Welcome to this Ansys How to Series video.
In this video, we will learn how to set up a simulation to analyze
the aerodynamics of a Formula SAE car using Ansys Fluent.
We will start from a mesh file and go through all the steps that are needed to set up the simulation,
such as setting up the boundary conditions, selecting the turbulence model,
and selecting the right solver for you simulation.
So, let's get started!
This is the computational domain that we will be using in this example.
As the car moves through the air, our working fluid in this simulation will be air.
In the real world, the car is moving at 20 m/s.
However, in our simulation, the car would remain stationary and everything else will
move relative to it.
The air would come in through this face at 20m/s and leave the domain through this face.
These surfaces represent the walls of our hypothetical wind tunnel and thus will be
modeled as slip walls since the effect of shear stresses
can be considered negligible along these walls.
This surface lies along the symmetry plane and thus will be modeled using the symmetry
boundary condition.
The ground will be moving at 20m/s relative to the car
and thus will be modeled as a moving wall.
Similarly, the wheels of the car rotate as the car moves forward, and thus we will be
modeling them as rotating walls having a speed of about 87 radians per second, which is obtained
by dividing the inlet speed by the wheel radius.
All the remaining surfaces of the car will be modeled as no slip walls.
For this simulation, the pseudo transient formulation of
the pressure based coupled solver would be used.
Let us begin by quickly checking the mesh.
As you can see the mesh check is complete without any errors.
Next, we will evaluate the mesh quality.
The orthogonal quality for this mesh is greater than the recommended minimum threshold of
0.1 confirming that it is of good quality.
Now let's go to the physics tab where we will set up the physics for this simulation.
We will retain the defaults in the general settings as we will be performing a steady
state simulation using the pressure-based solver.
Open the Operating Conditions.
We can see that the operating pressure is set to the atmospheric pressure.
Next, we need to update the reference values which will be used
to calculate the pressure coefficients.
Click on Reference values and type 20 m/s as velocity.
Now, in the case of external aerodynamics of cars, the reference area corresponds to
the area facing the flow, or the frontal area.
To calculate this, let’s switch to the results tab, and click on Projected Areas.
Select ‘X’ as the direction of projection as it is the direction of the flow and in
the list of the surface, select all the surfaces that correspond to the car.
An important parameter in this calculation is the Minimum feature size.
You can try reducing this value to find out when the projected surface area begins to
converge towards a particular value.
In our case, using a minimum feature size of 0.001 or smaller,
the frontal area converges towards 0.5m^2.
Copy this area from the console and paste it into the reference area field.
Now let's switch back to the physics tab.
Open the viscous model dialog box to set up the turbulence model.
The Reynolds Number based on the car length is about 4 million
so we will assume the flow to be fully turbulent,
and, therefore, we will use the k-omega sst model for this simulation.
Let's also go ahead and activate the curvature correction option to take into account the
streamline curvature and system rotation.
You can find more information about different models and their settings in the Help section.
Click on the Create/Edit button under Materials to edit the materials for this simulation.
Since the flow in this simulation is expected to be incompressible
we will be using constant density.
So let's stick with the default material properties of air, as shown here.
Clicking on the Cell zones will open the Cell zones conditions panel.
We can see that the air is assigned here as the default material.
Now click on Boundaries to open the boundary conditions panel.
Let us group the boundary conditions by ‘Zone Type.’
This can prove helpful when you are dealing with fluid flow problems with many boundaries.
Set the inlet velocity magnitude to 20m/s.
The turbulence intensity at the inlets of wind tunnels
is usually very low and therefore, we will set the turbulent intensity at 0.5%
and Turbulent viscosity ratio at 2%.
Make sure that the outlet is set to zero-gauge pressure because the outlet is exposed to
the atmosphere and keep the same turbulence quantities for the outlet in case of any reversed flow
For the back wheel
activate the rotational moving wall
and input a rotation axis origin
as shown on the screen.
These values were obtained from SpaceClaim during the geometry preparation stage.
Set a rotational speed of 87.489 rad/s
The axis of rotation is in the positive Z direction according to the right-hand rule.
Now repeat the steps for the front wheel and input the rotation axis origin as shown on the screen.
Make sure that chassis, front wing, rear wing, and rods are all set to no-slip stationary walls.
Set the ground as a moving wall with a 20m/s translational speed
as it will be moving with respect to the car.
Set the tunnel walls as a zero specified shear to simulate a free slip wall.
Repeat this step for wheel radii.
Let's switch to the Solutions tab and click on Solution Methods to set-up the numerical solver.
Make sure that the Spatial Discretization scheme for Turbulent Kinetic Energy
and Specific Dissipation Rate is set to Second Order Upwind.
Click on Controls to access the Under-Relaxation Factors.
For this simulation we will use the default values.
You can set the convergence conditions using the Residual Monitors as shown.
We'll use the default values for this simulation.
Next, we will set up a drag monitor for the entire car.
In the Drag Report Definition box, change the name to ‘cd-car'.
Make sure that the force vector is aligned with the flow direction.
Select the Wall Zones associated with the car as shown
and enable report plot and print to console options.
Similarly, repeat the steps to create a monitor for the lift coefficient.
You can add more report definitions depending on the goal of your simulation.
Click on Initialize to initialize the solution.
Next, we will use the Quick search feature of Fluent to perform FMG initialization.
Type fmg as shown and select the first command under TUI.
In the console hit enter,
and type yes and hit enter again.
This will begin the FMG initialization. FMG is generally used to initialize complex flows.
A better initial solution helps accelerate simulation convergence.
Set the number of iterations to 600 and hit ‘Calculate’ to run the simulation.
We can see that both the global residuals and the monitored quantities are oscillating.
This is due to vortex shedding caused by the interaction of the car and the air.
As this is an inherently unsteady flow problem this behavior of the solution is expected.
The plots of Cd and Cl seem to have stabilized past 300 iterations and oscillate around an
average value.
We can take the data output file to Excel.
In Workbench, click view and toggle on files.
Here we can find the location of the files.
The output files can be opened in Excel for further processing.
The results can be clipped, and we can estimate averages, root means square, and so on...
Both values are in an acceptable range for this car model, and we can conclude that the
simulation has reached an acceptable convergence for the steady state analysis.
So, to summarize – in this video we setup up a simulation for analyzing
the external aerodynamics of a formula SAE car.
We performed mesh checks to ensure that our mesh is of good quality.
Then we assigned material to the domain and set up the correct boundary conditions
of our flow problem.
Lastly, we set up the numerical solver for the problem and added a solution monitor to
help us keep track of the drag on the vehicle as the simulation progresses.
The monitors also helped us to understand if we reached a reasonable convergence for
the steady state analysis of this inherently unsteady problem.
Keep these tips in your mind when setting up your fluid dynamics simulation.
If you found this video helpful, please like, share, and subscribe.
To find more information about Ansys Fluent or other topics, check out our channel
for more how-to videos and visit ansys.com/courses today!