CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Problems with interFoam usage (http://www.cfd-online.com/Forums/openfoam-solving/59252-problems-interfoam-usage.html)

vrecha January 4, 2008 08:51

Hi all, I am trying to calcul
 
Hi all,
I am trying to calculate a free surface flow around fixed body using interFoam solver. But I didn't came far ...
What can be seen from the log is that time step keeps decreasing trying to keep the Courant number under specified value. When time step reaches values around 10^(-10) the solver crashes (segmentation fault ...).

What I have already done:
- checked mesh : It reports 131 severely non-orthogonal faces out of 3000000. All other tests are OK, and the checker concludes that mesh is OK.

- played with MaxCo and allowed it even to reach maximum of 0.5 . Made no significiant difference, a solver took a little more time to crash.

- played a little with PISO settings: increased nCorrectors, nNonOrthogonalCorrectors, nGammaCorr, nGammaSubCycles. -> no difference.

Any idea of what to try/do will be appreciated.

Regards,
Damjan.

hjasak January 4, 2008 09:06

Well, it is likely that someth
 
Well, it is likely that something is badly and obviously wrong with the case set-up. Dump the results in every time-step and see where the velocity increases without bounds: what you are seeing is the automatic time-step control trying to "save you" from increasing velocity.

Incidentally, if you're interested, I will be delivering a lecture on my work and OpenFOAM in general at the University of Ljubljana next Thursday (10/Jan/2008) - not too far from you.

Enjoy,

Hrv

caw January 4, 2008 09:12

I would suspect your interFoam
 
I would suspect your interFoam-chrash is caused by a bad mesh. I have observed the same thing on a mesh with big changes in cell size. After remeshing everthing went fine.

Regards
Christian

vrecha January 4, 2008 17:44

Thank you, both suggestions
 
Thank you,

both suggestions were extremely useful. Some pictures of what is going on:

http://lmmri.fri.uni-lj.si/damjan/beforeCrash.png
http://lmmri.fri.uni-lj.si/damjan/beforeCrash_1.png
http://lmmri.fri.uni-lj.si/damjan/beforeCrash_2.png

The problems with velocity arise exactly at mesh seam. So remeshing is inevitable ...

Any othr suggestions/remarks/comments etc are welcome. As you can see I am at a very early stage of learning the art of CFD.


---
PS (to Hrvoje): I will try my best to attend your talk in Ljubljana, tnx for invitation.

caw January 5, 2008 04:34

Yes, i see.... First of all
 
Yes, i see....

First of all, from my experience free surface codes usually do not like tetrahedral meshes. Also size jumps from cell to cell are to be avoided. So for you there are same ways to follow:

1) if you have to stick to tetrahedrons, use reasonable size functions with growth rates of about 1.2
2) Try to use a polyhedra mesh, this can be made out of a tet mesh using polydualmesh in FOAM
3) Best mesh for interFoam (goes for CFD in general) is still a hex mesh, you might want to give this a try. Your geometry is not that complex, so at least a hex dominant mesh shold be possible without to much effort. I heard some rumors about a hexdominant auto-mesher being available in the next release of OF, but there are others available right now as well (harpoon for example, but: commercial)

Suggestion: Use a good tet mesh and convert it to polyhedrons then you should be fine....

Regards
Christian


All times are GMT -4. The time now is 05:19.