This tutorial includes:
In this tutorial you will learn about:
Solving and postprocessing a case where the geometry has been omitted on one side of a symmetry plane.
Using free-slip wall boundaries as a compromise between accurate flow modeling and computational grid size.
Accurately modeling the near-wall flow using Shear Stress Transport (SST) turbulence model.
Running the CFX-Solver in parallel (optional).
Creating vector plots in CFD-Post with uniform spacing between the vectors.
Creating a macro using power syntax in CFD-Post.
|
Component |
Feature |
Details |
|---|---|---|
|
CFX-Pre |
User Mode |
General mode |
|
Analysis Type |
Steady State | |
|
Fluid Type |
Constant Property Gas | |
|
Domain Type |
Single Domain | |
|
Turbulence Model |
Shear Stress Transport | |
|
Boundary Conditions |
Inlet (Subsonic) | |
|
Outlet (Subsonic) | ||
|
Symmetry Plane | ||
|
Wall: No-Slip | ||
|
Wall: Free-Slip | ||
|
Timestep |
Physical Time Scale | |
|
CFX-Solver Manager |
Parallel Processing | |
|
CFD-Post |
Plots |
Default Locators |
|
Outline Plot (Wireframe) | ||
|
Sampling Plane | ||
|
Streamline | ||
|
Vector | ||
|
Volume | ||
|
Other |
Changing the Color Range | |
|
Instancing Transformation | ||
|
Lighting Adjustment | ||
|
Symmetry | ||
|
Viewing the Mesh |
In this tutorial, a generic vehicle body is placed into an oncoming side wind of 15 m/s. The turbulence will be set to Intensity and Length scale with a value of 0.05, which corresponds to 5% turbulence, a medium level intensity, and with an Eddy Length scale value of 0.1 m.
The goal of this tutorial is to set up, simulate, and then visualize the flow around the body. Since both the geometry and the flow are symmetric about a vertical plane, you will only use half of the geometry to find the solution. You will use free-slip wall boundaries on some sides of the domain to model external flow. The flow near the body is modeled using Shear Stress Transport. Since compressibility effects are not expected to be significant, you can model this as incompressible flow.
If this is the first tutorial you are working with, it is important to review the following topics before beginning:
Create a working directory.
Ansys CFX uses a working directory as the default location for loading and saving files for a particular session or project.
Download the
blunt_body.zipfile here .Unzip
blunt_body.zipto your working directory.Ensure that the following tutorial input file is in your working directory:
BluntBodyMesh.gtm
Set the working directory and start CFX-Pre.
For details, see Setting the Working Directory and Starting Ansys CFX in Stand-alone Mode.
In CFX-Pre, select File > New Case.
Select General and click .
Select File > Save Case As.
Under File name, type
BluntBody.Click .
Right-click
Meshand select Import Mesh > CFX Mesh.The Import Mesh dialog box appears.
Configure the following setting(s):
Setting
Value
File name
BluntBodyMesh.gtm
Click Open.
The flow of air in the domain is expected to be turbulent. The Shear Stress Transport (SST) turbulence model with automatic wall function treatment will be used because of its highly accurate predictions of flow separation. To take advantage of the SST model, the boundary layer should be resolved with at least 10 mesh nodes. In order to reduce computational time, the mesh in this tutorial is much coarser than that.
As stated in the overview, this tutorial models incompressible
flow. Incompressible flow is specified by choosing an incompressible
fluid. You will use Air at 25 C as the incompressible
fluid.
As part of the domain settings, you will specify a reference pressure. CFX requires this when modeling incompressible flow.
Click Domain
,
and set the name to BluntBody.Configure the following setting(s) of
BluntBody:Tab
Setting
Value
Basic Settings
Location and Type
> Location
B1.P3
Fluid and Particle Definitions
Fluid 1
Fluid and Particle Definitions
> Fluid 1
> Material
Air at 25 C [ a ]
Domain Models
> Pressure
> Reference Pressure
1 [atm]
Fluid Models
Heat Transfer
> Option
None
Turbulence
> Option
Shear Stress Transport
Click .
An imported mesh may contain many 2D regions. For the purpose of creating boundary conditions, it can sometimes be useful to group several 2D regions together and apply a single boundary to the composite 2D region. In this case, you are going to create a Union between two regions that both require a free-slip wall boundary.
From the main menu, select Insert > Regions > Composite Region.
