[gryphaea1635]

Hi everyone,

I have two volScalarFields, theta, and alpha.CO2. I want alpha.CO2 at a wall to have a value that depends on the value of theta at the wall.

I've set theta as 0.5 everywhere at the boundary in the solver file at the end of the while loop:

...
while(pimple.correct())
{
     #include "pEqn.H"
}

if (pimple.turbCorr())
{
     turbulence.correct();
}
}

//End of while(pimple.loop())
//Set theta as 0.5 on the boundary

forAll(mesh.boundary(), patchID){
     forAll (mesh.boundary()[patchID],facei)
     {
          theta.boundaryFieldRef()[patchID][facei]=0.5;
     }
}

runTime.write();

Info<< "ExecutionTime = "
     << runTime.elapsedCpuTime()
     ...

Then, I'm using the boundary condition to try to set alpha.CO2 to 1 at the boundary, by adding 0.5 to the value of theta (0.5):

walls                                                                           
{                                                                                      
        type codedFixedValue; 
        value uniform 0;                                                          
        name wallAdsorption;                                                                
        code    #{                                                            
           const fvPatch& boundaryPatch = patch();                                             
           const fvBoundaryMesh& boundaryMesh = boundaryPatch.boundaryMesh();
           const fvMesh& mesh = boundaryMesh.mesh();                                           
           const vectorField& Cf = boundaryPatch.Cf();
           scalarField& field = *this;
           field=patchInternalField();                                                         
           const volScalarField& theta = mesh.lookupObject<volScalarField>("theta");
            forAll(Cf, faceI){
                        field[faceI]=0.5+theta[faceI];
                }
    #};

        }

Yet after running the solver, the the boundary and plotting their values at the boundary with paraview, both alpha.CO2 and theta seem to have a value of 0.5 at the wall. Is there something I'm doing wrong?

Thanks!

[raumpolizei]

Short answer: Issue seems to be your codedFixedValue code. You are accessing your volScalarField with a faceid and this will get you the cell value with the id faceid. The solution to that problem is already there (in your first code snippet. There, the boundary faces, no cells, are accessed correctly). Something like that could work:

const label patchid = mesh.boundaryField().findPatchID(this->name()); // could work, not sure though

const volScalarField& theta(mesh.lookupObject<volScalarField>("theta"));
const auto& thetaPatchField = theta.boundaryField()[patchid];

forAll(field, facei) // face loop

{
    field[facei] = 0.5 + thetaPatchField[i];

}

Cheers, RP

[gryphaea1635]

Thanks for the response! Unfortunately, I'm still having some issues.

I put your code into alpha.CO2:

const fvPatch& boundaryPatch = patch();
                const fvBoundaryMesh& boundaryMesh = boundaryPatch.boundaryMesh();
                const fvMesh& mesh = boundaryMesh.mesh();
                const vectorField& Cf = boundaryPatch.Cf();                                                                             scalarField& field = *this;                                                                                             field=patchInternalField();
                const label patchid = mesh.boundaryField().findPatchID(this->name());
                const volScalarField& theta((mesh.lookupObject<volScalarField>("theta")));
                const auto& thetaPatchField = theta.boundaryField()[patchid];
                forAll(field, facei) {                                                                                                                               
                         field[facei] = 0.5+thetaPatchField[i];
                }

However, after running the code, I got an error that said:

error: 'const class Foam::fvMesh' has no member named 'boundaryField'
error: 'class Foam::wallAdsorptionFixedValueFvPatchScalarField' has no member named 'name'
error: 'i' was not declared in this scope
warning: unused variable 'Cf'

If I replace "thetaPatchField[i]" with "thetaPatchField[facei]", the third error message goes away, but since I'm new to OpenFOAM I'm not sure if that would do what I want it to do.
Also, how should I fix the first two error messages? Should I be replacing "name" with something?

[raumpolizei]

Hey,

which version of OF are you using?

Yes, of course this is not compiling, my bad. Just wrote without compiling and thought you would only take the hints out of that pseudo-like code..
Try to use mesh.boundary().findPatchID(this->patch().name()) instead of mesh.boundaryField... and like you suggested 'i' is not defined in your code so replace it with 'facei' in the loop. (+ delete the line with Cf, it looks like it is not used anywhere, see compiler warning message).

Cheers, RP