Welcome to this Ansys How to Series video.
In this lesson, we will learn how to use Ansys Fluent post-processing to visualize and analyze
the model results on the Formula SAE car.
First, we will learn to estimate the total lift and drag forces on the car.
We will then create and interpret contours of velocity magnitude and static pressure.
We will also learn how to create a velocity vector plot to help us understand the fluid
flow behavior around the FSAE car.
Are you interested in learning these post-processing techniques?
Let’s get started!
Most of the post-processing in Ansys Fluent is done from the ‘Results’ tab.
In this tab, we can create additional surfaces for post-processing, and add graphics such
as contours, vectors, pathlines to visualize the results.
We can also calculate the surface and volume integrals, fluxes, and forces from the ‘Reports’
section in this tab.
First, we will estimate both drag and lift forces on the car by clicking on ‘Forces’
under ‘Reports’.
We will highlight all wall zones related to the FSAE car as shown.
Ensure that the direction vector is pointing in the direction of the flow.
Here, the value 1 for X means that the forces are estimated along the X-direction.
The drag force experienced by each part as well as the total drag force on the car is
printed in the Fluent console.
The corresponding drag coefficients are also printed here.
As highlighted, the rear wing and the car chassis contribute significantly to the overall drag.
It is important here to note that these printed values are at the end of the 600th iteration.
Since the drag values are fluctuating in the simulation, the best way to estimate the steady
value would be to calculate the average over several hundred iterations.
The average drag coefficient is approximately 1.14.
Now, let’s change the direction vector as shown here to estimate the lift force experienced
The total lift force, as well as the corresponding lift coefficient, have a negative sign.
It means that the car is experiencing a net force in the negative Y direction, which acts
to keep the car on the ground at this speed.
This downward force on the car is commonly referred to as downforce.
The front and rear wings of the car contribute significantly to the overall downforce experienced by the car.
Next, we will create some contour plots to understand the general flow field around the car.
Before doing this, let us first display the entire car geometry.
Click on ‘Display’ from the ‘Mesh’ section of the Domain tab and highlight all the surfaces related to the car.
We only see half the car.
To show the entire car model, click on the ‘Views’ tab and open the ‘Views’ panel under the ‘Display’ section.
Select the ‘Symmetry’ face zone as the mirror plane.
Click on ‘Apply’ and Ansys Fluent will display the full model of the car in the graphics window.
Now, click on ‘new’ under ‘Contours’ in the ‘Graphics’ section to create a new contour.
Let us first display the contours of ‘velocity magnitude’ on the ‘symmetry’ plane.
Open a new contour, select ‘Velocity’ from the ‘Contours of’ dropdown, and highlight the ‘Symmetry’ surface.
Ensure that the ‘Global Range’ is deselected.
Hit ‘compute’ to obtain the range and click ‘Save/Display’ to show the contour in the graphics window.
The velocity plot helps us identify the low and high-velocity regions.
We can see that the velocity at the front of the car decelerates sharply to zero.
This is called a fluid stagnation point.
Similar stagnation points are observed on the driver helmet and the top portion of the rear wing.
If we zoom into the rear wing, we see flow acceleration near the bottom as it turns around the wing.
A low-velocity region is created right behind the car due to flow separation, which is generally referred to as the wake.
Similar wake regions are created behind the rear wing of the FSAE car.
We will learn more about flow separation and how to identify these regions a bit later.
To complete our understanding of the aerodynamic forces experienced by the car, we will plot
the static pressure contour on the plane of symmetry to analyze the pressure distribution around the car.
Change the drop-down to select ‘Pressure’.
Hit ‘compute’ to obtain the range and deselect both ‘auto range’ and ‘clip to range’ options.
Change the ‘Min’ to -250 Pa, to facilitate a distinguishable difference between the high
and low-pressure values, and click ‘Save/Display’ to show the contour.
Change the view to see the XY plane.
We observe a high-pressure region at the nose of the car and a low-pressure region behind the car.
The high-pressure in front of the car is due to flow stagnation and the low-pressure region
in the wake is due to the flow separation and subsequent flow reversal behind the car.
Similar high-pressure regions are created on the top side of the front and rear wings.
On the other hand, the bottom side of these wings experiences low pressure.
This uneven distribution of pressure around the wings, and other car parts, manifests
itself into the drag force and downforce.
We can obtain a general qualitative understanding of the flow field by looking at vector plots.
Let us create an IsoSurface of the Z-coordinate to plot the vectors on.
To do this, click on ‘Create’ under the Surface section and select ‘Iso-Surface’.
Pick ‘Mesh’ from the drop-down list of ‘Surfaces of Constant’ and select the ‘Z-Coordinate’.
Clicking ‘Compute’ should estimate the min and max ranges of Z-Coordinate in the computational domain.
We should either be able to provide the input by entering a value under ‘Iso-Values’
or use the slider bar to identify the correct plane we wish to create.
Enter 0.6 m under the ‘Iso-values’ input field, change the name to ‘z=0.6’, and hit ‘Create’.
Now, click on ‘Vectors’ in the ‘Results’ tab and pick ‘new’ to set-up a vector plot.
Rename this to ‘Velocity Vector’ and choose the isosurface that we just created and deselect the ‘global range’.
Also, change the ‘scale’ to 3.
Before hitting ‘Save/Display’ to show the velocity vectors, let us select the ‘draw
mesh’ option to display the FSAE car geometry.
Also, go into the ‘Views’ panel and deselect the ‘mirror’ plane.
In the ‘Vectors’ window, click ‘Save/Display’.
We can now visualize the fluid flow behavior around the front wing and the wheels.
Because of the rotational motion of the wheels, we see that the airflow near the wheels also
has a strong rotational component.
We also observe flow vortices, which are regions of rotating flow, behind the front wing and the tires.
That brings us to the end of our first lesson on post-processing.
To summarize, we learned how to extract the drag force and downforce experienced by the
car, and also create contours and vectors to study pressure distribution on different
car components, flow stagnation points, and recirculating regions behind the wheels and rear wing.
If you found this video helpful, please like, share, and subscribe.
To find additional tutorials related to our Meshing tools or other topics, check out our
channel for more how-to videos and visit ansys.com/courses today!