CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   Failed 1 mesh check (http://www.cfd-online.com/Forums/openfoam/92425-failed-1-mesh-check.html)

camoesas September 14, 2011 04:04

Failed 1 mesh check
 
Hello Everybody,

I have imported a simple mesh of a backwardfacingstep from icem by fluent3DmeshtoFoam. Import worked fine and the mesh looks good. But i dont get convergence so I checked the mesh in OpenFoam. And as a result i got this message:
Quote:

***Number of edges not aligned with or perpendicular to non-empty directions: 854
<<Writing 1348 points on non-aligned edges to set nonAlignedEdges
What does this mean??

jhoepken September 14, 2011 04:29

A 2D mesh in OpenFOAM is a 3D mesh with only one cell in planar direction and the planar patches have to be of type empty. For a proper 2D mesh, the start and end points of the edges normal to the planar patches have to be at the same "not empty" coordinates. This is not the case with your mesh and that is why your 2D simulation does not converge and checkMesh complains about those edges.

camoesas September 14, 2011 05:13

HI jhoepken,

Thanks for the fast and skilled reply. I have to check this in icem.
Or is there a possibility in OF to increase tolerance for this problem?

jhoepken September 14, 2011 05:38

When it comes to icem, I am definitely the wrong guy to talk to. I made some bad experiences with importing an icem mesh to OpenFOAM. This is the reason, I don't use icem any more ;). You may increase the tolerance, but I don't know where that switch is. Maybe somewhere in etc/controlDict, but I am not sure.

camoesas September 14, 2011 11:29

HI Jens,

I´ve sorted the mesh problem out by making the third direction in icem really small. So I dont get this error message. About convergence can´t say anything at the moment. (Going home now sun is shining ;). I´ll test it tomorrow)

chauchau

malaboss December 27, 2012 04:53

Hi,
I don't get it, why for a 2D simulation would we have a different meshing in the empty faces ? If the geometry is really 2D, then there should not be any difference between those two meshes.
Even if I try to make the size in the empty coordinates smaller, It does not change anything for the convergence. Anyway I don't see why it would have changed anything.

wyldckat December 27, 2012 07:10

Greetings to all!

@malaboss: I can only guess that the problem was that the mesh was in fact tetrahedral, even if only one cell thick. This would lead to having the cell centers not aligned with each other in the Z plane; making the cells small enough will lead to an acceptable numerical "deception".

Another solution would be to create an extrusion and remove the original cells, as explained here for snappyHexMesh: http://openfoamwiki.net/index.php/Ma...Examples/2DsHM

Best regards,
Bruno

malaboss December 27, 2012 09:52

Oh thanks for the reply !
In fact I was imaginating that the mesher was starting to mesh one empty patch, then one other, eventually stitching both.
Thank your for the link It really helped me !
I also found a great explanation of the snappyHexMeshing here : https://www.dropbox.com/s/jibjooemkg8makz/memory.pdf

s.m March 2, 2013 05:11

Quote:

Originally Posted by jhoepken (Post 324056)
A 2D mesh in OpenFOAM is a 3D mesh with only one cell in planar direction and the planar patches have to be of type empty. For a proper 2D mesh, the start and end points of the edges normal to the planar patches have to be at the same "not empty" coordinates. This is not the case with your mesh and that is why your 2D simulation does not converge and checkMesh complains about those edges.

hi jhoepken
whould you please explain it more obviously,i can't understand :(
thanks :)
Regards.

wyldckat March 2, 2013 05:41

Greetings saeidehmohamadi,
Quote:

Originally Posted by s.m (Post 410989)
hi jhoepken
whould you please explain it more obviously,i can't understand :(
thanks :)
Regards.

You didn't specify what you didn't understand... :rolleyes:
So I'll address the first part about 2D in OpenFOAM - if you read the first tutorial on the OpenFOAM User Guide, you'll find in section "2.1.1.1 Mesh Generation" the following description:
Quote:

Originally Posted by http://www.openfoam.org/docs/user/cavity.php
OpenFOAM always operates in a 3 dimensional Cartesian coordinate system and all geometries are generated in 3 dimensions. OpenFOAM solves the case in 3 dimensions by default but can be instructed to solve in 2 dimensions by specifying a ‘special’ empty boundary condition on boundaries normal to the (3rd) dimension for which no solution is required.

Best regards,
Bruno

faraz22 May 2, 2013 11:30

hello all, im facing the same error while creating blockmesh. do u know how to figure out this error?


