[Researcher23]

Hi all,

I would like to introduce a mass source in the fluid part of chtMultiRegionFoam. My first try was to introduce a semiImplicitSouce:

 
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  5                                     |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      fvOptions;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
scalarSource
{
    type            scalarSemiImplicitSource;
    duration        1000.0;
    selectionMode   all;
    volumeMode      absolute;
    injectionRateSuSp
    {
        rho           (-0.1 0);
    }
}

My problem is, that rho does not change with this source. Another try was a scalarCodedSource, with the same negative result: rho does not change in my fluid volume!

It is possible to change other fields (energy,...) with this kind of source, but I am interested in changing the masses.

Please could you give me a hint what's going wrong and how can I change rho in chtMultiRegionFoam?

Thanks a lot,
J.

[Researcher23]

Did somebody have an answer to my question?

[Researcher23]

Okay, I solved the problem. The bug (or missing feature) was that there is no fvOptions-term in the pressure equation of chtMultiRegionFoam. With adding this missing term my fvOptions mass term works fine. Here is our code fix:

 
        fvScalarMatrix p_rghEqn
        (
            p_rghEqnComp + p_rghEqnIncomp
          ==
          + fvOptions(psi, p_rgh, rho.name())
        );

[jherb]

Included in OpenFOAM-dev branch with https://bugs.openfoam.org/view.php?id=3146