[alexB]

Hi Gareth,

perhaps a bit late, but (7 8 17 16) is no proper defined face.
7 and 16, and 8 and 17 define the same points in your blockMesh.

greetings
Alex

[adkar]

If you want 2d mesh, set the same points again like follows.
vertices
(
(0 0 0)
(1 0 0)
(1 1 0)
(0 1 0)
(0 0 0)
(1 0 0)
(1 1 0)
(0 1 0)
);

[alexB]

Hi Adkar,

I don't know where you are referring to...

But your idea won't work.
If you want to set up a two-dimensional case you still have to make your mesh three-dimensional, but define the front and back boundaries as empty boundaries.

Just have a look at the cavity tutorial /incompressible/icofoam/cavity

regards
Alex

[adkar]

Originally Posted by adkar

If you want 2d mesh, set the same points again like follows.
vertices
(
(0 0 0)
(1 0 0)
(1 1 0)
(0 1 0)
(0 0 0)
(1 0 0)
(1 1 0)
(0 1 0)
);

Yeah..i was wrong. Sorry for the inconvinence.

[vigneshTG]

Hello everyone,

I made my own axi-symmetric mesh in 2D following the steps listed in this page. I get these warnings ...

--> 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: -1.13485e-07 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: -5.67424e-08 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: -5.67424e-08 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: -5.67424e-08 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: -5.67424e-08 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 somebody tell me what i am doing wrong ??

here is the blockMeshDict file

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1.0;
// a- 0.024976
//b- 0.0010905
vertices
(
    (0 0 0)                 // pt_0
    (0.024976 0 0.0010905)         // pt_1
    (0.024976 0.0125 0.0010905)     // pt_2
    (0 0.0125 0)                 // pt_3
    (0.024976 0 -0.0010905)           // pt_4
    (0.024976 0.0125 -0.0010905)       // pt_5

);

blocks
(
    hex (0 4 1 0 3 5 2 3) (20 1 20) simpleGrading (1 1 1)
//    hex (0 1 4 0 3 2 5 3) (20 20 1) simpleGrading (1 1 1)
);

edges
(
);

boundary
(
     front
     { 
           type wedge;
           faces  
           (
               (0 1 2 3)
           );
      }
     back
     { 
           type wedge;
           faces  
           (
               (0 3 5 4)
           );
      }
     right
     { 
           type wall;
           faces  
           (
               (1 4 5 2)
           );
      }
    bottom
     { 
           type wall;
           faces  
           (
               (0 4 1 0)
           );
      }
     top
     { 
           type wall;
           faces  
           (
               (3 5 2 3)
           );
      }
     axis
     { 
           type empty;
           faces  
           (
               (0 3 3 0)
           );
      }
);
 
mergePatchPairs
(
);
// ************************************************************************* //

[alexeym]

Hi,

In general negative volume of cells is a result of wrong vertex numbering. If you change

hex (0 4 1 0 3 5 2 3) (20 1 20) simpleGrading (1 1 1)

to

hex (3 5 2 3 0 4 1 0) (20 1 20) simpleGrading (1 1 1)

Errors disappear.

[vigneshTG]

Originally Posted by alexeym

Hi,

In general negative volume of cells is a result of wrong vertex numbering. If you change

hex (0 4 1 0 3 5 2 3) (20 1 20) simpleGrading (1 1 1)

to

hex (3 5 2 3 0 4 1 0) (20 1 20) simpleGrading (1 1 1)

Errors disappear.

Thank you alexeym !!

[usv001]

Hello everyone,

I have written a very simple script in m4 to create the points of the wedge:

divert(-1)
define([wedge],
[ifelse(calc(([$2]==0)),1,
[($1 0 0)],
[($1 calc($2*cos(2.5*pi/180)) calc($2*sin(2.5*pi/180)))
   ($1 calc($2*cos(-2.5*pi/180)) calc($2*sin(-2.5*pi/180)))])])dnl
divert

If you input the points in the x,y plane, it will return two points revolved 2.5deg on either side about x-axis. So,

wedge(1,2) -> two points
(1 1.99809837241304 0.0871945764388748)
(1 1.99809837241304 -0.0871945764388748)
wedge(1,0) -> only one point returned if point is on x-axis
(1 0 0)

It's a little primitive but works for me.

[sourav90]

Thanks https://www.cfd-online.com/Forums/members/trt.html, very much for sharing your code! Was pulling my hair to get a simple example go wedge geometry until I found this...