Node220 - CFD SUPPORT

Previous: New solver Up: Creating new OpenFOAM solver Next: Test case set up
_{This is an automatically generated documentation by LaTeX2HTML utility. In case of any issue, please, contact us at info@cfdsupport.com.}

Implementation

Solver already exists, make sure by listing:
# ls $FOAM_USER_APPBIN

In file createFields.H create new constant for heat constant coefficient kappa and new quantity T :

    Info<< "Reading transportProperties\n" << endl;

    IOdictionary transportProperties
    (
        IOobject
        (
            "transportProperties",
            runTime.constant(),
            mesh,
            IOobject::MUST_READ,
            IOobject::NO_WRITE
        )
    );

    dimensionedScalar nu
    (
        "nu",
        dimViscosity,
        transportProperties.lookup("nu")
    );

    dimensionedScalar kappa
    (
        "kappa",
        dimViscosity,
        transportProperties.lookup("kappa")
    );

    Info<< "Reading field p\n" << endl;
    volScalarField p
    (
        IOobject
        (
            "p",
            runTime.timeName(),
            mesh,
            IOobject::MUST_READ,
            IOobject::AUTO_WRITE
        ),
        mesh
    );

    Info<< "Reading field T\n" <<endl;
    volScalarField T
    (
        IOobject
        (
            "T",
            runTime.timeName(),
            mesh,
            IOobject::MUST_READ,
            IOobject::AUTO_WRITE
        ),
        mesh
    );

    Info<< "Reading field U\n" << endl;
    volVectorField U
    (
...

Now, in source code file icoTempFoam.C implement equation for temperature.

Temperature is dependent on velocity field, let us place the temperature equation right after the PISO loop:

            #include "continuityErrs.H"

            U = HbyA - rAU*fvc::grad(p);
            U.correctBoundaryConditions();
        }
        
        fvScalarMatrix TEqn
        (
            fvm::ddt(T)
            + fvm::div(phi, T)
            - fvm::laplacian(kappa, T)
        );
        
        TEqn.solve();

        runTime.write();

        Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s"

Each term of temperature equation is discretized and written in matrix of linear system
Compile solver:
# wmake

OpenFOAM Training by CFD Support, CFD SUPPORT, info@cfdsupport.com +420 212 243 883 © CFD support, s.r.o., Sokolovská 270/201, 190 00 Praha 9, Czech Republic