[evrikon]

Hello forum,

I have simulated a steady-state, incompressible, isotherm flow with simplePorousFoam. I rewritten rhoPorousFoam to this task in order to avoid compressibility.

The case runs without problem and converges well. The solution looks good except some few number of cells where the pressure explosures to the very high values (see attached velocity & pressure plot). All of these "bad cells" lie in the porous zone.

I'm currently lloking what is going wrong. my first idea was: well, my mesh which I got form the customer has some defects. But checkMesh does not found any problems. I also checked:

1) if the case works on 1 processor - no changes, still the same strange numerical artefacts in the porous zone.

2) I computed the whole case with 1.5.git - no changes in comparison to 1.5-dev.

3) I tryed to solve further with the standard simpleFoam and recognized that the solution gets more stable. Maximal values for U and p in the field decreases rapidly.

I tried this solver on a simple case (channel flow with porous zone) and it did not produced any difficulties.

Does anybody have any further idea what can be a reason for such strange pressure jumps?

[evrikon]

Fixed it.

I scaled the mesh not in ICEM but with fluent3DMeshtoFoam. And I increased "write precision" in controlDict.

[eugene]

Please post your porousZones file. If you have high differentials in the directional resistances this kind of thing tends to happen. If you are running explicit porosity, I suggest you limit your differential resistance to a factor of 20 or less.

[evrikon]

Hallo eugene,

thank you for comment.
I had the same idea because my porous zone is very anysotropic. It is a honeycomb which has directional multipliers -1000 in the x and y directions. I agree with you that a big multiplier can lead to instabilities because we get a huge source term.

As I wrote I solved the problem by re-writing the mesh with increased tolerance in ICEM, scaling of mesh with fluent3DMeshToFoam and increasing writePrecision in controlDict.


An here is my porousZone if you like:

1
(
FLUID_2
{
coordinateSystem
{
e1 (1 0 0);
e2 (0 1 0);
}

Darcy
{
d d [0 -2 0 0 0 0 0] (0 0 0);
f f [0 -1 0 0 0 0 0] (-1000 -1000 587.8648);
}
}
)

Originally Posted by eugene

Please post your porousZones file. If you have high differentials in the directional resistances this kind of thing tends to happen. If you are running explicit porosity, I suggest you limit your differential resistance to a factor of 20 or less.