[gaottino]

Hi,
I have a problem when I try to create a mesh with blockMesh. Using this command I generate the mesh,
but in the shell window these messages of warning appear:

Reading block mesh description dictionary

Creating block mesh

Creating blockCorners

Creating curved edges

Creating blocks

Creating patches

Creating block mesh topology
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.0211275 for face 0
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.0211275 for face 1
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.007549 for face 2
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.034706 for face 3
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.0153432 for face 4
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.0269118 for face 5
--> FOAM Warning :
From function blockMesh::createTopology(IOdictionary& meshDescription)
in file createTopology.C at line 372
negative volume block : 0, probably defined inside-out
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.0377207 for face 0
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.0377207 for face 1
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.034706 for face 2
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.0407353 for face 3
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.0319363 for face 4
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.043505 for face 5
--> FOAM Warning :
From function blockMesh::createTopology(IOdictionary& meshDescription)
in file createTopology.C at line 372
negative volume block : 1, probably defined inside-out
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.00063 for face 0
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.00063 for face 1
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.00063 for face 2
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.00063 for face 3
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.00063 for face 4
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.00063 for face 5
--> FOAM Warning :
From function blockMesh::createTopology(IOdictionary& meshDescription)
in file createTopology.C at line 372
negative volume block : 2, probably defined inside-out
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.192724 for face 0
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.192724 for face 1
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.192724 for face 2
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.192724 for face 3
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.19937 for face 4
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.186079 for face 5
--> FOAM Warning :
From function blockMesh::createTopology(IOdictionary& meshDescription)
in file createTopology.C at line 372
negative volume block : 3, probably defined inside-out
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -1.59 for face 0
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -1.59 for face 1
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -1.59 for face 2
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -1.59 for face 3
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -1.68 for face 4
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -1.5 for face 5
--> FOAM Warning :
From function blockMesh::createTopology(IOdictionary& meshDescription)
in file createTopology.C at line 372
negative volume block : 4, probably defined inside-out
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.51 for face 0
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.51 for face 1
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.51 for face 2
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.51 for face 3
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.42 for face 4
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.6 for face 5
--> FOAM Warning :
From function blockMesh::createTopology(IOdictionary& meshDescription)
in file createTopology.C at line 372
negative volume block : 5, probably defined inside-out
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -1.31 for face 0
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -1.31 for face 1
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -1.21 for face 2
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -1.41 for face 3
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.32 for face 4
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -2.3 for face 5
--> FOAM Warning :
From function blockMesh::createTopology(IOdictionary& meshDescription)
in file createTopology.C at line 372
negative volume block : 6, probably defined inside-out

Default patch type set to empty
--> FOAM Warning :
From function polyMesh::polyMesh(... construct from shapes...)
in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 573
Found 14 undefined faces in mesh; adding to default patch.

Check block mesh topology

Basic statistics
Number of internal faces : 8
Number of boundary faces : 26
Number of defined boundary faces : 26
Number of undefined boundary faces : 0

Checking patch -> block consistency

Creating block offsets

Creating merge list .

Creating points

Creating cells

Creating patches

Creating mesh from block mesh

Default patch type set to empty

Creating merge patch pairs


Writing polyMesh

end

The mesh is created, but I don't know what do these warnings mean, and I'm not so sure that the mesh is created correctly.
So, someone could help me, please?
I thank you in advance.

Gabriele

[hjasak]

Yup, this is bad: your mesh is inside out. Have a look at the point ordering rules for mesh blocks in the documentation.