Set the name to
FreeWallsand click .Configure the following setting(s):
Tab
Setting
Value
Basic Settings
Dimension (Filter)
2D
Click
beside the Region List dialog
box, to display the Selection Dialog. Hold down
the Ctrl key and select Free1andFree2.Click to confirm your selection.
Click to create the composite region.
The simulation requires inlet, outlet, wall (no slip and free-slip) and symmetry plane boundaries. The regions for these boundaries were defined when the mesh was created (except for the composite region just created for the free-slip wall boundary).
Click Boundary
.Under Name, type
Inlet.Configure the following setting(s):
Tab
Setting
Value
Basic Settings
Boundary Type
Inlet
Location
Inlet
Boundary Details
Flow Regime
> Option
Subsonic
Mass and Momentum
> Option
Normal Speed
Mass and Momentum
> Normal Speed
15 [m s^-1]
Turbulence
> Option
Intensity and Length Scale
Turbulence
> Fractional Intensity
0.05 [ a ]
Turbulence
> Eddy Length Scale
0.1 [m] [ a ]
Click .
Create a new boundary named
Outlet.Configure the following setting(s):
Tab
Setting
Value
Basic Settings
Boundary Type
Outlet
Location
Outlet
Boundary Details
Mass and Momentum
> Option
Static Pressure
Mass and Momentum
> Relative Pressure
0 [Pa]
Click .
The top and side surfaces of the rectangular region will use free-slip wall boundaries.
On free-slip walls the shear stress is set to zero so that the fluid is not retarded.
The velocity normal to the wall is also set to zero.
The velocity parallel to the wall is calculated during the solution.
This boundary is an approximation that may not accurately represent the true flow conditions. By using a free-slip wall boundary, the flow modeling will be less accurate but the computational grid size can be reduced by modeling less of the surroundings. If this case were modeling a wind tunnel experiment, the geometry would match the size and shape of the wind tunnel and use no-slip walls. If this case were modeling a blunt body open to the atmosphere, a much larger domain would be used to minimize the effect of the far-field boundary, and the far-field boundary type would be set to either a free-slip wall or a pressure-specified entrainment opening.
You will apply a single boundary to both walls by using the composite region defined earlier.
Create a new boundary named
FreeWalls.Configure the following setting(s):
Tab
Setting
Value
Basic Settings
Boundary Type
Wall
Location
FreeWalls
Boundary Details
Mass and Momentum
> Option
Free Slip Wall
Click .
Create a new boundary named
SymP.Configure the following setting(s):
Tab
Setting
Value
Basic Settings
Boundary Type
Symmetry
Location
SymP
Click .
Create a new boundary named
Body.Configure the following setting(s):
Tab
Setting
Value
Basic Settings
Boundary Type
Wall
Location
Body
Boundary Details
Mass and Momentum
> Option
No Slip Wall
Click .
The remaining 2D regions (in this case, just the low Z face) will be assigned the default boundary which is an adiabatic, no-slip wall condition. In this case, the name of the default boundary is BluntBody Default. Although the boundaries Body and BluntBody Default are identical (except for their locations), the Body boundary was created so that, during postprocessing, its location can be conveniently distinguished from the other adiabatic, no-slip wall surfaces.
The initial conditions are consistent with inlet boundaries.
Click Global Initialization
.Configure the following setting(s):
Tab
Setting
Value
Global Settings
Initial Conditions
> Cartesian Velocity Components
> Option
Automatic with Value
Initial Conditions
> Cartesian Velocity Components
> U
15 [m s^-1]
Initial Conditions
> Cartesian Velocity Components
> V
0 [m s^-1]
Initial Conditions
> Cartesian Velocity Components
> W
0 [m s^-1]
Click .
Click Solver Control
.Configure the following setting(s):
Tab
Setting
Value
Basic Settings
Convergence Control
> Max. Iterations
60
Convergence Control
> Fluid Timescale Control
> Timescale Control
Physical Timescale
Convergence Control
> Fluid Timescale Control
> Physical Timescale
2 [s][ a ]
Convergence Criteria
> Residual Target
1e-05
Click .
Click Define Run
.Configure the following setting(s):
Setting
Value
File name
BluntBody.def
Click .
CFX-Solver Manager automatically starts and, on the Define Run dialog box, Solver Input File is set.
If using stand-alone mode, quit CFX-Pre, saving the simulation (
.cfx) file at your discretion.
This tutorial introduces the parallel solver capabilities of CFX.
