[milad653279]

Dear foamer

I am confused about phi in openfoam. as you know, convection term in incompressible Navier-Stokes is div(UU). in openfoam is writen by div (phi,U) which phi= interpolate (U) & mesh.sf(). why does phi product mesh.sf()???!!! I think that phi must be U (phi=U) NOT phi=U*sf(). please help me at it.

[Lorena2fdez]

Hi Milad,

In openFoam you use
div ( psi , phi )
where
psi is an explicit SurfaceScalarField
phi is an implicit Vol<type>Field

fvc::interpolate() or fvm:interpolate(): generates a face flux field (surfaceScalarField) from a cell based volumetric field (volScalarField).
mesh.Sf(): return the face area magnitude of a face flux field (surfaceScalarField).

For your case U is a volScalarField and phi is its respective surfaceScalarField.

Best regards,
Lorena.

[milad653279]

Originally Posted by Lorena2fdez

Hi Milad,

In openFoam you use
div ( psi , phi )
where
psi is an explicit SurfaceScalarField
phi is an implicit Vol<type>Field

fvc::interpolate() or fvm:interpolate(): generates a face flux field (surfaceScalarField) from a cell based volumetric field (volScalarField).
mesh.Sf(): return the face area magnitude of a face flux field (surfaceScalarField).

For your case U is a volScalarField and phi is its respective surfaceScalarField.

Best regards,
Lorena.

Dear Lorena
OF integrates momentum equation over a cell, I think if phi is (phi=interpolate (U) & mesh.sf()) is wrong because the value of surface area is product twice into equation. once in phi and other time when OF integrates from equation.

[Lorena2fdez]

Originally Posted by milad653279

Dear Lorena
OF integrates momentum equation over a cell, I think if phi is (phi=interpolate (U) & mesh.sf()) is wrong because the value of surface area is product twice into equation. once in phi and other time when OF integrates from equation.

Probably the solver is thinking for don't make twice the product into equation. When the solver integrates the equation if it has a SurfaceScalarField, It won't make the product by value of surface area, again.

Maybe it help you, in a manual about OpenFOAM I saw a description of phi used for solve the Navier-Stokes equations:
In OpenFOAM, it's common that phi is the flux of velocity u . Other times, phi represents the flux of rho*u.

I saw the code of different solver in OpenFOAM and it's usual to do that product when it interpolate a field. For example (in KinematicSingleLayer.C):

... fvc::interpolate(rho_*gTan()) & regionMesh().Sf() ...
phiAdd += fvc::interpolate(pp) * fvc::snGrad(delta_) * regionMesh().magSf();
phi_ = fvc::interpolate(deltaRho_*U_) & regionMesh().Sf();

I don't know more about this subject but it's really strange a fail like that in the code.

Best regards,
Lorena

[turbulo]

I know this is long overdue, but since I just stumbled on it, I'll try to answer:

As you rightly pointed out, (or depending on the solver), but, for instance, if you look at fvmDiv in gaussConvectionScheme.C you'll see that OpenFOAM doesn't compute the integral of the divergence itself, but constructs a coefficients matrix (an fvMatrix in OF parlance) from phi and the velocity simply by multiplying them, there is no extra involved. I'll let you see for yourself (gaussConvectionScheme.C):

    forAll(vf.boundaryField(), patchi)
    {
        const fvPatchField<Type>& psf = vf.boundaryField()[patchi];
        const fvsPatchScalarField& patchFlux = faceFlux.boundaryField()[patchi];
        const fvsPatchScalarField& pw = weights.boundaryField()[patchi];

        fvm.internalCoeffs()[patchi] = patchFlux*psf.valueInternalCoeffs(pw);
        fvm.boundaryCoeffs()[patchi] = -patchFlux*psf.valueBoundaryCoeffs(pw);
    }