Welcome to this Ansys How To Series video.
In this lesson, we will learn how to use the Fluent Meshing Watertight workflow to mesh
the Formula SAE car geometry.
We will first understand how to create a surface mesh on the car, and then learn to setup prism
layers around the car.
Finally, we will create a poly-hexcore volume mesh.
Are you interested?
Let’s go!
The modeling objective of our simulation is to analyze an external flow around the Formula
SAE car.
To solve this turbulent flow problem using Ansys Fluent, we will create a computational
mesh using the Fluent meshing watertight workflow.
Before launching the Fluent meshing session, in the Workbench window, right-click on the
‘mesh’ cell, go to properties, and make sure ‘Use workflow’ is selected and the
‘Workflow type’ is set to Watertight geometry as shown.
Since the geometry was created in ‘mm’, ensure that ‘units’ is set to ‘mm’.
Double-click the “mesh” cell to launch Fluent Meshing.
Poly-hexcore meshing is parallelized allowing you to create a mesh faster on multiple cores.
To enable this, insert the number of physical cores as needed in the Meshing Processes box
in the Fluent meshing launcher.
Ensure that Double-Precision is checked in the launcher.
Once Fluent Meshing is launched, in the first step, import the linked geometry.
Once the geometry has been successfully imported, enable local sizing.
Here, we will first add a “body of influence” sizing to the geometry.
When air flows over the car, a turbulent wake is generated behind the car body.
In this wake region, the variation of flow properties such as pressure and velocity are
sharp, and a refined mesh is required to capture these gradients as well as the dynamic nature
of turbulence.
The body of influence sizing will help create a local volumetric mesh refinement.
To create a BOI, choose the body of influence under the size control type and select ‘boi-nearfield’
from zone labels.
Assign a value of 16 millimeters as target mesh size.
Name this local sizing as boi-nearfield and add the local sizing.
Note that the mesh sizes are chosen such that the larger wake features are accurately captured.
If resolution of the smaller features is also required, very fine cell sizes should be used,
which can dramatically increase the overall grid size.
Next, we will add curvature local sizing to some specific parts.
Using the curvature setting, we will be able to accurately resolve the curved features
of the geometry.
This will allow areas of high curvature like the leading edge of the rear wing as well
as the front and rear wheel suspensions to be accurately captured.
Add curvature local sizing by picking curvature under the size control type.
Pick both rear and front wings from the zone labels and assign 0.5 millimeters as the local
min size and 12 millimeters as the max size.
Name this local sizing ‘curvature-wing’ and click add.
Similarly, we can add more curvature local sizing tasks for rods, wheels, chassis, brakes
and the wheelradii parts, and a BOI local sizing task for the boi-farfield zone.
The settings for these local sizings are shown here.
We are now ready to create the surface mesh.
In the ‘Generate the Surface Mesh’ task, enter 0.5 mm as the minimum size and 256 millimeters
as the maximum sizing.
Enter three cells per gap to resolve small gaps and to obtain a good-quality volume mesh.
Leave the rest of the settings to default.
These settings will dictate the global parameters.
Once the surface mesh is created, insert a clipping plane, and inspect the surface mesh.
The settings we used captured all the features accurately.
If your geometry is different, additional local sizing may be required.
Next, we need to prepare the geometry to create the volume mesh.
Since this geometry has only fluid regions, select the appropriate setting from the ‘Describe
Geometry’ task and leave the rest of the settings to default.
Next, we will assign the boundary conditions to the different boundary faces in the Update
Boundaries task.
Based on the named selections employed during the geometry creation in Lesson 1, Fluent
meshing tries to automatically assign the appropriate boundary conditions to the different
faces.
Make sure that the correct boundary conditions are assigned and select ‘Update Boundaries’.
In the ‘Update Regions’ task, ensure that the cell zone is set to the fluid region type.
In the next step, we will define settings for creating boundary layer mesh.
Because we are modeling viscous flow around the car, it is important to create a good
mesh in the near wall region to capture the effect of boundary layer that forms along
the walls.
The thickness of the boundary layer is generally very small compared to the characteristic
dimensions of the car and as a result, a refined mesh is required to accurately capture the
flow physics in these thin regions.
In the ‘Add Boundary Layers’ task, select ‘yes’ for the ‘Would you like to add
boundary layers?’
question.
In the ‘Add Boundary Layers’ section of the same task, select ‘last-ratio’ as
the Offset Method Type.
Enter 10 for ‘Number of Layers’, 0.2 for Transition Ratio and 0.5 mm for First Height.
Based on the incoming airflow for the simulation i.e., 20 m/s, the estimated y+ using this
first cell height is about 30.
Additional mesh refinement studies are needed to understand the number of prisms in the
boundary layer required for this external flow problem.
Generally, for a y+ of 30, five to ten layers are a good starting point.
More info about the different methods and variables can be found in the user’s guide.
Set ‘Grow on’ to ‘Selected labels’ and select the walls on which you want the
prism layers to be created.
In this case, we will select all the wall faces except ‘tunnel-walls’ and ‘ground
’. Select ‘Add Boundary Layers’ after employing all the above changes.
In the ‘Generate the volume mesh’ task, change the fill with option to ‘poly-hexcore’.
Set the minimum cell length to 0.5mm and max cell length to 512mm.
Click on ‘generate the volume mesh’ button to create the volume mesh.
Once meshing is done, we can visually inspect the volume using cut planes.
Here, we can see the poly-hexcore mesh distribution, and the boundary layers created on different
wall faces.
We can also check the quality of the mesh to ensure that it meets the standards.
The best practice is to have the mesh inverse orthogonal quality value to be less than 0.9.
To achieve this, right click on the ‘Generate the Volume Mesh’ task and select ‘Improve
Volume Mesh’.
Change the ‘Cell Quality Limit’ value to 0.1 and click ‘Improve the Volume Mesh’.
Once the algorithm finishes running, check the quality of the mesh to ensure that it
meets the standards.
Save the workflow for future use with similar geometries.
The mesh is now ready to be taken into the Ansys Fluent solver for performing CFD analysis.
To summarize, we learned about creating a computational mesh for a watertight geometry
using Fluent Watertight Meshing Workflow.
In this process, we understood the significance of local sizings such as curvature and body
of influence.
Finally, we discussed the importance of boundary layers and how we can setup the prism layers
using the watertight workflow