[shahilc]

Hi,

I am working on a 2D problem (please check the attached image), where a very small heat source is placed inside of the box, with penetrating into the solid. I am facing problems in creating the blockMesh. Please advice if it is the correct way of creating a blockMesh for this case. Also, please help resolving the current error found while running the blockMesh

face 0 in patch 1 does not have neighbour cell face: 4(1 7 6 0)

blockMeshDict File:

convertToMeters 0.001;

vertices
(
(-505 -400 0)
(505 -400 0)
(505 150 0)
(-505 150 0)
(-505 0 0)
(505 0 0)
(-505 -400 1)
(505 -400 1)
(505 150 1)
(-505 150 1)
(-505 0 1)
(505 0 1)
(-10 0 0)
(-10 -10 0)
(10 -10 0)
(10 0 0)
(-10 0 1)
(-10 -10 1)
(10 -10 1)
(10 0 1)
(-10 -400 0)
(10 -400 0)
(-10 -400 1)
(10 -400 1)
);

blocks
(
hex (0 20 12 4 6 22 16 10) (40 80 1) simpleGrading (1 1 1)

hex (20 21 14 13 22 23 18 17) (40 78 1) simpleGrading (1 1 1)

hex (21 1 5 15 23 7 11 19) (20 80 1) simpleGrading (1 1 1)

hex (4 5 2 3 10 11 8 9) (100 50 1) simpleGrading
(
(
(0.5 0.5 0.25)
(0.5 0.5 4)
)
10
1
)
);

edges
(
);

boundary
(
maxY
{
type wall;
faces
(
(2 3 9 8)
);
}

minY
{
type wall;
faces
(
(1 7 6 0)
);
}

solidLeft
{
type wall;
faces
(
(6 10 4 0)
);
}

inlet
{
type patch;
faces
(
(10 9 3 4)
);
}

solidRight
{
type wall;
faces
(
(1 5 11 7)
);
}

outlet
{
type patch;
faces
(
(5 2 8 11)
);
}

frontAndBack
{
type empty;
faces
(
(0 4 5 1)
(7 11 10 6)
(4 3 2 5)
(11 8 9 10)
);
}
);

mergePatchPairs
(
);


Error in Solver

--> FOAM FATAL ERROR:
face 0 in patch 1 does not have neighbour cell face: 4(1 7 6 0)

From function polyMesh::facePatchFaceCells(const faceList& patchFaces,const labelListList& pointCells,const faceListList& cellsFaceShapes,const label patchID)
in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 127.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 Foam:olyMesh::facePatchFaceCells(Foam::List<Foam ::face> const&, Foam::List<Foam::List<int> > const&, Foam::List<Foam::List<Foam::face> > const&, int) const at ??:?
#3 Foam:olyMesh::setTopology(Foam::List<Foam::cellS hape> const&, Foam::List<Foam::List<Foam::face> > const&, Foam::List<Foam::word> const&, Foam::List<int>&, Foam::List<int>&, int&, int&, Foam::List<Foam::cell>&) at ??:?
#4 Foam:olyMesh:olyMesh(Foam::IOobject const&, Foam::Xfer<Foam::Field<Foam::Vector<double> > > const&, Foam::List<Foam::cellShape> const&, Foam::List<Foam::List<Foam::face> > const&, Foam::List<Foam::word> const&, Foam::PtrList<Foam::dictionary> const&, Foam::word const&, Foam::word const&, bool) at ??:?
#5 Foam::blockMesh::createTopology(Foam::IOdictionary const&, Foam::word const&) at ??:?
#6 Foam::blockMesh::blockMesh(Foam::IOdictionary const&, Foam::word const&) at ??:?
#7 ? at ??:?
#8 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9 ? at ??:?
Aborted (core dumped)


Please check attached image

[clktp]

Have you tried to mesh the blocks separately? You may have a ordering error. I remember the error message but I can't recall when I received it.

[Antimony]

Hi,

Based on a quick look at your block definitions, I don't see any one block that has all the vertices 1, 7 6 and 0. Double check and see that the vertices that you use to define a face belong to a particular block.

Cheers,
Antimony

[shahilc]

Hello guys,
Thanks for your quick advice. I specified the blocks separately and the mesh worked out.
The following is what I did:

minYa
{
type wall;
faces
(
(0 20 22 6)
);
}

minYb
{
type wall;
faces
(
(20 21 23 22)
);
}
minYc
{
type wall;
faces
(
(21 1 7 23)
);
}
......................................

frontAndBack
{
type empty;
faces
(
(0 4 12 20)
(20 13 14 21)
(21 15 5 1)
(22 16 10 6)
(23 18 17 22)
(7 11 19 23)
(4 3 2 5)
(11 8 9 10)
);
}
--------------------------------------------------
Keeping the rest of the conditions same. Thanks