[joel.lehikoinen]

Hi,

I need to create a solver based on buoyantPimpleFoam which solves an arbitrary (around 10) scalar transport equations. I have written a solver which solves one passive scalar transport equation. I could just copy-paste that code enough many times, but I would like to know if a more elegant solution is possible: Namely, how easy it would be to implement a for-loop that solves N scalar transport equations, where N is specified by the user? The problem is, I don't know C++ and I'm not too familiar with the classes present in OpenFOAM.

As far as I know, the vectors in OpenFOAM are always 3-dimensional. But could I use a tensor of rank (1,N) or (N,1) to store the scalars? Or is using a tensor a bad idea, if I want to have different BCs for the scalars? Tensor would be nice because then I wouldn't have to worry about how to get OF to read/write files with indices in their names (scalar1, scalar2, etc.).

This is not a critical problem, as I said I can just copy-paste the code snippet that solves one scalar transport equation N times, but if I want to change the number of scalars later it becomes cumbersome to recompile the solver every time. I was just wondering if anyone with more knowledge of C++ and OF source code knows these things.

Regards,
Joel

[l_r_mcglashan]

Sure, you can use a PtrList. Here's how you initialise them:

//  Create a list of pointers to the mass fraction field of each species.
    PtrList<volScalarField> chemicalSpecies(numberOfSpecies);
    for (label i=0; i<numberOfSpecies; ++i)
    {
        Info << "Creating Species " << namesOfSpecies[i] << endl;
        chemicalSpecies.set
        (
            i,
            new volScalarField
            (
                IOobject
                (
                    namesOfSpecies[i],
                    runTime.timeName(),
                    mesh,
                    IOobject::NO_READ,
                    IOobject::AUTO_WRITE
                ),
                mesh,
                dimensionedScalar("zero", dimless, 0.0),
                mixtureFraction.boundaryField().types()
            )
        );
    }

Then use a for loop to solve the equations, as done in, for example, YEqn.H in solvers/combustion/chemFoam

[joel.lehikoinen]

Thank you very much for your help, I managed to create the solver I will need.

[dinksy]

I am also trying to solve a similar problem of solving transport equation of n scalars, say c, and would like to define them as an array, such as c[n] instead of defining n separate scalarfields. The above thread was of some help but if you can tell me which solver it is a part of then I could look into it to clarify my doubts. The main problem I face is with the definition of c as an array in the initial time folder [0].
Regards