Note: The results produced will be identical, whether produced by a parallel or serial run.
If you do not want to solve this tutorial in parallel (on more than one processor) or you do not have a license to run the CFX-Solver in parallel, proceed to Obtaining a Solution in Serial.
If you do not know if you have a license to run the CFX-Solver in parallel, you should either ask your system administrator, or query the license server (see the Ansys, Inc. Licensing Guide (which is installed with the Ansys License Manager) for details). Alternatively proceed to Obtaining a Solution in Serial.
If you would like to solve this tutorial in parallel on the same machine, proceed to Obtaining a Solution with Local Parallel.
If you would like to solve this tutorial in parallel across different machines, proceed to Obtaining a Solution with Distributed Parallel.
When CFX-Solver Manager has started, you can obtain a solution to the CFD problem by using the following procedure.
Click Start Run.
When CFX-Solver is finished, select the check box next to Post-Process Results.
If using stand-alone mode, select the check box next to Shut down CFX-Solver Manager.
Click . Continue this tutorial from Viewing the Results Using CFD-Post.
Using the parallel capability of the CFX-Solver enables you to divide a large CFD problem so that it can run on more than one processor/machine at once. This saves time and, when multiple machines are used, avoids problems that arise when a CFD calculation requires more memory than a single machine has available. The partition (division) of the CFD problem is automatic.
A number of events occur when you set up a parallel run and then ask the CFX-Solver to calculate the solution:
Your mesh will be divided into a number of partitions.
The CFX-Solver runs separately on each of the partitions on the selected machine(s).
The results that one CFX-Solver process calculates affects the other CFX-Solver processes at the interface between the different sections of the mesh.
All of the CFX-Solver processes are required to communicate with each other and this is handled by the leader process.
The leader process always runs on the machine that you are logged into when the parallel run starts. The other CFX-Solver processes are follower processes and may be run on other machines.
After the problem has been solved, a single results file is written. It will be identical to a results file from the same problem run as a serial process, with one exception: an extra variable
Real partition numberwill be available for the parallel run. This variable will be used later in this tutorial during post processing.
In CFX-Solver Manager, the Define Run dialog box should already be open.
To run in local parallel mode:
Leave Type of Run set to
Full.If Type of Run was instead set to
Partitioner Only, your mesh would be split into a number of partitions but would not be run in the CFX-Solver afterwards.Set Run Mode to a parallel mode suitable for your configuration; for example,
Intel MPI Local Parallel.This is the recommended method for most applications.
If required, click Add Process
to increase the maximum number of processes.Ideally, the number of processes should not exceed the number of available processor cores. The number of processes used will be the number of partitions for the mesh.
Select Show Advanced Controls.
Click the Partitioner tab at the top of the dialog box.
Use the default
MeTiSpartitioner.Your model will be divided into a number of sections, with each section running in its own CFX-Solver process. The default is the
MeTiSpartitioner because it produces more efficient partitions than eitherRecursive Coordinate BisectionorUser Specified Direction.Click Start Run.
When CFX-Solver is finished, select the check box next to Post-Process Results.
If using stand-alone mode, select the check box next to Shut down CFX-Solver Manager.
Click .
Continue this tutorial from Text Output when Running in Parallel.
Before running in Distributed Parallel mode, ensure that your system has been configured as described in the installation documentation.
In CFX-Solver Manager, the Define Run dialog box should already be open.
Leave Type of Run set to
Full.If Type of Run was instead set to
Partitioner Only, your mesh would be split into a number of partitions but would not be run in the CFX-Solver afterwards.Set Run Mode to a parallel mode suitable for your environment; for example,
Intel MPI Distributed Parallel.The name of the machine that you are currently logged into should be in the Host Name list. You are going to run with two partitions on two different machines, so another machine must be added.
Click Insert Host
to specify a new host machine.The Select Parallel Hosts dialog box is displayed. This is where you choose additional machines to run your processes.
Your system administrator should have set up a hosts file containing a list of the machines that are available to run the parallel CFX-Solver.
The Host Name column displays names of available hosts.
The second column shows the number of processors on that machine.
The third shows the relative processor speed: a processor on a machine with a relative speed of 1 would typically be twice as fast as a machine with a relative speed of 0.5.
The last column displays operating system information.
This information is read from the hosts file; if any information is missing or incorrect your system administrator should correct the hosts file.
Note: The # processors, relative speed and system information does not have to be specified to be able to run on a host.
