[Democritus]

I used to adopt following way in order to impose a complex fixedValue type BC:
1. Implement a program to manipulate the value of boundary field directly and write the field into file. The code is as follow:

    const fvBoundaryMesh & thisBoundary = mesh.boundary(); //here I get the boundary of the mesh
    forAll( thisBoundary, fvPatchID ) // go through all the patchs of the boundary
    {
      const fvPatch & thisPatch = thisBoundary[ fvPatchID ];
      Info << "\n Imposing the boundary condition on the fvPatch of " <<
      thisPatch.name() << endl;

      const vectorField & position = thisPatch.Cf(); // get the cell face centers' positions
      forAll( thisPatch, elmtID ) // imposing values on the centers of all the cell faces of this patch   
      {
        const scalar & x = position[elmtID].component(0);
        const scalar & y = position[elmtID].component(1);

        //you can replace your function on the right side of the =
        pS.boundaryField()[fvPatchID][elmtID] = -1 * Foam::exp(-1 * x) * Foam::cos( x );
        pC.boundaryField()[fvPatchID][elmtID] = Foam::exp(-1 * x) * Foam::sin( x );

        vS.boundaryField()[fvPatchID][elmtID].component(0) = -1 * Foam::exp(-1 * x) * Foam::cos( x );
        vS.boundaryField()[fvPatchID][elmtID].component(1) = 2 * Foam::cos( x ) * Foam::sin( y ) ;

        vC.boundaryField()[fvPatchID][elmtID].component(0) = Foam::exp(-1 * x) * Foam::sin( x );
        vC.boundaryField()[fvPatchID][elmtID].component(1) = Foam::sin( x ) * Foam::cos( y );

      }

    }

2. Then I open the file, change the BC type from "calculated" to "fixedValue"

3. After that, I can run my solver

But!!!
Now in new 4.0 version OpenFOAM, the boundary field is read only! When I compile the BC implement program, the compiler indicates that

vC.boundaryField()[fvPatchID][elmtID].component(0) is read only!

For information the detailed error is as follow:

error: assignment of read-only location ‘(&(&(& u2.Foam::GeometricField<Type, PatchField, GeoMesh>::boundaryField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>())->Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>::Boundary::<anonymous>.Foam::FieldField<Foam::fvPatchField, Foam::Vector<double> >::<anonymous>.Foam::PtrList<Foam::fvPatchField<Foam::Vector<double> > >::<anonymous>.Foam::UPtrList<T>::operator[]<Foam::fvPatchField<Foam::Vector<double> > >(fvPatchID))->Foam::fvPatchField<Foam::Vector<double> >::<anonymous>.Foam::Field<Foam::Vector<double> >::<anonymous>.Foam::List<Foam::Vector<double> >::<anonymous>.Foam::UList<T>::operator[]<Foam::Vector<double> >(elmtID))->Foam::Vector<double>::<anonymous>.Foam::VectorSpace<Form, Cmpt, Ncmpts>::component<Foam::Vector<double>, double, 3u>(1)’
           vC.boundaryField()[fvPatchID][elmtID].component(1) = 0.1*x*y

What can I do for that? Can I have the full control over every single elements of fields in new 4.0 OF?
Thanks!

[hk318i]

I think it is related to this commit [LINK]

[kittychunk]

Originally Posted by hk318i

I think it is related to this commit [LINK]

This solved the problem for me.

The summary version is that you need to replace instances of "boundaryField()" and "internalField()" with "boundaryFieldRef()" and "internalFieldRef()" if you want to modify them in your code. The non-"Ref" calls are const now.

Update

Seems like internalField and internalFieldRef have been replaced by direct calls to the field variable. Eg: U.internalField() becomes U() for a const reference to the internal field, or U.ref() for non-const access. See associated bug report.

[Democritus]

Originally Posted by hk318i

I think it is related to this commit [LINK]

Thank you very much!

[Democritus]

Originally Posted by kittychunk

This solved the problem for me.

The summary version is that you need to replace instances of "boundaryField()" and "internalField()" with "boundaryFieldRef()" and "internalFieldRef()" if you want to modify them in your code. The non-"Ref" calls are const now.

Thank you very much! My problem is solved~!

[Zhiheng Wang]

Originally Posted by Democritus

Thank you very much! My problem is solved~!

Hi my createField.H has defination of T as

const volScalarField& T = thermo.T();
I want to impliment my code on boundaryCondition correction as

forAll(T.boundaryField()[patchID],i)
{

T.boundaryField)([patchID][i] = T.boundaryField()[patchID][i]-DT;
------------
-------------------------- (some code for spoces) ........
T.write();

}

I am getting following error

error: assignment of read-only location ‘(&(&(& T)->Foam::GeometricField<Type, PatchField, GeoMesh>::boundaryField<double,.....

How to resolve this condition I want to correct the temperature T with some differet function based on spices flux. please help

[Sugajen]

Hi all,

I had a similar problem of read-only and added Ref to the boundaryField. But the values that I assign are not reflected on the output. Where am I going wrong ?

 label upMem = mesh.boundaryMesh().findPatchID("upperMembrane");
forAll( U.boundaryFieldRef()[upMem], i)
{
	U.boundaryFieldRef()[upMem][i].component(vector::X) = 0;
	U.boundaryFieldRef()[upMem][i].component(vector::Y) = 0;
	U.boundaryFieldRef()[upMem][i].component(vector::Z) = Jw.boundaryFieldRef()[upMem][i];

}

[Zhiheng Wang]

Store script in some file "patch.H" and include file as #include "patch.H" in pEqn.H before U.correctBoundary()
This will reflect effect of code in boundary

Sent from my Lenovo K50a40 using CFD Online Forum mobile app

[Sugajen]

Thank you Zhiheng!

It worked after I changed the boundary conditions to (0.0, 0.0, 0.0) instead of noSlip. Looks like noSlip overwrites whatever we do!

[Zhiheng Wang]

Yes you need to write type fixedValue ;
Uniform (0.0 0.0 0.0);

Sent from my Lenovo K50a40 using CFD Online Forum mobile app

[superkelle]

Originally Posted by kittychunk

This solved the problem for me.

The summary version is that you need to replace instances of "boundaryField()" and "internalField()" with "boundaryFieldRef()" and "internalFieldRef()" if you want to modify them in your code. The non-"Ref" calls are const now.

Update

Seems like internalField and internalFieldRef have been replaced by direct calls to the field variable. Eg: U.internalField() becomes U() for a const reference to the internal field, or U.ref() for non-const access. See associated bug report.

I now searched a whole day for this. For me it is nearly impossible to get solutions for those problems by myself. Does anybody has an advice how to find those problems that occure by changes in the "openfoam language"? I mean I read many codes where

.boundaryField()

worked fine, and I got nearly crazy when it did not work for me. What is the best workflow to find the root of the problem in openfoam? I mean, I would never have assumed that they changed the functionality of ".boundaryField()" in the src code.