[basneb]

Hello there,

I am currentliy running simpleFoam on my mesh, which contains half an automotive geometry (station wagon) in order to find out the drag coefficient Cd. The mesh has a total of about 12 million cells and with my settings now, I get convergence after about 2000 iterations. This actually is very time consuming and an entire simulation (up to 5000 iterations) takes about 14 hours. The same case can be run in Fluent, which converges already after about 500 iterations. Is it somehow possible, to speed up the simulation?
So for further information, I'm using simpleFoam and the realizable k-epsilon-model with the default values. In order to intialize the pressure field, I run potentialFoam first. I use the GAMG solver for the pressure and the DILUPBiCG solver for the rest. Usually I run in double precision.
Hope that somebody can help me.

[dVoglander]

Hi,

if you don't have stability problems, you could maybe try to increase the relaxation factors in system/fvSolution.

[askjak]

Try smoothSolver instead of DILUPBiCG to improve performance.

[bastil]

Originally Posted by basneb

Hello there,
The same case can be run in Fluent, which converges already after about 500 iterations. Is it somehow possible, to speed up the simulation

I guess it is the "coupled" solver in FLUENT? Simple will behave very similar to OpenFOAM. Regards.

[basneb]

Originally Posted by dVoglander

Hi,

if you don't have stability problems, you could maybe try to increase the relaxation factors in system/fvSolution.

I tried this already, but unfortunately I get stability problems then, but thx anyway.

Originally Posted by askjak

Try smoothSolver instead of DILUPBiCG to improve performance.

I will definitely try this, thx.

Originally Posted by bastil

I guess it is the "coupled" solver in FLUENT? Simple will behave very similar to OpenFOAM. Regards.

Unfortunately, I did not do the Fluent simulations, so I don't know, which solver was used, but actually it should have been the same one. Will try to find it out, thx.

[askjak]

I don't know fluent but I know the definition of residuals differ among CFD packages. So don't base convergence on the absolute residual levels.

I have found simpleFoam to convergence in as many steps as StarCD on the same mesh.

[basneb]

After trying some stuff today, I can state that playing with the URFs really helps a lot in getting faster convergence. Now I am almost at Fluent-level. For the rest the use of the "applyBoundaryLayer" function seems to help speeding up the simulation as well. Setting the nonOrthogonalCorrectors to 0 gives a significant change.

[Thomas Baumann]

Hi basneb,

After trying some stuff today, I can state that playing with the URFs really helps a lot in getting faster convergence. Now I am almost at Fluent-level. For the rest the use of the "applyBoundaryLayer" function seems to help speeding up the simulation as well. Setting the nonOrthogonalCorrectors to 0 gives a significant change.

But don't you need nonOrthogonalCorrectors? I think a mesh of a station wagon is complex and should have deformed mesh cells. Have you compared the results of your flow problem with different numerical models, especially with and without nonOrthogonalCorrectors?

Regards Thomas

[basneb]

Originally Posted by Thomas Baumann

Hi basneb,

But don't you need nonOrthogonalCorrectors? I think a mesh of a station wagon is complex and should have deformed mesh cells. Have you compared the results of your flow problem with different numerical models, especially with and without nonOrthogonalCorrectors?

Regards Thomas

Hi Thomas,

I don't need the nonOrthogonalCorrectors, since the mesh is really really good. The max. nonOrthogonolaty is very low. However, you are right, you cannot run every mesh without the nonOrthogonalCorrectors. In my case, I compared the results (i.e. drag coefficient) for both simulations (with and without nonOrthogonalCorrectors) and they are really similar, so I conclude that there is no problem for me.

Best regards