Select the name of another machine in the Host Name list.
Select a machine that you can log into.
Click Add.
The name of the machine is added to the Host Name column.
Note: Ensure that the machine that you are currently logged into is in the Hosts Name list in the Define Run dialog box.
Close the Select Parallel Hosts dialog box.
Select Show Advanced Controls.
Click the Partitioner tab at the top of the dialog box.
Use the default
MeTiSpartitioner.Your model will be divided into two sections, with each section running in its own CFX-Solver process. The default is the
MeTiSpartitioner because it produces more efficient partitions than eitherRecursive Coordinate BisectionorUser Specified Direction.Click Start Run to begin the parallel run.
Click on the dialog box.
When CFX-Solver is finished, select the check box next to Post-Process Results.
If using stand-alone mode, select the check box next to Shut down CFX-Solver Manager.
Click .
The text output area shows what is being written to the CFX-Solver Output file. You will see information similar to the following:
+--------------------------------------------------------------------+ | Job Information at Start of Run | +--------------------------------------------------------------------+ Run mode: partitioning run +------------------------------+------+--------+----------+----------+ | Host | Mesh | PID | Job Started | | | Part | | DD/MM/YY | hh:mm:ss | +------------------------------+------+--------+----------+----------+ | fastmachine1 | 1 | 5952 | 19/02/13 | 10:50:09 | +------------------------------+------+--------+----------+----------+
This tells you that the information following is concerned with the partitioning. After the partitioning job has finished, you will find:
+--------------------------------------------------------------------+
| Partitioning Information |
+--------------------------------------------------------------------+
Partitioning information for domain: BluntBody
+------------------+------------------------+-----------------+
| Elements | Vertices | Faces |
+------+------------------+------------------------+-----------------+
| Part | Number % | Number % %Ovlp | Number % |
+------+------------------+------------------------+-----------------+
| Full | 131878 | 37048 | 11318 |
+------+------------------+------------------------+-----------------+
| 1 | 67873 50.4 | 19431 50.4 4.0 | 5705 49.5 |
| 2 | 66865 49.6 | 19151 49.6 4.0 | 5820 50.5 |
+------+------------------+------------------------+-----------------+
| Sum | 134738 100.0 | 38582 100.0 4.0 | 11525 100.0 |
+------+------------------+------------------------+-----------------+
+--------------------------------------------------------------------+
| Partitioning CPU-Time Requirements |
+--------------------------------------------------------------------+
- Preparations 3.689E-01 seconds
- Low-level mesh partitioning 5.599E-02 seconds
- Global partitioning information 9.998E-03 seconds
- Element and face partitioning information 7.999E-03 seconds
- Vertex partitioning information 0.000E+00 seconds
- Partitioning information compression 0.000E+00 seconds
- Summed CPU-time for mesh partitioning 4.609E-01 seconds
+--------------------------------------------------------------------+
| Job Information at End of Run |
+--------------------------------------------------------------------+
+---------------------------+------+----------+----------+-----------+
| Host | Mesh | Job Finished | CPU |
| | Part | DD/MM/YY | hh:mm:ss | seconds |
+---------------------------+------+----------+----------+-----------+
| fastmachine1 | 1 | 19/02/13 | 10:50:09 | 8.020E-01 |
+---------------------------+------+----------+----------+-----------+
Total wall clock time: 7.990E-01 seconds
or: ( 0: 0: 0: 0.799 )
( Days: Hours: Minutes: Seconds )This marks the end of the partitioning job. The CFX-Solver now begins to solve your parallel run:
+--------------------------------------------------------------------+ | Job Information at Start of Run | +--------------------------------------------------------------------+ Run mode: parallel run (Intel MPI) +------------------------------+------+--------+----------+----------+ | Host | Mesh | PID | Job Started | | | Part | | DD/MM/YY | hh:mm:ss | +------------------------------+------+--------+----------+----------+ | fastmchine1 | 1 | 6044 | 19/02/13 | 10:50:11 | | | 2 | 3276 | 19/02/13 | 10:50:11 | +------------------------------+------+--------+----------+----------+
The machine that you are logged into runs the leader process, and controls the overall simulation. The second machine selected will run the follower process. If you had more than two processes, each additional process is run as a follower process.
The leader process in this example is running on the mesh partition number 1 and the follower is running on partition number 2. You can find out which nodes and elements are in each partition by using CFD-Post later on in the tutorial.
