CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM (
-   -   GAMG problem in interDyMFoam? (

ribe May 13, 2010 00:07

GAMG problem in interDyMFoam?

I want to combine mesh refinement from interDyMFoam with interPhaseChangeFoam and as a first step I ran a cavitating foil for a while to then having the developed bubble being transported using interDyMFoam. But when I start interDyMFoam I get the following error:

Courant Number mean: 0.00223322 max: 0.161259
Time = 0.160004

Selected 8597 cells for refinement out of 48796.
Refined from 48796 to 108975 cells.
Selected 0 split points out of a possible 8597.
Execution time for mesh.update() = 0.97 s
time step continuity errors : sum local = 0.000223602, global = 3.57329e-13, cumulative = -3.24457e-08

field does not correspond to level 0 sizes: field = 108975 level = 48796

From function void GAMGAgglomeration::restrictField(Field<Type>& cf, const Field<Type>& ff, const label fineLevelIndex) const
in file lnInclude/GAMGAgglomerationTemplates.C at line 48.

This is the second time step, the first went fine. dynamicMeshDict is copied from the damBreak-case.

Any ideas on how to get around this?


sean_mcintyre July 15, 2010 13:29

I've also been experiencing this same problem for quite a while. It doesn't seem that GAMG is currently set up to handle topological changes with meshes. It could be that some other agglomeration method works. I believe that amgSolver out of the 1.5-dev version does handle this, but it might not be readily brought over to 1.6. If anyone has gotten GAMG to work with topology change, I'm sure a lot of us would like to hear about it.

Sean McIntyre

MartinB July 15, 2010 14:13

Hi Sean, hi Rickard,

you must disable the cacheAgglomeration option, i.e. set it to "cacheAgglomeration off;" in fvSolution.


sean_mcintyre July 15, 2010 14:24

Well that certainly does work! Thank you so much Martin. It's actually pretty funny how long I fought with it and never figured that out.

yhaomin2007 July 17, 2013 22:23

1 Attachment(s)
Hey, guys,
How is your adaptive mesh refinement going? I also tried to put AMR in rhoSimplecFoam, now seems it is working. But I met another problem. My case is a 2D case, it seems this AMR can only divide cell into 8 sub cells. Is there any way we can specify the direction it split the cell?
And, this AMR function will make cells really awkward at buffer zone.
Does any one how to get around with this?~

All times are GMT -4. The time now is 13:30.