[Joanne]

I apologise in advance if this has been asked already.

I am building a custom solver based in simpleFoam where I solve a continuity equation along the lines of:

    fvScalarMatrix rhoEEqn
    (
        fvm::ddt(rhoE)
        - fvc::laplacian(sigma, phiE)
        ==
        - fvc::div(phi, rhoE)
    );

Where rhoE is defined elsewhere in the solver code as:

volScalarField rhoE = A * B;

Where A and B are calculated, temperature dependent values. This all compiles fine and I have div(phi,rhoE) defined in my fvSchemes and fvSolutions.

However, whenI run the solver, it states:

--> FOAM FATAL IO ERROR:
keyword div(phi,(q*(I|((A*pow((((8*k)*T)|(p*m)),0.5))*q))) is undefined in dictionary "/home/OpenFOAM/user/run/test/system/fvSchemes.divSchemes"

so the error brings up rhoE expressed as its component parts, rather than rhoE itself which is defined in createFields and also in fvSchemes and fvSolutions but the case won't run.

If anyone has any advice, I'd be truly grateful.

Kind regards

[akidess]

You need to tell OpenFOAM how to discretize your div-operator. RTM, and understand the fvSchemes file.

[Joanne]

Hi Anton,

Thank you for your fast response! I think you might have misunderstood my issue or perhaps I am misunderstanding your response! I apologize!

In my fvSchemes, my div(phi, rhoE) is defined with a discretization scheme.

However, when I run the solver, the error shows rhoE to be made of all it's constituent parts. And that these constituent parts are not defined in fvSchemes, despite div(phi,rhoE) being defined.

I can use the "default ___some_discretization_scheme___" to correct the fvSchemes file, but then the same error shows under fvSolutions>solvers.

keyword q*(I|((A*pow((((8*k)*T)|(p*m)),0.5))*q) is undefined in dictionary /home/OpenFOAM/user/run/test/system/fvSolution.solvers"

And here again, a solver type is defined for rhoE, but again rhoE appears as it's total constituent parts.

I'm not exactly sure how to deal with this.

Kind regards,
Joanne

[RobertHB]

Its a crude workaround, but your problem might be fixed by replacing "rhoE" with "q*(I|((A*pow((((8*k)*T)|(p*m)),0.5))*q)" whenever OpenFOAM complains.

[akidess]

You can add e.g. "div(phi,(q*(I|((A*pow((((8*k)*T)|(p*m)),0.5))*q)) ) Gauss upwind" to your fvSchemes and be done with it. You expect to see div(phi, rhoE), but you never explicitly created rhoE, since you constructed it implicity by A*B. If you had defined an IOobject with a name the error message would be different.