CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Meshing & Mesh Conversion

problem in axisymmetric Mesh.

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   October 27, 2013, 02:58
Default problem in axisymmetric Mesh.
  #1
Member
 
sajad
Join Date: Aug 2013
Posts: 64
Rep Power: 4
seju is on a distinguished road
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 200simpleGrading (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 face4(3 2 5 3)

    
From function polyMesh::facePatchFaceCells(const faceListpatchFaces,const labelListListpointCells,const faceListListcellsFaceShapes,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
HTML Code:
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
seju is offline   Reply With Quote

Old   November 2, 2013, 23:48
Default Using wedge elements
  #2
Member
 
Ken
Join Date: Aug 2012
Posts: 65
Blog Entries: 1
Rep Power: 6
Nucleophobe is on a distinguished road
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,
Quote:
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:
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
(

(0.0999 -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:
Quote:
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' :

Code:
....
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
Nucleophobe is offline   Reply With Quote

Old   November 25, 2014, 12:23
Default Negative pyramid volume warning
  #3
Member
 
Vignesh
Join Date: Oct 2012
Location: Darmstadt, Germany
Posts: 59
Rep Power: 5
vigneshTG is on a distinguished road
Dear All,

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

Code:
/*--------------------------------*- 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
Code:
--> 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 !!
__________________
Thanks and Regards

Vignesh
vigneshTG is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
3D Hybrid Mesh Errors DarrenC ANSYS Meshing & Geometry 11 August 5, 2013 06:42
[ICEM] Problem making structured mesh on a surface froztbear ANSYS Meshing & Geometry 4 November 10, 2011 09:52
Dynamic Mesh Problem. Tom Clark FLUENT 9 July 7, 2010 07:56
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10
Gambit problems Althea FLUENT 21 February 6, 2001 08:05


All times are GMT -4. The time now is 00:25.