[bigbang]

So I've extracted a list of cell IDs from paraview after meshing. I want to create a cellZones file that contains a list of all these cells for use in simplePorousFoam.

Any ideas?

[tomislav_maric]

Originally Posted by bigbang

So I've extracted a list of cell IDs from paraview after meshing. I want to create a cellZones file that contains a list of all these cells for use in simplePorousFoam.

Any ideas?

Here's an idea:

      // Define a cellZoneMesh of size 0.

    cellZoneMesh zones
    (
        IOobject
        (
            "zones",
            runTime.timeName(),
            mesh,
            IOobject::NO_READ
        ),
        mesh, 
        0
    );

    // Bogus label list definition, replace with your ID list here:
    // if you have created it from some outside app and written it 
    // onto the HDD, you will need to read and register it using a
    // LabelLiist<T> constructor.

        // Bogus label list of ten elements.  
    labelList selectCells (10,0);

        // Bogus selection, just for this example: select cells with
        // labels 0-9.
    forAll (selectCells, I)
    {
        selectCells[I] = I;
    }

    // Define a cellZone from the selectCells label list (not a cell list, a list of IDs is not 
    // a cell list, it's a label list :) )
    cellZone myZone
    (
        "myZone",
        selectCells, 
        0,
        zones
    );

    // Brute force write.
    OFstream outFile("myZone");
    myZone.write(outFile);

This is just the first thing I thought of. You probably won't be happy with the myZone.write(IOstream) approach.

What i find interesting is that the

cellZone

constructor requires a const reference to the

cellZoneMesh

which is a list of

cellZone

basically.

Hope this is of any help...

T.

[bigbang]

Hi T,

Thanks for this reply.

I'm still relatively new to programming in openFoam.

I tried to splice your code into some tutorials that I've done, but when I compile I get the following error:

myZones.C:42:30: error: createFields.H: No such file or directory
myZones.C: In function ‘int main(int, char**)’:
myZones.C:88: error: ‘OFstream’ was not declared in this scope
myZones.C:88: error: expected ‘;’ before ‘outFile’
myZones.C:89: error: ‘outFile’ was not declared in this scope
/opt/openfoam201/src/finiteVolume/lnInclude/initContinuityErrs.H:37: warning: unused variable ‘cumulativeContErr’
make: *** [Make/linux64GccDPOpt/myZones.o] Error 1
alexander@alexander-G50VT:~/OpenFOAM/alexander-2.0.1/applications/myZones$ gedit myZones.C

Basically, what do I need to include to run your code?

Thanks for helping out a newbie.

[tomislav_maric]

Originally Posted by bigbang

Hi T,

Thanks for this reply.

I'm still relatively new to programming in openFoam.

I tried to splice your code into some tutorials that I've done, but when I compile I get the following error:

myZones.C:42:30: error: createFields.H: No such file or directory
myZones.C: In function ‘int main(int, char**)’:
myZones.C:88: error: ‘OFstream’ was not declared in this scope
myZones.C:88: error: expected ‘;’ before ‘outFile’
myZones.C:89: error: ‘outFile’ was not declared in this scope
/opt/openfoam201/src/finiteVolume/lnInclude/initContinuityErrs.H:37: warning: unused variable ‘cumulativeContErr’
make: *** [Make/linux64GccDPOpt/myZones.o] Error 1
alexander@alexander-G50VT:~/OpenFOAM/alexander-2.0.1/applications/myZones$ gedit myZones.C

Basically, what do I need to include to run your code?

Thanks for helping out a newbie.

Can you post the whole app here and I can try to plug the code in? I have tried to attach the .zip of my app to this post. If it doesn't help, post your code and we'll figure it out.

Btw, don't worry about being new to the code, without proper documentation everybody is new to the code, especially if they step out of their "comfort zone".

Best regards,
Tomislav

[bigbang]

Thanks again T.

When I compile your application (wmake) from my $FOAM_RUN/myCellZone,
I get the following error:

Making dependency list for source file myCellZone.C
SOURCE=myCellZone.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/opt/openfoam201/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/openfoam201/src/OpenFOAM/lnInclude -I/opt/openfoam201/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/myCellZone.o
myCellZone.C: In function ‘int main(int, char**)’:
myCellZone.C:85: error: ‘OFstream’ was not declared in this scope
myCellZone.C:85: error: expected ‘;’ before ‘outFile’
myCellZone.C:86: error: ‘outFile’ was not declared in this scope
make: *** [Make/linux64GccDPOpt/myCellZone.o] Error 1
alexander@alexander-G50VT:~/OpenFOAM/alexander-2.0.1/applications/myCellZone$

[bigbang]

And then if I add: #include "OFstream.H" in the main, I get this error:

