Working on a cfd around a simplified model of a formula student car to check how certain volumes affect the airflow around our car.
link: SimScale
The thing is that I don’t have an understanding of what is wrong with the mesh or simulation
Hi dani_marciu,
First of all, welcome to the SimScale Forum, and thanks for posting your question,
Almost every divergence in a simulation is because of bad mesh quality. So if we have a look at the meshing log, we can clearly see that you have a super-high max values for many of the mesh metrics as shown below
Now the important question is where do these bad cells lie? Can they be ignored? If they are at important or critical regions, then they should be resolved to better capture the physics.
So let’s switch to mesh quality and look at these metrics.
Below we have cells with an aspect ratio above 50, and there are a lot of cells spread across the domain
It is also a good practice to check your results and look for regions where the values begin to explode. You can do this by creating an isovolume filter, selecting velocity magnitude for coloring, and filtering the very high velocities. This gives me the below-highlighted region, which is the exact location mentioned in the error message
Now if we create a cutting plane and look at the mesh, we can see that the mesh here is not that great also we are getting super high y+ values here. This indicates that the boundary layer is not well resolved. Perhaps you can read more about y+in this nice article: what is y+
All in all, I would recommend you improve your mesh quality. You can read more here on How to Check and Improve Mesh Quality?
Also, I noticed that your geometry is symmetric. For this you can make use of the symmetry boundary condition, this will greatly reduce the complexity, as well as the mesh size and run time. There is an exact tutorial that makes use of symmetry, you can check it out here Incompressible Flow around a Formula Student Car
I hope this helps.
Best,
Paresh
Hi dani_marciu,
Welcome to our Forum!
As I see, Paresh has already given you a very comprehensive response on what might be the issues of your model not behaving as expected. Please try to follow the considerations for mesh quality are suggested.
I also had a look at your model and looks like the cause of the very high aspect ratio is your boundary layers. The surface mesh looks nice but you are trying to grow some really small boundary layers (First layer Size)
What you can try, is increase the overall relative thickness to a value around 0.3-0.4 and then also increase the First layer size a bit. The very small First layer height might be the cause of the mesh Aspect Ratio getting too high.
Good luck with it and lets us know if any new questions arise,
Ioannis
Thanks a lot, having a finer mesh helped running the simulation but after it was done the showing results are unsatisficatory.
What can be done to reach realistic values?
Hello dani_marciu,
On a second look, it looks like your run was actually successful with accurate results, so congratulations!
Your screenshot does present a uniform velocity everywhere around the flow domain, however, you’ll want to ensure the legend is properly scaled. Sometimes, the legend may be heavily skewed to large values by default (like 2633 m/s in your case due to a few outlier diverged nodes in your large mesh domain), but as you can see below, you’ll simply need to modify the scaling by re-inputting the expected minimum/maximum in the legend to dynamically change the visualization of the field quantities.
Hope you have a great start to the new year and continue gaining insight with the SimScale simulations you perform!
Cheers,
-Omar
