[t.oliveira]

Dear all,

From a Foam::fvMesh object and a Foam::labelHashSet object, I create a submesh:

Foam::fvMeshSubset subsetter(mesh);
subsetter.setLargeCellSubset(voidCells);
Foam::fvMesh& subMesh = subsetter.subMesh();

From this submesh, I create a Foam::fvMesh object:

Foam::fvMesh mesh
(
    Foam::IOobject
    (
        Foam::fvMesh::defaultRegion,
        runTime.timeName(),
        runTime,
        Foam::IOobject::MUST_READ
    ),
    Xfer < pointField > (subMesh.points()),
    Xfer < faceList >   (subMesh.faces()),
    Xfer < labelList >  (subMesh.faceOwner()),
    Xfer < labelList >  (subMesh.faceNeighbour())
);

When I run, I receive the error

cannot find file /home/user/solver/case/constant/polyMesh/pointZones at line 0.

However, if replace it by

Foam::fvMesh mesh
(
    Foam::IOobject
    (
        Foam::fvMesh::defaultRegion,
        runTime.timeName(),
        runTime,
        Foam::IOobject::MUST_READ
    ),
);

I receive no error. Can you please help me identify the problem?

Best wishes,

Thomas

[t.oliveira]

Dear Thomas,

When you use

Foam::fvMesh mesh
(
    Foam::IOobject
    (
        Foam::fvMesh::defaultRegion,
        runTime.timeName(),
        runTime,
        Foam::IOobject::MUST_READ
    ),
);

you call Foam::fvMesh::fvMesh(const IOobject& io), which calls Foam::polyMesh::polyMesh(const IOobject& io), which initialises pointZones_ using the read option Foam::IOobject::READ_IF_PRESENT.

When you use

Foam::fvMesh mesh
(
    Foam::IOobject
    (
        Foam::fvMesh::defaultRegion,
        runTime.timeName(),
        runTime,
        Foam::IOobject::MUST_READ
    ),
    Xfer < pointField > (subMesh.points()),
    Xfer < faceList >   (subMesh.faces()),
    Xfer < labelList >  (subMesh.faceOwner()),
    Xfer < labelList >  (subMesh.faceNeighbour())
);

you call Foam::fvMesh::fvMesh(const IOobject& io, const Xfer<pointField>& points, const Xfer<faceList>& faces, const Xfer<labelList>& allOwner, const Xfer<labelList>& allNeighbour, const bool syncPar), which calls Foam::polyMesh::polyMesh(const IOobject& io, const Xfer<pointField>& points, const Xfer<faceList>& faces, const Xfer<labelList>& owner, const Xfer<labelList>& neighbour, const bool syncPar), which initialises pointZones_ using the read option io.readOpt(), which is Foam::IOobject::MUST_READ in your case.

That is why you get the error if the file pointZones doesn't exist just in this second case. You may want to use this instead:

Foam::fvMesh mesh
(
    Foam::IOobject
    (
        Foam::fvMesh::defaultRegion,
        runTime.timeName(),
        runTime,
        Foam::IOobject::READ_IF_PRESENT
    ),
    Xfer < pointField > (subMesh.points()),
    Xfer < faceList >   (subMesh.faces()),
    Xfer < labelList >  (subMesh.faceOwner()),
    Xfer < labelList >  (subMesh.faceNeighbour())
);

so that io.readOpt() will be Foam::IOobject::READ_IF_PRESENT.

Best wishes,

Thomas