[nlc]

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

  --> 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 !

[nlc]

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

    ground
    {
      type ABLz0kWall;
      //z0       uniform 0.1;
      /**/
      #include        "include/z0Field"
      z0 nonuniform   $z0Field;
      /**/
      kappa           0.41;
      Cmu             0.09;
    }

with include/z0Field

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
              );

[nlc]

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:

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:

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

[nlc]

apparently the too errors

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

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++ !!

but still this error remains

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

[nlc]

Found the reason for the error :

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

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

instead of

fvPatchField::rmap(ptf, addr);

And the error is gone !!

works fine now tanks for reading