CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   interFoam: hydrostatic pressure drives flow in non-orthogonal mesh (http://www.cfd-online.com/Forums/openfoam-solving/75980-interfoam-hydrostatic-pressure-drives-flow-non-orthogonal-mesh.html)

 kaergaard May 11, 2010 05:23

interFoam: hydrostatic pressure drives flow in non-orthogonal mesh

1 Attachment(s)
Dear Forum.
I have a problem wiith interFoam. With a plane water surface and no flow trough any boundaries I get a flow along the bottom boundary when the mesh elements near the boundary are non-orthogonal. I expected zero velocity everywhere.
The flow velocity increases as time goes and ends up blowing up the computation. I have attatched an image showing the same simulation with slightly different meshes the top one has a maximum non-orthogonality of 65, the middle 35 and the bottom 15 (mesh is made using snappyMesh). The shown time is 0.01 s.
I would like to be able to run the simulaiton with a larger non-orthogonality since this will describe my bottom better. I have tried
nOrthoCorrectors = 5, with no improvement, I have also tried different combinations of schemes for laplace (MUSCL uncorrected, corrected linear, upwind), and div (MUSCL, upwind, linear). Any ideas are most welcome.

Best regards Kasper

My fvSolution file is:
solvers
{
pcorr PCG
{
preconditioner DIC;
tolerance 1e-10;
relTol 0;
};
p PCG
{
preconditioner DIC;
tolerance 1e-10;
relTol 0;
};
pFinal PCG
{
preconditioner DIC;
tolerance 1e-10;
relTol 0;
};
U PBiCG
{
preconditioner DILU;
tolerance 1e-10;
relTol 0;
};
}

PISO
{
pdRefCell 0;
pdRefValue 0;
momentumPredictor yes;
nCorrectors 3;
nNonOrthogonalCorrectors 5;
nAlphaCorr 1;
nAlphaSubCycles 1;
cAlpha 1;
}
fvSchemes:
ddtSchemes
{
default Euler;
}

{
default Gauss linear;
}

divSchemes
{
default Gauss linear;
// div(rho*phi,U) Gauss MUSCL;
// div(phi,alpha) Gauss vanLeer;
// div(phirb,alpha) Gauss interfaceCompression;
}

laplacianSchemes
{
default Gauss upwind phi corrected;
}

interpolationSchemes
{
default linear;
}

{
default corrected;
}

fluxRequired
{
default yes;
p;
pcorr;
alpha;
}

 m.afshar September 28, 2010 12:40

Hi Casper

I have faced the same problem as you. The case is a 3D wave tank with a sloping bed. For a simple test (still water in the basin with hydrostatic pressure and no wave) interFoam gives non-physical flows over and around the sloping bed. The DeltaT decreases continuously and finally the run blows up.
Could you please kindly tell me if you have found any way out of this problem?

Best Regards
Mostafa

 kaergaard September 29, 2010 05:17

 cheng1988sjtu September 5, 2011 10:56

Could you explain how you solve the problem?

Hi kaergaard,

Since I'm sending wave into a box at one inlet, and top as atmosphere, other 4 walls. however, It keeps blowing up after few seconds of simulation.
Could you share with us how you solve the problem? Thanks !

Zhen

Quote:
 Originally Posted by kaergaard (Post 277065) As I remember: use quad as grad scheme :)

 kaergaard September 6, 2011 01:09

An even better solution to solve the original problem in this thread is to upgrade to openfoam 1.7.x where the formulation in interfoam has been changed back so it again (like in 1.5.x) solve for excess pressure. Since I switched to 1.7.x I have not has the problem.

Zhen: I don't think I can help with your wave simulation which is blowing up, but an idea is to use upwing scheme for all your divergence schemes and all your interpolation schemes.

 cheng1988sjtu September 6, 2011 07:39

Thanks, runs wells now!

Hi kaergaard,