[camoesas]

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:

***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]

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]

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]

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]

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]

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]

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]

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]

Originally Posted by jhoepken

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]

Greetings saeidehmohamadi,

Originally Posted by s.m

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

You didn't specify what you didn't understand...
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:

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]

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]

Originally Posted by faraz22

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]

Originally Posted by wyldckat

Greetings saeidehmohamadi,

You didn't specify what you didn't understand...
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]

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:

mv 0 0.org
checkMesh -constant

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

Best regards,
Bruno

[faraz22]

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]

Originally Posted by faraz22

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]

Originally Posted by wyldckat

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]

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]

Originally Posted by s.m

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]

Originally Posted by faraz22

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.