The following picture demonstrates what should be visible after importing the tutorial project.
1.2. CAD Mode
The first step for this simulation is the creation of an enclosure. This will be the domain that will be used for the external CFD analysis. To enter the CAD mode click on the following icon:
Select ‘Create flow volume’, at the top right of the page:
The ‘External’ option that is listed on the drop down menu is used to create the flow domain around the model:
Then fill in the dimensions of the domain, like below, where L is the diameter of the golf ball:
In more details, the size of the domain is as following. After you apply the dimensions, click on ‘Seed face’, and proceed to select a face of the ball that is inside the domain:
After you are done, click ‘Apply‘. Then select the ‘Delete’ feature next to the Body section, to remove the whole solid part:
Select the solid body from the scene tree on the right and click ‘Apply’:
When the operation is finished and the ball is removed successfully, click on the ‘Finish’ option at the top right so you get redirected to the Workbench:
When the Workbench loads, another geometry appears, which is the copy created from the original model, after the CAD mode operations. You can delete the initial version:
Then rename the new version as ‘Golf ball’:
1.3. Create Topological Entities
Create a topological entity set for the golf ball:
Hide the walls of the Enclosure by selecting each one of them on the Workbench, then right-click and choose the ‘Hide selection’ option.
Activate the box selection at the top of the page.
Drag it across the model until all the faces are selected.
Click on the ‘+’ next to the Topological Entity Sets.
Name your new set and click on the checkmark.
1.4. Create the Simulation
After you finish with the topological entity set, proceed to click the ‘Create simulation‘ option to get started.
Select the ‘Compressible‘ analysis, which is used for cases where the Mach number in any point of the domain reaches a value bigger than 0.3. This golf ball simulation will be using a high velocity, so the compressible analysis is the best fitting.
Switch the Turbulence model to ‘k-omega SST‘ in the panel that appears:
2. Assigning the Material and Boundary Conditions
Now we will set up the physics for the simulation.
2.1. Define a Material
In this simulation, we want to analyze the airflow around a solid body. Therefore we need to assign properties to the fluid region. Click on the ‘+’ icon next to the Materials option of the simulation tree on the left of the page, and then choose ‘Air‘ in the panel that pops up, and apply:
The flow region that was created due to the Geometry operation at the beginning of the simulation is automatically selected for the material.
Just confirm the selection by hitting the check button next to the material’s name. You can also create a custom fluid by changing the properties and the materials name.
2.2. Assign the Boundary Conditions
In order to assign Boundary Conditions on the golf ball, click on the ‘+’ icon next to the BoundaryConditions, and click on the types described in this section.
In order to have an overview, the following picture shows the boundary conditions applied for this simulation:
a. Velocity Inlet
Assign a ‘Velocity Inlet‘ of 59 \(m/s\). This is close to the average Ball Speed an average male golf player achieves.
b. Pressure Outlet
Assign a ‘Pressure Outlet‘ condition of 101325 (Pa) at the highlighted face below:
c. Slip Walls
Add a Slip Wall boundary condition on the top, bottom, and right face of the domain. Leave only the symmetry plane unassigned.
Assign a Symmetry condition on the symmetry plane. If you want to learn more about this boundary condition, click here.
e. Rotating Walls
Did you know?
The golf ball rotates like the following photo, so the negative z direction is chosen for the rotation axis, in regards to the coordinate system of the CAD model.
We will define the condition according to the spin rate of an average male golf player. Create a new ‘wall’ boundary condition:
Select ‘Rotating wall’ for (U) velocity.
Set the Turbulence wall to ‘full resolution’.
The spin rate of an average male golf player (rotational velocity) is 343 \(rad \over \ s \) .
According to the coordinate system, we need to orientate it on the negative z-direction.
Assign it to the topological entity set of the golf ball by clicking on it as you can see below:
2.3. Simulation Control & Numerics
Fill the simulation control panel in like below:
Leave the Numerics panel at its’ default state.
Access the global mesh settings by clicking on ‘mesh’ in the simulation tree:
Choose the ‘Standard‘ algorithm, and keep the default settings.
