[OpenFOAM] How to correctly show the result of #codeStream# internalField?

chengdi · May 7, 2017, 06:38

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.

wyldckat · May 7, 2017, 08:34

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
    #};

chengdi · May 8, 2017, 02:08

Dear Bruno

Thank you so much for you reply!

chengdi · May 8, 2017, 02:18

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?

Antimony · May 8, 2017, 04:44

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

wyldckat · May 8, 2017, 19:19

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.

chengdi · May 9, 2017, 02:51

Dear Bruno

Thanks for your suggestion. I will try foamToVTK.

gtarang · May 18, 2017, 15:58

Hi,
I am using OpenFOAM 4.1 for melting and solidification problem. I am following this thread Marangoni bc 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

chengdi · May 19, 2017, 23:47

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

gtarang · May 20, 2017, 00:54

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

chengdi · May 20, 2017, 22:38

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.

gtarang · May 21, 2017, 06:33

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?

chengdi · June 12, 2017, 10:34

Quote:

Originally Posted by gtarang

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.

gaza · September 7, 2017, 10:08

Hi
I use codeStream BC for U
I tried to access time as you posted in How to correctly show the result of #codeStream# internalField?

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?

rarnaunot · July 4, 2018, 09:14

Hi Foamers,

I got the same error as you:

Quote:

Originally Posted by gaza

Hi
I use codeStream BC for U
I tried to access time as you posted in How to correctly show the result of #codeStream# internalField?

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:

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

Do you know what is wrong?

How did you solve this error?

Thanks!

gaza · July 5, 2018, 08:34

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

rarnaunot · July 5, 2018, 10:18

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

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

gaza · July 5, 2018, 13:04

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

or search on the forum

Ali Amarloo · September 21, 2018, 08:41

Quote:

Originally Posted by gaza

Hi
I use codeStream BC for U
I tried to access time as you posted in How to correctly show the result of #codeStream# internalField?

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?

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"?

gaza · September 21, 2018, 14:25

change

Code:

fixedValue

into

Code:

codedFixedValue

May 7, 2017, 08:34		#2
wyldckat Retired Super Moderator Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,974 Blog Entries: 45 Rep Power: 128	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 #}; tariq and anon_q like this. __________________ OpenFOAM: FAQ \| Getting started Forum: How to get help, to post code/output and forum guide Read this before sending me PM

May 8, 2017, 19:19		#6
wyldckat Retired Super Moderator Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,974 Blog Entries: 45 Rep Power: 128	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. tariq and virengos like this.

July 5, 2018, 08:34		#16
gaza Senior Member Przemek Join Date: Jun 2011 Posts: 249 Rep Power: 15	Hi I did not solve this. I used codedFixedValue instead of fixedValue. rarnaunot likes this. __________________ best regards pblasiak

July 5, 2018, 13:04		#18
gaza Senior Member Przemek Join Date: Jun 2011 Posts: 249 Rep Power: 15	you can find basic info here https://www.openfoam.com/documentati...xed-value.html or search on the forum __________________ best regards pblasiak

September 21, 2018, 14:25		#20
gaza Senior Member Przemek Join Date: Jun 2011 Posts: 249 Rep Power: 15	change Code: fixedValue into Code: codedFixedValue atulkjoy likes this. __________________ best regards pblasiak

May 8, 2017, 02:08		#3
chengdi Member Di Cheng Join Date: May 2010 Location: Beijing, China Posts: 47 Rep Power: 15	Dear Bruno Thank you so much for you reply!

May 8, 2017, 04:44		#5
Antimony Senior Member Join Date: Aug 2013 Posts: 407 Rep Power: 15	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

May 9, 2017, 02:51		#7
chengdi Member Di Cheng Join Date: May 2010 Location: Beijing, China Posts: 47 Rep Power: 15	Dear Bruno Thanks for your suggestion. I will try foamToVTK.

May 19, 2017, 23:47		#9
chengdi Member Di Cheng Join Date: May 2010 Location: Beijing, China Posts: 47 Rep Power: 15	I think you can use post-processor to calculate grad(T)

May 20, 2017, 00:54		#10
gtarang Member Tarang Join Date: Feb 2011 Location: Delhi, India Posts: 47 Rep Power: 15	Will I be able to use "post process"ed grad(T) as volVectorField in boundaryConditionFvPatchField?

May 20, 2017, 22:38		#11
chengdi Member Di Cheng Join Date: May 2010 Location: Beijing, China Posts: 47 Rep Power: 15	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.

May 21, 2017, 06:33		#12
gtarang Member Tarang Join Date: Feb 2011 Location: Delhi, India Posts: 47 Rep Power: 15	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?

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Difference of the max function result with full field, internalField and boundaryFiel	cyss38	OpenFOAM Programming & Development	1	October 2, 2018 05:39
CFD post cannot load results-Error appeared?	mariam.sara	ANSYS	9	September 17, 2018 15:23
[Workbench] Current result file may not contain requested result data	zhizhuo	ANSYS Meshing & Geometry	0	December 13, 2017 04:18
Simulation won't show turbulence	pete_87	OpenFOAM Running, Solving & CFD	4	June 25, 2014 11:35
Geometry show in Result Display	ShFlow	FLOW-3D	3	January 11, 2009 20:51