Hello! After successfull 2D steady-state Ercoftac results I transfered settings (boundary conditions) to 3D Ercoftac. it runs firm with no error message, but there it diverges very bad.



I have attached the files which I suppose to be important for you. I would be glad, if someone will check it and give me some hints. (Sorry for c&p the files, but couldn't attach normal text files)

FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 2 -2 0 0 0 0];

internalField uniform 0;

boundaryField
{
INTERFACE_R //innenliegender rotierender GGI-Teil
{
type ggi;
// value uniform 0;
}
EINTRITT // hier strömt die Luft in die Maschine
{
type zeroGradient;
// value uniform 0;
}
ROTOR_EINTRITT //Ende des Einlaufkanals und Übergang in den Rotor
{
type ggi;

}
INTERFACE //außenliegender stehender GGI-Teil; Gegenstück zu INTERFACE_R
{
type ggi;
// value uniform 0;
}
EINTRITT_WAND //begrenzt den Einlaufkanal
{
type zeroGradient;
}
EINTRITT_INTERFACE //
{
type ggi;
}
HUB_R
{
type zeroGradient;
}
WAND_ROT
{
type zeroGradient;
}
WAND_STAT
{
type zeroGradient;
}

OUTLET
{
type fixedMeanValue;
meanValue 0;
}
}


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

FoamFile
{
version 2.0;
format ascii;
class volVectorField;
location "0";
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 1 -1 0 0 0 0];

internalField uniform (0 0 0);

boundaryField
{
INTERFACE_R //innenliegender rotierender GGI-Teil
{
type ggi;
value uniform (0 0 0);
}
EINTRITT // hier strömt die Luft in die Maschine
{
type flowRateInletVelocity;
flowRate 0.292;
value uniform (0 0 0);
}
ROTOR_EINTRITT //Ende des Einlaufkanals und Übergang in den Rotor
{
type ggi; //
}
INTERFACE //außenliegender stehender GGI-Teil; Gegenstück zu INTERFACE_R
{
type ggi;
value uniform (0 0 0);
}
EINTRITT_WAND //begrenzt den Einlaufkanal
{
type fixedValue;
value uniform (0 0 0);
}
EINTRITT_INTERFACE
{
type ggi;
}
HUB_R //"Halbkugel" auf dem 1.GGI
{
type movingRotatingWallVelocity;
centre (0 0 0);
axis (0 0 -1);
rpm 2000;
value uniform (0 0 0);
}
WAND_ROT
{
type movingRotatingWallVelocity;
centre (0 0 0);
axis (0 0 -1);
rpm 2000;
value uniform (0 0 0);
}
WAND_STAT // Boden, außen, stillstehend
{
type fixedValue;
value uniform (0 0 0);
}

OUTLET
{
type zeroGradient;
}
}


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

FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSchemes;
}

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

ddtSchemes
{
default backward;
}

gradSchemes
{
default Gauss linear;
grad(p) Gauss linear;
}

divSchemes
{
default none;
div(phi,U) Gauss linearUpwind Gauss;
div((nuEff*dev(grad(U).T()))) Gauss linear;
div(phi,epsilon) Gauss upwind;
div(phi,k) Gauss upwind;
}

laplacianSchemes
{
default none;
laplacian(nu,U) Gauss linear corrected;
laplacian(rAU,pcorr) Gauss linear corrected;
laplacian(rAU,p) Gauss linear corrected;
laplacian(nuEff,U) Gauss linear corrected;
laplacian((1|A(U)),p) Gauss linear corrected;
laplacian(DepsilonEff,epsilon) Gauss linear corrected;
laplacian(DkEff,k) Gauss linear corrected;
laplacian(1,p) Gauss linear corrected;
}

interpolationSchemes
{
default linear;
interpolate(HbyA) linear;
interpolate(1|A) linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
pcorr;
p;
}


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

FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
p
{
solver GAMG;
tolerance 1e-8;
relTol 0.05;

smoother GaussSeidel;

cacheAgglomeration true;

nCellsInCoarsestLevel 20;
agglomerator faceAreaPair;
mergeLevels 1;
}

U
{
solver smoothSolver;
smoother GaussSeidel;
nSweeps 2;
tolerance 1e-7;
relTol 0.1;
}

k
{
solver smoothSolver;
smoother GaussSeidel;
nSweeps 2;
tolerance 1e-7;
relTol 0.1;
}

epsilon
{
solver smoothSolver;
smoother GaussSeidel;
nSweeps 2;
tolerance 1e-7;
relTol 0.1;
}
}

SIMPLE
{
nNonOrthogonalCorrectors 2;
pRefCell 0;
pRefValue 0;
}

relaxationFactors
{
p 0.3;
U 0.7;
k 0.5;
epsilon 0.5;
}

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

So now I can add a little warning for everyone:

If you make a conversion from icemcfd to OpenFoam by typing Fluent3DMeshToFoam check the size of your mesh in Paraview. mm Can be changed into meters.

So you'll have to add fluent3DMeshToFoam -scale 0.001

Remember that! (I hope my mistake will help to avoid such problems at other simulations people do).

Best regards
Christian

Dear Christian and other OpenFOAM® users,

It is good practice to run checkMesh before running any simulation. There you can see the domain extent as a bounding box. The problem you describe is typical when you don't remember that you have made the mesh in mm. You can also see if OpenFOAM® consider any of your control volumes to have negative volume, or any faces to be negative. Note that such things are evaluated differently, so even if your mesh generator sais that the mesh is ok, you should also ask your solver OpenFOAM®/CFX/Fluent... OpenFOAM® might in fact run with negative volumes and faces, but I wouldn't rely much in the results!

When you convert a mesh from any format to any other format, you simply re-organize the point positions and miscellaneous definitions into a new format. That means that if you have a mesh defined in mm, the converted mesh will be in mm. Then you will have to tell your solver that the mesh is in mm so that it can transform it. OpenFOAM® uses m only, so the mesh must be transformed before it is used. As you mention, it can be done with -scale, but also with:
transformPoints -scale "(1e-3 1e-3 1e-3)"

In other CFD solvers you might do it differently, but you need to do it somehow. As they say: Garbage in, garbage out. There is no magic.

Best regards,
Håkan.