[MartinB]

Hi again,

I found the bug: a bracket related problem... so here comes the (hopefully) correct parallel version:

#include "RASModel.H"
// write matlab file

{
    Info << "Writing Area of the cells on the patch!" << endl;

    word wallPatchName = "obstacle";
    Info << "Searching for patch " << wallPatchName << endl;

    // Check, if the patch name exists:
    label patchID = mesh.boundaryMesh().findPatchID(wallPatchName);
    if (patchID < 0)
    {
        Info << "No patch found with name \"" << wallPatchName << "\"!"
        << endl;
    }

    // Pointer to the patch we want to have shear stress for:
    const polyPatch& cPatch = mesh.boundaryMesh()[patchID];
    label nFaces = cPatch.size();

    pointField faceAreas(nFaces, vector(0,0,0));

    label runFaces = 0;

    // collecting the interesting data
    for (int i=0; i<nFaces; i++)
    {
        faceAreas[runFaces] = mesh.Sf().boundaryField()[patchID][i];
        runFaces++;
    }

    // for parallel
    reduce(nFaces, sumOp<label>());
    Info << "Number of global faces: " << nFaces << endl;

    // make a cute filename
    fileName casePath = cwd();//casePath.name();
    fileName caseName = casePath.name();
    fileName myFile = "area.dat";
    Info << "Data is written to file " << myFile << endl;

    // create a new file
    OFstream *myStream = NULL;
    if (Pstream::master())
    {
        myStream = new OFstream(myFile);
    }

    // slaves send data to master, master writes data to file
    if (Pstream::parRun())
    {
        if (Pstream::myProcNo() != Pstream::masterNo())
        {
            OPstream toMaster(Pstream::blocking, Pstream::masterNo());
            toMaster << faceAreas;
        }
        else // master part
        {
            // first write own data
            for (int i=0; i<faceAreas.size(); i++)
            {
                *myStream << i << ";"
                << mag(faceAreas[i]) << endl;

            }

            label run = faceAreas.size();

            // then receive slave data and write
            pointField bufferFaceAreas;

            for (int slave=Pstream::firstSlave(); slave <= Pstream::lastSlave(); slave++)
            {
                IPstream fromSlave(Pstream::blocking, slave);
                fromSlave >> bufferFaceAreas;

                for (int i=0; i<bufferFaceAreas.size(); i++)
                {
                    *myStream << run << "; "
                    << mag(bufferFaceAreas[i]) << endl;
                    run++;
                }
            }
        }
    }
    else // single processor only
    {
        for (int i=0; i<nFaces; i++)
        {
            *myStream << i << "; "
            << mag(mesh.Sf().boundaryField()[patchID][i]) << endl;
        }
    }

}

Have fun

Martin

[Andrea_85]

Hi Martin,

after wclean and wmake i got this error (i dont know if the instructions that you had given to compile simpleFoam are the same for interFoam (the solver that i use) but seems that there is some error on #include RASModel.H)

Making dependency list for source file interFoam.C
could not open file RASModel.H for source file interFoam.C
SOURCE=interFoam.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-40 -I/opt/OpenFOAM/OpenFOAM-1.7.0/src/transportModels -I/opt/OpenFOAM/OpenFOAM-1.7.0/src/transportModels/incompressible/lnInclude -I/opt/OpenFOAM/OpenFOAM-1.7.0/src/transportModels/interfaceProperties/lnInclude -I/opt/OpenFOAM/OpenFOAM-1.7.0/src/turbulenceModels/incompressible/turbulenceModel -I/opt/OpenFOAM/OpenFOAM-1.7.0/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude -I/opt/OpenFOAM/OpenFOAM-1.7.0/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/interFoam.o
In file included from interFoam.C:125:
write.H:1:22: error: RASModel.H: No such file or directory
/opt/OpenFOAM/OpenFOAM-1.7.0/src/finiteVolume/lnInclude/readPISOControls.H: In function â:
/opt/OpenFOAM/OpenFOAM-1.7.0/src/finiteVolume/lnInclude/readPISOControls.H:11: warning: unused variable â
/opt/OpenFOAM/OpenFOAM-1.7.0/src/finiteVolume/lnInclude/readPISOControls.H:14: warning: unused variable â
/opt/OpenFOAM/OpenFOAM-1.7.0/src/finiteVolume/lnInclude/readPISOControls.H:3: warning: unused variable â
/opt/OpenFOAM/OpenFOAM-1.7.0/src/finiteVolume/lnInclude/readPISOControls.H:8: warning: unused variable â
/opt/OpenFOAM/OpenFOAM-1.7.0/src/finiteVolume/lnInclude/readPISOControls.H:11: warning: unused variable â
/opt/OpenFOAM/OpenFOAM-1.7.0/src/finiteVolume/lnInclude/readPISOControls.H:14: warning: unused variable â

