Floworks: basic vehicle simulation
 

Hello folks, I'm a complete newbie to this. I'm looking for a little guidance in setting up some simulations, basically I'm looking to run virtual windtunnel calculations.

My goal is to use a simplified model of a race car's body to evaluate the overall affect of various diffuser angles and shapes on the back of the car with regard to drag and downforce production.

My vehicle body is approximately 12 ft long by 4.5 ft wide, and I have a ride height of 2" set up, with symmetry along the Y axis to reduce the calculation time. I am also using a moving ground plane set at the air speed.

What size computational domain would be appropriate for such a vehicle? How many cells would be required for the analysis to accurately model the trends of drag/downforce for a model of this size? Can anyone point me to some information on narrow gap size settings?

Thanks!

Hi,
This is not that easy to say. Usually we recommend 3 cells over a small gap if there is some flow and more cells (8 -12) if the flow there is important for example the opening of a nozzle is of course the most important flow of the nozzle.
You can then in addition use the solution adaptive refinement (SAR) which you find in the calculation control options. This can be applied to the global computational domain (CD) or just to local meshes which you might have used for the diffusor to resolve the mesh here finer as it is the key interest on the flow and forces etc.

So to give you a rough idea, if your car is around 12ft long I would suggest to have the CD start 1/2 to one full lenght of the car in front of the car and depending on the velocity and your interest on the wake of the car for example for following cars you should consider 3-4 lenghts of the car behind it. For the height you should use 3-4 car height above the car. These are some rough ideas, over the time you will learn how much is enough by looking at the velocity and pressure field to see if it has dissipated already in the far field.
It is enough to have the CD range into the ground by a few milimeters as there is no flow anyway. Often the road is modelled as a thin plate anyway and you extend the CD into it just a little to have the solid surface in the CD for the moving wall boundary condition (BC).

There is no "number of cells" that I can tell you as it is heavily dependent on the car geometry as the partial cells should resolve the features and surface of the car especially where they are thin in order to resolve the airflow on such locations such as the front wing leading tip or any ribs etc. This is really the point where you need to do a mesh convergent study in order so see what mesh settings you need until the results are not changing anymore. Usually this is done once to get a feeling for it for simulations you are working on repeatedly. If you have constantly changing types of models for example pumps, valves, a whole car or just the exhaust, then of course you will have to find that experience for all of them over time.

The narrow gap settings are mostly usefull for local meshes in order not to have a huge mesh because the settings were applied to the whole CD. For example you can use it for the local region of the under car flow to reach the ~8 cells. In general the level here limits the maximum level to be used to reach the defined cell number in such a gap. The level is always based on the basic mesh which corresponds to Level 0. Each level step means a octree refinement of a cell of the previous level. Meaning a level 1 refines a level 0 cell in all tree directions by halving the cell lenght, so it makes 8 level 1 cells out of one level 0 cell, hence "octree" refinement. And level two does the same to a level 1 cell etc.

I hope this helps,
Boris