[petr.f.]

Hi guys,

recently I've been playing with chtMultiRegionFoam but cannot get it to work. My test case is simple - an iron ball hanging in the air with the initial temperature of 300 K over which I blow the air with temperature of 620 K. I'd like to see the ball slowly heating. However in a really short time the temperature in the vicinity of the ball starts to drop and continues dropping towards the absolute zero until the solver diverges. I attach the configuration files - nothing fancy, I've just used the tutorial settings and tweaked them a bit. The mesh is generated in snappy and is of quite a decent quality.

the max Courant Nos I use are
maxCo 0.5;
// Maximum diffusion number
maxDi 10.0;

and for the boundary conditions for temperature I prescribe the standard options for inlet/outlet and for T
fluid region:
domain0_to_ball
{
type compressible::turbulentTemperatureCoupledBaffleMix ed;
value uniform 620;
Tnbr T;
kappaMethod fluidThermo;
}

solid region:
ball_to_domain0
{
type compressible::turbulentTemperatureCoupledBaffleMix ed;
value uniform 300;
Tnbr T;
kappaMethod solidThermo;
}


I've done quite a lot computations with chtMultiRegionSimpleFoam but never seen such a behaviour... So any help would be really appreciated.

Configuration for the fluid region:
fvSchemes

ddtSchemes
{
    default                   Euler;
}

gradSchemes
{
    default                   Gauss linear;
    grad(U)                   cellLimited Gauss linear 1;
}

divSchemes
{
    default                   none;
    
    div(phi,U)                bounded Gauss linearUpwindV grad(U);
    
    div(phi,h)                bounded Gauss upwind;
    div(phi,e)                bounded Gauss upwind;
    div(phi,K)                bounded Gauss upwind;
    div(phi,k)                bounded Gauss upwind;
    div(phi,R)                bounded Gauss upwind;
    div(R)                    Gauss linear;
    div(phi,epsilon)          bounded Gauss upwind;
    div(phi,omega)          bounded Gauss upwind;
   div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
    default                   Gauss linear corrected;
}

interpolationSchemes
{
    default                     linear;
}

wallDist
{
    method meshWave;
}

snGradSchemes
{
    default                   corrected;
}

fluxRequired
{
    default                     no;
    p;
}

fvSolution

solvers
{
    rho
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-7;
        relTol          0.1;
    }

    rhoFinal
    {
        $rho;
        tolerance       1e-7;
        relTol          0;
    }
    
    "(p_rgh|p)"
    {
        solver           GAMG;
        tolerance        1e-7;
        relTol           1e-2; // def. 1e-2
        smoother         DICGaussSeidel;
        nPreSweeps       0;
        nPostSweeps      2;
        cacheAgglomeration on;
        agglomerator     faceAreaPair;
        nCellsInCoarsestLevel 10;
        mergeLevels      1;
        minIter          2;
        maxIter          50;
    }
    
    p_rghFinal
    {
        $p_rgh;
        tolerance        1e-7;
        relTol           0;
    }    

    "(U|h|e|k|epsilon|omega|R)"
    {
        solver           smoothSolver;
        smoother         DILUGaussSeidel;
        tolerance        1e-7;
        relTol           0.1;//0.01;// def. 0.1;
        nSweeps          2;
    }
    
    "(U|h|e|k|epsilon|omega|R)Final"
    {
        $U;
        tolerance        1e-7;
        relTol           0;
    }
}


PIMPLE
{
    momentumPredictor   on;
    nCorrectors         2;
    nOuterCorrectors    2;
    nNonOrthogonalCorrectors 0;
}


relaxationFactors
{
  rho               1;
  "(p_rgh|p)"       0.7;  
  U                 0.3;
  "(h|e)"           0.3;

  k                 0.8;
  "(epsilon|omega)" 0.8;
}

Configuration for the solid region:
fvSchemes:

ddtSchemes
{
    default Euler;
}

gradSchemes
{
    default         Gauss linear;
}

divSchemes
{
    default         none;
}

laplacianSchemes
{
    default             none;
    laplacian(alpha,h)  Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}

fvSolution

solvers
{
    h
    {
        solver           PCG;
        preconditioner   DIC;
        tolerance        1e-06;
        relTol           0.1;
    }

    hFinal
    {
        $h;
        tolerance        1e-06;
        relTol           0;
    }
}

PIMPLE
{
    nNonOrthogonalCorrectors 0;
}

P.

[petr.f.]

Got it solved - the (obvious) error was in usage of the bounded schemes, should anyone be interested...

[manuc]

@petr.f.
How did u solve this issue , Is it just by using some unbounded schemes?
Thanks

[petr.f.]

Just remove the "bounded" keyword. Detailed explanation is here:

http://openfoam.org/release/2-2-0/numerics-boundedness/