CFD Online Discussion Forums - Describing div terms in fvSchemes

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

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

- - Describing div terms in fvSchemes (https://www.cfd-online.com/Forums/openfoam-programming-development/85542-describing-div-terms-fvschemes.html)

Describing div terms in fvSchemes

Hi FOAMers, I have a solver with this code:

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:

Code:

--> 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:

Code:

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:

Quote:

--> 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.

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?

Code:

 fvVectorMatrix UEqn

    (

        fvm::ddt(rhom, U)

      + fvm::div(phi, U)

      + fvc::div

        (

            alpha*rhop*Vdrp*Vdrp

        )

      - fvm::laplacian(mum, U, "laplacian(mum,U)")

    );

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

Code:

    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:

Code:

--> 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

Quote:

--> 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.

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.

Anton, the correct entry in fvSchemes is:

Code:

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.