Hrv

[aldo.iannetti]

Hi Hrvoje,
I'm trying to mesh a pipe for a DNS simulation. here the blockMeshDict:
########################
convertToMeters 1;
vertices
(
(0 0 1) //0
(8 0 1) //1
(8 1 0) //2
(0 1 0) //3
(0 1 1) //4
(8 1 1) //5
(8 2 1) //6
(0 2 1) //7
(0 1 2) //8
(8 1 2) //9
);
blocks
(
// block 1
hex (
0 1 2 3
4 5 5 4
)
(400 128 500) //(600 60 200)
simpleGrading (1 1 10)
// block 2
hex (
3 2 6 7
4 5 5 4
)
(400 128 500) //(600 60 200)
simpleGrading (1 1 10)
// block 3
hex (
7 6 9 8
4 5 5 4
)
(400 128 500) //(600 60 200)
simpleGrading (1 1 10)
// block 4
hex (
8 9 1 0
4 5 5 4
)
(400 128 500) // (600 60 200)
simpleGrading (1 1 10)
);
//create the quarter circles
edges
(
arc 3 0 (0 0.292893219 0.292893219)
arc 2 1 (8 0.292893219 0.292893219)
arc 0 8 (0 0.292893219 1.707106781)
arc 1 9 (8 0.292893219 1.707106781)
arc 7 3 (0 1.707106781 0.292893219)
arc 6 2 (8 1.707106781 0.292893219)
arc 8 7 (0 1.707106781 1.707106781)
arc 9 6 (8 1.707106781 1.707106781)
);
patches
(
cyclic inout1
(
(0 4 4 3)
(1 2 5 5)
)
cyclic inout2
(
(3 4 4 7)
(2 6 5 5)
)
cyclic inout3
(
(7 4 4 8)
(6 9 5 5)
)
cyclic inout4
(
(8 4 4 0)
(9 1 5 5)
)
wall wall1
(
(0 3 2 1)
)
wall wall2
(
(3 7 6 2)
)
wall wall3
(
(7 8 9 6)
)
wall wall4
(
(8 0 1 9)
)
);
mergePatchPairs
(
);

########################################
There are 100 Mln cells, I'm using CINECA (bologna, Italy) HPC Plx:


Model: IBM PLX (iDataPlex)
Architecture: Linux Infiniband Cluster
Processor Type: Intel Xeon X5550 2.66 GHz / Intel Xeon X5570 2.93 GHz (Quad Core Nehalem) / nVidia Quadro
Number of Processors: 578(2290 core): 564 (2192 cores) X5550 + 12 (96 cores) X5570 + 2 nVidia Quadro
Nodes: 274 IBM X360M2 + 12 X3650M2 + 2 nVidia Quadro Plex 2200 S4
RAM: 8624 GB: 24 Gb * 274 + 128Gb * 16
Internal Network: Infiniband with 4 QDR switches
Disk Space: 100 TB
Operating System: Red Hat RHEL4
Peak Performance: 24 TFlop/s

I know (correct me if it is not true) blockMesh run not in parallel, so I started a serial session. BlockMesh seem to need 10 Gb memory and of course after 18 hours the mesh seem to be closed but I have not output, here the log file (only the writing message is missing):

Creating blockCorners
Creating curved edges
Creating blocks
Creating patches
Creating block mesh topology
Default patch type set to empty
Check block mesh topology
Basic statistics
Number of internal faces : 6
Number of boundary faces : 12
Number of defined boundary faces : 12
Number of undefined boundary faces : 0
Checking patch -> block consistency
Creating block offsets
Creating merge list .
Creating points with scale 1
Creating cells
Creating patches
Creating mesh from block mesh
Default patch type set to empty


Can you please help me understand why it doesn't work? Is there any broblem for blockMesh to handle large mesh even in HPC systems? Have you got any advice or me?
Ask me whatever you need to understand better

thanks
Aldo

[PaGgiE]

Hi,
I am trying to run a 2D fluid flow with an obstacle in its path and it is able to creat the mesh proprly but when i run icoFoam its giving the error as:



Create time

Create mesh for time = 0

Reading transportProperties

Reading field p

Reading field U

Reading/calculating face flux field phi


Starting time loop

Time = 0.005

Courant Number mean: 0 max: 7.5


This mesh contains patches of type empty but is not 1D or 2D
by virtue of the fact that the number of faces of this
empty patch is not divisible by the number of cells.

