[HHOS]

Hello everyone;

I am trying to solve a case in which two rotating bodies share part of the volume where their rotating mesh domain would be. For that reason I need to make a dynamic mesh.

I am trying to get a nice setup, but the best I achieved was a case that was getting negative cells after 100 time steps.

What I would like to understand is the setup. In the remeshing tab, which I guess is the most important, I understand that it will remesh the cells which are "smaller than", "bigger than", and have a "higher skewness than". However I don't get how the new cells will be. Will their size be between the two borders I wrote?

Do you think that my setup is correct for the given mesh details?

Mesh Scale Info

Minimum Length Scale: 7.3281e-5
Maximum Length Scale: 0.01169608
Maximum Cell Skewness: 0.9477243
Maximum Face Skewness: 0.9309621

Smoothing:

By diffusion
Diffusion Function: Boundary-distance
Duffusion Parameter: 0

Remeshing:

Local cell
Minimum length scale: 0.003
Maximum length scale: 0.011
Maximum Cell Skewness: 0.93
Size remeshing Interval: 1

At the moment it is running, but with a really small timestep. I would like to increase it, but it always dies.

Any suggestion??

Thank you!

[himanshume89]

Hi HHOS,

i guess you were working on some kind of positive displacement pump. I would like to know that have you found any solution with your setup. Please let me know as i am working on same kind of project and facing same kind of problem.

Thanks.

[HHOS]

Hello!

So, the setup went well as follows:

Smoothing:

By Spring
Constant factor: 0.5
Convergence Tolerance: 0.001
Number of iterations: 40
Tet in tet zones

Remeshing:

Local cell
Minimum length scale: 0.00115
Maximum length scale: 0.003
Maximum Cell Skewness: 0.9
Size remeshing Interval: 1

That taken into consideration, it makes no sense to have the transient formulation as second order because it will always switch to 1st order when remeshing. If you change the size remeshing interval, might make sense to have it in second order, I don't know.

Another important thing is that the Pressure-Velocity coupling must be set to Coupled. It resulted in very fluctuating pressure field otherwise, at least in my case.

[himanshume89]

Thanks HHOS, it will be very helpful.