[Tobi-R]

Hi,

I have a problem running a case with SimpleFoam. The geometry is quite complex. I'm running the case with turbulence off. I made the mesh with netgen (1.4M cells, no layers). As you can see in the attached File the case doesn't converge although the solution looks physical to me.
My checkMesh complains only about some non-orthogonal Faces and a lot of under-determined Cells.
Could these cells effect the convergence?
Or what can I change in fvSolution / fvSchemes so that the case converge?

Thanks in advance.

Checking geometry...
Overall domain bounding box (-876.472 -48 -63.9999) (884.528 48 273)
Mesh (non-empty, non-wedge) directions (1 1 1)
Mesh (non-empty) directions (1 1 1)
Boundary openness (2.12129e-17 -1.9514e-16 1.29017e-16) OK.
Max cell openness = 3.51972e-16 OK.
Max aspect ratio = 33.8371 OK.
Minumum face area = 0.146015. Maximum face area = 287.294. Face area magnitudes OK.
Min volume = 0.0386411. Max volume = 1541.7. Total volume = 3.29777e+07. Cell volumes OK.
Mesh non-orthogonality Max: 84.8534 average: 16.5116
*Number of severely non-orthogonal faces: 42.
Non-orthogonality check OK.
<<Writing 42 non-orthogonal faces to set nonOrthoFaces
Face pyramids OK.
Max skewness = 1.45798 OK.
Min/max edge length = 0.224133 28.1059 OK.
All angles in faces OK.
All face flatness OK.
Cell determinant (wellposedness) : minimum: 0 average: 1.36798
***Cells with small determinant found, number of cells: 10537
<<Writing 10537 under-determined cells to set underdeterminedCells

Failed 1 mesh checks.

End

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.0.0 |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
default steadyState;
}

gradSchemes
{
default Gauss linear;
}

divSchemes
{
default Gauss linear;
div(phi,U) Gauss linearUpwindV Gauss linear
div(phi,k) Gauss upwind;
div(phi,omega) Gauss upwind;
div((nuEff*dev(T(grad(U))))) Gauss linear;
div((nuEff*dev(grad(U).T()))) Gauss linear;
}

laplacianSchemes
{
default Gauss linear corrected;
}

interpolationSchemes
{
default linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
}

// ************************************************** *********************** //

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.0.0 |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
p
{
solver GAMG;
tolerance 1e-7;
relTol 0.1;
smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2; //2
cacheAgglomeration on;
agglomerator faceAreaPair;
nCellsInCoarsestLevel 10;
mergeLevels 1;
}

U
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1; //1
}

k
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}

omega
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}
}

SIMPLE
{
nNonOrthogonalCorrectors 0;
}

potentialFlow
{
nNonOrthogonalCorrectors 10;
}

relaxationFactors
{
p 0.3;
U 0.7;
k 0.7;
omega 0.7;
}

cache
{
grad(U);
}

// ************************************************** *********************** //

[wyldckat]

Greetings Tobi-R and welcome to the forum!

You better try removing those undetermined cells: http://openfoamwiki.net/index.php/SetSet

The best solution would be for the mesh to be "100% OK" according to checkMesh, but since there are strange cells in it, you would either have to edit the mesh manually to fix it (I don't know how to do that), or you can use the setSet utility to manipulate the mesh based on the sets created by checkMesh.

Best regards and good luck!
Bruno

[chegdan]

Tobi-R

I encountered this a lot over the summer and tried to figure out how to remove these. Though i am not exactly sure what under-determined cells can do to the solution (if anyone can answer i would appreciate that as well), i do know that more of them correlated to terrible convergence. The best and possibly quickest solution I can offer is to re-mesh your geometry. I know you say it's a complex one, but you might better off in the long run. I ended up moving to extremely small mesh sizes (with more than 20 million delauney tetrahedral cells) and then converting it to a polyhedral mesh (less than 8 million cells). This of course has its own problems, but you will get better results (from my experience of course). Good luck and I hope this helps.

Dan

[Tobi-R]

Hi,

thanks for the answers. Unfortunately none of your hints worked. I tried to work with the setSet utility as well as converting the mesh into a polyhedral mesh but both just made things even worse.
I also tried to re-mesh the geometry. I made a finer mesh with Netgen ( ~5 million Cells) an 3 different meshes with EnGrid (1, 2.5, 8 million Cells) . All of them blew up except the mesh made with Engrid with ~8 million Cells and the results looks nearly the same as in the first post, although the checkMesh is better ( only ~ 50 under-determined cells but ~5000 non-orthogonal faces). The other EnGrid meshes had also just ~ 50 under-determined cells and only ~50 non-orthogonal faces.

Has anyone another hint what I can do?

[Aurelien Thinat]

Hi Tobi,

I didn't face problems with underdetermined cells. But I already faced problems with cells non-orthogonality : you have to change your fvScheme.

"divSchemes
{
default Gauss linear;
div(phi,U) Gauss linearUpwindV Gauss linear
div(phi,k) Gauss upwind;
div(phi,omega) Gauss upwind;
div((nuEff*dev(T(grad(U))))) Gauss linear;
div((nuEff*dev(grad(U).T()))) Gauss linear;
}

laplacianSchemes
{
default Gauss linear corrected;
}
"

These schemes are used on "perfect" mesh only and you have to use limited 0,5 (or 0,33) schemes, it depends on the mesh's quality.