Convergence problem - Formula SAE CFD


#1

I’m trying to simulate a Formula SAE car (First test rsracing).

However, I’m getting a huge velocity profile underneath the car. I’m not sure how should I set up the ground of the car. I’ve tried to set up as the tire was at exact contact with the ground. But I’m not sure if I achived it and I was thinking in setting up as the tire was just a little bit “inside” of the ground.

https://www.simscale.com/projects/rfensterseifer/simscale_-_first_test_careen/


#2

Hi @rfensterseifer, I think that the way you have your model right now should work fine but truth be told I haven’t really done much on cars. The F1 workshop is a good place to do your research! Check it out! Also, if I am not wrong @akosior was doing something along these lines, @dylan too? Good luck!


#3

Hi @rfensterseifer, I agree some odd results here:

I certainly wouldn’t expect velocities of these extremes (1.3Km/s? in some areas), however your simulation setup looks very reasonable.

So I would look at doing these changes:

  • Increase your bounding box. To me it looks like we are getting a bit of interference from the walls… I’d say treble the height and width and maybe double length (behind).
  • Add layers to the ground. I know the ground is moving the same velocity as the air however under the car, velocity will increase a lot and therefore will have a boundary layer.

Apart from that I think its a solid setup so beyond this I don’t think I can give any further advice, if this still produces odd results we might need backup :slight_smile:

Kind regards,
Darren Lynch


#4

Hi @rfensterseifer,

Darren is right; there are a couple of things you should do to get back on track:

  • Add boundary layers to the ground. But if you keep your settings for the mesh, you’ll end up with about 50 M-cells, so you might want to reduce the refinement level of your refinement boxes.
  • Recalculate the reference area of your model. I measured the frontal area of your model to be 0.807 m^2; but since you are running a symmetry simulation you should specify the half of it.
  • Write coefficients every 1 iteration. Besides checking the convergence of residuals, you will want your drag and lift to reach an asymptote. Thus, you need to monitor their values every timestep.

With this changes I was reaching values of about 0.7 and 0.3 for the drag and lift coefficients of your model; which is in the order of magnitude I would expect those values to be.

Regards,


#5

I saw the post but forgot to reply. Been very busy recently.

pfernandez has mentioned a key mesh setup - prism layers on the ground. There is a finite wall-normal velocity gradient on the ground plane where the car sits, and this gradient extends downstream. This gradient exists even though the velocity immediately next to the ground has the velocity of the ground. Expect large wall shear on the ground under a well-designed underbody. The four wheels also create jetting phenomena that accelerate local flow.

With a high-Re turbulence model, use at least 2-layers on the ground. If you can afford more, use more.


#6

Hi @jjanczyk,

Take a look to this post, I think you’ll find it very interesting and useful for what you are trying to do:

Best, ML