When the CFX-Solver finishes, the CFX-Solver Output file displays the job information and a dialog box to indicate completion of the run.
In CFD-Post, you will:
Create an instance transform object to recreate the full geometry
Create a vector plot that shows how the flow behaves around the body
Create a pressure plot that shows the pressure distribution on the body
Make a surface streamline that shows the path of air along the surface of the body
Examine the values of the dimensionless wall distance
to make sure that the mesh is sufficiently fine
near the walls
Earlier in this tutorial you used a symmetry plane boundary because the entire blunt body is symmetrical about a plane. Due to this symmetry, it was necessary to use only half of the full geometry to calculate the CFD results. However, for visualization purposes, it is helpful to use the full blunt body. CFD-Post is able to recreate the full data set from the half that was originally calculated. This is done by creating an Instance Transform object.
You need to manipulate the geometry so that you will be able to see what happens when you use the symmetry plane. The CFD-Post features that you have used in earlier tutorials will not be described in detail. New features will be described in detail.
Right-click a blank area in the viewer and select Predefined Camera > View From +X.
Instance Transforms are used to visualize a full geometry representation in cases where the simulation took advantage of symmetry to solve for only part of the geometry. There are three types of transforms that you can use: Rotation, Translation, Reflection/Mirroring. In this tutorial, you will create a Reflection transform located on a plane.
Click Location > Plane and set the name to
Reflection Plane.Configure the following setting(s):
Tab
Setting
Value
Geometry
Definition
> Method
ZX Plane
Definition
> Y
0.0 [m]
Render
Show Faces
(cleared)
Click .
This creates a plane at y=0, the same location as the symmetry plane defined in CFX-Pre. Now the instance transform can be created using this plane:
From the main menu, select Insert > Instance Transform and accept the default name.
Configure the following setting(s):
Tab
Setting
Value
Definition
Instancing Info From Domain
(Cleared)
Apply Rotation
(Cleared)
Apply Reflection
(Selected)
Apply Reflection
> Plane
Reflection Plane
Click .
You can apply the new transform to graphics objects. For example, you can modify the display of the wireframe as follows:
Under the Outline tab, in
User Locations and Plots, configure the following setting(s) ofWireframe:Tab
Setting
Value
View
Apply Instancing Transform
> Transform
Instance Transform 1
Click .
Zoom so that the geometry fills the Viewer.
You will see the full blunt body.
In this case, you created a new instance transform and applied it to the wireframe. This caused only the wireframe object to be mirrored. If you had modified the default transform instead of creating a new one, then all graphics (including those not yet made) would be mirrored by default.
You are now going to create a vector plot to show velocity vectors behind the blunt body. You need to first create an object to act as a locator, which, in this case, will be a sampling plane. Then, create the vector plot itself.
A sampling plane is a plane with evenly spaced sampling points on it.
Right-click a blank area in the viewer and select Predefined Camera > View From +Y.
This ensures that the changes can be seen.
Create a new plane named
Sample.Configure the following setting(s) to create a sampling plane that is parallel to the ZX plane and located at x= 6 m, y= 0.001 m and z= 1 m relative to blunt object:
Tab
Setting
Value
Geometry
Definition
> Method
Point and Normal
Definition
> Point
6, -0.001, 1
Definition
> Normal
0, 1, 0
Plane Bounds
> Type
Rectangular
Plane Bounds
> X Size
2.5 [m]
Plane Bounds
> Y Size
2.5 [m]
Plane Type
Sample
Plane Type
> X Samples
20
Plane Type
> Y Samples
20
Render
Show Faces
(Cleared)
Show Mesh Lines
(Selected)
Click .
You can zoom in on the sampling plane to see the location of the sampling points (where lines intersect). There are a total of 400 (20 * 20) sampling points on the plane. A vector can be created at each sampling point.
Turn off the visibility of
Sample.
Click Vector
and accept the default name.Configure the following setting(s):
Tab
Setting
Value
Geometry
Definition
> Locations
Sample
Definition
> Sampling
Vertex
Symbol
Symbol Size
0.25
Click .
Zoom until the vector plot is roughly the same size as the viewer.
You should be able to see a region of recirculation behind the blunt body.
Ignore the vertices on the sampling plane and increase the density of the vectors by applying the following settings:
Tab
Setting
Value
Geometry
Definition
> Sampling
Equally Spaced
Definition
> # of Points
1000
Click .
