Slant edges in blockMesh
 

Hello All!

I have this questions which has been bugging me from quite sometime now. I think many of you might find it very trivial.

So attached with this post is blockMeshDict for a very simple square box. The image following the box is that of a slice of the volume. I dont understand despite defining all block such that all the local axes are aligned along the real x, y, z coordinates, why am I getting those slanting edges for every cell?

BlockMesh:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;

vertices
(
(0 0 0)
(10 0 0)
(10 5 0)
(0 5 0)
(0 0 10)
(10 0 10)
(10 5 10)
(0 5 10)
);

blocks
(
hex (0 1 2 3 4 5 6 7) (20 10 20) simpleGrading (1 1 1)
);

edges
(
);

boundary
(
floor
{
type wall;
faces
(
(1 5 4 0)
);
}
ceiling
{
type wall;
faces
(
(3 7 6 2)
);
}
fixedWalls
{
type wall;
faces
(
(0 4 7 3)
(2 6 5 1)
(0 3 2 1)
(4 5 6 7)
);
}
);

mergePatchPairs
(
);

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

This is an artifact of post-processing in ParaFoam and using the slice filter. If you run checkMesh you will see that you only have hexahedra as the actual cells.

In other words, don't worry and be happy!

Thanks for your reply Marco! I used to think so too. However, as apparent in the attached screenshot, the Temperature distribution is not symmetrical; and I am forced to think that it is because of the slant edge in the bottom left corner of the CV-which is oriented differently compared to other slant edges. The temperature should be symmetrical as the geometry and the meshing are symmetrical. So is it this problem because of paraFoam's slice filter or my blockMesh?

Thanks again!

-Nikunj

Hmmm, a little more involved. How did you create the hole in the domain? I don't see that in your blockMeshDict. Also, what was the result of checkMesh?

blockMeshDict:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;

vertices
(
(0 0 0) //0
(0.56 0 0)
(0.7 0 0)
(1.26 0 0)
(0 0.56 0)
(0.56 0.56 0)
(0.7 0.56 0)
(1.26 0.56 0)
(0 0.7 0)
(0.56 0.7 0)
(0.7 0.7 0)
(1.26 0.7 0)
(0 1.26 0)
(0.56 1.26 0)
(0.7 1.26 0)
(1.26 1.26 0)
(0 0 4) //0
(0.56 0 4)
(0.7 0 4)
(1.26 0 4)
(0 0.56 4)
(0.56 0.56 4)
(0.7 0.56 4)
(1.26 0.56 4)
(0 0.7 4)
(0.56 0.7 4)
(0.7 0.7 4)
(1.26 0.7 4)
(0 1.26 4)
(0.56 1.26 4)
(0.7 1.26 4)
(1.26 1.26 4)
(0 0 12) //0
(0.56 0 12)
(0.7 0 12)
(1.26 0 12)
(0 0.56 12)
(0.56 0.56 12)
(0.7 0.56 12)
(1.26 0.56 12)
(0 0.7 12)
(0.56 0.7 12)
(0.7 0.7 12)
(1.26 0.7 12)
(0 1.26 12)
(0.56 1.26 12)
(0.7 1.26 12)
(1.26 1.26 12)

);

blocks
(
hex (0 1 5 4 16 17 21 20) (8 8 40) simpleGrading (1 1 1)//0
hex (1 2 6 5 17 18 22 21) (2 8 40) simpleGrading (1 1 1)
hex (2 3 7 6 18 19 23 22) (8 8 40) simpleGrading (1 1 1)
hex (4 5 9 8 20 21 25 24) (8 2 40) simpleGrading (1 1 1)
hex (6 7 11 10 22 23 27 26) (8 2 40) simpleGrading (1 1 1)//4
hex (8 9 13 12 24 25 29 28) (8 8 40) simpleGrading (1 1 1)
hex (9 10 14 13 25 26 30 29) (2 8 40) simpleGrading (1 1 1)
hex (10 11 15 14 26 27 31 30) (8 8 40) simpleGrading (1 1 1)
hex (16 17 21 20 32 33 37 36) (8 8 80) simpleGrading (1 1 1)//8
hex (17 18 22 21 33 34 38 37) (2 8 80) simpleGrading (1 1 1)
hex (18 19 23 22 34 35 39 38) (8 8 80) simpleGrading (1 1 1)
hex (20 21 25 24 36 37 41 40) (8 2 80) simpleGrading (1 1 1)
hex (21 22 26 25 37 38 42 41) (2 2 80) simpleGrading (1 1 1)//12
hex (22 23 27 26 38 39 43 42) (8 2 80) simpleGrading (1 1 1)
hex (24 25 29 28 40 41 45 44) (8 8 80) simpleGrading (1 1 1)
hex (25 26 30 29 41 42 46 45) (2 8 80) simpleGrading (1 1 1)
hex (26 27 31 30 42 43 47 46) (8 8 80) simpleGrading (1 1 1)//16
);