make: *** [Make/linux64GccDPOpt/interFoam.o] Error 1


Thanks again

Andrea

[MartinB]

Hi Andrea,

just remove the line "#include RASModel.H". It was necessary for wall shear stress calculation in the original piece of code...

Martin

[Andrea_85]

I figured that was enough to remove that line. I just launched a test. I write to you in case there are errors. Thank you very much for all your help.

Andrea

[Andrea_85]

Hi Martin, everything works fine!

I am taking advantage of your patience to ask another thing. I would like to calculate the gradient of alpha1 for each cell and each time step. I tried to write this piece of code: writeGradientAlpha1.C (writeCellVolumes.C them).
Please look if is ok. I do not know if i have included the right source file (.H).
I guess the function to calculate gradient is fvcGrad:field).

#include "argList.H"
#include "timeSelector.H"
#include "Time.H"
#include "fvMesh.H"
#include "vectorIOField.H"
#include "volFields.H"
#include "fvcGrad.H"

using namespace Foam;

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

// Main program:

int main(int argc, char *argv[])
{
    timeSelector::addOptions();

#   include "setRootCase.H"
#   include "createTime.H"

    instantList timeDirs = timeSelector::select0(runTime, args);

#   include "createMesh.H"

    forAll(timeDirs, timeI)
    {
        runTime.setTime(timeDirs[timeI], timeI);

        Info<< "Time = " << runTime.timeName() << endl;

        // Check for new mesh
        mesh.readUpdate();

        volVectorField gradAlpha1
    (
            IOobject
            (
                    "GradAlpha1",
                    runTime.timeName(),
                    mesh,
                    IOobject::NO_READ,
                    IOobject::AUTO_WRITE
            ),
            volVectorField gradAlpha1 = fvc::grad(alpha1)

    );



         Info<< "Writing gradAlpha1 to " << gradAlpha1.name() << " in "
             << runTime.timeName() << endl;

         gradAlpha1.write();

    }

    Info<< "\nEnd" << endl;

    return 0;
}


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

thanks a lot
andrea

[MartinB]

Hi Andrea,

you must read the alpha1 field from disk first, otherwise your tool doesn't know what to work on.

Extract the attached tool to your user directory, for example .../OpenFOAM/andrea-1.7.1/ and call wmake in the new folder.

Have fun

Martin

[Andrea_85]

Hi,

can i put this code in the /home/../applications/utilities/postProcessing/miscellaneous/ like writeCellCenter?

for the next help I guess I will have to pay!!

Thanks

andrea

[MartinB]

Yes, you can.

Please have a look at the file
Make/options

Right now the executable is written to
$(FOAM_USER_APPBIN)
so only you have access to it. If you want to make it available globally (for other users), you may want to change this variable to
$(FOAM_APPBIN)

Martin

[Andrea_85]

Yes, i know that.

Thanks a lot
andrea

[Andrea_85]

Hi Martin,
I have copied all file in the right directory and then wmake. When i call writeGradientAlpha1 from my case directory i got this error:

| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 1.7.0-21131bcbd876
Exec : writeGradientAlpha1
Date : Feb 14 2011
Time : 12:28:14
Host : master.cluster
PID : 25375
Case : /home/aferrari/Simulation/OstacoliRandom/simm2e-2alpha30/simmetricou2e-2
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Time = 0
Reading field alpha1



--> FOAM FATAL IO ERROR:
Unknown patchField type constantAlphaContactAngle for patch type wall

Valid patchField types are :

