CFD Online Discussion Forums - [OpenFOAM] How to correctly show the result of #codeStream# internalField?

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

- ParaView (https://www.cfd-online.com/Forums/paraview/)

- - [OpenFOAM] How to correctly show the result of #codeStream# internalField? (https://www.cfd-online.com/Forums/paraview/187463-how-correctly-show-result-codestream-internalfield.html)

How to correctly show the result of #codeStream# internalField?

Hi, everyone

I just used codeStream to generate some initial condtion and codedFixedValue to generate some boundary condtion. The codedFixedValue BC can be correctly executed and loaded using paraFoam (I am using OF1612+ in docker), however, the codeStream initial condition can be correctly interpreted and executed but cannot be loaded in paraFoam.

I was running the forwardStep with following "0/U" file

Code:

/*--------------------------------*- C++ -*----------------------------------*\



| =========                 |                                                 |



| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |



|  \\    /   O peration     | Version:  plus                                  |



|   \\  /    A nd           | Web:      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 (3 0 0);







internalField  #codeStream



{



    code



    #{



        const IOdictionary& d = static_cast<const IOdictionary&>(dict);



        const fvMesh& mesh = refCast<const fvMesh>(d.db());



        



        vectorField T(mesh.nCells());







        const vectorField& CC = mesh.C(); //cell center 



        



        forAll(CC,cellI)



        {



            



            //spatial coordinates, type: scalar



                scalar x = CC[cellI].x();



                scalar y = CC[cellI].y(); 



                scalar z = CC[cellI].z();



                



                T[cellI] = vector(3+0.2*sin(10*x),0,0);



        }



                



        //void Foam::Field<Type>::writeEntry(const word& keyword, Ostream& os) const



        T.writeEntry("", os); 



    #};







    //! Optional:



    codeInclude



    #{



        #include "fvCFD.H"



    #};











    //! Optional:



    codeOptions



    #{



        -I$(LIB_SRC)/finiteVolume/lnInclude \



        -I$(LIB_SRC)/meshTools/lnInclude



    #};







    //! libs:



    codeLibs



    #{



        -lmeshTools



    #};



};







boundaryField



{







    inlet



    {



        type            codedMixed;



        refValue        uniform (3 0 0); //default value



        refGradient     uniform (0 0 0); //default value



        valueFraction   uniform 1;



        redirectType    linearOscillatingBC; //name of new BC type



        code



        #{



        const vectorField& Cf = patch().Cf(); // get face center coordinate;



        



        scalar ymax = max(Cf&vector(0,1,0)); // `&` is dot product



        scalar ymin = min(Cf&vector(0,1,0));



        // Info<<"ymax="<<ymax<<",ymin="<<ymin<<nl;



        



        vectorField& rvf = this->refValue();



        vectorField& rgf = this->refGrad();



        scalarField& vf = this->valueFraction();



        



        //temporal coordinate, type: scalar



        scalar t =this->db().time().value(); // get time



        //Oscillating parameters



        scalar omega = 5;



        scalar A = 0.2;



        scalar tt = (1+A*sin(omega*t)); // temporal term, separated



        



        forAll(Cf,faceI)



        {



                //spatial coordinates, type: scalar



                //scalar x = Cf[faceI].x();



                scalar y = Cf[faceI].y(); 



                //scalar z = Cf[faceI].z();



                rvf[faceI] = vector(((y-ymin)/(ymax-ymin)+2.5)*tt,0.0,0.0); 



                rgf[faceI] = Zero;



                vf[faceI] = 1.0;



        }







        #};



        



        //I do not know why I need to add those things



        //codeInclude



        //#{



        //    #include "fvCFD.H"



        //#};



        



        //codeOptions



        //#{



        //    -I$(LIB_SRC)/finiteVolume/lnInclude



        //#};



    }







    outlet



    {



        type            inletOutlet;



        inletValue      uniform (3 0 0);



        value           uniform (3 0 0);



    }







    bottom



    {



        type            symmetryPlane;



    }







    top



    {



        type            symmetryPlane;



    }







    obstacle



    {



        type            slip;



    }







    defaultFaces



    {



        type            empty;



    }



}







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

And here is the output of crashing paraFoam when I try to load the data.

