (spf), Turbulent Viscosity, Velocity (spf), Velocity xy, Wall Resolution (spf)
1
In the Model Builder window, under Results, Ctrl-click to select Velocity (spf), Pressure (spf), Wall Resolution (spf), Turbulent Viscosity, and Velocity xy.
2
Right-click and choose Group.
Frozen Rotor
In the Settings window for Group, type Frozen Rotor in the Label text field.
Time Dependent
1
Right-click Frozen Rotor and choose Duplicate.
2
In the Settings window for Group, type Time Dependent in the Label text field.
Velocity (spf) 1
1
In the Model Builder window, expand the Time Dependent node, then click Velocity (spf) 1.
2
In the Settings window for 3D Plot Group, locate the Data section.
3
From the Dataset list, choose Study 2/Solution 3 (sol3).
4
In the Model Builder window, expand the Velocity (spf) 1 node.
Deformation 1
1
In the Model Builder window, expand the Results > Time Dependent > Velocity (spf) 1 > Surface 1 node.
2
Right-click Deformation 1 and choose Delete.
Update the dataset for all remaining plots in this group.
Study 2
Step 1: Time Dependent
1
In the Model Builder window, under Study 2 click Step 1: Time Dependent.
2
In the Settings window for Time Dependent, click to expand the Results While Solving section.
3
Select the Plot checkbox.
4
In the table, enter the following settings:
Plot group
Plot window
Velocity (spf) 1
Graphics
Solver Configurations
In the Model Builder window, expand the Study 2 > Solver Configurations node.
Solution 3 (sol3)
1
In the Model Builder window, expand the Study 2 > Solver Configurations > Solution 3 (sol3) node.
2
In the Model Builder window, click Time-Dependent Solver 1.
3
In the Settings window for Time-Dependent Solver, click to expand the Time Stepping section.
4
From the Minimum BDF order list, choose 2.
The BDF order must be larger than 1 to accurately capture the surface movement.
5
In the Study toolbar, click  Compute.
Results
Velocity (spf) 1
1
In the Settings window for 3D Plot Group, locate the Data section.
2
From the Time (s) list, choose Last (1.8).
3
In the Velocity (spf) 1 toolbar, click  Plot.
Turbulent Viscosity 1
1
In the Model Builder window, click Turbulent Viscosity 1.
2
In the Settings window for 3D Plot Group, locate the Data section.
3
From the Time (s) list, choose Last (1.8).
4
In the Turbulent Viscosity 1 toolbar, click  Plot.
xz-Plane, Time Dependent
1
In the Results toolbar, click  Cut Plane.
2
In the Settings window for Cut Plane, type xz-Plane, Time Dependent in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study 2/Solution 3 (sol3).
4
Locate the Plane Data section. From the Plane list, choose xz-planes.
Velocity xz
1
In the Results toolbar, click  2D Plot Group.
2
In the Settings window for 2D Plot Group, type Velocity xz in the Label text field.
3
Locate the Plot Settings section. Clear the Plot dataset edges checkbox.
Surface 1
Right-click Velocity xz and choose Surface.
Arrow Surface 1
1
In the Model Builder window, right-click Velocity xz and choose Arrow Surface.
2
In the Settings window for Arrow Surface, locate the Arrow Positioning section.
3
Find the x grid points subsection. In the Points text field, type 20.
4
Find the y grid points subsection. In the Points text field, type 20.
5
Locate the Coloring and Style section.
6
Select the Scale factor checkbox. In the associated text field, type 0.1.
7
In the Velocity xz toolbar, click  Plot.