[cutmountain]

Hello everybody,



I am working (trying to ) on an external aerodynamic case with a compressible flow and I need to use a steady state solver.


So I need to use rhoSimpleFoamm but the problem is that I am not able to let it run.



What I know is the velocity field at the inlet Ma=0.6 and the p_inf (static) which is 35000 Pa. So I imposed the correspondent velocity at the inlet and the value of p_inf at the outlet.



At first I had the problem that the sim was not able to start, but then I managed to limit the temperature between a maximum value and a minimum value and the sim started but after 50 iteration I had the temperature residual equal to 1 and then crashed.



I know that the problem is due to the BCs.



I add the BCs for U,T,p. Let me know if u need something else.


T

dimensions      [0 0 0 1 0 0 0];

internalField   uniform 236;

boundaryField
{
    inlet
    {
        type            fixedValue;
        value           uniform 236;
    }

    outlet
    {
        type            inletOutlet;
        value           uniform 236;
        inletValue      uniform 236;
    }

    "nose|body|wings|tail"
    {
        type            fixedValue;
        value           uniform 236;
    }    
    SphereW
    {
        type            cyclicAMI;
        value           $internalField;
    }
    SphereS
    {
        type            cyclicAMI;
        value           $internalField;
    }

}

U

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

internalField   uniform (0 0 0);

boundaryField
{
    inlet
    
    {
    type        fixedValue;
    value        uniform (0 185 0);
    }
                    
    

    outlet
    {
        type            zeroGradient;
    }

    "nose|body|wings|tail"
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    SphereW
    {
        type            cyclicAMI;
        value           $internalField;
    }
    SphereS
    {
        type            cyclicAMI;
        value           $internalField;
    }

}

p

dimensions      [1 -1 -2 0 0 0 0];

internalField   uniform 35687;

boundaryField
{
    inlet
    {
        type            zeroGradient;

    }
    outlet
    {
        type        fixedValue;                    
        value           uniform  35687;
    }
    "nose|body|wings|tail"
    {
        type            zeroGradient;
    }
    SphereW
    {
        type            cyclicAMI;
        value           $internalField;
    }
    SphereS
    {
        type            cyclicAMI;
        value           $internalField;
    }

Cheers,


CutMountain.

[Swagga5aur]

Hello cutmountain, would it be possilbe to upload the case for potential debugging? It could be an issue with fv solution oe schwme, I had a similar problem recently, being due to no residual control of h as e was specified inatead.
Regards Lasse

[cutmountain]

Dear Swagga,



thanks for caring.



here there are my fvSolution, fvSchemes and fvOptions.



I hope that my problem is the same as yours. You think that the boundary conditions are well posed?






fvSolution

solvers
{
    p
    {
        solver          GAMG;
        tolerance       1e-08;
        relTol          0.1;
        smoother        GaussSeidel;
        nCellsInCoarsestLevel 20;
    }

    "(U|e|k|omega)"
    {
        solver          GAMG;
        tolerance       1e-08;
        relTol          0.1;
        smoother        GaussSeidel;
        nCellsInCoarsestLevel 20;
    }
}

SIMPLE
{
    nNonOrthogonalCorrectors 10;
    rhoMin          0.1;
    rhoMax          10.0;
    transonic       no;
    consistent      yes;


}

relaxationFactors
{
    fields
    {
        p               0.4;
        rho             0.01;
    T        0.01;
    }
    equations
    {
        p               0.4;
        U               0.6;
        e               0.4;
        k               0.6;
        omega           0.6;
    }
}

fvSchemes

 ddtSchemes
{
    default         steadyState;
}

gradSchemes
{
    default         cellLimited Gauss linear 0.333;
}

divSchemes
{
    default         none;

    div(phi,U)                         bounded Gauss upwind;
    div(phi,k)                       bounded Gauss upwind;
    div(phi,omega)                   bounded Gauss upwind;
    div(((rho*nuEff)*dev2(T(grad(U)))))     Gauss linear;
    div(phi,e)                  bounded Gauss upwind;
    div(phid,p)                 bounded Gauss upwind;
    div(phi,Ekp)                bounded Gauss upwind;
    div((phi|interpolate(rho)),p)      bounded Gauss upwind;


}

laplacianSchemes
{
    default         Gauss linear uncorrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         limited 0.333;
}

wallDist
{
method meshWave;
}


fluxRequired
{
    default         no;
    p               ;
}

fvOptions

limitT
{
    type        limitTemperature;
    active        true;

    limitTemperatureCoeffs
    {
        Tmin         30;
        Tmax            1000;
        selectionMode     all;
    }
}

Cheers,



CutMountain.

