[Clementhuon]

Hi everyone,

I'm using Star-ccm to simulate the cooling of a brake system on a car. The purpose here is to compare the mass flow rate threw the wheel rim in a steady and in an implicit unsteady simulation.

I set a rotating wall condition on the wheel, and the wheel rim. I also set a MRF condition on the brake disk (I need to move the air volume in the cooling channel in the brake disk). I also set a translation on the road.

The simulation run really good in steady state. Convergence and results are allright ( I am using a standard model my company use for this kind of study). But when I try to make the conversion in unsteady (with the implicit unsteady model) the calculation diverge.

I set a time step of 7.5E-5 s (velocity of 140 km/h and a mesh size of 2 mm on the wheel) a number of inner iteration of 10.

I also try to make the simulation without MRF and without any rotation. Every time the steady simulation run fine but when I try to set the model in unsteady and run it (with the initialisation of the steady simulation) the calculation diverge.

If someone get an idea ? I woud really appreciate some help.

Thanks

[willimanili]

I would try to reduce the time step to see if you can get the simualtion stable with it. Especially at the beginning when you switch to transient calculation. If it works you can try to increase the timestep after some timesteps to get an faster simulation result. Another thing you could do is to reduce the URF. And also an combination of both could be targeted. If you reduce the URF, maybe some more inner iterations are necessary to get an converged result for each timestep.
Is there any warning or limit overstepping before the solution diverge?

[Josh]

In addition to willi's suggestions, I'd try ramping the Courant number.

[Clementhuon]

Thanks for the answers !!

I succeed in solving my problem in using the coupled solver (and not the segragated)

The simulation seems to work but after 1000 iterations a got an error message because of a problem of Interface Updating, my mesh doesn't seem to support the rotation.......

[Josh]

How did you model your tire in the unsteady simulation? Did you isolate it and create a cylindrical domain around it with an interface between the domain and tire?

[Clementhuon]

No, for the moment the BC on the tires is just a wall tangential velocity. Only the wheel rim and the brake disk are defined as MRF. Those two boundaries are defined in another regions and (with the interface) every regions are closed.
But I found out the problem, the simulation run in coupled and the only problem are coming from my interface. After a few iterations the two parts (master and slave) of my interfaces are not coupled anymore (between 30 and 90 % of intersection).
I didn't succeed in solving the problem but I think this is coming from the rotation axis of my MRF. I'm trying to work on the coordinate system to make it perfectly adjusted with my geometry but this is not so easy.
If someone get any idea. I'm working with ANSA to develop the geometry and then (after importing the geometry) with starccm+. The problem is that I can't export my coordinate axis from ANSA to STAR-CCM+ and creating it in STAR-CCM+ is not enough accurate.

Bye and thanks for the interest ....

[Josh]

This is probably an obvious point, but did you try defining the coordinate system in the scene using three points on a circle of the initial surface, e.g., on the tire, rims, or suspension? This works very accurately for me.

[Clementhuon]

The problem is more to find the center of rotation as the axis. But I think I succeed in doing something relevant. I found another problem in my geometry.
The brake disk wasn't really a disk but a kind of elipsoid. That could explane the problem of Interface during the rotation. I will run it in the next days, and say it to you how good it worked.

Anyway, than you for your help.

clement