3.1. Meshing Refinements
This project needs some refinements. If you want to learn more about using the Standard meshing tool, and using refinements, click on this.
a. Create Geometry Primitives
Prior to adding refinements, you must create some Geometry Primitives sets.
Click on the ‘+’icon under the Geometry Primitives at the right of the screen.
Choose the ‘Sphere‘ option.
Name your entities, and define its’ center and 0.1 (m) radius.
Create a second Sphere with a smaller radius (0.05 (m)):
b. Assign Region Refinements to the Spheres
In order to add refinement regions, click on the under theMesh:
Add a region refinement to the first sphere:
And one more fine region refinement to the smaller sphere, to create a more dense mesh there:
Do not click on the ‘Generate’ button after you are done with the mesh settings, otherwise the physics of the simulation will not be taken into consideration during the meshing procedure. Instead of generating it at this point, your mesh will be automatically created after you start a new run later on.
4. Start the Simulation
After all the settings are completed, proceed to clicking the ‘+’ icon next to the Simulation Runs, in order to get started with the analysis. Initially, your mesh will be generated, and then the program will go on with the run.
While the results are being calculated you can already have a look at the intermediate results in the post-processor.
Did you know?
Your results are being updated in real time! That means that you can already look into the intermediate results during the solver calculates the simulation.
5.1. Convergence Plot
When the simulation is completed, you can check the convergence of the simulation. You can access them under the completed run:
The convergence plot indicates whether the solution is reliable, or whether some changes should be made in the settings, like making the mesh finer, or increasing the simulation time. In the following picture you can see how the residuals of your simulations will appear in the plot if you set the end time to 2000 seconds and let it fully converge:
5.2 Surface Visualization
In order to view the results of your golf ball simulation, click on the ‘Solution Fields’ tab under your finished run. This will redirect you to the post-processor.
You can use several post-processing filters to further analyze the results. If you wish to see the pressure distribution on your golf ball :
Make sure the post-processor shows the results for the final timestep – 2000 \(sec\)-;
Go to the Parts Color and choose ‘Pressure’ from the Coloring drop-down menu. When entering the post-processor, the whole model may be colored with this parameter at default. Feel free to change the parameter if you wish;
Click on the faces of the enclosure, then right-click on the Workbench, and choose the ‘Hide selection’ option:
Make sure to right-click on the color scale at the bottom of the screen and select the ‘Use continuous scale option’, for smoother transition between color contours:
This is how the results will appear afterwards if you include the symmetry plane too:
It is seen that at the front of the ball, an area of high pressure is created, and a low-pressure region is observed at the back. As the velocity is decelerating when reaching the back of the ball, there is flow separation, resulting in this low-pressure area.
Finally, for streamline visualization:
Click on the ‘Add Filter’ option;
Select ‘Particle Trace’.
Click on the circle icon next to the Pick Position;
Apply the seed point on the inlet face, as close to the symmetry face and the center of the y-axis as possible;
The # Seeds horizontally represents the number of streamline rows along the z-axis. Set it to ‘2’. The # Seeds vertically represents the number of rows along the y-axis. Make sure it is big enough that it covers the whole y dimension of the domain. An input of ‘100′ should be fine for this case;
Select ‘Velocity’ as Coloring;
For this case, you can have the Trace both directions option disabled, as the flow here travels from the inlet only towards the positive x-direction.
With these settings, this is how the streamlines will finally appear:
In Figure 39, the behavior of the flow can be observed. The decrease in velocity is obvious in the downstream, where low pressure was previously noticed (Figure 36). Towards the end of the domain, the streamlines gradually tend to become parallel again, reaching ambient conditions.
Animations can be started by choosing ‘Animation’ from the Filters panel:
Click the play button to start the animation. Below is an example of animating the streamlines , colored with the velocity magnitude, during the final timestep:
For more information, have a look at our post-processing guide to learn how to use the post-processor. Congratulations! You finished the tutorial!
Strictly Necessary Cookies
Strictly Necessary Cookie should be enabled at all times so that we can save your preferences for cookie settings.
If you disable this cookie, we will not be able to save your preferences. This means that every time you visit this website you will need to enable or disable cookies again.