Multiple reference frames
 

Hi, I have to perform an CFD analysis on an car body and I have to consider also the rotating wheel, how can I consider the wheel rotation??? Probably the best solution is to use MRF but how bis i the volume of fluid that I have to consider??? thanks raffap

Re: Multiple reference frames
 

Firstly you create a cylindrical coordinate system and enforce a wall boundary condition for each wheel. Then You define the angular velocity (RPM). To calculate it: Consider distance between the axis of rotation and the ground,and the car velocity. Ex. d=300 mm V=50 m/s w=50/0.3=166.67 rad/s /0.10472 = 1591.55 rpm By

Re: Multiple reference frames
 

you also need to ensure you have a nice circular interface round the weel mesh, that is the tricky bit, you have to be quite careful. You could just use rotating walls of course

Re: Multiple reference frames
 

so julien, you mean I have only to assign a wall boundary (with angular velocity)for each wheel??? But what about MRF???, with MRF I have to force the fluid to rotate, so I have to assign to that fluid a different spin index...and I can consider the wall with zero velocity...it's ok what about if I have also more components like for example rotating like brake disc????

Re: Multiple reference frames
 

Hi Raffap, in my opinion there's no need to use MRF. I think it's ok if you do this way: i suppose you simulate, for the symmetry, only half model. So you define two wall boundary conditions and two cylindrical coordinate systems, with z axis coincident with the rotation axis, for the two wheels. For the ground you enforce another wall boundary condition in which you specify the car velocity component. The others boundary conditions are: inlet, pressure for the outlet section, and symplane for the plane of symmetry. If you have other rotating components it depends by what you want to get by the analysis. By

Re: Multiple reference frames *NM*
 

Re: Multiple reference frames
 

ok I'll try your method. i'm doingtwo kind of analysis: 1) only external car body, so wheels have very simple geometry... 2) I'm intersted in the airflow direct to the brake disc, so the geometry for this second analysis is more complex,I need to simulate alle the components, disc, caliper, wheel and so on.. I think that for the second analysis is more difficult apply simple boudary condition...what do you think???

Re: Multiple reference frames
 

This kind of simulation are often done in steps: - Make a model and run the simulation of the complete car. - Make a sub-model of the wheelhouse and surroundings. In the sub-model you can use a much smaller cell size than in the complete car model, which make it possible to resolve all the details. - Use SMAP command to transfer the solution of the complete car model to the sub-model. - Run the sub-model 1 iteration without solving anything with restart from the SMAP generated file. You now have a proper *pst file. - Read in the *pst file of the submodel and create boundaries to the sub-model, write a nice macro to to that. -Run the sub-model with boundaries created from the complete car solution.

The submodel needs to be divided so you can apply the MRF-model just around the brake disk and wheel rim, on the wheel rubber you can use a rotating wall boundary.

You need some experience to do this, so if you are a beginner I suggest you call CD-Adapco support.

Re: Multiple reference frames
 

Thanks tobbe, My idea was to perform an analysis according your steps, but I have not experience in use SMAP command, anyway I'll try to do it...

Re: Multiple reference frames
 

yes this is correct.

There is no need for MRF if there no solid part rotating inside the fluid volume. Only on the boundary of the fluid domain

You can imagine you stand inside the fluid cell during one period and look if a solid traverses it at a time t.

Re: Multiple reference frames
 

I totally agree.

On top of that doing it in step also allows you to quantity the importance of each term, model or option you add or turn on at each step. This is powerful because you know what is preponderant in your analysis.

- start invisicid -> get the drag - do RANS -> how much does the viscous term modify the drag/force - add MRF -> how much does it account for the drag

then in your report to your boss you show how cfd is providing insightful information. You also increase your expertise/knowledge much faster although you are doing more runs.

If there is a problem -> you know where it comes from. If there is an option that does not make a difference -> you know.

If you do 1 run with the full model straight away...what did you really learn?