Code:

Created temporary 'forwardStepMod3.OpenFOAM'

Using #codeStream at line 21 in file "/home/di/OpenFOAM/di-v1612+/run/forwardStepMod3/0/U"

Using #codeStream with "/home/di/OpenFOAM/di-v1612+/run/forwardStepMod3/dynamicCode/platforms/linux64GccDPInt32Opt/lib/libcodeStream_ba5ce8457724532859ca03bd0612f92a5665a90f.so"

Invoking wmake libso /home/di/OpenFOAM/di-v1612+/run/forwardStepMod3/dynamicCode/_ba5ce8457724532859ca03bd0612f92a5665a90f

wmake libso /home/di/OpenFOAM/di-v1612+/run/forwardStepMod3/dynamicCode/_ba5ce8457724532859ca03bd0612f92a5665a90f





--> FOAM FATAL IO ERROR: 

Failed loading library "/home/di/OpenFOAM/di-v1612+/run/forwardStepMod3/dynamicCode/platforms/linux64GccDPInt32Opt/lib/libcodeStream_ba5ce8457724532859ca03bd0612f92a5665a90f.so"

Did you add all libraries to the 'libs' entry in system/controlDict?



file: /home/di/OpenFOAM/di-v1612+/run/forwardStepMod3/0/U from line 17 to line 17.



    From function static void (* Foam::functionEntries::codeStream::getFunction(const Foam::dictionary&, const Foam::dictionary&))(Foam::Ostream&, const Foam::dictionary&)

    in file db/dictionary/functionEntries/codeStream/codeStream.C at line 309.



FOAM exiting

I also tried to add "/home/di/OpenFOAM/di-v1612+/run/forwardStepMod3/dynamicCode/platforms/linux64GccDPInt32Opt/lib/libcodeStream_ba5ce8457724532859ca03bd0612f92a5665 a90f.so" to my system/controlDict 's libs entry. Here is the output:

Code:

Created temporary 'forwardStepMod3.OpenFOAM'

--> FOAM Warning : 

    From function void* Foam::dlOpen(const Foam::fileName&, bool)

    in file POSIX.C at line 1244

    dlopen error : /home/di/OpenFOAM/di-v1612+/run/forwardStepMod3/dynamicCode/platforms/linux64GccDPInt32Opt/lib/libcodeStream_ba5ce8457724532859ca03bd0612f92a5665a90f.so: undefined symbol: _ZTIN4Foam6fvMeshE

--> FOAM Warning : 

    From function bool Foam::dlLibraryTable::open(const Foam::fileName&, bool)

    in file db/dynamicLibrary/dlLibraryTable/dlLibraryTable.C at line 101

    could not load "/home/di/OpenFOAM/di-v1612+/run/forwardStepMod3/dynamicCode/platforms/linux64GccDPInt32Opt/lib/libcodeStream_ba5ce8457724532859ca03bd0612f92a5665a90f.so"

Using #codeStream at line 21 in file "/home/di/OpenFOAM/di-v1612+/run/forwardStepMod3/0/U"

Using #codeStream with "/home/di/OpenFOAM/di-v1612+/run/forwardStepMod3/dynamicCode/platforms/linux64GccDPInt32Opt/lib/libcodeStream_ba5ce8457724532859ca03bd0612f92a5665a90f.so"

Invoking wmake libso /home/di/OpenFOAM/di-v1612+/run/forwardStepMod3/dynamicCode/_ba5ce8457724532859ca03bd0612f92a5665a90f

wmake libso /home/di/OpenFOAM/di-v1612+/run/forwardStepMod3/dynamicCode/_ba5ce8457724532859ca03bd0612f92a5665a90f





--> FOAM FATAL IO ERROR: 

Failed loading library "/home/di/OpenFOAM/di-v1612+/run/forwardStepMod3/dynamicCode/platforms/linux64GccDPInt32Opt/lib/libcodeStream_ba5ce8457724532859ca03bd0612f92a5665a90f.so"

Did you add all libraries to the 'libs' entry in system/controlDict?



file: /home/di/OpenFOAM/di-v1612+/run/forwardStepMod3/0/U from line 17 to line 17.



    From function static void (* Foam::functionEntries::codeStream::getFunction(const Foam::dictionary&, const Foam::dictionary&))(Foam::Ostream&, const Foam::dictionary&)

    in file db/dictionary/functionEntries/codeStream/codeStream.C at line 309.