Change the location of the Vector plot by applying the following setting:
Tab
Setting
Value
Geometry
Definition
> Locations
SymP
Click .
Configure the following setting(s) of the boundary named
Body:Tab
Setting
Value
Color
Mode
Variable
Variable
Pressure
View
Apply Instancing Transform
> Transform
Instance Transform 1
Click .
Configure the following setting(s) of
SymP:Tab
Setting
Value
Render
Show Faces
(Cleared)
Show Mesh Lines
(Selected)
Click .
You will be able to see the mesh around the blunt body, with the mesh length scale decreasing near the body, but still coarse in the region of recirculation. By zooming in, you will be able to see the layers of inflated elements near the body.
In order to show the path of air along the surface of the blunt body, surface streamlines can be made as follows:
Turn off the visibility of
Body,SymPandVector 1.Create a new plane named
Starter.Configure the following setting(s):
Tab
Setting
Value
Geometry
Definition
> Method
YZ Plane
X
-0.1 [m]
Click .
Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up).
The plane appears just upstream of the blunt body.
Turn off the visibility of the plane.
This hides the plane from view, although the plane still exists.
Click Streamline
and click to accept
the default name.Configure the following setting(s):
Tab
Setting
Value
Geometry
Type
Surface Streamline
Definition
> Surfaces
Body
Definition
> Start From
Locations
Definition
> Locations
Starter
Definition
> Max Points
100
Definition
> Direction
Forward
Click .
The surface streamlines appear on half of the surface of the blunt body. They start near the upstream end because the starting points were formed by projecting nodes from the plane to the blunt body.
In CFD-Post, you can reposition some locator objects directly in the viewer by using the mouse.
Turn on the visibility of the plane named
Starter.Select the
Single Select mouse pointer
from the Selection Tools toolbar.In the viewer, click the
Starterplane to select it, then drag it along the X axis.Notice that the streamlines are redrawn as the plane moves. The rate at which the streamlines are redrawn is dependent on your computer's speed. If the streamlines are updated infrequently, you may find it useful to move the mouse very slowly.
The velocity next to a no-slip wall boundary changes rapidly from a value of zero at the wall to the free stream value a short distance away from the wall. This layer of high velocity gradient is known as the boundary layer. Many meshes are not fine enough near a wall to accurately resolve the velocity profile in the boundary layer. Wall functions can be used in these cases to apply an assumed functional shape of the velocity profile. Other grids are fine enough that they do not require wall functions, and application of the latter has little effect. The majority of cases fall somewhere in between these two extremes, where the boundary layer is partially resolved by nodes near the wall and wall functions are used to supplement accuracy where the nodes are not sufficiently clustered near the wall.
One indicator of the closeness of the first node to the wall
is the dimensionless wall distance 
. It is good practice to examine the values of 
at the end of your simulation. At the lower limit,
a value of 
less than
or equal to 11 indicates that the first node is within the laminar
sublayer of the boundary flow. Values larger than this indicate that
an assumed logarithmic shape of the velocity profile is being used
to model the boundary layer portion between the wall and the first
node. Ideally you should confirm that there are several nodes (3 or
more) resolving the boundary layer profile. If this is not observed,
it is highly recommended that more nodes be added near the wall surfaces
in order to improve simulation accuracy. In this tutorial, a coarse
mesh is used to reduce the run time. Thus, the grid is far too coarse
to resolve any of the boundary layer profile, and the solution is
not highly accurate.
A surface plot is one which colors a surface according to the
values of a variable: in this case, 
. A surface plot of 
can be obtained as follows:
Turn off the visibility of all previous plots.
Under the Outline tab, configure the following settings of
BluntBodyDefault:Tab
Setting
Value
Color
Mode
Variable
Variable
Yplus [ a ]
View
Apply Instancing Transform
> Transform
Instance Transform 1
Click .
Under the Outline tab, configure the following settings of
Body:Tab
Setting
Value
Color
Mode
Variable
Variable
Yplus
View
Apply Instancing Transform
> Transform
Instance Transform 1
Click .
If you solved this tutorial in parallel, then an additional
variable named Real partition number will be
available in CFD-Post
Create an isosurface of
Real partition numberequal to1.Create a second isosurface of
Real partition numberequal to1.999.
The two isosurfaces show the edges of the two partitions. The gap between the two plots shows the overlap nodes. These were contained in both partitions 1 and 2.
When you have finished looking at the results, quit CFD-Post.