edges
(
);

boundary
(
top
{
type wall;
faces
(
(32 36 37 33)
(33 37 38 34)
(34 38 39 35)
(36 40 41 37)
(37 41 42 38)
(38 42 43 39)
(40 44 45 41)
(41 45 46 42)
(42 46 47 43)
);
}
bottom
{
type wall;
faces
(
(0 1 5 4)
(1 2 6 5)
(2 3 7 6)
(4 5 9 8)
(6 7 11 10)
(8 9 13 12)
(9 10 14 13)
(10 11 15 14)
);
}
assembly
{
type wall;
faces
(
(9 5 21 25)
(10 9 25 26)
(6 10 26 22)
(5 6 22 21)

);
}
sides
{
type wall;
faces
(
(0 4 20 16)
(4 8 24 20)
(8 12 28 24)
(16 20 36 32)
(20 24 40 36)
(24 28 44 40)

(12 13 29 28)
(13 14 30 29)
(14 15 31 30)
(28 29 45 44)
(29 30 46 45)
(30 31 47 46)

(15 11 27 31)
(11 7 23 27)
(7 3 19 23)
(31 27 43 47)
(27 23 39 43)
(23 19 35 39)

(3 2 18 19)
(2 1 17 18)
(1 0 16 17)
(19 18 34 35)
(18 17 33 34)
(17 16 32 33)
);
}
);

mergePatchPairs
(
);

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

Check Mesh Result:

Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
points: 43641
faces: 120964
internal faces: 111356
cells: 38720
boundary patches: 5
point zones: 0
face zones: 0
cell zones: 0

Overall number of cells of each type:
hexahedra: 38720
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0

Checking topology...
Boundary definition OK.
***Total number of faces on empty patches is not divisible by the number of cells in the mesh. Hence this mesh is not 1D or 2D.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
Patch Faces Points Surface topology
top 324 361 ok (non-closed singly connected)
bottom 320 360 ok (non-closed singly connected)
assembly 320 328 ok (non-closed singly connected)
sides 8640 8712 ok (non-closed singly connected)
defaultFaces 4 9 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (0 0 0) (1.26 1.26 12)
Mesh (non-empty, non-wedge) directions (1 1 0)
Mesh (non-empty) directions (1 1 0)
All edges aligned with or perpendicular to non-empty directions.
Boundary openness (-6.31812e-19 6.31812e-19 0) OK.
Max cell openness = 8.85063e-17 OK.
Max aspect ratio = 1 OK.
Minumum face area = 0.0049. Maximum face area = 0.007. Face area magnitudes OK.
Min volume = 0.00049. Max volume = 0.00049. Total volume = 18.9728. Cell volumes OK.
Mesh non-orthogonality Max: 0 average: 0
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 5.11632e-12 OK.
Coupled point location match (average 0) OK.

Mesh OK.

End

In the checkMesh I see there are some unassigned boundary conditions. The Solver complains of the 1D/2D nature of the sim. Try a run where you assign something to the boundary and let me know how it goes.

Could you tell me what do u mean by "unassigned BCs" as i couldnt see it in checkMesh output.

As far as slant edges are concerned, I changed the orientation of blocks and even then, I am seeing the exact same slant edges, which is quite unexpected. I hoped them to atleast change, if not improve. But that didnt happen, and I am starting to believe, unwillingly though, that may be it is just a paraFoam concoction.

You have 4 faces (on the tip of the square protrusion into the domain) that are empty, when they should probably have a boundary condition assigned to them. I think what is happening is that the empty boundary condition is causing paraview to not interpolate properly. Try assigning those faces a BC (it seems like they should be part of "assembly").

Hope this helps,
Marco

The issue with the T distribution is due to how paraview interpolates values, and has nothing to do with your numerical solution. Use "extract cells by region" instead of simple slicing, and these issues goes away.

K

Thanks for you reply Kalle! This was precisely the issue. Is there a way to extract a 'slice', as when I use 'extract cells by region' a part of 3D geometry is extracted instead of a face.

Thanks a lot for your help.

Regards,
Nikunj.

Click the "extrcat only intersected" and "extract intersected" after selecting "extract cells by region". You cannot get an infinitely thin plane, but you get a sample of cells intersecting a plane... To actually see cell values choose to view cell data instead of point data. In point data mode, paraview interpolates. (which together with an interpolated triangulated surface gives the problem above)

K

Thanks a lot for your valuable inputs Kalle!

Regards,
Nikunj.