CFD Online Discussion Forums - surface and volume fields multiplication

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

- OpenFOAM Programming & Development (https://www.cfd-online.com/Forums/openfoam-programming-development/)

- - surface and volume fields multiplication (https://www.cfd-online.com/Forums/openfoam-programming-development/85629-surface-volume-fields-multiplication.html)

surface and volume fields multiplication

Greetings !

I have two fields: volVectorField X and surfaceScalarField M. Is there any method to multiply them to get volume field on new time step like that :
X(n+1,i) = X(n,i-1)*M(n,1-1/2)-X(n,i+1)*M(n,i+1/2)
there n timestep index and i index of a cell. i+1/2 - right face of a cell i-1/2 - left face.

I assumed that this will look like interpolate(interpolate(X)*M) with upwind interpolation schemes, but as i know there is no method for interpolating face field onto cell volumes.
Is there any way to make such construction in solver ?

Best regards !

Something along these lines should do the trick. You're going to have to sort out the the discretization and mathematical correctness of it all. Since the mesh is unstructured you'll probably need to use the face normal vector or something to get the direction. Also take a look at finiteVolume/finiteVolume/fvc/fvcReconstruct.C, which does something similar.

Code:

    vectorField& Xi = X.internalField();

    const vectorField& X0i = X.oldTime().internalField();

    const scalarField& M0i = M.oldTime().internalField();



    const unallocLabelList& owner = mesh.owner();

    const unallocLabelList& neighbour = mesh.neighbour();



    Xi = vector::zero;

    

    forAll(owner, faceI)

    {

        label P = owner[faceI];

        label N = neighbour[faceI];



        // You're gonna have to sort out the sign issue here

        // This will probably need the face normal

        Xi[P] += X0i[N]*M0i[faceI];

        Xi[N] -= X0i[P]*M0i[faceI];

    }



    forAll(mesh.boundaryMesh(), patchI)

    {

        fvPatchVectorField& pf = X.boundaryField()[patchI];

        const fvPatchVectorField& pf0 = X.oldTime().boundaryField()[patchI];

        const fvsPatchScalarField& psf = M.oldTime().boundaryField()[patchI];



        const unallocLabelList& faceCells = mesh.boundaryMesh()[patchI].faceCells();



        if (pf.coupled())

        {

            // I'm going to leave this one up to you

        }

        else

        {

            forAll(pf, faceI)

            {

                Xi[faceCells[faceI]] += pf0[faceI]*psf[faceI];

            }

        }        

    }



    X.correctBoundaryConditions();

This might be a much simpler alternative. Again, you need to sort out the discretization and mathematical correctness.
X = fvc::surfaceSum(fvc::interpolate(X.oldTime())*M.ol dTime())

Hi Ivor , thank you very much for your reply !

It was really helpful for me. I'm trying to add some another algorithms in OpenFoam like FLIC or Big particles method, but there is a very little information about classes and methods in OpenFoam and tutorials for their usage, except Doxygen documentation. Construction proposed by you in your second post looks to be that i need. I used it for coding 3rd step in FLIC method and solver is compiling well now. I will try to solve some test cases and work out correctness issue.

Best regards !

Hi ivor,
I have a similar doubt.
I have interface area as a surfaceScalarField and my thermal conductivity as a volume scalar field. how to multiply them and get a volScalarField
Thanks in advance

Dear Hari,
I think you need to be more specific about what you're trying to achieve. What value are you trying to get at the cell centres. Are you trying to get face-area-averaged value for each cell? Are you trying to get the total interface area?
OpenFOAM has the surfaceSum function that might do what you want.

Thanks ivor surfaceSum solved my problem

Hi ivor,
Can you tell me where can we find surfaceSum in openfoam libraries? I hope it is from surface integrals.C but if surfaceSum integrates and converts a surfaceScalar field to volScalarField then what does volIntegrals do?
Thanks in advance

#include "fvcSurfaceIntegrate.H"

fvc::surfaceSum sums the face values for each cell and returns a volField.

fvc::volumeIntegrate simply multiples the cell values by the cell volume.