[seju]

Greetings to all.
I want run this mesh but I see the error.

PHP Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 0.012;
 
vertices
(
(0 0 0)
(0.0999 0.04362 0)
(0.0999 0.04362 5) 
(0 0 5)
(0.0999 -0.04362 0) 
(0.0999 -0.04362 5)
);
 
blocks
(
hex (0 4 1 0 3 5 2 3) (40  1 200) simpleGrading (1 1 1)
);
 
edges
(
);
 
boundary
(
     front
     { 
           type wedge;
           faces  
           (
               (0 1 2 3)
           );
      }
     back
     { 
           type wedge;
           faces  
           (
               (0 3 5 4)
           );
      }
     fixedkWall
     { 
           type wall;
           faces  
           (
               (1 4 5 2)
           );
      }
     bottom
     { 
           type patch;
           faces  
           (
               (0 4 1 0)
           );
      }
     top
     { 
           type patch;
           faces  
           (
               (3 2 5 3)
           );
      }
     axis
     { 
           type empty;
           faces  
           (
               (0 3 3 0)
           );
      }
);
 
mergePatchPairs
(
);

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


ERROR:

PHP Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.1-57f3c3617a2d
Exec   : blockMesh
Date   : Oct 28 2013
Time   : 10:24:38
Host   : "sajad-K55VD"
PID    : 7306
Case   : /home/sajad/OpenFOAM/sajad-2.2.1/run/tutorials/multiphase/interFoam/laminar/ellipsoidal
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

Creating block mesh from
    "/home/sajad/OpenFOAM/sajad-2.2.1/run/tutorials/multiphase/interFoam/laminar/ellipsoidal/constant/polyMesh/blockMeshDict"
Creating curved edges
Creating topology blocks
Creating topology patches

Creating block mesh topology

 --> FOAM FATAL ERROR: 
face 0 in patch 4 does not have neighbour cell face: 4(3 2 5 3)

    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::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::polyMesh::facePatchFaceCells(Foam::List<Foam::face> const&, Foam::List<Foam::List<int> > const&, Foam::List<Foam::List<Foam::face> > const&, int) const at ??:?
#3  Foam::polyMesh::setTopology(Foam::List<Foam::cellShape> 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::polyMesh::polyMesh(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) 


you can see similar mesh in this link

http://openfoamwiki.net/index.php/Main_ContribExamples/AxiSymmetric

I even copy that code from above link and I saw this error again.
after change polyMesh in terminal I run: blockMesh
is it wrong?
where is my drawback??
*best regards*
sajad

[Nucleophobe]

Sajad,

In order to create wedge elements with blockMesh, you must be careful to follow the guidelines provided in the OpenFOAM documentation (5.3.3):
http://www.openfoam.org/docs/user/blockMesh.php

Also, note that when specifying patches,

The order in which the vertices are given must be such that, looking from inside the block and starting with any vertex, the face must be traversed in a clockwise direction to define the other vertices.

I'm not sure where the problem was, but this works:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 0.012;
 
vertices
(

(0.0999 -0.04362 0) // new 0, old 4
(0.0999 -0.04362 5) // new 1, old 5
(0.0999 0.04362 5) // new 2, old 2
(0.0999 0.04362 0) // new 3, old 1
(0 0 0) // new 4, old 0
(0 0 5) // new 5, old 3

// Old vertices:
//(0 0 0) //0
//(0.0999 0.04362 0) //1
//(0.0999 0.04362 5) //2
//(0 0 5) //3
//(0.0999 -0.04362 0) //4
//(0.0999 -0.04362 5) //5
);
 
blocks
(
hex (0 1 2 3 4 5 5 4) (40  1 200) simpleGrading (1 1 1)
);
 
edges
(
);
 
boundary
(
     front
     { 
           type wedge;
           faces  
           (
               (0 1 5 4) 
           );
      }
     back
     { 
           type wedge;
           faces  
           (
               (2 3 4 5)
           );
      }
     fixedkWall
     { 
           type wall;
           faces  
           (
               (0 1 2 3)
           );
      }
     bottom
     { 
           type patch;
           faces  
           (
               (1 2 5 5)
           );
      }
     top
     { 
           type patch;
           faces  
           (
               (0 3 4 4)
           );
      }
     axis
     { 
           type empty;
           faces  
           (
               (4 5 5 4)
           );
      }
);
 
mergePatchPairs
(
);

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

Finally, before you use this mesh in a simulation, you will want to modify the geometry such that the angle between the 'front' and 'back' patches is ~5 degrees:

wedge
For 2 dimensional axi-symmetric cases, e.g. a cylinder, the geometry is specified as a wedge of small angle (e.g. ) and 1 cell thick running along the plane of symmetry, straddling one of the coordinate planes, as shown in Figure 5.4. The axi-symmetric wedge planes must be specified as separate patches of wedge type. The details of generating wedge-shaped geometries using blockMesh are described in section 5.3.3.

(http://www.openfoam.org/docs/user/boundaries.php)
As defined, the angle is closer to 25 degrees. You can check this with 'checkMesh' :

....
Checking geometry...
    Overall domain bounding box (0 -0.00052344 0) (0.0011988 0.00052344 0.06)
    Mesh (non-empty, non-wedge) directions (1 0 1)
    Mesh (non-empty) directions (1 1 1)
    Wedge front with angle 23.587845 degrees
    Wedge back with angle 23.587845 degrees
    All edges aligned with or perpendicular to non-empty directions.
    Boundary openness (-8.8718496e-14 -3.0464533e-16 -1.9670129e-19) OK.
    Max cell openness = 2.5596435e-16 OK.
    Max aspect ratio = 500.5005 OK.
    Minimum face area = 1.5687497e-11. Maximum face area = 1.57032e-06.  Face area magnitudes OK.
    Min volume = 2.3531245e-14. Max volume = 9.3889668e-12.  Total volume = 3.7649992e-08.  Cell volumes OK.
    Mesh non-orthogonality Max: 0 average: 0
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 1.0915773 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End

Good luck,
-Nuc

[vigneshTG]

Dear All,

I am trying to create an axisymmetric mesh. The blockMeshDict i edited is shown below.

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
// angle 5 deg
// radius 1
convertToMeters 1;

vertices
(
    (0 0 0)
    (0.49952 0 0.02180)
    (0.49952 1 0.02180)
    (0 1 0)
    (0.49952 0 -0.02180)
    (0.49952 1 -0.02180)
);

blocks
(
    hex (0 4 1 0 3 5 2 3) (60 1 60) simpleGrading (1 1 1)
);

edges
(
);

boundary
(
    front
     { 
           type wedge;
           faces  
           (
               (0 1 2 3)
           );
      }
     back
     { 
           type wedge;
           faces  
           (
               (0 3 5 4)
           );
      }
     sideWall
     { 
           type wall;
           faces  
           (
               (1 4 5 2)
           );
      }
     bottom
     { 
           type wall;
           faces  
           (
               (0 4 1 0)
           );
      }
     top
     { 
           type patch;
           faces  
           (
               (3 5 2 3)
           );
      }
     axis
     { 
           type empty;
           faces  
           (
               (0 3 3 0)
           );
      }
);

mergePatchPairs
(
);


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

When i run blockMesh, i get the following warning of negative pyramid volume

--> 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: -0.00362985 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: -0.00181492 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: -0.00181492 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: -0.00181492 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: -0.00181492 for face 5
--> FOAM Warning : 
    From function blockMesh::createTopology(IOdictionary&)
    in file blockMesh/blockMeshTopology.C at line 255
    negative volume block : 0, probably defined inside-out

Can someone tell me what i am doing wrong !!