[baezacaljo]

Dear All


I am looking for help, how to add temperature equation or any other equation to InterFoam solver?, i noticed, that now everything is called modular solver and even the name changed to incompressibleVoF.


i know everything is with classes, however, openFoam is improving faster and now i am a bit lost.


Finally the version is OpenFoam11



thanks in advance

[LongGe]

Hello baezacaljo

I would add to the class method "thermophysicalPredictor" in "incompressibleVoF.C".
The solver "foamRun" always calls this class method.


OpenFOAM-11/applications/modules/incompressibleVoF

void Foam::solvers::incompressibleVoF::thermophysicalPredictor()
{}

OpenFOAM-11/applications/solvers/foamRun/foamRun.C

        // PIMPLE corrector loop
        while (pimple.loop())
        {
            solver.moveMesh();
            solver.fvModels().correct();
            solver.prePredictor();
            solver.momentumPredictor();
            solver.thermophysicalPredictor();
            solver.pressureCorrector();
            solver.postCorrector();
        }

[baezacaljo]

Thank you for your help LongGe

Now I assume I have to copy both folder the one called incompressibleVoF and compile it. And the other other one that contains the solver foamRun.C and compile it, right?

Finally in the controlDict file in solver I have to write myFoamRun, right?


By the way, i was reading the code carefully and the fie incompressibleVoF.C already has

void Foam::solvers::incompressibleVoF::thermophysicalPr edictor() {}

and the file incompressibleVoF.H has

// Member Functions //- Called at the start of the PIMPLE loop virtual void prePredictor(); //- Construct and solve the energy equation, // convert to temperature // and update thermophysical and transport properties virtual void thermophysicalPredictor();

Hence, i am not getting the code.


is the incompressibleVoF.C and foamRun considering the temperature already?


Best regards

[LongGe]

Hello

Since "foamRun" is simply a client using the "solver" class, you do not need to make any changes. All you have to do is copy "incompressibleVoF" and create your "yourincompressibleVoF". The controlDict is as follows.

application     foamRun;
solver          yourincompressibleVoF

foamRun" always calls the class method "thermophysicalPredictor()". This is as I have shown before. The following is the inheritance relation of the "incompressibleVoF" class. The "thermophysicalPredictor" is declared as a pure virtual function in the "fluidSolver" class.

incompressibleVoF->twoPhaseVoFSolver->twoPhaseSolver->VoFSolver->fluidSolver

virtual void thermophysicalPredictor() = 0;

The class "incompressibleVoF" must implement "thermophysicalPredictor", but "incompressibleVoF" does not solve the temperature, so its implementation is empty. And you will be the one to specifically do this implementation.

[baezacaljo]

Thank you LongGe


So rry for the late reply i was testing and writing the code, look this is what i achieved so far (see attached files), however, in the case of the Make folder and the other two folder, do i have to modify them and then COMPILE THEM? or what to do?


i only modify the folder name from incompressibleVoF to incompressibleVoFTemp and the files stick with the same name incompressibleVoF.C and incompressibleVoF.H but with some modifications.


Thanks in advance

[LongGe]

Hello

You will need to create a new class. I don't think you can just copy it.

For example:

class incompressibleVoFTemp
:
    public twoPhaseVoFSolver
{

...
...

    //- Runtime type information
    TypeName("incompressibleVoFTemp");

Other changes will need to be made to ctor and dtor as well....

[K.C.]

I found this thread via Google and have to admit, that I am facing the same problem.


I copied an existing solver module, modified it and then compiled it into an shared library with .so extension via "wclean" and "wmake libso".
Compilation worked fine, but my new solver class is not available to foamRun


I tried

foamRun -solver {nameOfMyOwnSolver}

while the .so was declared inside of my controlDict with

libs("{pathToMyLibrary.so}");

and I also tried

foamRun -libs '("{pathToMyLibrary.so}")' -solver {nameOfMyOwnSolver}

and my last attempt was to extend the searchPath for libraries with

export LD_LIBRARY_PATH=$LD_LIBRARY_PATH:/{absolutePathToMyLibraryFolder}

In all ways foamRun complains with "solvers table is empty"

So how can I declare to foamRun to use my new created solver module?
The




Kind regards,
K.C.