[ChrisWe]

I'm doing DDES calculation in OpenFoam and want to show me the gridcells, that are calculated with RANS and those that are calculated with LES.

Therefore I created a new turbulenceModel called mySpalartAllmarasDDES that is a simple copy of the standard SpalartAllmarasDDES. There are the following lines in the mySpalartAllmarasDDES.C file:

volScalarField mySpalartAllmarasDDES::dTilda(const volScalarField& S) const
{
    return max
    (
        y_
      - fd(S)
       *max(y_ - CDES_*delta(), dimensionedScalar("zero", dimLength, 0)),
        dimensionedScalar("small", dimLength, SMALL)
    );
}

The first step I want to do is to write out dTilda in the time directories. My Problem is, that dTilda is only virtual as a tmpField.

So my Question is: is there any possibility, to write out tmp-datas?
For example anything like

volScalarField dTilda_output...
(
   NO_READ
   MUST_WRITE...
)

dTilda_output = dTilda;

Thank you all for the amazing help that this forum gives me all the time...

[hismother]

Originally Posted by ChrisWe

I'm doing DDES calculation in OpenFoam and want to show me the gridcells, that are calculated with RANS and those that are calculated with LES.

Therefore I created a new turbulenceModel called mySpalartAllmarasDDES that is a simple copy of the standard SpalartAllmarasDDES. There are the following lines in the mySpalartAllmarasDDES.C file:

volScalarField mySpalartAllmarasDDES::dTilda(const volScalarField& S) const
{
    return max
    (
        y_
      - fd(S)
       *max(y_ - CDES_*delta(), dimensionedScalar("zero", dimLength, 0)),
        dimensionedScalar("small", dimLength, SMALL)
    );
}

The first step I want to do is to write out dTilda in the time directories. My Problem is, that dTilda is only virtual as a tmpField.

So my Question is: is there any possibility, to write out tmp-datas?
For example anything like

volScalarField dTilda_output...
(
   NO_READ
   MUST_WRITE...
)

dTilda_output = dTilda;

Thank you all for the amazing help that this forum gives me all the time...

Does anyone have the answer for this problem??

[Daniel_Khazaei]

Hi, cant you just use the following method? I use it for temperature dependent density to be written during simulation...

tmp<volScalarField> incompressibleTwoPhaseThermoMixture::rho1() const
{
    return tmp<volScalarField>
    (
        new volScalarField
        (
            IOobject
            (
                "rho1",
                mesh_.time().timeName(),
                mesh_,
                IOobject::NO_READ,
                IOobject::AUTO_WRITE
            ),
            rho1_ + linearCoeff1_ * (T().oldTime() - TRef1_)
          + polyCoeff1_ * sqr(T().oldTime() - TRef1_)
        )
    );
}

But it seems that your function returns a volScalarField instead of tmp<volScalarField>, which the above method that I have described may not work for you! (although I can see that it is define as tmp<volScalarField> in my OpenFOAM version, so perhaps we are running different versions)
second method would be to define dTilda as volScalarField globally (don't define it in local scope of your function as you are not allowed to return local variable) and do the calculation in your function and then return it:

in your header file define dTilda_ as private variable:

volScalarField dTilda_;

then initialize it in the constructor in your C file:

    dTilda_
    (
        IOobject
        (
            "dTilda",
            U.time().timeName(),
            U.mesh(),
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
         U.mesh(),
        dimensiondScalar("zero", dimension, scalar(0))

     )