[lourencosm]

Hello,

I'm trying to calculate the tke in interfoam but I can't call k.
This file goes next to the Courant calculation in the solver structure.
Can anybody help me to call k? Thank you.

This is the code:

scalar TkeSum = 0.0;

if (mesh.nInternalFaces())
{
    scalarField Tke (rho*mesh.V().field()*k);
    TkeSum = gSum(Tke);
}

Info<< "All phases tke: " << TkeSum << endl;
Info<< "tke units: kg*m^2/s^2" << endl;
Info<< "  " << endl;

I get this error:

allTke.H: In function ‘int main(int, char**)’:
allTke.H:39:43: error: ‘k’ was not declared in this scope
     scalarField Tke (rho*mesh.V().field()*k);
                                           ^
allTke.H:39:43: note: suggested alternative:
In file included from /opt/OpenFOAM/OpenFOAM-2.2.2/src/OpenFOAM/lnInclude/constants.H:46:0,
                 from /opt/OpenFOAM/OpenFOAM-2.2.2/src/finiteVolume/lnInclude/fvCFD.H:17,
                 from ihFoamLSM.C:69:
/opt/OpenFOAM/OpenFOAM-2.2.2/src/OpenFOAM/lnInclude/fundamentalConstants.H:79:36: note:   ‘Foam::constant::physicoChemical::k’
     extern const dimensionedScalar k;
                                    ^

[T.D.]

Hi lourencosm,

You should do: scalarField Tke (rho*mesh.V().field()*k.value());


Best Regards,

GoodLuck !

T.D.

Originally Posted by lourencosm

Hello,

I'm trying to calculate the tke in interfoam but I can't call k.
This file goes next to the Courant calculation in the solver structure.
Can anybody help me to call k? Thank you.

This is the code:

scalar TkeSum = 0.0;

if (mesh.nInternalFaces())
{
    scalarField Tke (rho*mesh.V().field()*k);
    TkeSum = gSum(Tke);
}

Info<< "All phases tke: " << TkeSum << endl;
Info<< "tke units: kg*m^2/s^2" << endl;
Info<< "  " << endl;

I get this error:

allTke.H: In function ‘int main(int, char**)’:
allTke.H:39:43: error: ‘k’ was not declared in this scope
     scalarField Tke (rho*mesh.V().field()*k);
                                           ^
allTke.H:39:43: note: suggested alternative:
In file included from /opt/OpenFOAM/OpenFOAM-2.2.2/src/OpenFOAM/lnInclude/constants.H:46:0,
                 from /opt/OpenFOAM/OpenFOAM-2.2.2/src/finiteVolume/lnInclude/fvCFD.H:17,
                 from ihFoamLSM.C:69:
/opt/OpenFOAM/OpenFOAM-2.2.2/src/OpenFOAM/lnInclude/fundamentalConstants.H:79:36: note:   ‘Foam::constant::physicoChemical::k’
     extern const dimensionedScalar k;
                                    ^

[lourencosm]

Thank you T.B. but it still no working.

(k is meant to be from the k-epsilon turbulent model)
Now I get this error:

allTke.H: In function ‘int main(int, char**)’:
allTke.H:40:43: error: ‘k’ was not declared in this scope
     scalarField Tke (rho*mesh.V().field()*k.value());
                                           ^
allTke.H:40:43: note: suggested alternative:
In file included from /opt/OpenFOAM/OpenFOAM-2.2.2/src/OpenFOAM/lnInclude/constants.H:46:0,
                 from /opt/OpenFOAM/OpenFOAM-2.2.2/src/finiteVolume/lnInclude/fvCFD.H:17,
                 from ihFoamLSM.C:69:
/opt/OpenFOAM/OpenFOAM-2.2.2/src/OpenFOAM/lnInclude/fundamentalConstants.H:79:36: note:   ‘Foam::constant::physicoChemical::k’
     extern const dimensionedScalar k;
                                    ^

Thank you.

[alexeym]

Hi,

@lourencosm

Where do you try to add this code? Inside the solver, inside the turbulence model, somewhere else?

Compiler tried to do its best to guess what you are trying to say, but was not successful as he suggested you Boltzmann constant instead of kinetic turbulent energy.

[lourencosm]

In the interfoam.C file, therefore the solver main file.

int main(int argc, char *argv[])
{
    #include "setRootCase.H"
    #include "createTime.H"
    #include "createMesh.H"

    pimpleControl pimple(mesh);

    #include "initContinuityErrs.H"
    #include "createFields.H"
    #include "readTimeControls.H"
    #include "correctPhi.H"
    #include "CourantNo.H"
    #include "setInitialDeltaT.H"


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

    Info<< "\nStarting time loop\n" << endl;

    while (runTime.run())
    {
        #include "readTimeControls.H"
        #include "CourantNo.H"
        #include "alphaCourantNo.H"
        #include "allTke.H"                            //-------------------here!!
        #include "setDeltaT.H"

        runTime++;

        Info<< "Time = " << runTime.timeName() << nl << endl;

[alexeym]

Hi,

In this case you have turbulence variable of type autoPtr<incompressible::turbulenceModel> turbulence, which is created in createFields.H file. incompressible::turbulenceModel class has k method which returns TKE.

So finally your code should be something like:

dimensionedScalar totalTKE(fvc::domainIntegrate(rho*turbulence->k()));

[lourencosm]

Thank you very much alexeym!

I was driving nuts!
I had already tried RASModel->k() and turbulenceModel->k() with no result. Thank you.

I ended up by using this function because I need the air, water and interface values as well:

scalar waterTkeSum = 0.0;
scalar airTkeSum = 0.0;
scalar interfaceTkeSum = 0.0;
scalar TkeSum = 0.0;

if (mesh.nInternalFaces())
{
    scalarField Tke(rho*turbulence->k());

    scalarField water (neg(0.99 - alpha1));
    scalarField waterTke(water*Tke);

    scalarField air (neg(alpha1 - 0.01));
    scalarField airTke (air*Tke);

    scalarField interface (pos(alpha1 - 0.01)*pos(0.99 - alpha1));
    scalarField interfaceTke (interface*Tke);

    waterTkeSum = gSum(waterTke);
    airTkeSum = gSum(airTke);
    interfaceTkeSum = gSum(interfaceTke);
    TkeSum = gSum(Tke);
}

Info<< "All phases tke: " << TkeSum << endl;
Info<< "Water tke : " << waterTkeSum << endl;
Info<< "Air tke : " << airTkeSum << endl;
Info<< "Interface tke : " << interfaceTkeSum << endl;
Info<< "tke units: kg*m^2/s^2" << endl;
Info<< "  " << endl;