CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM (https://www.cfd-online.com/Forums/openfoam/)

- - Laplacian(A*B) (https://www.cfd-online.com/Forums/openfoam/122138-laplacian-b.html)

you could try to implement it implicitly
fvc::laplacian(delta*F,Psat) = fvc::div( delta*F*grad(Psat) )

volVectorField dps = delta * fvc::grad(Psat);
surfaceScalarField dpsf = fvc::interpolate(dps) & mesh.Sf();

then you can view the dps field as a 'convective' change of F due to the Psat gradient
and rewrite it like this

fvc::laplacian(delta*F,Psat) = fvm::div(dpsf, F)

...should work

Hi

That's a pitty. But the code of niklas seems to be promissing. Ricardo, I didn't get your approach in total. Could you explain it in a little more detail? Especially the part of the lduAddressing.

Regards

Fabian

Quote:

Originally Posted by niklas (Post 445771)

fvc::laplacian(delta*F,Psat) = fvm::div(dpsf, F)
...should work

implementation to solver >> solve (fvm::ddt(dw,F)==fvm::laplacian(lambdaD*Psat,F)+fv m::div(dpsf, F)); doen't works, too :(

Quote:

Originally Posted by fabian_roesler (Post 445791)

This is my code, but it I am still working ...

a part of code ...

Code:

    float tdelta = 1.0;

    float tdeltaN = 1.0;

    

    float fdelta = 1.0;

    float fdeltaN = 1.0;



    double relFaktor = 1.0;

    int iter = 0;

    

    #include "boundaryCalculation.H"

    

    do 

    {



    Tt = T;

    

    #include "heatParameters.H"



    solve

            (

               fvm::ddt(cap,T)==fvm::laplacian(lambda, T)//+hv*fvc::laplacian(lambdaD, Psat*F)

         );



    T=(relFaktor)*T+(1-relFaktor)*Tt;

    

    tdeltaN=diffFields(T,Tt);



    #include "saturatedpressure.H"

    #include "moistureParameters.H"





    fvScalarMatrix mat1

    (

          fvm::laplacian(lambdaD,F)

     );



    

    label Nc = mesh.nCells(); //Total number of cells

    

    // Diagonal coefficients calculation

        for(label i=0; i<Nc; i++)

        {

          mat1.diag()[i]*=Psat[i];

        }

        

    //Off-diagonal coefficients calculation

        for(label faceI=0; faceI<mat1.lduAddr().lowerAddr().size(); faceI++)

        {

    mat1.lower()[faceI]*=Psat[mesh.faceOwner()[faceI]];

      mat1.upper()[faceI]*=Psat[mesh.faceNeighbour()[faceI]];

        }





      dimensionedScalar Pa ("Pa",dimensionSet(1,-1,-2,0,0,0,0), 1.0 );



    mat1*=Pa;

 

    solve

        (

            fvm::ddt(dw,F)==mat1

    //fvm::laplacian(lambdaD*Psat,F)//+fvc::laplacian(dT,T)// //  

         );

    

    F=(relFaktor)*F + (1-relFaktor)*Ft;



    fdeltaN=diffFields(F,Ft);

     

    #include "w_prepocet.H"

    iter++;

    

    if (iter==1)

    {

    tdelta=tdeltaN;

    fdelta=fdeltaN;

    }



    if ((tdeltaN>tdelta) || (fdeltaN>fdelta))

    {

    relFaktor=relFaktor/2;

    T=(relFaktor)*T+(1-relFaktor)*Tt;

    F=(relFaktor)*F + (1-relFaktor)*Ft;

    }

    

    } while (((tdeltaN>maxDeltaT) || (fdeltaN>maxDeltaH)) && iter < maxIter);

my approach to laplacian(labmbdaD,F*Psat) is in code, maybe for expert it could be ridiculous :D , but I am working with openFoam and C++ 2 weeks, and this code gives some "expected" values. Other approach gives unstability or doesn't work...

I tried next approach, rewrite partial pressure by gradient of temperature, it seems, that gives similar values like lduaddressing script :)

I don't know where is problem, I have to check all functions, material parameters and other properties again,...

thanks to all for support and advices
Richard

you REALLY need to be more specific when you say 'it doesnt work'.

I was wrong :o, It works, but obtained values ...

dimensions [0 0 0 0 0 0 0];

internalField nonuniform List<scalar>
4000
(
-1.35814e-10
4.58031e-11
4.58031e-11
4.58031e-11
4.5803e-11
4.58031e-11
4.58031e-11
4.58031e-11
-1.82592e-10
-1.77054e-12
-2.23032e-11

So it seems (two scheme unstable), that a problem could be somewhere else,

Is right using parameters (lambda), stored as volScalaField and (ununiform field) calculated in each step equation by this way? (fvm::laplacian(lambda,T)) Is it interpreted correctly to scheme or is used average values?

Thanks
Richard

Quote:

Originally Posted by fabian_roesler (Post 445542)

Hi,

when psat is a function of temperature, you are not allowed to pull it out of the gradient in the laplacian function. But you could use the chain rule to get an implicit term of F and an explicit term of psat. Here we go:

Eqn (1): This is your starting point

Code:

fvm::ddt(dw,F) + fvm::laplacian(delta,psat*F)

Eqn (2): Split the gradient term

Code:

fvm::ddt(dw,F) + fvc::div(delta*F*fvc::grad(psat) + delta*psat*fvc::grad(F))

Eqn (3): Split the divergence term

Code:

fvm::ddt(dw,F) + fvc::div(delta*F*fvc::grad(psat)) + fvm::div(delta*psat*fvc::grad(F))

Eqn (4): form the last two terms into laplacians again

Code:

fvm::ddt(dw,F) + fvc::laplacian(delta*F,psat) + m::laplacian(delta*psat,F)

Eqn 4 should work for you. Try it out.

Regards

Fabian

Hi, anyone manage to solve the problem?

I face similar problem whereby I need to convert

Code:

fvm::laplacian((alpha*rho*DkEff(F1)), k_)

Code:

fvm::laplacian((alpha*DkEff(F1)), rho*k_)

I used eqn4 as recommended to get:

Code:

fvm::laplacian((alpha*rho*DkEff(F1)), k_) + fvc::laplacian((alpha*k_*DkEff(F1)), rho)

but seems like I can't place rho there in:

Code:

fvc::laplacian((alpha*k_*DkEff(F1)), rho)

The error is "error: no matching function for call to ‘laplacian(Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> >, const rhoField&)’"

Another error is "note: template argument deduction/substitution failed"

Any idea how to solver it? Must been trying to solve it for a month.

Thanks