FOAM exiting

I thought "_ZTIN4Foam6fvMeshE" must be something important. However, there is only one result from Google and I cannot see any related information in it.

Quick answer: You have this:

Code:

    codeOptions

    #{

        -I$(LIB_SRC)/finiteVolume/lnInclude \

        -I$(LIB_SRC)/meshTools/lnInclude

    #};







    //! libs:

    codeLibs

    #{

        -lmeshTools

    #};

Notice that in the first block here you mention "finiteVolume", but in the "codeLibs" block you don't mention it. This isn't a problem when using the solver, because the solver already has this library loaded in. Therefore, you need to update the second block to this:

Code:

    //! libs:

    codeLibs

    #{

        -lmeshTools \

        -lfiniteVolume

    #};

Dear Bruno

Thank you so much for you reply!

Hi Bruno,

I just tried to use "paraview" rather than "paraFoam" to post-process the result after time "0".

However, the "U" field cannot be read and here is the errors:

Code:

ERROR: In /home/buzz2/pawan/OpenFOAM/ThirdParty-1606_plus/ParaView-5.0.1/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 6497

vtkOpenFOAMReaderPrivate (0x40ace10): Error reading line 16332 of /home/di/OpenFOAM/di-v1612+/run/forwardStepMod3/8/U: Unsupported directive {

And here is content in "8/U"

Code:

internalField   nonuniform List<vector>

16128

(

(2.877288422651 -3.144469067245e-05 0)

...

)

;

        name            linearOscillatingBC;

        code            #{

        const vectorField& Cf = patch().Cf(); // get face center coordinate;



        scalar ymax = max(Cf&vector(0,1,0)); // `&` is dot product

        scalar ymin = min(Cf&vector(0,1,0));

        // Info<<"ymax="<<ymax<<",ymin="<<ymin<<nl;



        vectorField& rvf = this->refValue();

        vectorField& rgf = this->refGrad();

        scalarField& vf = this->valueFraction();



        //temporal coordinate, type: scalar

        scalar t =this->db().time().value(); // get time

        //Oscillating parameters

        scalar omega = 5;

        scalar A = 0.2;

        scalar tt = (1+A*sin(omega*t)); // temporal term, separated



        forAll(Cf,faceI)

        {

                //spatial coordinates, type: scalar

                //scalar x = Cf[faceI].x();

                scalar y = Cf[faceI].y();

                //scalar z = Cf[faceI].z();

                rvf[faceI] = vector(((y-ymin)/(ymax-ymin)+2.5)*tt,0.0,0.0);

                rgf[faceI] = Zero;

                vf[faceI] = 1.0;

        }



        #};

    }

    outlet 

    {

...

Is there any way to solve this problem?

Hi,

AFAIK, there isn't a very straightforward way to do this.

What I do is to open up the result file and modify the type from 'coded...' to 'fixedValue'. OF seems to write the values in any case (usually in the line/lines right below type) and so making this change allows Paraview to understand and display the velocity.

Hope this helps.

Cheers,
Antimony

Quick answer: If the file extension ".OpenFOAM" is not used and instead the built-in reader with ".foam" is used instead, then it will not work. You could try with ParaView 5.3, but I haven't tested it yet.

The only other solution is to use foamToVTK and then open the VTK files in ParaView.

Dear Bruno

Thanks for your suggestion. I will try foamToVTK.

Implementing a new IOobject

Hi,
I am using OpenFOAM 4.1 for melting and solidification problem. I am following this thread https://www.cfd-online.com/Forums/op...angoni-bc.html for writing marangoni BC. The boundary condition uses an IOobject of volVectorField gradT. The thread suggest putting IOobject in solver. I want to know the possibility of calculating gradT from controlDict using functionObjects or codeStream.