[Swagga5aur]

How does your thermophysical property file look?
I havn't used cyclicAMI before, but could you give an illustration of the domain with the different patch names?

I would suggest simply changing all the patches that aren't inlet or outlet to a simple wall to determine if its the boundary conditions, however the conditions seems fine from an initial glance.

Just a side note is it correct that the temperature is 236Kelvin?

Regards Lasse

[cutmountain]

This is the thermo

thermoType
{
    type            hePsiThermo;
    mixture         pureMixture;
    transport       sutherland;
    thermo          hConst;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleInternalEnergy;
}

mixture
{
    specie
    {
        nMoles      1;
        molWeight   28.9;
    }
    thermodynamics
    {
        Cp          1005;
        Hf          0;
    }
    transport
    {
        As          1.4792e-06;
        Ts          116;
    }
}

The domain is a body inside a "windtunnel" that has a shape close to a bullet so I have just an inlet (the lateral surface of the bullet) and the outlet. I used the AMI because I had done two mesh separately and then merged because later I will have the necessity to turn the geometry, so instead of remeshing everytime I just rotate one of the two mesh and then I will merge them.



But this work because I firt run some incompressible sim and they went very well and all of them converged.



Maybe this mesh done in that way is not good for the compressible solver? (I can try to have a unique mesh and see if it works in that way)



But the think that (from what I've learned, cause I always did incompressible sim) the pressure boundary conditions works differently between inc and compr solver so my concern is about the pressure BC. You think that it is ok?

[Swagga5aur]

I don't see any issues with your pressure BC's, maybe check out the tutorial case in tutorials->compressible->rhoSimpleFoam->angledDuctExplicitFixedCoeff or aerofoilNACA0012 for some comparability to your case.

Note that the tutorials are based upon openFOAM v6 don't know if its different from other distributions.

You are welcome to share your case if able, I'm not certain what else to suggests.

You could try the following fvSolution code:

solvers
{
    p
    {
        solver          GAMG;
        tolerance       1e-08;
        relTol          0.1;
        smoother        GaussSeidel;
        nCellsInCoarsestLevel 20;
    }

    "(U|e|k|omega)"
    {
        solver          GAMG;
        tolerance       1e-08;
        relTol          0.1;
        smoother        GaussSeidel;
        nCellsInCoarsestLevel 20;
    }
}

SIMPLE
{
    nNonOrthogonalCorrectors 10;
    pMinFactor          0.1;
    pMaxFactor          10.0;
    transonic       yes;
    consistent      yes;


}

relaxationFactors
{
    fields
    {
        p               1;
    }
    equations
    {
        p               1;
        U               0.9;
        e               0.8;
        k               0.9;
        omega       0.9;
    }
}

[giovanni.medici]

Have you tried decreasing the number of SIMPLE -> nNonOrthogonalCorrector,?
As you are solving with a steady state solver, there is no requirement of convergence on each tilmestep, you will reach it through relaxation factor. If the reason of an high nNonOrthogonalCorrector is mesh quality, I would tackle that problem in the first place.
You may find some interesting infos here:

• OFtipsandtricks.pdf
• non-orthogonal-correction-simplefoam thread

By the way rhoSimpleFoam is a quite picky solver, hence maybe an initialization of the flow field (in particular U), with potentialFoam may help.
Have you tried initializing the U domain with potentialFoam? and with an internal value different than 0 (in your case something like (0 185 0) )?

In order to cross check BC may I suggest you to take a look to the aerofoilNACA0012 tutorial?

[mAlletto]

Maybe it's a bit late but there is a OneraM6 wing tutorial available which was run with rhoSimpleFoam:


https://wiki.openfoam.com/OneraM6_by_Michael_Alletto