[lynx]

Hello Foamers,

i have a problem. I simulate a so called "ZickZack"-separator with the "turbFoam" solver.
All solvers and their options are set to default, which means i didn't changed values there in any way. Through this separator flows air with 20 m/s at the outlet ("fixedVelocityOutlet") and the inlet ("pressureInlet") is set to normalpressure.

At first i simulated an empty separator.. all runs fine, which means the residual for the velocities "Ux", "Uy" and "Uz" and the pressure "p" became smaller with the time and i got a good result.

Now i placed some "material" inside, just to place there a few obstacles for the airflow (like the separator in real works). But now the residuals doesn't converge. It converges at first a bit, then it holds the value and then its increasing again and then - finaly - the courant number 'explodes'.
I changed different times the value for "delta_t" (decreased it), but with no improvement.

My question is.. what can i do, to make the residual running smaller? I read about the "under_relaxion factors" in the manual, but i don't find the place where they are stored and how i can change them.

Please can you give me some tips? Thank you in advance.

[graser]

I assume you use "adjustTimeStep yes" and already decreased maxCo

relaxation factors are appended to root/case/system/fvSolution
Here is an example:
SIMPLE
{
...
}

relaxationFactors
{
p 0.2;
U 0.5;
k 0.2;
epsilon 0.2;
}

but they only work for steady state solvers like simpleFoam etc.

maybe you should try to initialize your mesh with potentialFoam:
potentialFoam <root> <case> -writep
another way to initialize is to decrease Reynolds-Number. Therefore lower your velocity or/and increase "nu" in
root/case/constant/transportProperties
After you have initialized your mesh you normally can change velocity and nu back to your desired values.

hf
Max

[lynx]

Hi Max,

at first, thank you for your hints.

1) Okay, relaxation factors are working only with steady state solvers - and so far i'm using "turbFoam", a transient solver, i can't use this
2) The option "adjustTimeStep" with "maxCo" is not available in "turbFoam" - i tried then "rhoTurbFoam", but with no better result..
3) I don't know if i looked right, but i didn't found the solver "potentialFoam" in the drop down menu of the FoamX - any idea where i find him?
4) I solved the problem in editing the mesh from scratch. "checkMesh" did not say something, but i think some skewed faces (4 of them) which i had before, were the problem. And it seems that bigger faces which are a bit skewed ("checkMesh" doesn't warn) are as bad as little faces which are more skewed ("checkMesh" warns)
5) I also changed the number from "nCorrectors" from 2 to 3 and the number from "nOrthogonalCorrectors" from 0 to 2, seems that improved the solution a bit - can you verify this on own experience?

[graser]

1) see my previous post
2) As far as I remember turbFoam and rhoTurbFoam are both capable of using adjustTimeStep. Maybe you just didn't put them in the controlDict? Look at the UserGuide for the available Options in controlDict.
3) I dont't use FoamX so I can't help you with this. But if you just type the command mentioned above potentialFoam should work. Maybe you will have to change the fvSolutions dictionary from PISO to SIMPLE because potentialFoam needs it. From my experience the settings you put in SIMPLE don't matter for potentialFoam. After you ran potentialFoam don't forget to switch back from SIMPLE to PISO.
4) reduced skew Faces and generaly fewer warnings from checkMesh are always positive
5) If I experience instability the first thing I do is to increse nCorrectors and nOrthogonalCorrectors by quite a bit. So from my experience I would do the same...maybe just a little more Correctors (5-10).
But I'm only a student yet so maybe some more experienced CFD expert could comment on how many Correctors to use?