[Mohammadmz]

Hi

I have error in codeStream at openFoam v10

Error:

error: ‘Foam::scalarField’ {aka ‘class Foam::Field<double>’} has no
member named ‘writeEntry’
make: *** [/opt/openfoam10/wmake/rules/General/transform:26:
Make/linux64GccDPInt32Opt/codeStreamTemplate.o] Error 1

I searched it, this error about syntax of "writeEntry()", this syntax is changed in new versions but i can't found it.

please help me to solve it.

[Mohammadmz]

please help me. i need it.

[Tobermory]

It's difficult, my friend, to help you without more information! Please attach the codestream and then we can maybe comment?

[Mohammadmz]

/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 10
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object alpha.water;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 0 0 0 0 0 0];

internalField uniform 0;

boundaryField
{

inlet
{
type fixedValue;
value #codeStream
{
codeInclude
#{
#include "fvCFD.H"
#};
codeOptions
#{
-I$(LIB_SRC)/finiteVolume/lnInclude \
-I$(LIB_SRC)/meshTools/lnInclude
#};
codeLibs
#{
-lmeshTools \
-lfiniteVolume
#};
code
#{
const IOdictionary& d = static_cast<const IOdictionary&>
(
dict.parent().parent()
);
const fvMesh& mesh = refCast<const fvMesh>(d.db());
const label id = mesh.boundary().findPatchID("inlet");
const fvPatch& patch = mesh.boundary()[id];
scalarField a(patch.size(), scalar(0));
const scalar h = 3;
forAll(a, i) //equivalent to for (int i=0; patch.size()<i; i++)
{
const scalar z = patch.Cf()[i][2];
if(z<h)
a[i] = scalar(1);
}
a.writeEntry("", os);
#};
};
}
outlet
{
type zeroGradient;
}
cylinder
{
type zeroGradient;
}
walls
{
type zeroGradient;
}
bed
{
type zeroGradient;
}
atm
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}
}

// ************************************************** *********************** //

[Tobermory]

Check your syntax: I think that the correct writeEntry method is in dictionaryTemplates.C (line 210 - you can find this by using Doxygen and seraching on the overloaded method version with the right parameters):

 template<class EntryType>
 void Foam::writeEntry
 (
     Ostream& os,
     const word& entryName,
     const EntryType& value
 )
 {
     writeKeyword(os, entryName);
     writeEntry(os, value);
     os << token::END_STATEMENT << endl;
 }

and the call to it should be written as:

writeEntry(os, "", a);

Try this instead, and see if it compiles.

[Mohammadmz]

It solved.
Thanks & Regards.