[samwong]

Hi all,

I followed the tutorial,
https://wiki.openfoam.com/Programming2
http://www.wolfdynamics.com/wiki/pro...streamINIT.pdf
and tried to learn using codeStream in Dictionary to set B.C.
And I found that OFv1906 has a different definition of writeEntry.

with the original line,
writeEntry(os, "", alpha);
this error pop up
error: ‘Foam::scalarField {aka class Foam::Field<double>}’ has no member named ‘writeEntry ’

then I follow the instruction in
src/OpenFOAM/db/dictionary/functionEntries/codeStream/codeStream.H
and change the line to
alpha.writeEntry("",os);

this error pop up
/home/sam/OpenFOAM/sam-v1906/run/codeStream_INIT/fillBox_BCIC/0/alpha.water.#codeStream:59:15: error: ‘Foam::scalarField {aka class Foam::Field<double>}’ has no member named ‘writeEntry ’

What's happening.?

[samwong]

Anyone? please help

[olesen]

Originally Posted by samwong

Hi all,

I followed the tutorial,
https://wiki.openfoam.com/Programming2
http://www.wolfdynamics.com/wiki/pro...streamINIT.pdf
and tried to learn using codeStream in Dictionary to set B.C.
And I found that OFv1906 has a different definition of writeEntry.

with the original line,
writeEntry(os, "", alpha);
this error pop up
error: ‘Foam::scalarField {aka class Foam::Field<double>}’ has no member named ‘writeEntry ’

then I follow the instruction in
src/OpenFOAM/db/dictionary/functionEntries/codeStream/codeStream.H
and change the line to
alpha.writeEntry("",os);

this error pop up
/home/sam/OpenFOAM/sam-v1906/run/codeStream_INIT/fillBox_BCIC/0/alpha.water.#codeStream:59:15: error: ‘Foam::scalarField {aka class Foam::Field<double>}’ has no member named ‘writeEntry ’

What's happening.?

The second one with

field.writeEntry(keyword, os);

must work. Need to check if there is something else wrong.



https://develop.openfoam.com/Develop...d/Field.H#L361

[missios]

I just wanted to add a small implementation based on the above discussion. It is not the same field but the procedure remains sort of similar.


So, scope of the folowing code stream is the generation of Taylor-Green Vortex initial conditions in order to simulate some canonical DNS case. The files that codestream needs to be used is the velocity file U under the 0 directory as well as the pressure file p under the same directory.


Here are attached the code snippets of those files



First is given the U file

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2006                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

//internalField   uniform (0 0 0);

internalField   #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);
            const fvMesh& mesh = refCast<const fvMesh>(d.db());
            vectorField U_0(mesh.nCells(), Foam::Vector<double>(0.,0.,0.));

            forAll(U_0, i)
            {
                const scalar x = mesh.C()[i][0];
                const scalar y = mesh.C()[i][1];
                const scalar z = mesh.C()[i][2];
                U_0[i] = Foam::Vector<double>(-Foam::cos(x)
                *Foam::sin(y), Foam::sin(x)
                *Foam::cos(y), 0.);   
            }

            U_0.writeEntry("",os)   ;
        #};
    };

boundaryField
{
    upperBoundary      
    {
        type            cyclic;
    }

    lowerBoundary      
    {
        type            cyclic;
    }

    leftBoundary
    {
        type            cyclic;
    }

    rightBoundary
    {
        type            cyclic;
    }

    frontAndBack    
    {
        type            empty;
    }
}
// ************************************************************************* //

and in the same logic is generated the p file

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2006                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -2 0 0 0 0];

//internalField   uniform 0;
internalField   #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);
            const fvMesh& mesh = refCast<const fvMesh>(d.db());
            scalarField p_0(mesh.nCells(), 0.);
            forAll(p_0, i)
            {  
                const scalar x = mesh.C()[i][0];
                const scalar y = mesh.C()[i][1];
                const scalar z = mesh.C()[i][2];
                p_0[i]=-0.25*(Foam::cos(2*x) + Foam::cos(2*y));
            }
            p_0.writeEntry("",os)   ;
        #};
    };


boundaryField
{
    upperBoundary
    {
        type            cyclic;
    }

    lowerBoundary
    {
        type            cyclic;
    }
    
    leftBoundary
    {
        type            cyclic;
    }

    rightBoundary
    {
        type            cyclic;
    }

    frontAndBack    
    {
        type            empty;
    }
}


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

I hope this can be useful.



Best

K