[santiagomarquezd]

Hi FOAMers, I have a solver with this code:

    fvVectorMatrix UEqn
    (
        fvm::ddt(rhom, U)
      + fvm::div(phi, U)
      + fvc::div
        (
            alpha*rhop*Vdrp*Vdrp,
            "div(phiVdrp,Vdrp)"
        )
      - fvm::laplacian(mum, U, "laplacian(mum,U)")
    );

when I run the solver I obtain this error:

--> FOAM FATAL IO ERROR:
keyword div(phiVdrp,Vdrp) is undefined in dictionary "/home/santiago/OpenFOAM/santiago-1.6.x/run/tankBubbles/system/fvSchemes::divSchemes"

file: /home/santiago/OpenFOAM/santiago-1.6.x/run/tankBubbles/system/fvSchemes::divSchemes from line 30 to line 32.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 396.

FOAM exiting

then if I add this:

divSchemes
{
    div(phi,U)  Gauss upwind; //limitedLinearV 1;
    div(rhop*phi,alpha) Gauss upwind;
    div(phiVdrp,alpha) Gauss upwind;
    div(phiVdrp,Vdrp) Gauss upwind;
}

to my system/fvSchemes dictionary I still get an error, but a different one:

--> FOAM FATAL IO ERROR:
attempt to read beyond EOF

file: /home/santiago/OpenFOAM/santiago-1.6.x/run/tankBubbles/system/fvSchemes::divSchemes::div(phiVdrp,Vdrp) at line 33.

From function ITstream::read(token& t)
in file db/IOstreams/Tstreams/ITstream.C at line 84.

FOAM exiting

Any clues about that?, I've checked some similar threads without success.

Regards.

[akidess]

The divergence schemes in fvSchemes apply to convective terms like fvm::div(phi, X), but your term in the equation seems to be a simple explicit divergence of a scalar field, so why not just write it in the following way?

 fvVectorMatrix UEqn
    (
        fvm::ddt(rhom, U)
      + fvm::div(phi, U)
      + fvc::div
        (
            alpha*rhop*Vdrp*Vdrp
        )
      - fvm::laplacian(mum, U, "laplacian(mum,U)")
    );

[santiagomarquezd]

Anton, I took this notation from settlingFoam, but on the other hand I'd tried you suggested with same results:

    fvVectorMatrix UEqn
    (
        fvm::ddt(rhom, U)
      + fvm::div(phi, U)
      + fvc::div
        (
            alpha*rhop*Vdrp*Vdrp
        )
      - fvm::laplacian(mum, U, "laplacian(mum,U)")
    );

error obtained at runtime:

--> FOAM FATAL IO ERROR:
keyword div((((alpha*rhop)*Vdrp)*Vdrp)) is undefined in dictionary "/home/santiago/OpenFOAM/santiago-1.6.x/run/tankBubbles/system/fvSchemes::divSchemes"

file: /home/santiago/OpenFOAM/santiago-1.6.x/run/tankBubbles/system/fvSchemes::divSchemes from line 30 to line 32.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 396.

FOAM exiting

adding corresponding line in system/fvSchemes

--> FOAM FATAL IO ERROR:
attempt to read beyond EOF

file: /home/santiago/OpenFOAM/santiago-1.6.x/run/tankBubbles/system/fvSchemes::divSchemes::div((((alpha*rhop)*Vdrp)*Vd rp)) at line 34.

From function ITstream::read(token& t)
in file db/IOstreams/Tstreams/ITstream.C at line 84.

FOAM exiting

Regards.

[akidess]

Ah, you are right, looking at fvcDiv.* it is indeed possible to name even an explicit term and force usage of a certain divergence scheme instead of plainly calling surfaceIntegrate. I'm sorry I don't really have other ideas what could cause the problem. Hopefully someone else will notice this thread and have an answer.

[santiagomarquezd]

Anton, the correct entry in fvSchemes is:

divSchemes
{
    div(phi,U)  Gauss upwind; //limitedLinearV 1;
    div(phi,alpha) Gauss upwind;
    div(phiVdrp,alpha) Gauss upwind;
   div(phiVdrp,Vdrp) Gauss upwind phiVdrp;
}

it's necessary to explicitly write the flux which will be used in order to interpolate the values at faces. Early alberto shown me the wording to include the flux properly.

Regards.