[sippanspojk]

Dear foamers, I need your help!


As the title says I am trying to change the value of the faces of a defined patch. I have modified the pimpleFoam solver to generate a dimensionless volScalarField that I have initialized to 0.0.

I would then like to within a functionObject loop over the faces of the desired patch and assign a specific value to each face.

As I start I did a very simple case where I wanted to try to change the initial value 0.0 to 1.0 but that didn't work.


In my myFunctionObject.C file I have the following code

    const volScalarField& myField = lookupObject<volScalarField>("myField");

    forAll(myField.boundaryField()["defined patch"], faceIt){
        myField.boundaryField()["defined patch"][faceIt] == 1.0;
        Info << myField.boundaryField()["defined patch"][faceIt] << endl;
    }

The functionObject does compile but with a warning saying:

myFunctionObject.C:178:41: warning: value computed is not used [-Wunused-value]
myField.boundaryField()[6][faceIt] == 1.0;


When I then run the case the output is still 0 and not 1 as I was hoping for.

Can someone help me whit this one??


Thank you!

David

[jherb]

[QUOTE=sippanspojk;752272]

        myField.boundaryField()["defined patch"][faceIt] == 1.0;

This compares your boundary field value with 1.0 and then throws away the result. You should use just one "=".

[sippanspojk]

[QUOTE=jherb;752291]

Originally Posted by sippanspojk

This compares your boundary field value with 1.0 and then throws away the result. You should use just one "=".

Ok that makes sence actually. "==" returns either false or true and then moves on, right?


I tried it out with only one "=" and then I couldn't compile my functionObject. I got the following error message:

myFunctionObject.C:178:41: error: assignment of read-only location '(&(&(& myField)->Foam::GeometricField<Type, PatchField, GeoMesh>::boundaryField<double, Foam::fvPatchField, Foam::volMesh>())->Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::Boundary::<anonymous>.Foam::FieldF ield<Foam::fvPatchField, double>::<anonymous>.Foam::PtrList<Foam::fvPatchFi eld<double> >::<anonymous>.Foam::UPtrList<T>:perator[]<Foam::fvPatchField<double> >(6))->Foam::fvPatchField<double>::<anonymous>.Foam::Fie ld<double>::<anonymous>.Foam::List<double>::<anony mous>.Foam::UList<T>:perator[]<double>(faceIt)'
myField.boundaryField()[6][faceIt] = 1.0;


Any idea of what this means?

[einstein_zee]

Hii there,

Looks like you should use boundaryFieldRef() instead of boundaryField().

[sippanspojk]

Originally Posted by einstein_zee

Hii there,

Looks like you should use boundaryFieldRef() instead of boundaryField().

Thanks Hosein, this helps!

However, only if I modify the solver and change the boundary value from there. But If I take the exact same row in my functionObject it complains:

myFunctionObject.C:179:34: error: passing ‘const volScalarField {aka const Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>}’ as ‘this’ argument of ‘Foam::GeometricField<Type, PatchField, GeoMesh>::Boundary& Foam::GeometricField<Type, PatchField, GeoMesh>::boundaryFieldRef() [with Type = double; PatchField = Foam::fvPatchField; GeoMesh = Foam::volMesh]’ discards qualifiers [-fpermissive]
myField.boundaryFieldRef()[patchIt][faceIt] = 1.0;

[einstein_zee]

I think this one "lookupObjectRef()" should solve the issue. This means now you don't need "const" qualifier.

[sippanspojk]

Originally Posted by einstein_zee

I think this one "lookupObjectRef()" should solve the issue. This means now you don't need "const" qualifier.

That did the trick!

Thank you very much for you quick and helpful response.