[LuisAlberto]

Good afternoon everyone,

I am trying to write a coded function object into my controlDict in order to play around with the calculation of yPlus and, by the way, learn more about programming in OpenFOAM.

At the moment, I am trying to do it in the way it is done in nutkWallFunctionFvPatchScalarField.C

The thing is that I need to include the header "incompressible/turbulenceModel/turbulenceModel.H" where the type turbulenceModel is defined, but when I run pisoFoam, he does not find the file.

However, he is able to find pointField.H (I don't need it, it is just for testing) Why does he find this one and not turbulenceModel.H? Code and errors below.

Any help is appreciated.

At the same time, any suggestions about how to compute the distance from the wall at the cells adjacent to it in a coded function objetct?

functions
{
    test
    {
        // Load the library containing the 'coded' functionObject
        functionObjectLibs ("libutilityFunctionObjects.so");
        type coded;
        // Name of on-the-fly generated functionObject
        redirectType error;

        codeInclude
        #{
        #include "pointField.H" // Why does he find this one but not the rest??
        #include "nutkWallFunctionFvPatchScalarField.H" // only in case he needed this to find the next, but not.
        #include "incompressible/turbulenceModel/turbulenceModel.H"
        #};

        codeOptions  // To try to fix the above files not found, but does not work
        #{
        -I /opt/openfoam231/src/turbulenceModels/
        #};

        code
        #{

        label patchID = mesh().boundaryMesh().findPatchID("movingWall");
        const turbulenceModel& turbModel =
                db().lookupObject<turbulenceModel>("turbulenceModel");
        const scalarField& y = turbModel.y()[patchID];
        #};
    }
}

could not open file nutkWallFunctionFvPatchScalarField.H for source file functionObjectTemplate.C due to No such file or directory
could not open file incompressible/turbulenceModel/turbulenceModel.H for source file functionObjectTemplate.C due to No such file or directory
Making dependency list for source file FilterFunctionObjectTemplate.C
could not open file nutkWallFunctionFvPatchScalarField.H for source file FilterFunctionObjectTemplate.C due to No such file or directory
could not open file incompressible/turbulenceModel/turbulenceModel.H for source file FilterFunctionObjectTemplate.C due to No such file or directory
In file included from functionObjectTemplate.C:26:0:

Thanks,

Luis

[mkraposhin]

The problem is that you must point include directory "-I" to lnInclude, for example

-I$(FOAM_SRC)/turbulenceModels/incompressible/turbulenceModel/lnInclude \
-I$(FOAM_SRC)/turbulenceModels/incompressible/RAS/lnInclude \

You can find how to add proper include directories for RAS/LES incompressible models in file Make/options of pimpleFoam solver ($FOAM_APP/solvers/incompressible/pimpleFoam)

[LuisAlberto]

Thank you very much mkraposhin,

Following your suggestion, it finally finds it using

        codeOptions
        #{
        -I$(FOAM_SRC)/turbulenceModels/incompressible/turbulenceModel/lnInclude \
        -I$(FOAM_SRC)/transportModels \
        #};

However, even after including turbulenceModel.H, it still says that 'burbulenceModel' does not name a type. Any clue why, or any suggestions for a work-around for obtaining the distances to the wall? (I am going to try to do it also following the way it is done in yPlusRAS or yPlusLES).

/home/lpadron/OpenFOAM/lpadron-2.3.1/run/tutorials/incompressible/pisoFoam/ras/cavity-test-yplus-coded/system/controlDict.functions.test:74:8: error: ‘turbulenceModel’ does not name a type

Any suggestiong?

thanks!

[mkraposhin]

Hello, are using incompressible or compressible turbulence model?

If turbulence mode is incompressible, then you must declare variable for it using namespace Foam::incompressible, for example:

const Foam::incompressible::turbulenceModel& turbModel =
                db().lookupObject<Foam::incompressible::turbulenceModel>("turbulenceModel");

You can see example in "createFields.H" of pimpleFoam solver sources

[LuisAlberto]

Thank you very much mkraposhin,

It indeed works that way. I should have realized that it was a TypeName that could be found in Doxygen and going to Namespaces->Incompressible (Foam::incompressible) ->class turbulenceModel (the one whose header I include), and there you find typeName turbulenceModel as the run-time information for the turbulence model. Of course, you can directly search for turbulence model in Doxygen. Thanks.

My only doubt there, perhaps you can help me, is why 'turbulenceModel' does not appear in Doxygne's Namespaces -> Namespace members.

In case it might be of use to someone in the future, the final working code to add at the end of controlDict is:

functions
{
    test
    {
        // Load the library containing the 'coded' functionObject
        functionObjectLibs ("libutilityFunctionObjects.so");
        type coded;
        // Name of on-the-fly generated functionObject
        redirectType error;

        codeInclude
        #{
        #include "turbulenceModel.H"
        #};

        codeOptions
        #{
        -I$(FOAM_SRC)/turbulenceModels/incompressible/turbulenceModel/lnInclude \
        -I$(FOAM_SRC)/transportModels \
        #};

        code
        #{

        label patchID = mesh().boundaryMesh().findPatchID("movingWall");
        const Foam::incompressible::turbulenceModel& turbModel =
                mesh().thisDb().lookupObject<Foam::incompressible::turbulenceModel>("turbulenceModel");

        const scalarField& y = turbModel.y()[patchID];

        Info << "y= " << y << endl;
        #};
    }
}