From function emptyFvPatchField<Type>::updateCoeffs()
in file fields/fvPatchFields/constraint/empty/emptyFvPatchField.C at line 148.

FOAM exiting



Can anyone suggest what is the problem?
Do i need to use any other solver than icoFoam?
or is there any problem with the mesh as while running blockMesh, i got a warning as:


Creating blockCorners

Creating curved edges

Creating blocks

Creating patches

Creating block mesh topology

Default patch type set to empty
--> FOAM Warning :
From function polyMesh: PolyMesh(... construct from shapes...)
in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 577
Found 8 undefined faces in mesh; adding to default patch.

Check block mesh topology

Basic statistics
Number of internal faces : 0
Number of boundary faces : 24
Number of defined boundary faces : 24
Number of undefined boundary faces : 0

Checking patch -> block consistency

Creating block offsets

Creating merge list .

Creating points with scale 1

Creating cells

Creating patches

Creating mesh from block mesh

Default patch type set to empty

Writing polyMesh

End



The blockMesh code is as follows:

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.6 |
| \\ / A nd | Web: http://www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;

vertices
(
(0 0 0)
(0.4 0 0)
(0.6 0 0)
(1 0 0)
(0.4 0.2 0)
(0.6 0.2 0)
(0.4 0.4 0)
(0.6 0.4 0)
(0 0.6 0)
(0.4 0.6 0)
(0.6 0.6 0)
(1 0.6 0)
(0 0 0.1)
(0.4 0 0.1)
(0.6 0 0.1)
(1 0 0.1)
(0.4 0.2 0.1)
(0.6 0.2 0.1)
(0.4 0.4 0.1)
(0.6 0.4 0.1)
(0 0.6 0.1)
(0.4 0.6 0.1)
(0.6 0.6 0.1)
(1 0.6 0.1)
);

blocks
(
hex (0 1 9 8 12 13 21 20) (30 45 1) simpleGrading (1 1 1)
hex (1 2 5 4 13 14 17 16) (15 15 1) simpleGrading (1 1 1)
hex (2 3 11 10 14 15 23 22) (30 45 1) simpleGrading (1 1 1)
hex (6 7 10 9 18 19 22 21) (15 15 1) simpleGrading (1 1 1)

);

edges
(
);

patches
(
patch
inlet
(
(0 8 20 12)
)

patch
outlet
(
(11 3 15 23)
)

wall upperWalls
(
(8 9 21 20)
(10 11 23 22)
(6 7 19 18)
(9 10 22 21)
)

wall lowerWalls
(
(1 0 12 13)
(3 2 14 15)
(5 4 16 17)
(2 1 13 14)
)

empty frontAndBack
(
(9 8 0 1)
(10 9 6 7)
(5 4 1 2)
(11 10 2 3)
(20 21 13 12)
(21 22 19 18)
(16 17 14 13)
(22 23 15 14)
)
);

mergePatchPairs
(
);

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

[bunni]

after you run blockMesh, I would run foamToVTK and look at the initial mesh. So, have a good look at the initial mesh, and see if it does what you think it should do. And, of course, draw it all out on paper, and write out all the hexes/faces on paper first. Somehow fewer errors than writing directly on the computer.
Good luck.

[hm86]

Hey all,

I am trying to create a quarter-cylinder mesh with cyclic boundary conditions on the two straight external faces. My blockMeshDict file is

| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.7.0 |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 1;

vertices
(
(0.00 0.053 -2.432) // 0
(0.357 0.363 -2.432) // 1
(0.651 0.003 -2.432) // 2
(0.3040 -0.3093 -2.432) // 3
(0.917 0.85 -2.432) // 4
(1.216 0.053 -2.432) // 5
(0.7816 -0.8785 -2.432) // 6
(0.00 0.053 2.432) // 7
(0.357 0.363 2.432) // 8
(0.651 0.003 2.432) // 9
(0.3040 -0.3093 2.432) // 10
(0.917 0.85 2.432) // 11
(1.216 0.053 2.432) // 12
(0.7816 -0.8785 2.432) // 13
);

blocks
(
hex (0 1 2 3 7 8 9 10) (10 10 10) simpleGrading (1 1 1)
hex (1 4 5 2 8 11 12 9) (10 10 10) simpleGrading (1 1 1)
hex (3 2 5 6 10 9 12 13) (10 10 10) simpleGrading (1 1 1)

