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

Failed 1 mesh check

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

Like Tree9Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   September 14, 2011, 05:04
Default Failed 1 mesh check
  #1
Senior Member
 
Join Date: Mar 2009
Posts: 138
Rep Power: 7
camoesas is on a distinguished road
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??
camoesas is offline   Reply With Quote

Old   September 14, 2011, 05:29
Default
  #2
Senior Member
 
Jens Höpken
Join Date: Apr 2009
Location: Duisburg, Germany
Posts: 139
Rep Power: 7
jhoepken is on a distinguished road
Send a message via Skype™ to 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.
wangxi and s.m like this.
jhoepken is online now   Reply With Quote

Old   September 14, 2011, 06:13
Default
  #3
Senior Member
 
Join Date: Mar 2009
Posts: 138
Rep Power: 7
camoesas is on a distinguished road
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?
camoesas is offline   Reply With Quote

Old   September 14, 2011, 06:38
Default
  #4
Senior Member
 
Jens Höpken
Join Date: Apr 2009
Location: Duisburg, Germany
Posts: 139
Rep Power: 7
jhoepken is on a distinguished road
Send a message via Skype™ to 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.
jhoepken is online now   Reply With Quote

Old   September 14, 2011, 12:29
Default
  #5
Senior Member
 
Join Date: Mar 2009
Posts: 138
Rep Power: 7
camoesas is on a distinguished road
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
camoesas is offline   Reply With Quote

Old   December 27, 2012, 04:53
Default
  #6
Member
 
Malik
Join Date: Dec 2012
Location: Austin, USA
Posts: 52
Rep Power: 4
malaboss is on a distinguished road
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.
malaboss is offline   Reply With Quote

Old   December 27, 2012, 07:10
Default
  #7
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 7,510
Blog Entries: 33
Rep Power: 74
wyldckat is a jewel in the roughwyldckat is a jewel in the roughwyldckat is a jewel in the roughwyldckat is a jewel in the rough
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
wyldckat is offline   Reply With Quote

Old   December 27, 2012, 09:52
Default
  #8
Member
 
Malik
Join Date: Dec 2012
Location: Austin, USA
Posts: 52
Rep Power: 4
malaboss is on a distinguished road
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
malaboss is offline   Reply With Quote

Old   March 2, 2013, 05:11
Default
  #9
s.m
Senior Member
 
saeideh mohamadi
Join Date: Aug 2012
Posts: 229
Rep Power: 5
s.m is on a distinguished road
Quote:
Originally Posted by jhoepken View Post
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.
s.m is offline   Reply With Quote

Old   March 2, 2013, 05:41
Default
  #10
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 7,510
Blog Entries: 33
Rep Power: 74
wyldckat is a jewel in the roughwyldckat is a jewel in the roughwyldckat is a jewel in the roughwyldckat is a jewel in the rough
Greetings saeidehmohamadi,
Quote:
Originally Posted by s.m View Post
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:
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
s.m likes this.
wyldckat is offline   Reply With Quote

Old   May 2, 2013, 12:30
Default
  #11
New Member
 
faraz
Join Date: May 2013
Posts: 7
Rep Power: 3
faraz22 is on a distinguished road
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
faraz22 is offline   Reply With Quote

Old   May 3, 2013, 04:45
Default
  #12
Member
 
Andreas Wendy
Join Date: Aug 2012
Posts: 73
Rep Power: 4
A.Wendy is on a distinguished road
Quote:
Originally Posted by faraz22 View Post
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?
A.Wendy is offline   Reply With Quote

Old   May 19, 2013, 05:22
Default
  #13
s.m
Senior Member
 
saeideh mohamadi
Join Date: Aug 2012
Posts: 229
Rep Power: 5
s.m is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
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
s.m is offline   Reply With Quote

Old   May 19, 2013, 06:37
Default
  #14
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 7,510
Blog Entries: 33
Rep Power: 74
wyldckat is a jewel in the roughwyldckat is a jewel in the roughwyldckat is a jewel in the roughwyldckat is a jewel in the rough
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
wyldckat is offline   Reply With Quote

Old   May 19, 2013, 09:07
Default hello s.m,
  #15
New Member
 
faraz
Join Date: May 2013
Posts: 7
Rep Power: 3
faraz22 is on a distinguished road
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.
wyldckat and s.m like this.
faraz22 is offline   Reply With Quote

Old   May 19, 2013, 11:58
Default
  #16
s.m
Senior Member
 
saeideh mohamadi
Join Date: Aug 2012
Posts: 229
Rep Power: 5
s.m is on a distinguished road
Quote:
Originally Posted by faraz22 View Post
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
Attached Files
File Type: txt blockMeshDict.txt (1.6 KB, 7 views)
s.m is offline   Reply With Quote

Old   May 19, 2013, 12:07
Default
  #17
s.m
Senior Member
 
saeideh mohamadi
Join Date: Aug 2012
Posts: 229
Rep Power: 5
s.m is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
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.
Attached Files
File Type: txt checkMesh.txt (3.4 KB, 11 views)
s.m is offline   Reply With Quote

Old   May 19, 2013, 13:48
Default
  #18
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 7,510
Blog Entries: 33
Rep Power: 74
wyldckat is a jewel in the roughwyldckat is a jewel in the roughwyldckat is a jewel in the roughwyldckat is a jewel in the rough
Hi s.m,

Have a look at this thread: Aerofoil blockMesh - it might have what you're looking for.

Best regards,
Bruno
s.m likes this.
wyldckat is offline   Reply With Quote

Old   May 21, 2013, 11:08
Default
  #19
New Member
 
faraz
Join Date: May 2013
Posts: 7
Rep Power: 3
faraz22 is on a distinguished road
Quote:
Originally Posted by s.m View Post
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 likes this.
faraz22 is offline   Reply With Quote

Old   May 23, 2013, 06:27
Default
  #20
s.m
Senior Member
 
saeideh mohamadi
Join Date: Aug 2012
Posts: 229
Rep Power: 5
s.m is on a distinguished road
Quote:
Originally Posted by faraz22 View Post
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.
Attached Files
File Type: txt blockMeshDict.txt (1.6 KB, 9 views)
File Type: txt checkMesh.txt (3.3 KB, 12 views)
s.m 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
mesh check failed / degenerated contact points shohin FLUENT 16 April 11, 2014 23:32
Transient boundary conditions Jarrod Sinclair (Sinclair) OpenFOAM Running, Solving & CFD 132 November 30, 2011 12:06
ParaView/Parafoam error when making animation Disco_Caine OpenFOAM Paraview & paraFoam 6 September 28, 2010 10:54
user subroutine error CFDUSER CFX 2 December 9, 2006 07:31
user defined function cfduser CFX 0 April 29, 2006 11:58


All times are GMT -4. The time now is 04:34.