***Number of edges not aligned with or perpendicular to non-empty directions: 4720

A.Wendy May 3, 2013 03:45

Quote:

Originally Posted by faraz22 (Post 424720)
hello all, im facing the same error while creating blockmesh. do u know how to figure out this error?


***Number of edges not aligned with or perpendicular to non-empty directions: 4720

i normally get this error if not all patches are defined in the 0-folder. maybe your naming is not consistant?

s.m May 19, 2013 04:22

Quote:

Originally Posted by wyldckat (Post 410993)
Greetings saeidehmohamadi,

You didn't specify what you didn't understand... :rolleyes:
So I'll address the first part about 2D in OpenFOAM - if you read the first tutorial on the OpenFOAM User Guide, you'll find in section "2.1.1.1 Mesh Generation" the following description:

Best regards,
Bruno

Hi Dear Bruno;
i didn't understand that how could we remove the " ***Number of edges not aligned with or perpendicular to non-empty directions: 71686" error from our checkMesh?
Thank you very much:)

wyldckat May 19, 2013 05:37

Hi saeidehmohamadi,

According to Andreas on the previous post, it looks like you did not reconfigure the files in the "0" folder. To confirm this hypothesis, run:
Quote:

mv 0 0.org
checkMesh -constant
This way the "0" folder will not be used when checkMesh is executed.

Best regards,
Bruno

faraz22 May 19, 2013 08:07

hello s.m,
 
i have removed this error by defining all the faces in blockMeshDict. this error mostly because of the remaining default patches in your background mesh so try to define all the faces in blockMeshDict so that blockMesh command wont create any default patches again, then it will work. i hope.

s.m May 19, 2013 10:58

1 Attachment(s)
Quote:

Originally Posted by faraz22 (Post 428540)
i have removed this error by defining all the faces in blockMeshDict. this error mostly because of the remaining default patches in your background mesh so try to define all the faces in blockMeshDict so that blockMesh command wont create any default patches again, then it will work. i hope.

Hi faraz,
i have used snappyHexMesh for meshing my airfoil. i use the blockMeshDict to create a background mesh for me, so it is a rectangular box that have inlet outlet topAndBottom and fron & back.
now how should i define airfoil in blockMeshDict?
thank you very much:)

s.m May 19, 2013 11:07

1 Attachment(s)
Quote:

Originally Posted by wyldckat (Post 428506)
Hi saeidehmohamadi,

According to Andreas on the previous post, it looks like you did not reconfigure the files in the "0" folder. To confirm this hypothesis, run:

This way the "0" folder will not be used when checkMesh is executed.

Best regards,
Bruno

hi Bruno,
i did what you said me, but my mesh has that error yet.:(

wyldckat May 19, 2013 12:48

Hi s.m,

Have a look at this thread: http://www.cfd-online.com/Forums/ope...blockmesh.html - it might have what you're looking for.

Best regards,
Bruno

faraz22 May 21, 2013 10:08

Quote:

Originally Posted by s.m (Post 428554)
Hi faraz,
i have used snappyHexMesh for meshing my airfoil. i use the blockMeshDict to create a background mesh for me, so it is a rectangular box that have inlet outlet topAndBottom and fron & back.
now how should i define airfoil in blockMeshDict?
thank you very much:)

hi S.m, yes we make background mesh in blockmesh and your file might be correct and the faces you have added at inlet outlet etc might be correct but still after having these faces blcokmesh creates default patches (faces) when your run the blockmesh command. so try to visualiye those default patches in paraView and when you will see where are they locate in backgound mesh try to define them also in blockmeshdict file at the bottom , then you will not get this error.. i hope it will works. good luck.

s.m May 23, 2013 05:27

2 Attachment(s)
Quote:

Originally Posted by faraz22 (Post 428917)
hi S.m, yes we make background mesh in blockmesh and your file might be correct and the faces you have added at inlet outlet etc might be correct but still after having these faces blcokmesh creates default patches (faces) when your run the blockmesh command. so try to visualiye those default patches in paraView and when you will see where are they locate in backgound mesh try to define them also in blockmeshdict file at the bottom , then you will not get this error.. i hope it will works. good luck.

Hi,faraz
i didn't get what do you mean:( sorry.
i put my blockMeshDict and the checkMesh files in the following, would you please tell me again.
thank you very much.


All times are GMT -4. The time now is 19:43.