);

edges
(

arc 4 5 (1.12 0.52 -2.432)
arc 5 6 (1.05 -0.557 -2.432)
arc 11 12 (1.12 0.52 2.432)
arc 12 13 (1.05 -0.557 2.432)

);

patches
(

wall a
(
(7 10 9 8)
(8 9 12 11)
(10 13 12 9)
)

wall b
(
(0 1 2 3)
(1 4 5 2)
(3 2 5 6)
)


wall c
(
(5 4 11 12)
(5 12 13 6)
)

cyclic cyclic
(
(0 1 8 7)
(1 4 11 8)
(3 8 7 10)
(6 3 10 13)
)


);

mergePatchPairs
(


);

But when I run blockMesh on this I get


/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.7.0 |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 1.7.0-21131bcbd876
Exec : blockMesh
Date : Jul 18 2010
Time : 06:43:56
Host : black1
PID : 6654
Case : /home/usr/run/zprop_single
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

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


Creating block mesh from
"/home/usr/run/zprop_single/constant/polyMesh/blockMeshDict"


Creating blockCorners

Creating curved edges

Creating blocks

Creating patches

Creating block mesh topology
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 128
zero or negative pyramid volume: -0.180065 for face 0
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 128
zero or negative pyramid volume: -0.176886 for face 1
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 128
zero or negative pyramid volume: -0.17966 for face 2
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 128
zero or negative pyramid volume: -0.17729 for face 3
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 128
zero or negative pyramid volume: -0.178475 for face 4
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 128
zero or negative pyramid volume: -0.178475 for face 5
--> FOAM Warning :
From function blockMesh::createTopology(IOdictionary&)
in file createTopology.C at line 397
negative volume block : 0, probably defined inside-out
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 128
zero or negative pyramid volume: -0.228153 for face 0
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 128
zero or negative pyramid volume: -0.428514 for face 1
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 128
zero or negative pyramid volume: -0.37968 for face 2
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 128
zero or negative pyramid volume: -0.276987 for face 3
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 128
zero or negative pyramid volume: -0.328333 for face 4
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 128
zero or negative pyramid volume: -0.328333 for face 5
--> FOAM Warning :
From function blockMesh::createTopology(IOdictionary&)
in file createTopology.C at line 397
negative volume block : 1, probably defined inside-out
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 128
zero or negative pyramid volume: -0.421065 for face 0
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 128
zero or negative pyramid volume: -0.26901 for face 1
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 128
zero or negative pyramid volume: -0.205004 for face 2
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 128
zero or negative pyramid volume: -0.485071 for face 3
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 128
zero or negative pyramid volume: -0.345038 for face 4
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 128
zero or negative pyramid volume: -0.345038 for face 5
--> FOAM Warning :
From function blockMesh::createTopology(IOdictionary&)
in file createTopology.C at line 397
negative volume block : 2, probably defined inside-out

Default patch type set to empty


--> FOAM FATAL ERROR:
face 2 in patch 3 does not have neighbour cell face: 4(3 8 7 10)

