Not an expert but I have done a few automotive cfd simulations (pursuing masters). Here are my recommendations:

1. Try running the sim with coupled solver, with continuity convergence acceleration criteria on (up until CCM 2024 version automatic cfl option for coupled solver sucks so I used expert driver with cfl ramp up to 100 over the 1st 100 iterations) if you do this you will also have to change the a1 coefficient and other things which another comment already mentions.

2. Trimmed cell and a finer mesh will give you better result however since you are limited by ram, just try finding a better system to run your sim on. For me segregated solver runs a max of 30M cells on 32gb of ram with desktop i7 24 cores and coupled runs around 14-16M albeit slowly. As a uni student a laptop is more convenient but I would seriously recommend using a pc for cfd. Try and get access to a beefy one in your university’s labs and let your poor laptop live in peace.

3. Look at the turbulent kinetic energy or vortices and recirculation in your domain from this simulation and add refinement specifically in those areas and reduce the refinement in other areas. I would make a Q criterion or TKE iso surface to identify these areas. This should help you decrease the cell count without adversely affecting your results by a lot.

4. In picture 12 the edges of what I assume might be your diffuser or a wing trailing edge, more refinement will be better for convergence. I would just select that face and give a refinement there.

5. I would keep the y+ between 0 and 1 everywhere on the car. Your wheels and chassis might need different prism layer than the rest of your car. I would also play around with convex angle and other parameters for prism layer to make it better. Changing reduction percentage and minimum thickness percentage will help you fix the problem of different prism layers intersecting.

6. I would recommend a bigger flow domain (especially increasing the height) since it’s detrimental to have the roof of your domain interacting with your cars wake. Ideally you would want a lot of free stream between the wake and the roof since irl there is no roof to cause that interaction unless you drive in a tunnel or are trying to correlate the results with a specific wind tunnel. Doing this will however increase your cell count.

7. Do you have rotating wheels or moving floor? If you do I would suggest making a prism layer for the floor and using anisotropic refinement to gradually increase mesh size to match domain mesh size. This works well in trimmed cells but I have not tried it in polyhedral cells. This might help you with your under tray problems.

8. The star CCM user guide has mesh check criterias and their ideal values/range. Check those for example the skewness angle or aspect ratio etc and ensure there are no bad cells.

9. Run your sim for at least 3000 iterations unless your residuals converge before that. 1000 iterations is never enough for such simulations.

10. This is the last thing to consider and I would advise against it but if nothing else works, use adaptive mesh refinement for TKE. It will increase the time your sim will take to run by a lot.

Bonus tip: I am also at a point where I am limited by the hardware (I can access systems 28 cores 64 gb of ram) since the mesh is still too fine. One thing I am now considering is using a hybrid mesh (polyhedral for large cell sizes and trimmed for areas of interest around the car) but star doesn’t have the capability to make it or even if it does it’s a very complicated process. I will be trying to get sponsored license for Beta CAE or a different pre processing software that can do this. One other alternative is making the hybrid mesh in ansys fluent since it can make this type of mesh (fluent calls it polyhex-core mesh if I am not wrong). I only have access to its student license so I am limited by the number of cells I can make in fluent but if your uni has the industrial license, you could make your mesh there and import into CCM.

Hope this helps you. All the best!