[kandelabr]

Hello,

is there a way to speed up temperature convergence in chtMultiRegionSimpleFoam? My velocity residuals have converged long ago but the temperature keeps rising, just awfully slowly.

For instance, could I fake density and/or specific heat because it's a steady state case? Increasing nNonOrthogonalCorrectors in solid regions doesn't help.

Thanks!

[Carlo_P]

Yes, there are at least three options:


-change fvSolution file
-change the fvSchemes file
-initialized in a different way the temperature.


The easiest way is to decrease the tollerance or nMinIt of the velocity and pressure in fvSolution and increase the number of iteration or tollerance of the temperature.


Probably you can also increase the relaxation factor of the temperature.


Can you attach the fvSolution file?
Thanks

[kandelabr]

Here is a fvSolution file for fluid region:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v1906                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    rho
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-7;
        relTol          0;
    }

    p_rgh
    {
        solver           GAMG;
        tolerance        1e-7;
        relTol           0.01;

        smoother         GaussSeidel;

    }

    "(U|h|k|omega|epsilon|G|Ii|gammaInt|ReThetat)"
    {
        solver           PBiCGStab;
        preconditioner   DILU;
        tolerance        1e-8;
        relTol           0.01;


    }

    "(f|v2)"
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-07;
        relTol          0.01;
    }

    G
    {
        $p_rgh;
        tolerance       1e-05;
        relTol          0.1;
    }
}

SIMPLE
{
    consistent yes;
    momentumPredictor yes;
    nNonOrthogonalCorrectors 2;

    // pRefCell        0;
    // pRefValue       100000;

    rhoMin          0.5;
    rhoMax          1.5;
}

relaxationFactors
{
    fields
    {
        rho             1.0;
        p_rgh           0.7;
    }
    equations
    {
        U                   0.5;
        h                   0.5;
        "(k|omega|epsilon|f|v2|gammaInt|ReThetat)" 0.7;
        G                   0.7;
        "ILambda.*"         0.7;
        qr                  0.7;
    }
}

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

And here is the solid region:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  5                                     |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    "h.*"
    {
        solver           PCG;
        preconditioner   DIC;
        tolerance        1e-07;
        relTol           0.01;
    }
}

SIMPLE
{
    nNonOrthogonalCorrectors 10; // faster temperature convergence (?)
}

relaxationFactors
{
    equations
    {
        h 1.0;
    }
}

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

[Carlo_P]

In the fvSolution of the Solid, you are using 10 Correctors,,normally it is not usefull to use more than 3, but only for very "shitty" mesh.
You can change the relTol, decreasing it.

In this way, you will have a faster convergence for the solid.


You can take a look here:
Conjugate Heat Transfer: slow solid temperature convergence





Normally is also not usefull to use 1 as relaxationFactor. Yes, you will have a faster convergence, but maybe it is unsteable, so in the end you can't reach a good convergence.




Can I aks you to share your project or at least the folders,without the geometry?


I would like to do something like this in the short future.

[kandelabr]

Here is my complete chtMultiRegionSimpleFoam case. The mesh is made in a separate directory, then I copy mesh files to simulation/ dir.
Check out readme.txt file for more explanations.

[Bloerb]

Change your h relaxation-factor (or e if you intend to solve for that) to 1.0 in all regions. This is the main cause of extremely slow temperature convergence. You basically shouldn't relax temperature unless you need it for stability. And in that case 0.99 should suffice. Another usefull thing is to use

SIMPLE / or PIMPLE depending on the solver
{
    ...
    frozenFlow yes;
}

This allows you to only solve for the temperature on a velocity field that isn't solved and hence does not change anymore.

[kandelabr]

Thank you, I will try that!