[rdbisme]

Hello,

I searched a bit on the forum and it seems that I'm one of the fewest lucky people that can afford to setup all the six Reynolds stress at the inlet from experimental data .
I'm doing a benchmark simulation to test the behavior of the several turbulence models in that specific case (divergent diffuser) and I would like to see how the RSM models behave.
It's the first time I use RSM models, sorry if I would result a bit unexperienced.

By the way I have experimental points for all the six (uu, uv, uw, vv, vw, ww) Reynolds stress components. In the case of scalar (or vectorial) fields what I do is:

Scalar

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.x                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      omega;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 1;

boundaryField
{
    inlet
    {
        type            groovyBC;
        value           $internalField;
        lookuptables (
            {
                name expInlet;
                outOfBounds clamp;
                fileName    "$FOAM_CASE/inlet/omega.dat";
            }
        );
        valueExpression "expInlet(pos().y)";
    }
    outlet
    {
        type            zeroGradient;
    }

    walls
    {   type            omegaWallFunction;
        value           uniform 1e-6;
    }

    front
    {
        type            wedge;
    }
    
    back
    {   
        type            wedge;
    }

    axis
    {
        type            empty;
    }

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

Vector

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.x                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform (0 0 2);


boundaryField
{
    inlet
    {
        type            groovyBC;
        value           $internalField;
        lookuptables (
            {
                name expInlet;
                outOfBounds clamp;
                fileName    "$FOAM_CASE/inlet/u_14_ort.dat";
            }
        );
        valueExpression "-expInlet(pos().y)*normal()";
    }
    outlet
    {
        type            zeroGradient;
    }

    walls
    {   type            noSlip;
    }

    front
    {
        type            wedge;
    }
    
    back
    {   
        type            wedge;
    }

    axis
    {
        type            empty;
    }
}
// ************************************************************************* //

Can I achieve the same for the R tensor field?

[Gerhard]

I am also interested to test RSM models on the ERCOFTAC conical diffuser for which experimental data is available.

Please let me know whether you managed to figure this out.

Thanks

[Gerhard]

Hi

I think I might have figured it out.
Let me know what you think.

Tensor

/*--------------------------------*- 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       volSymmTensorField;
    object      R;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform (0 0 0 0 0 0);

boundaryField
{
	inlet
    {
	        type			groovyBC;
		value			uniform (0 0 0 0 0 0);

		lookuptables (
			{
				name		Ruu;
				file		"$FOAM_CASE/0/Ruu.data";
				outOfBounds	clamp;
			}
            {
                name		Rww;
                file		"$FOAM_CASE/0/Rww.data";
                outOfBounds	clamp;
            }
            {
                name		Rvv;
                file		"$FOAM_CASE/0/Rvv.data";
                outOfBounds	clamp;
            }
            {
                name		Ruw;
                file		"$FOAM_CASE/0/Ruw.data";
                outOfBounds	clamp;
            }
            {
                name		Ruv;
                file		"$FOAM_CASE/0/Ruv.data";
                outOfBounds	clamp;
            }
            {
                name		Rvw;
                file		"$FOAM_CASE/0/Rvw.data";
                outOfBounds	clamp;
            }
		);

		variables (
			"origin=vector(0,0,0.025);"  // Patch centre (vector)
			"rp=pos()-origin;"           // Radii from centre (vector)
			"r=mag(rp);"				 // Radii from centre (scalar)
			"vv=symmTensor(1,0,0,0,0,0);"
            "vw=symmTensor(0,1,0,0,0,0);"
            "uv=symmTensor(0,0,1,0,0,0);"
            "ww=symmTensor(0,0,0,1,0,0);"
            "uw=symmTensor(0,0,0,0,1,0);"
            "uu=symmTensor(0,0,0,0,0,1);"
            "xDir=vector(1,0,0);"
            "yDir=vector(0,1,0);"
            "zDir=vector(0,0,1);"
		);

        valueExpression "Rvv(r)*vv + Rww(r)*ww + Ruu(r)*uu + Rvw(r)*vw + Ruw(r)*uw + Ruv(r)*uv";
    }

	casing
    {
        type            kqRWallFunction;
        value           $internalField;
    }

    diffuser
    {
        type            kqRWallFunction;
        value           $internalField;
    }

    dump
    {
        type            zeroGradient;
    }

    outlet
    {
        type            zeroGradient;
    }

	axis
	{
		type			symmetryPlane;
	}

	front
	{
		type			wedge;
	}

	back
	{
		type			wedge;
	}
}

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

[silviliril]

I have been trying to simulate nucleate boiling in OpenFOAM. With present model in phaseChangeHeatFoam the wall constant wall temperature can be applied throughout the wall having fixed value. Which generates a thin vapor layer first and then it breaks into several nucleation sites due to density difference. (See bottom nucleation image file attached below)

Now, What I want to do is, apply random value of wall temperature only at certain provided locations (also randomly chosen locations) in lookup table (see posx image file attached below).

I want the nucleation to start only at certain locations and not from entire wall.

One such possibility is to use lookup table feature in groovyBC and another is codedFixedValue BC. But, I could not really figure out that how to use it for my specific purpose.