CFD Online Discussion Forums - Problem running simpleFoam with kOmegaSST turbulence model

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

- - Problem running simpleFoam with kOmegaSST turbulence model (https://www.cfd-online.com/Forums/openfoam-solving/108774-problem-running-simplefoam-komegasst-turbulence-model.html)

Problem running simpleFoam with kOmegaSST turbulence model

Hello,
I'm trying to run a channel-case (4m^2) with a smaller cross-section (0.05m^2) in between. My boundary-conditions are:

Code:

inlet_velocity (0.3 0 0)

inlet_pressure zeroGradient

inlet_k uniform 2e-04

inlet_omega uniform 0.2

inlet_nut uniform 0



outlet_velocity zeroGradient

outlet_pressure uniform 0

outlet_k zeroGradient

outlet_omega zeroGradient

outlet_nut uniform 0



wall_velocity (0 0 0)

wall_pressure zeroGradient

wall_k kqRWallFunction uniform 2e-04

wall_omega omegaWallFunction uniform 0.2

wall_nut nutkWallFunction uniform 0

fvSchemes:

Code:

ddtSchemes

{

    default         steadyState;

}



gradSchemes

{

    default         Gauss linear;

}



divSchemes

{

    default         none;

    div(phi,U)      Gauss linear;

    div(phi,k)      Gauss linear;

    div(phi,omega)  Gauss linear;

    div((nuEff*dev(T(grad(U))))) Gauss linear;

}



laplacianSchemes

{

    default         Gauss linear corrected;

}



interpolationSchemes

{

    default         linear;

}



snGradSchemes

{

    default         corrected;

}



fluxRequired

{

    default         no;

    p;

}

and finally fvSolution:

Code:

solvers

{

    p

    {

        solver           GAMG;

        tolerance        1e-06;

        relTol           0.01;

                smoother         DICGaussSeidel;

        cacheAgglomeration on;

                agglomerator         faceAreaPair;

        nCellsInCoarsestLevel 50;

        mergeLevels      1;

    }

    U

    {

        solver           PBiCG;

                preconditioner         DILU;        

                tolerance        1e-05;

        relTol           0.1;

    }

    k

    {

        solver           PBiCG;

                preconditioner         DILU;

        tolerance        1e-05;

        relTol           0.1;

    }



    omega

    {

        solver           PBiCG;

        preconditioner          DILU;

                tolerance        1e-05;

        relTol           0.1;

    }

}



SIMPLE

{

    nNonOrthogonalCorrectors 0;

}



potentialFlow

{

    nNonOrthogonalCorrectors 10;

}



relaxationFactors

{

    fields

    {

        p               0.3;

    }

    equations

    {

        U               0.7;

        k               0.7;

                epsilon                        0.7;

        omega           0.7;

                nuTilda                        0.7;

                R                                0.7;

    }

}

The problem is that the calculation diverges with bounding k and omega. Any suggestions?

can you post images of the mesh? have you tried to visualize where the k and omega rises to high values?

Quote:

Originally Posted by sail (Post 389663)

can you post images of the mesh? have you tried to visualize where the k and omega rises to high values?

there is no defined location where the k and omega values reach the high values. it depends on the timestep... attached you can find two screenshots of a slice through the fluid domain.

mmm the mesh looks good from here,

are the layers correctly added even in the corners?

maybe increasing the number of nonOrtogonalCorrectors in the simple loop?

if the issue arises in the early timesteps you might want to try to increase the value of the initial omega internal field to artificially stabilize the solution.

this is what comes to mind right now...

tried to solve it without turbulence, but also no convergence. I have no idea what the problem is...

Hi,

Just looking at your fvSchemes, try changing:

Code:

divSchemes

{

    default         none;

    div(phi,U)      Gauss linear;

    div(phi,k)      Gauss linear;

    div(phi,omega)  Gauss linear;

    div((nuEff*dev(T(grad(U))))) Gauss linear;

}

to:

Code:

divSchemes

{

    default         none;

    div(phi,U)      Gauss GammaV 0.5;

    div(phi,k)      Gauss Gamma 0.5;

    div(phi,omega)  Gauss Gamma 0.5;

    div((nuEff*dev(T(grad(U))))) Gauss linear;

}

You are now introducing some filtering, because I doubt that you have the required resolution (Cell Reynolds number <2) for pure central differencing (linear scheme). Or maybe look at limitedLinear instead of Gamma.

You may even want to use upwind for the turbulence variables if that is needed for convergence, to my experience the end result is not affected significantly.

Especially if you have a lot of nonOrthogonality this may help:

Code:

laplacianSchemes

{

    default         Gauss linear limited 0.333;

}

Regards,
Tom