Making dependency list for source file myCellZone.C
SOURCE=myCellZone.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/opt/openfoam201/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/openfoam201/src/OpenFOAM/lnInclude -I/opt/openfoam201/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/myCellZone.o
In file included from /usr/include/c++/4.4/fstream:42,
                 from /opt/openfoam201/src/OpenFOAM/lnInclude/OFstream.H:42,
                 from myCellZone.C:42:
/usr/include/c++/4.4/bits/codecvt.h: In function ‘int main(int, char**)’:
/usr/include/c++/4.4/bits/codecvt.h:42: error: expected ‘=’ before ‘__attribute__’
/usr/include/c++/4.4/bits/codecvt.h:42: error: expected identifier before ‘__attribute__’
/usr/include/c++/4.4/bits/codecvt.h:42: error: expected ‘;’ before ‘__attribute__’
/usr/include/c++/4.4/bits/codecvt.h:42: error: expected primary-expression before ‘__attribute__’
/usr/include/c++/4.4/bits/codecvt.h:42: error: expected ‘;’ before ‘__attribute__’
myCellZone.C:95: error: expected ‘}’ at end of input
make: *** [Make/linux64GccDPOpt/myCellZone.o] Error 1

[tomislav_maric]

Which OF version are you using? I'm on 1.6-ext.

Originally Posted by bigbang

And then if I add: #include "OFstream.H" in the main, I get this error:

Making dependency list for source file myCellZone.C
SOURCE=myCellZone.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/opt/openfoam201/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/openfoam201/src/OpenFOAM/lnInclude -I/opt/openfoam201/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/myCellZone.o
In file included from /usr/include/c++/4.4/fstream:42,
                 from /opt/openfoam201/src/OpenFOAM/lnInclude/OFstream.H:42,
                 from myCellZone.C:42:
/usr/include/c++/4.4/bits/codecvt.h: In function ‘int main(int, char**)’:
/usr/include/c++/4.4/bits/codecvt.h:42: error: expected ‘=’ before ‘__attribute__’
/usr/include/c++/4.4/bits/codecvt.h:42: error: expected identifier before ‘__attribute__’
/usr/include/c++/4.4/bits/codecvt.h:42: error: expected ‘;’ before ‘__attribute__’
/usr/include/c++/4.4/bits/codecvt.h:42: error: expected primary-expression before ‘__attribute__’
/usr/include/c++/4.4/bits/codecvt.h:42: error: expected ‘;’ before ‘__attribute__’
myCellZone.C:95: error: expected ‘}’ at end of input
make: *** [Make/linux64GccDPOpt/myCellZone.o] Error 1

[bigbang]

Hmmm,

I'm on 2.0.1. Don't know why I keep upgrading.. it's nothing but trouble

[tomislav_maric]

Originally Posted by bigbang

Hmmm,

I'm on 2.0.1. Don't know why I keep upgrading.. it's nothing but trouble

That's where the problem lies.... updates are evil.

I think the only thing differences are in the Make/options file, I haven't used some new fancy functionality or a backward incompatible class...

[bigbang]

Maybe it's possible that you can just post your cellZones file created from the program and I can use it as a template and replace the values for the cell Ids?

[bigbang]

I found a whole pdf on porous Zones. Click here

It says:
"Many porous zones can be added to the case. The number of porous zones is limited to the number
of cell zones in the mesh.
1
(
<cellZoneName>
{
Defintions.
}
)
2
(
<anotherCellZoneName>
{
Defintions.
}
)
"

So my questions is how do you replace "Definitions." with a list of cell IDs to define a zone? Or can you even define a zone with a list of cell IDs?

[tomislav_maric]

Here's the 2.0 app. It's in the attachment.

Look at the cellZone constructor: it needs a label list naturally, because the cellZone --> zone --> labelList (check out the doxygen). So, basically, cellZone is a kind of labelList.

class zone
: public labelList
 { 
    protected:      // Protected data

How will you populate the lists is up to you of course. Have fun!

[fly_light]

A very delayed answer; I think the people in the post don't need the code. But I have such a problem, and I found a way to solve it. I hope it is helpful. Please contact me if anyone wants to discuss this.

   // Initialise OF case
    #include "setRootCase.H"

    // These two create the time system (instance called runTime) and fvMesh (instance called mesh).
    #include "createTime.H"
    #include "createMesh.H"

    List<label> selectCellList;

    // add your procedure to append the list
    if (xxx)
    {
          selectCellList.append(cellid)
    }


    mesh.cellZones().append
    (
        new cellZone
        (
            "selectCellZone",
            selectCellList,
            // index, the max index of original cellzones is "size-1". 
            // The value is used as only a cellzone is added  
            mesh.cellZones().size(),  
            mesh.cellZones()
        )
    );

    mesh.cellZones().write();