41
(
advective
buoyantPressure
calculated
cyclic
directMapped
directionMixed
empty
fan
fixedFluxPressure
fixedGradient
fixedInternalValue
fixedPressureCompressibleDensity
fixedValue
freestream
freestreamPressure
inletOutlet
inletOutletTotalTemperature
mixed
oscillatingFixedValue
outletInlet
partialSlip
processor
rotatingTotalPressure
sliced
slip
symmetryPlane
syringePressure
timeVaryingMappedFixedValue
timeVaryingMappedTotalPressure
timeVaryingTotalPressure
timeVaryingUniformFixedValue
timeVaryingUniformInletOutlet
totalPressure
totalTemperature
turbulentInlet
turbulentIntensityKineticEnergyInlet
uniformDensityHydrostaticPressure
uniformFixedValue
waveTransmissive
wedge
zeroGradient
)


file: /home/aferrari/Simulation/OstacoliRandom/simm2e-2alpha30/simmetricou2e-2/0/alpha1::boundaryField::wall.4 from line 263883 to line 263885.

From function fvPatchField<Type>::New(const fvPatch&, const DimensionedField<Type, volMesh>&, const dictionary&)
in file /opt/OpenFOAM/OpenFOAM-1.7.0/src/finiteVolume/lnInclude/newFvPatchField.C at line 110.


I use constantAlphaContactAngle patch instead of simply wall.

Thanks
andrea

[MartinB]

Hi Andrea,

to use the writeGradientAlpha1 tool in OpenFOAM-1.7.0 replace the lines in writeGradientAlpha1/Make/options with:

EXE_INC = \
    -I$(LIB_SRC)/transportModels \
    -I$(LIB_SRC)/transportModels/incompressible/lnInclude \
    -I$(LIB_SRC)/transportModels/interfaceProperties/lnInclude \
    -I$(LIB_SRC)/turbulenceModels/incompressible/turbulenceModel \
    -I$(LIB_SRC)/finiteVolume/lnInclude

EXE_LIBS = \
    -ltwoPhaseInterfaceProperties \
    -lincompressibleTransportModels \
    -lincompressibleTurbulenceModel \
    -lincompressibleRASModels \
    -lincompressibleLESModels \
    -lfiniteVolume

Rebuild with
wclean
wmake

Martin

[Andrea_85]

Thanks Martin,

the correct library for the interface properties is : -linterfaceProperties \ .
I had an error with -ltwoPhaseInterfaceProperties \.

Thanks again

andrea

[Andrea_85]

Hi Martin

I tried to edit your file to calculate the curvature of the interface, according to the calculations found in interfaceProperties.C
Attached my writeCurvature.C.

i got this error
SOURCE=writeCurvature.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-40 -I/opt/OpenFOAM/OpenFOAM-1.7.0/src/transportModels -I/opt/OpenFOAM/OpenFOAM-1.7.0/src/transportModels/incompressible/lnInclude -I/opt/OpenFOAM/OpenFOAM-1.7.0/src/transportModels/interfaceProperties/lnInclude -I/opt/OpenFOAM/OpenFOAM-1.7.0/src/turbulenceModels/incompressible/turbulenceModel -I/opt/OpenFOAM/OpenFOAM-1.7.0/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude -I/opt/OpenFOAM/OpenFOAM-1.7.0/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/writeCurvature.o
In file included from /opt/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude/GeometricField.C:1273,
from /opt/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude/GeometricField.H:586,
from /opt/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude/GeometricScalarField.H:38,
from /opt/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude/GeometricFields.H:34,
from /opt/OpenFOAM/OpenFOAM-1.7.0/src/finiteVolume/lnInclude/volFields.H:37,
from writeCurvature.C:35:
/opt/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude/GeometricFieldFunctions.C: In function â:
/opt/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude/GeometricFieldFunctions.C:950: instantiated from â
writeCurvature.C:98: instantiated from here
/opt/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude/GeometricFieldFunctions.C:950: error: no matching function for call to â
/opt/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude/scalarField.H:77: note: candidates are: void Foam::add(Foam::Field<double>&, const Foam::scalar&, const Foam::UList<double>&)
/opt/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude/scalarField.H:77: note: void Foam::add(Foam::Field<double>&, const Foam::UList<double>&, const Foam::scalar&)
/opt/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude/labelField.H:53: note: void Foam::add(Foam::Field<int>&, const Foam::label&, const Foam::UList<int>&)
/opt/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude/labelField.H:53: note: void Foam::add(Foam::Field<int>&, const Foam::UList<int>&, const Foam::label&)
/opt/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude/GeometricFieldFunctions.C:950: instantiated from â
writeCurvature.C:98: instantiated from here
/opt/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude/GeometricFieldFunctions.C:950: error: no matching function for call to â
/opt/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude/scalarField.H:77: note: candidates are: void Foam::add(Foam::Field<double>&, const Foam::scalar&, const Foam::UList<double>&)
/opt/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude/scalarField.H:77: note: void Foam::add(Foam::Field<double>&, const Foam::UList<double>&, const Foam::scalar&)
/opt/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude/labelField.H:53: note: void Foam::add(Foam::Field<int>&, const Foam::label&, const Foam::UList<int>&)
/opt/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude/labelField.H:53: note: void Foam::add(Foam::Field<int>&, const Foam::UList<int>&, const Foam::label&)
make: *** [Make/linux64GccDPOpt/writeCurvature.o] Error 1


