How to compute cellZone volume
 

Dear OpenFoamers,

I am currently trying to develop a solver derived from simpleFoam. In this one I add a source term S which is zero almost everywhere except on a cellZone. In my equation I would need to divide S by the volume of this cellZone.
Does anybody know how I could compute this volume in the code. For example, I know there is something like mesh.V() in order to get the volume of one cell. How should I proceed to get the volume of my whole cellZone.
Any help would be appreciated.

Regards,

Vincent

Hi Vincent

I have never worked with cellZones, however, I do expect that addressing these will give you a list of cell-numbers referring to the mesh. Then loop over these indices and sum the volumes.

E.g.

scalar vol(0);
forAll(cellZonesIndices, cI)
{
vol += mesh.V()[cellZonesIndices[cI]];
}

Best regards

Niels

Hi Niels,

And thanks a lot for your fast reply.
I am going to try your solution which seems rather logical.
However, one more question, what do you mean by "adressing" the cellZone? and how do you get the cellIndices?
I guess it is a newbie question but I never went deep into the openFoam code, so I don't know how to do it.
If you have already some hints, that would be nice!

Regars,

Vincent

I tried this in my code since the name of my zone in cellZones file is "boundaryZone"

word boundaryZone;
label cellZoneID = mesh.cellZones().findZoneID(boundaryZone);
const cellZone& zone = mesh.cellZones()[cellZoneID];
const cellZoneMesh& zoneMesh = zone.zoneMesh();
const labelList& cellsZone = zoneMesh[cellZoneID];


scalar cellZoneVol(0);
forAll(cellsZone, cI)
{
cellZoneVol += mesh.V()[cellsZone[cI]];
}

It compiles but crashes straight at the first iteration with this message:

#0 Foam::error::printStack(Foam::Ostream&) in "/CFDBB/vincent/OpenFOAM//OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigSegv::sigSegvHandler(int) in "/CFDBB/vincent/OpenFOAM//OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 __restore_rt at sigaction.c:0
#3 Foam::cellZone::zoneMesh() const in "/CFDBB/vincent/OpenFOAM//OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 main in "/CFDBB/vincent/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64GccDPOpt/adSimpleFoam"
#5 __libc_start_main in "/lib64/libc.so.6"
#6 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/CFDBB/vincent/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64GccDPOpt/adSimpleFoam"
Segmentation fault

Any idea on what is going on?
Thanks!

Ok I reply to myself, here is the solution which works now:

const label cellZoneID = mesh.cellZones().findZoneID("boundaryZone");
const cellZone& zone = mesh.cellZones()[cellZoneID];
const cellZoneMesh& zoneMesh = zone.zoneMesh();
const labelList& cellsZone = zoneMesh[cellZoneID]; //list of all radiatorZone cell ID's

scalar cellZoneVol(0);
forAll(cellsZone, cI)
{
cellZoneVol += mesh.V()[cellsZone[cI]];
}

Info<< "cellZoneVol = " << cellZoneVol << nl << endl;

tmp<fvVectorMatrix> UEqn
(
fvm::div(phi, U)
+ turbulence->divDevReff(U)
);

UEqn().relax();

eqnResidual = solve
(
UEqn() == -fvc::grad(p) - force/cellZoneVol
).initialResidual();


However this solution only works in serial mode. If I decompose my case and try to run it in parallel it crashes since apparently the cellZoneVol is equal to 0 at some point??
Does someone know how to run this in parallel?

Regards,

Vincent

Just reduce the value of the volume after computing it, so that all the processors have the whole result (I've added output command to show you the result):

scalar cellZoneVol(0);
forAll(cellsZone, cI)
{
cellZoneVol += mesh.V()[cellsZone[cI]];
}

Pout << "before reduce: cellZoneVol = " << cellZoneVol << endl;
reduce(cellZoneVol,sumOp<scalar>());
Pout << "after reduce: cellZoneVol = " << cellZoneVol << endl;


Hope this helps,
Francesco

Hi everybody,

And Thanks a lot Francesco, that works perfectly now!
I hope I'll get some results that I can post here later on.

Regards,

Vincent

Dear Vincent,

How to compute cellZone area? my problem is similar like you had but only this time S = area/volume. I know there is a function like mag(mesh.Sf().boundaryField()[cellZoneID][cI]), but that is for the boundary area i think. My object is a hemisphere.

Please anyone give me a feedback. Very much appreciate it.

Kind Regards,
Robert.

Here's a rough idea of how you could calculate the outside surface area of a cellZone:



NOTE: this code has not been tested (at all). You'll need to add some extra operations to ensure that it also works in parallel. Nonetheless, it should help get you going.

Hi all,
Anybody knows how to access the normal vector of a specific face (facei) of a specific -cubical- cell (celli)?
It should look like something like this:
vector normal_vector=mesh[celli].faceAreas[facei];
Because they are all cubical cells, facei varies from 0 to 5.
Thanks a lot for your help!
Maxime

If your faceI is a globe index or a local index.

For fvMesh
if a globe one, you can use
mesh.Sf()[facei];
a local one
convert it to globe face index
mesh.Sf()[mesh.cells()[cellI][faceI] ]

for polyMesh
you can also use mesh.faceArea() instead of mesh.Sf()

Junwei

Hello Junwei,
Everything works perfectly!
Thanks again for your help.
Maxime