[D.B]

Hi All,
I want to monitor residuals at specific points in the domain. I have checked the residual function objects which gives max initial residuals in the entire domain. I have checked probes as well which writes various fields at various probe locations.

I have found no examples of writing residuals at specific points.

Can someone enlighten me of any functionality present in OpenFOAM which would help me get residuals at specific points in the domain, or if someone has an idea of how to change the source code for the same purpose.

Thanks,

[coloursfordirectors]

Hi D. B.! I'm looking for exactly the same – have you found a solution in the meantime?

[jherb]

A long time ago, I submitted a patch for something related to this:
http://bugs.openfoam.org/view.php?id=270

Perhaps this is a starting point: You can access the residual field of the solver object. Also the normalization constant should be accessible via the object registry. So you have to modify the solver and store the residuals as field at each (to be saved) time step.

In createFields.H of your solver, you have to add fields for the residuals, e.g.:

    volVectorField uResidual
    (
        IOobject
        (
            "uResidual",
            runTime.timeName(),
            mesh,
            IOobject::NO_READ,
            IOobject::NO_WRITE
        ),
        mesh,
        dimensionedVector("zero", dimensionSet(0,0,-1,0,0,0,0), vector(0.0, 0.0, 0.0))
    );

    volScalarField uxRes
    (
        IOobject
        (
            "uxRes",
            runTime.timeName(),
            mesh,
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        mesh,
        dimensionedScalar("zero", dimensionSet(1,-2,-2,0,0,0,0), 0.0)
    );

    volScalarField uyRes
    (
        IOobject
        (
            "uyRes",
            runTime.timeName(),
            mesh,
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        mesh,
        dimensionedScalar("zero", dimensionSet(1,-2,-2,0,0,0,0), 0.0)
    );

    volScalarField uzRes
    (
        IOobject
        (
            "uzRes",
            runTime.timeName(),
            mesh,
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        mesh,
        dimensionedScalar("zero", dimensionSet(1,-2,-2,0,0,0,0), 0.0)
    );



    volScalarField pResidual
    (
        IOobject
        (
            "pResidual",
            runTime.timeName(),
            mesh,
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        mesh,
        dimensionedScalar("zero", dimensionSet(0,0,-1,0,0,0,0), 0.0)
    );

In your solver you have to set these fields after every time step (bofore call to .solve()):

      pResidual.internalField() = p_rghEqn.residual();

            uResidual.internalField() = UEqnRes.residual();
            uxRes.internalField() = mag(uResidual.component(0));
            uyRes.internalField() = mag(uResidual.component(1));
            uzRes.internalField() = mag(uResidual.component(2));

To be honest, at the moment, I do not know how to access the normalization factor, but perhaps, the above code is enough, if you see where the largest residuals occur.