Welcome to this Ansys How To Series video.
In this video, we will focus on how to use Ansys SpaceClaim to prepare the geometry of
a FSAE car for aerodynamic analysis using Ansys Fluent.
You will learn how to create an enclosure around the car, how to set up bodies of influence
to drive the meshing phase, and finally how to create named selections.
Ready? Let’s go!
This is the solid model of an FSAE car that we will be using in this example. It is about
3 meters long, 1.2 meters high, and 1.4 meters wide. In the model, we can identify the front
wing, the rear wing, the chassis with the pilot, front and rear wheels, suspensions,
and brakes.
If you look close to the tires, you can see that we have added a fillet in the region
where the tire would touch the ground. This is a practical trick to avoid sharp angles
between the tire and the ground that would lead to bad quality cells during the meshing
phase.
First, we will create an enclosure. This is the volume we will analyze to study how the
air interacts with the car and what forces are generated. The analysis would look as
if we were testing the car inside a wind tunnel.
As you can see the car is symmetric. For our analysis we will only use half of the enclosure,
to reduce the mesh size and the computational cost of the simulation.
Next, we will generate bodies of influence (BOIs) that would help us control the mesh
size, and refine only the regions of interest, during the meshing phase. This is a useful
step to have accurate results in the vicinity of the car.
Lastly, we will create named selections that will be fundamental for quickly specifying
local meshing controls, during the meshing phase, and defining the proper boundary conditions,
for the simulation.
Start a Workbench session. Bring the geometry module onto the project schematic window and
link a Fluent meshing module.
Right click on the geometry tab and import the car model. Then open the model in Ansys
SpaceClaim.
Hold CTRL and select the X and Z axis and then click on the plane tool, to create the
bottom plane. Repeat the same for the X and Y axis to create a middle plane. These planes
will be used later so let's hide them for now.
Our geometry is relatively clean, but if you are using a different geometry, you may find
the tools under the repair tab useful. These tools can be used to fix features of the model
that are important in creating a high-quality mesh.
Create an enclosure around the car by clicking enclosure and then box selecting all the components.
Have the enclosure length behind the car about three times the length of the car, in our
case 9000 mm, to capture the wake and place the outlet away from the region of interest.
Have the enclosure width and height to one car length, in our case 3000 mm, and click
the complete button. Make sure to conduct a domain study by varying its dimensions and
understanding how it affects the flow.
In the structure tree, toggle on the midplane and hide the enclosure. Double click on the
Z axis on the bottom right corner to align the view. Select the plane and, under the
design tab, activate the rectangle tool. Sketch a rough rectangle around the car. Switch to
the 3D mode and select the pull tool. Now click on the pull in both directions option
for the pull tool and pull the rectangle by 1,500 millimeters in both directions. This
is a body of influence that will be renamed BOI 1 for simplicity. Copy-and-paste BOI 1
using CTRL+C and then CTRL+V and rename this to BOI 2.
Hide BOI 1 and select only these five faces. We will now pull these faces of BOI 2 in all
the directions by typing 500 millimeters and hitting enter. Unhide the enclosure. Hold
ctrl and scroll the middle mouse wheel to choose the BOI 2 back face. Click on the face
and pull it up to the end of the enclosure. Triple-click the bodies of influence and change
the transparency for both.
Hide everything except the wheels. Triple click it to select the front one and create
an origin at the center of the wheel. Then, hold control and select both the axis systems
to find the location of the center of the wheel. Note down the X, Y and Z coordinates,
you will need them later to define the boundary conditions. Repeat the same process for the
back wheel and make a note of those coordinates as well. Next, delete the origin in the wheels
as it is not needed anymore.
Unhide the enclosure and the planes. Using the split body tool cut the model with the
planes we have created before. Cut the body as shown. Hold CTRL when choosing the cutting
planes and then select the part to delete as shown. As the car is symmetrical, for the
simulation we would only use half of the enclosure, saving computational cost and time.
The bodies of influence don't necessarily need to be cut as the excess geometry will
not be considered during meshing.
Select the front face of the enclosure and then go to groups to create named selections.
Name this as Inlet. Create the named selections for the remaining external boundaries by repeating
these steps. The named selections for the external boundaries are shown here: inlet,
outlet, symmetry and tunnel walls.
Select all the faces and hide them. Triple-click to select the body and create a name selection
called BOI far-field. Repeat the same process for BOI near-field. When selecting geometry
holding the left mouse button and dragging from different corners has different functions:
dragging from the bottom right to the top left will select face as it touches, dragging
from top left to bottom right will select only those that are within the selection box.
Call this rear wing and repeat the same process for all the components of the car. We have
the rear wing, the wheels radii that are the fillets we discussed before, the rods, the
rear wheel and the front wheel, similarly rear brakes and front brakes, the front wing
and lastly the chassis. Show all the components and suppress the car for physics this ensures
the car model does not come into the fluent mesh
and save the geometry.
So, let's summarize. The geometry preparation for an external aerodynamics analysis requires
the creation of an enclosure around the model which would be the volume of analysis.
Bodies of influence can help simplify the meshing process and refine specific regions
of the enclosure, where we want more accurate results. For example, around the car body
and in the car’s wake. Another very good practice is to set named selections. As you
will see, this step simplifies both meshing and simulation setup processes.
Keep these tips in your mind when preparing the geometry for a fluid dynamic simulation.
If you found this video helpful, please like, share, and subscribe. To find more information
about Ansys SpaceClaim tools or other topics, check our channel for more how-to videos and
visit ansys.com/courses today!