Formula Student Car Simulation


Hi all,

After having read many topics about FS car simulations and having followed the related webinars, I still cannot find the solutions to the problems that I am facing. Apologies in advance if these kind of issues have already been solved.

-Firstly, the result for the mesh is not ok (mesh ‘FUC3M18_V1’). The setup indicated in last year webinars has been followed (adapted to our specific CAD), but the resulting mesh features too many illegal cells. Since I realized (I am pretty sure about it, though not 100 %) that these illegal cells appeared due to the surface refinements, I tried the following alternatives:
- Increasing the number of max. iterations for layer addition from 3 to 5 (mesh ‘FUC3M18_V1 - 5 iterations layer addition’): this seemed to reduce the number of illegal cells from > 8000 to ~ 2000. As a consequence, I am now trying to get a mesh with 7 max. iterations for layer addition, which I suppose will yield a lower number of cells. But I do not know neither when it will be enough (i.e. which number of illegal cells can be considered to be low enough), nor whether this is the reason why simulations fail.
- Repeating the same mesh, but with a lower surface refinement (mesh ‘FUC3M18_V1 - Less layer (2, 1.1)’) / without surface refinement (mesh ‘FUC3M18_V1 - No layer car’): in these cases, the number of illegal cells just rocketed!!! (?)

-Simulations were then performed for the meshes ‘FUC3M18_V1’ (the original one, 8000 illegal cells) and ‘FUC3M18_V1 - 5 iterations layer addition’ (2000 illegal cells). In both cases, the simulation just diverged massively, which led to incoherent results -it can be checked in the results control: forces in the wings and the car-. Just in case it was the reason of the trouble, both simulations were also run without the rotating BC for the wheels, but again the same kind of results were obtained. Note that, when the simulations stopped, a window saying that ‘numerical inestabilities’ may be the cause of our problem appeared. But I do not know how to interpret that information.

To sum up: would it be possible for you to take a look to this meshes / simulations and tell us about what could be the origin of our problems? @AnnaFless @pfernandez Thank you so much, any help will be welcomed.


Hi @D_Izquierdo,

The first thing I noticed is that you are using an anisotropic block mesh, and snappyHexMesh doesn’t like that at all.

Try to get cells as isotropic in dimensions as possible. For that, you can take the same wind tunnel dimensions and number of cells as in the workshops.

Regarding full car simulation, just skip the MRF and porous zone steps of the tutotials. For the wheels you just have to specify a rotating wall boundary condition, like is done for the tires.

Kind regards,


good answer you beat me to it :smiley:

I created a mesh last night, just made it public with the above mentioned.

Kind regards


Thank you for the advice, I had mixed up the coordinates when creating the block mesh, now I have done it properly and the mesh result is excellent:
-‘FUC3M18_V1 - ISOTROPIC’ mesh: only 93 illegal cells
-‘FUC3M18_V1 - 9 iter, ISOTROPIC’ mesh: 0 illegal cells (by allowing more surface add. iterations)

However, the simulation only converges for the case of no rotating wheels. When I include the rotating boundary condition for the wheels, the solution for the forces just rockets up to huge values:

I have also tried to change the sense of rotation, just in case that was the problem, but the result is still the same. Do you know what may be happening? @pfernandez @1318980

NOTE: simulation ‘V1 - Rotating wheels (ISO)’ is exactly the same as ‘V1 - Not rotating wheels (ISO)’, but just changing the BC for the wheels. So the problem might be likely in the rotating BC definition. I explain here exactly what I have changed from one simulation to the other:

  1. For the car BC, I have undo the selection of the wheels faces
  2. For the rotating BC, I have selected those same faces. The absolut origin of the cad is just at the middle of the front axle, so for the case of the front tyres, I have left (0,0,0) as origin and x as rotating axis direction.


Hi @D_Izquierdo,

For the rotating wheels case you’ve specified the centre of rotation of the rear wheel at (0, 0, -1600). There’s the problem… the simulation is using the meter as the unit of length. Considering that the STL measures about 3 m, which seems OK, then I guess the actual centre of rotation of the rear wheel would be placed at (0, 0, -1.6).



Ok, problem solved. It works nicely now. Thank you so much.