[jdw135]

Hello,

I've been attempting to learn how to use scalarCodedSource, and I've hit a brick wall of sorts. I am using rhoPimpleFoam for my case, and I would like to add a source to the energy equation via the fvOptions. My fvOptions code is its own file in the constant directory, and is as follows:

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      fvOptions;
}

ICM
    {
        type            scalarCodedSource;
        name            sourceTime;

        active          yes;

        scalarCodedSourceCoeffs
        {
            selectionMode   all;
            fields          (he);

            codeInclude
            #{
            #};

            codeCorrect
            #{
                Pout<< "**codeCorrect**" << endl;
            #};

            codeAddSup
            #{
                const Time& time = mesh().time();
                const volScalarField& rhoS = mesh_.lookupObject<volScalarField>("rho");
                const volVectorField& uS = mesh_.lookupObject<volVectorField>("U");
                const volScalarField& pS = mesh_.lookupObject<volScalarField>("p");
                const vectorField& C = mesh_.C();
                const scalarField& V = mesh_.V();
                scalarField& SoS = sqrt(1.4*(pS/rhoS));
                scalarField& mach = uS/SoS;
                scalarField& qq = -(pS*(1-(mach*mach))1005)/(1.4*(mach*mach)*287.058);
                scalarField& heSource = eqn.source();
                heSource -= qq;
            #};

            codeConstrain
            #{
                Pout<< "**codeSetValue**" << endl;
            #};

            // Dummy entry. Make dependent on above to trigger recompilation
            code
            #{
                $codeInclude
                $codeCorrect
                $codeAddSup
                $codeConstrain
            #};
        }
        sourceTimeCoeffs
        {
            // Dummy entry
        }
    }

Unfortunately, I can't find reliable documentation on what else to do to implement this code. I have added the following to my controlDict file based on what I've read on these forums:

ICM
  {
    type            scalarTransport;
    libs            ("libsolverFunctionObjects.so");
    field           he;
  }

I'm basing the field name on the rhoPimpleFoam solver Eeqn.h, where it calls

fvOptions(rho,he)

I keep getting the error message, "Source ICM defined for field he but never used", and prior to running I get a warning saying, "cannot find file "/afs/crc.nd.edu/user/j/jwells4/ShearLayer/OpenFoam/Rennie/processor0/0/he". Can someone please point out where I'm missing the point, and maybe tell me the full steps to implementing this kind of source? Should I be naming the field something else and supplying a 0 file for it?

[jdw135]

Can anyone please help with this issue? There are zero actual tutorials for this and I cannot find a reason that it's not implementing the fvOption. The code is definitely reading the file.

[jdw135]

This is the portion that is returning the error, but I'm unsure why it's not applying the source. This is from fvOption.C

void Foam::fv::option::checkApplied() const
 {
     forAll(applied_, i)
     {
         if (!applied_[i])
         {
             WarningInFunction
                 << "Source " << name_ << " defined for field "
                 << fieldNames_[i] << " but never used" << endl;
         }
     }
 }

[Yann]

Hello Jonathan,

Depending on your thermophysicalProperties setup, you can use either internal energy (e) or enthalpy (h).

There is no "he" variable and this is what the solver complains about in your first warning. In your fvOptions, just replace "he" in fields (he); with the energy variable you use in your case (h or e)

The scalarTransport function object is, I guess, useless for what you are trying to achieve here.

I don't know which OpenFOAM version you are using, but there is an example to add a source on the energy equation here : https://www.openfoam.com/documentati...ces-coded.html

I hope this helps,
Yann

[jdw135]

Originally Posted by Yann

Hello Jonathan,

Depending on your thermophysicalProperties setup, you can use either internal energy (e) or enthalpy (h).

There is no "he" variable and this is what the solver complains about in your first warning. In your fvOptions, just replace "he" in fields (he); with the energy variable you use in your case (h or e)

Thanks for clarifying this. I did eventually change my case to apply the source to the h field, but I was getting a separate error so I got confused. It makes sense that the field would be my energy variable defined in thermophysicalProperties. Now, though, when I run the case, I get an error saying "Unknown variable 'WM_OPTIONS'. From looking online, it seems like this is an environment variable? I can't find much else on it, though.