what the problem for you?

andrea

[MartinB]

Hi Andrea,

without doing testing, just removed some typos... have a look...

Martin

[Andrea_85]

It runs!

do you know what OF calculate in these lines?

const surfaceVectorField& Sf = mesh.Sf();
surfaceScalarField nHatf_ = nHatfv & Sf;

thanks
andrea

[MartinB]

The face unit interface normal flux...

See the comments here, line 00113ff:
http://foam.sourceforge.net/doc/Doxy...8C_source.html

Martin

[Andrea_85]

Yeah,
but what does it means? If i want the geometric curvature of the interface ([1/L]) which is linked to the capillary pressure that i would like to calculate, do i need the flux? Or is OF that needs the flux to calculate the interfacial forces to put in the equation?

thanks
andrea

[Andrea_85]

Hi,

I still have a problem when i calculate the curvature. I find high value of curvature where there is no interface (values higher than the values at the interface!!)and that's no possible.
what is wrong?

thanks
andrea

[tju_shq]

hello, foamers
I encounter a problem, when initializes the alpha in 0 files as bellow. i don't know why. anyone can help me.
thank you for your help in advance

Unknown patchField type constantAlphaContactAngle for patch type patch

Valid patchField types are :

62
(
advective
calculated
codedFixedValue
codedMixed
cyclic
cyclicACMI
cyclicAMI
cyclicSlip
directionMixed
empty
externalCoupled
fan
fanPressure
fixedFluxPressure
fixedGradient
fixedInternalValue
fixedJump
fixedJumpAMI
fixedMean
fixedPressureCompressibleDensity
fixedValue
freestream
freestreamPressure
inletOutlet
inletOutletTotalTemperature
mapped
mappedField
mappedFixedInternalValue
mappedFixedPushedInternalValue
mixed
nonuniformTransformCyclic
oscillatingFixedValue
outletInlet
outletMappedUniformInlet
partialSlip
phaseHydrostaticPressure
prghPressure
processor
processorCyclic
rotatingTotalPressure
sliced
slip
symmetry
symmetryPlane
syringePressure
timeVaryingMappedFixedValue
totalPressure
totalTemperature
turbulentInlet
turbulentIntensityKineticEnergyInlet
uniformDensityHydrostaticPressure
uniformFixedGradient
uniformFixedValue
uniformInletOutlet
uniformJump
uniformJumpAMI
uniformTotalPressure
variableHeightFlowRate
waveSurfacePressure
waveTransmissive
wedge
zeroGradient
)

[David*]

Originally Posted by hyperion

Hi Andrea - Just in case you want it I have attached the source file that I use to get cell Volumes (Thanks to Martin). I put the file in a directory I created called writeCellVolumes that is in the same directory as writeCellCentres. I also copied over the the other make files (Make/files and Make/options) from writeCellCentres then update those files with the correct EXE = path names then wmake it. The application is executed within a case directory. Good Luck

Back to the original topic of this thread: Since OpenFOAM 4.0 the quoted tool does not compile anymore. In order to make it work again you have to change line 77 to:

cv.ref() = mesh.V();