From function polyMesh::facePatchFaceCells(const faceList& patchFaces,const labelListList& pointCells,const faceListList& cellsFaceShapes,const label patchID)
in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 124.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) in "/home/usr/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/usr/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 Foam:olyMesh::facePatchFaceCells(Foam::List<Foam ::face> const&, Foam::List<Foam::List<int> > const&, Foam::List<Foam::List<Foam::face> > const&, int) const in "/home/usr/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libOpenFOAM.so"
#3 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::List<Foam::word> const&, Foam::word const&, Foam::word const&, Foam::List<Foam::word> const&, bool) in "/home/usr/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 Foam::blockMesh::createTopology(Foam::IOdictionary &) in "/home/usr/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linux64GccDPOpt/blockMesh"
#5 Foam::blockMesh::blockMesh(Foam::IOdictionary&) in "/home/usr/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linux64GccDPOpt/blockMesh"
#6 main in "/home/usr/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linux64GccDPOpt/blockMesh"
#7 __libc_start_main in "/lib64/libc.so.6"
#8 _start at /usr/src/packages/BUILD/glibc-2.10.1/csu/../sysdeps/x86_64/elf/start.S:116
Aborted

This should be relatively simple I think but I dont know what I am doing wrong! Any help would be greatly appreciated! Thanks!

[MartinB]

Hi,
there are problems in the numbering of your hex blocks, as well as in one of the patches. I don't have experience regarding the cyclic patch you want to use, but using a symmetry patch might work as well... otherwise search for cyclic in the forum, there are threads about it...
See the corrections below:

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.7.0 |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 1;

vertices
(
(0.00 0.053 -2.432) // 0
(0.357 0.363 -2.432) // 1
(0.651 0.003 -2.432) // 2
(0.3040 -0.3093 -2.432) // 3
(0.917 0.85 -2.432) // 4
(1.216 0.053 -2.432) // 5
(0.7816 -0.8785 -2.432) // 6
(0.00 0.053 2.432) // 7
(0.357 0.363 2.432) // 8
(0.651 0.003 2.432) // 9
(0.3040 -0.3093 2.432) // 10
(0.917 0.85 2.432) // 11
(1.216 0.053 2.432) // 12
(0.7816 -0.8785 2.432) // 13
);

blocks
(
//hex (0 1 2 3 7 8 9 10) (10 10 10) simpleGrading (1 1 1) // wrong
//hex (1 4 5 2 8 11 12 9) (10 10 10) simpleGrading (1 1 1) // wrong
//hex (3 2 5 6 10 9 12 13) (10 10 10) simpleGrading (1 1 1) // wrong
hex (0 3 2 1 7 10 9 8) (10 10 10) simpleGrading (1 1 1) // correction
hex (3 6 5 2 10 13 12 9) (10 10 10) simpleGrading (1 1 1) // correction
hex (5 4 1 2 12 11 8 9) (10 10 10) simpleGrading (1 1 1) // correction
);

edges
(

arc 4 5 (1.12 0.52 -2.432)
arc 5 6 (1.05 -0.557 -2.432)
arc 11 12 (1.12 0.52 2.432)
arc 12 13 (1.05 -0.557 2.432)

);

patches
(

wall a
(
(7 10 9 8)
(8 9 12 11)
(10 13 12 9)
)

wall b
(
(0 1 2 3)
(1 4 5 2)
(3 2 5 6)
)


wall c
(
(5 4 11 12)
(5 12 13 6)
)

//cyclic cyclic
symmetryPlane symmetry // try this
(
(0 1 8 7)
(1 4 11 8)
//(3 8 7 10)    // wrong
(0 3 10 7) // correction
(6 3 10 13)
)
);

mergePatchPairs
(
);

The numeration problem in the patches can be found easily with pyFoamDisplayBlockMesh. The problem with the hex numbering will vanish with gaining experience ;-)

Martin

[hm86]

Thank you Martin! You got rid of a lot of the errors - you are right about the hex numbering but thank you for the quick response!! I want to implement cyclic bcs but i will look through the forums for some help. Thanks again!

Actually - I'm not sure if I need cyclic BCs. I am trying to use the above grid to simulate a wind turbine and was wondering if I needed cyclic BCs or symmetry planes? Usually people use periodic BCs and I think cyclic BCs are the closest to that - but I dont know if the symmetry plane will do the same thing. Any suggestions?

Update- I managed to get cyclic BCs to work by using createPatch and increasing the merge Tolerance. However now snappyHexMesh gives me an error. (face 0 area does not match neighbor ... )