I have written the controlDict in this way

Code:

/*--------------------------------*- C++ -*----------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  4.1                                |

|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

FoamFile

{

    version     2.0;

    format      ascii;

    class       dictionary;

    location    "system";

    object      controlDict;

}

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



application     buoyantPimpleFoam;



startFrom       startTime;



startTime       0;



stopAt          endTime;



endTime         30.0;



deltaT          1.0;



writeControl    adjustableRunTime;



writeInterval   10;



purgeWrite      0;



writeFormat     ascii;



writePrecision  8;



writeCompression off;



timeFormat      general;



timePrecision   10;



runTimeModifiable yes;



adjustTimeStep  yes;



libs 

(

    "libmyBoundaryConditions.so"

    "libOpenFOAM.so"

);

/*

maxCo           0.25;



maxDeltaT       1;

maxAlphaCo      1;

*/



    #codeStream

    {

        code

        #{

            const IOdictionary& d = static_cast<const IOdictionary&>(dict);

            const fvMesh& mesh = refCast<const fvMesh>(d.db());

            volVectorField gradT

            (

                IOobject

                (

                    "gradT",

                    runTime.timeName(),

                    mesh,

                    IOobject::READ_IF_PRESENT,

                    IOobject::AUTO_WRITE

                ),

                fvc::grad(T)

            );



        #};

        /*codeInclude

        #{

            #include "fvCFD.H"

        #};*/

        codeOptions

        #{

            -I$(LIB_SRC)/finiteVolume/lnInclude \

            -I$(LIB_SRC)/meshTools/lnInclude \

        #};

        codeLibs

        #{

            -lmeshTools

        #};

    }





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

Kindly suggest me how can I calculate gradT.

--
Tarang

I think you can use post-processor to calculate grad(T)

Will I be able to use "post process"ed grad(T) as volVectorField in boundaryConditionFvPatchField?

sorry, I misunderstood your purpose.

As far as I know. #codeStream is just used to generate some "TEXT" in the controlDict or other text-based configuration file for OpenFOAM. If you want to use some volVectorField grad(T) in your BC. you must modify your solver.

Thanks chengdi. I have modified my solver to calculate gradT. One thing about the #codestream in controlDict I want to ask is that where in the execution flow process the code is executed?

Quote:

Originally Posted by gtarang (Post 649708)

Thanks chengdi. I have modified my solver to calculate gradT. One thing about the #codestream in controlDict I want to ask is that where in the execution flow process the code is executed?

I think #codeStream is just used to generate texts.

You may understand it like this:

When the foam app read the controlDict, what your app actually read is the text generated by your #codeStream at the start of the dict-entry-reading.

Hi
I use codeStream BC for U
I tried to access time as you posted in https://www.cfd-online.com/Forums/op...tml#post647952

However I got error "error: invalid use of ‘this’ in non-member function"
in the line scalar t = this->db().time().value();

My U file is

Code:

dimensions      [0 1 -1 0 0 0 0];



internalField   uniform (16 0 0);



boundaryField

{

    WALL

    {

        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("WALL");

                const fvPatch& patch = mesh.boundary()[id];

                

                vectorField U(patch.size(), vector(0, 0, 0));



                scalar t = this->db().time().value(); 



                forAll(U,i)

                {

                    U[i] = vector(1, 0., 0.);

                }



                U.writeEntry("", os);

            #};

        };

    }

Do you know what is wrong?

Hi Foamers,

I got the same error as you:

Quote:

Originally Posted by gaza (Post 663550)

Code:

.

.

.

.

                scalar t = this->db().time().value(); 

.

.

.

.

Do you know what is wrong?

How did you solve this error?

Thanks!

Hi
I did not solve this. I used codedFixedValue instead of fixedValue.

:confused: I'm not really into the difference between codedFixedValue and fixedValue. But i am initializing a IC so I use: internalField #codeStream

Quote:

Originally Posted by gaza (Post 698282)

Hi
I did not solve this. I used codedFixedValue instead of fixedValue.

you can find basic info here
https://www.openfoam.com/documentati...xed-value.html

or search on the forum

Quote:

Originally Posted by gaza (Post 663550)

Code:

dimensions      [0 1 -1 0 0 0 0];



internalField   uniform (16 0 0);



boundaryField

{

    WALL

    {

        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("WALL");

                const fvPatch& patch = mesh.boundary()[id];

                

                vectorField U(patch.size(), vector(0, 0, 0));



                scalar t = this->db().time().value(); 



                forAll(U,i)

                {

                    U[i] = vector(1, 0., 0.);

                }



                U.writeEntry("", os);

            #};

        };

    }

Do you know what is wrong?

I have the same problem
It seems that by "scalar t = this->db().time().value(); " we can access time just for codedFixedvalue
Does anybody know how can I access time (of simulation) in "codeStream"?

change

Code:

fixedValue

into

Code:

codedFixedValue