[ufocfd]

Hi guys, I'm trying to use rhoSimplecFoam from the OpenFOAM v2.1.x distribution (therein lies the problem).

It keeps crashing after a few iterations, with what seems to be a density spike, causing the epsilon equation to crash. When I view the solution from just before the crash, I see a high density cell just upstream of the aircraft. I'm imposing limits on the density (0.5min and 2.0max) within the fvSolution file.

Has anyone actually got rhoSimplecFoam (or rhoSimpleFoam for that matter) to work??? My testcase is an aircraft at 100m/sec and I'm using freestream boundaries. rhoSimpleFoam does not even get past the 1st iteration.

I think its likely something to do with the fvSchemes and fvSolution file settings... any help much appreciated. Thanks.

[ufocfd]

...and it seems to have something to do with the location specified in pRefPoint:
pRefPoint (-15 35 35);
pRefValue 100000;

[ufocfd]

Finally got rhoSimpleFoam working for an aircraft at 100m/sec.
Having consistent boundary conditions, and turbulence values,
seems to be the key factors, and not using pRefPoint also.
Got a nice convergence plot from rhoSimpleFoam below.

[vale94]

Originally Posted by ufocfd

Finally got rhoSimpleFoam working for an aircraft at 100m/sec.
Having consistent boundary conditions, and turbulence values,
seems to be the key factors, and not using pRefPoint also.
Got a nice convergence plot from rhoSimpleFoam below.

Hi ufoCFD,
I know quite a lot time has passed, but do you still have the fvschemes and fvsolution to post? I'd like to know how you obtained such a beautiful convergence! Thank you

[ufocfd]

I will have a look for them...

[ufocfd]

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.x |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
default steadyState;
}

gradSchemes
{
default Gauss linear;
}

divSchemes
{
default none;

div(phi,U) Gauss upwind;
div((muEff*dev2(T(grad(U))))) Gauss linear;
div(phi,h) Gauss upwind;
div(phi,epsilon) Gauss upwind;
div(phi,k) Gauss upwind;

div(phid,p) Gauss upwind;
div(phi,K) Gauss upwind;
}

laplacianSchemes
{
default Gauss linear corrected;
}

interpolationSchemes
{
default linear;
UD upwind phid;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
pCorr;
}

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

[ufocfd]

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.x |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
p
{
solver GAMG;
tolerance 1e-08;
relTol 0.1;
smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
nFinestSweeps 2;
cacheAgglomeration true;
nCellsInCoarsestLevel 20;
agglomerator faceAreaPair;
mergeLevels 1;
}

"(U|h|k|epsilon)"
{
solver GAMG;
tolerance 1e-08;
relTol 0.1;
smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
nFinestSweeps 2;
cacheAgglomeration true;
nCellsInCoarsestLevel 20;
agglomerator faceAreaPair;
mergeLevels 1;
}
}

SIMPLE
{
nNonOrthogonalCorrectors 0;
rhoMin rhoMin [1 -3 0 0 0] 0.5;
rhoMax rhoMax [1 -3 0 0 0] 2.0;
transonic no;
}

relaxationFactors
{
fields
{
p 0.3;
rho 0.1;
}
equations
{
// pEqn 0.3;
U 0.5;
h 0.5;
k 0.5;
epsilon 0.5;
}
}

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

[ufocfd]

Those (supplied) are the fvSchemes and fvSolution for the rhoSimple solver.
I have also done same for rhoSimplec solver if you need them.
Contact me on garcfd (at) gmail (dot) com if you need any help.

[vale94]

Thank you very much!

[witega]

Originally Posted by ufocfd

Finally got rhoSimpleFoam working for an aircraft at 100m/sec.
Having consistent boundary conditions, and turbulence values,
seems to be the key factors, and not using pRefPoint also.
Got a nice convergence plot from rhoSimpleFoam below.

Hi ufoCFD,
I know quite a lot time has passed, but do you have also the consistent boundary condition to post? I'd like to know how you obtained such a beautiful convergence, because I'm having a lot of trouble with rhoSimpleFoam! Thank you

[ufocfd]

message me on garcfd@gmail.com and I can look into it for you...