CFD Online Discussion Forums - boundary condition scalarField in parallel

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM (https://www.cfd-online.com/Forums/openfoam/)

- - boundary condition scalarField in parallel (https://www.cfd-online.com/Forums/openfoam/81011-boundary-condition-scalarfield-parallel.html)

boundary condition scalarField in parallel

I'm trins to compile my boundary condition using a scalarField It work but in parallel I get this warning:

Code:

  --> FOAM Warning : 

    From function Field<Type>::Field(const word& keyword, const dictionary&, const label)

    in file /home/niko/OpenFOAM/OpenFOAM-1.7.1/src/OpenFOAM/lnInclude/Field.C at line 262

    Reading "/home/niko/OpenFOAM/niko-1.7.1/run/AEMN/testcase/ABL_kepsilonGroundShear/processor0/0/U::boundaryField::ground" from line 102 to line 105

    expected keyword 'uniform' or 'nonuniform', assuming deprecated Field format from Foam version 2.0.

Reading/calculating face flux field phi

And the const scalarField z0_ change but it is not suppose to !

To do this patch I use fixed shear stress and nut rough wall as example.

Thanks for the help !

The k file in the 0 folder has the ground boundary define:

Code:

    ground

    {

      type ABLz0kWall;

      //z0       uniform 0.1;

      /**/

      #include        "include/z0Field"

      z0 nonuniform   $z0Field;

      /**/

      kappa           0.41;

      Cmu             0.09;

    }

with include/z0Field

Code:

z0Field            List<scalar> 

        75(0.1 0.1 0.1 0.1 0.1 

           0.1 0.1 0.1 0.1 0.1 

           0.1 0.1 0.1 0.1 0.1 

           0.1 0.1 0.1 0.1 0.1 

              0.1 0.1 0.1 0.1 0.1 

              0.1 0.1 0.1 0.1 0.1 

              0.1 0.1 0.1 0.1 0.1 

             0.4 0.4 0.4 0.4 0.4 

              0.4 0.4 0.4 0.4 0.4 

              0.4 0.4 0.4 0.4 0.4 

              0.4 0.4 0.4 0.4 0.4 

              0.4 0.4 0.4 0.4 0.4 

              0.4 0.4 0.4 0.4 0.4 

              0.4 0.4 0.4 0.4 0.4 

              0.4 0.4 0.4 0.4 0.4

              );

I found an error that solve part of the problem, but now I try to use rmap and automap to make it possible to use in parallel.

My error was that in the write function I did not use the right function too write z0_ so I change it for:

Code:

z0_.writeEntry("z0", os);

now z0 write correctly but it is still a problem with parallel since rmap and automap are not define.

I try to add them as it is add in turbulentHeatFluxTemperatureFvPatchScalarField but i get this error:

Code:

Wall/epsilonWallFunctions/ABLz0epsilonWallFunction/ABLz0epsilonWallFunction.C: In member function ‘virtual void Foam::incompressible::RASModels::ABLz0epsilonWallFunction::autoMap(const Foam::fvPatchFieldMapper&)’:

Wall/epsilonWallFunctions/ABLz0epsilonWallFunction/ABLz0epsilonWallFunction.C:286: error: passing ‘const Foam::scalarField’ as ‘this’ argument of ‘void Foam::Field<Type>::autoMap(const Foam::FieldMapper&) [with Type = float]’ discards qualifiers

Wall/epsilonWallFunctions/ABLz0epsilonWallFunction/ABLz0epsilonWallFunction.C: In member function ‘virtual void Foam::incompressible::RASModels::ABLz0epsilonWallFunction::rmap(const Foam::fvPatchScalarField&, const Foam::labelList&)’:

Wall/epsilonWallFunctions/ABLz0epsilonWallFunction/ABLz0epsilonWallFunction.C:296: error: ‘template<class Type> class Foam::fvPatchField’ used without template parameters

Wall/epsilonWallFunctions/ABLz0epsilonWallFunction/ABLz0epsilonWallFunction.C:304: error: passing ‘const Foam::scalarField’ as ‘this’ argument of ‘void Foam::Field<Type>::rmap(const Foam::UList<T>&, const Foam::unallocLabelList&) [with Type = float]’ discards qualifiers

make: *** [Make/linux64GccSPOpt/ABLz0epsilonWallFunction.o] Erreur 1

thanks for the help

autoMap tryed to modify my const scalarField z0_ !!

apparently the too errors

Code:

Wall/epsilonWallFunctions/ABLz0epsilonWallFunction/ABLz0epsilonWallFunction.C:294: error: passing ‘const Foam::scalarField’ as ‘this’ argument of ‘void Foam::Field<Type>::autoMap(const Foam::FieldMapper&) [with Type = float]’ discards qualifiers

and

Code:

Wall/epsilonWallFunctions/ABLz0epsilonWallFunction/ABLz0epsilonWallFunction.C:313: error: passing ‘const Foam::scalarField’ as ‘this’ argument of ‘void Foam::Field<Type>::rmap(const Foam::UList<T>&, const Foam::unallocLabelList&) [with Type = float]’ discards qualifiers

are in my case related to the fact that I used a:

const scalarField z0_;

I change it for a:

scalarField z0_;

And those too error disappear. I guess it means i tried to modify the constant class z0_ with autoMap. So autoMap modify the member of the class !!! One day I'll get use to c++ error message. But now I'm still learning c++ :D !!

but still this error remains

Code:

Wall/epsilonWallFunctions/ABLz0epsilonWallFunction/ABLz0epsilonWallFunction.C: In member function ‘virtual void Foam::incompressible::RASModels::ABLz0epsilonWallFunction::rmap(const Foam::fvPatchScalarField&, const Foam::labelList&)’:

Wall/epsilonWallFunctions/ABLz0epsilonWallFunction/ABLz0epsilonWallFunction.C:304: error: ‘template<class Type> class Foam::fvPatchField’ used without template parameters

If some one can give me a cue on this error it will help me !!!
Regards

Found the reason for the error :

Code:

Wall/epsilonWallFunctions/ABLz0epsilonWallFunction/ABLz0epsilonWallFunction.C: In member function ‘virtual void Foam::incompressible::RASModels::ABLz0epsilonWallFunction::rmap(const Foam::fvPatchScalarField&, const Foam::labelList&)’:

Wall/epsilonWallFunctions/ABLz0epsilonWallFunction/ABLz0epsilonWallFunction.C:304: error: ‘template<class Type> class Foam::fvPatchField’ used without template parameters

As rmap is a virtual function and the mother of my class is a template with no rmap define I got confuse. The problem was that I was calling the rmap function without template parameters. So I had to define the parameters I used. In my case : <scalar>.

I use

Code:

fvPatchField<scalar>::rmap(ptf, addr);

instead of

Code:

fvPatchField::rmap(ptf, addr);

And the error is gone !!

works fine now tanks for reading