CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ANSYS Meshing] Problem with structured meshing pipe elbow

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

Like Tree3Likes
  • 1 Post By flotus1
  • 2 Post By Gweher

Reply
 
LinkBack Thread Tools Display Modes
Old   July 23, 2012, 07:45
Default Problem with structured meshing pipe elbow
  #1
New Member
 
Anna
Join Date: Jun 2012
Location: Finland
Posts: 19
Rep Power: 5
Kirjain is on a distinguished road
Hi all,

I am having problems with generating a structured mesh on a pipe with a 90-degree bend. I am using Ansys Meshing and don't have any access to other applications.
Otherwise things would be going fine but just at the bending point the mesh breaks apart into something well peculiar: Random 3D ripples form on the side of the pipe mesh no matter what sort of sizing options I have chosen. I added a few pictures so you can see the abnormality. What am I doing wrong or is it really just a quirk in the software?
Attached Images
File Type: jpg ripples1.jpg (81.4 KB, 148 views)
File Type: jpg ripples.jpg (85.5 KB, 87 views)
Kirjain is offline   Reply With Quote

Old   July 23, 2012, 08:03
Default
  #2
Member
 
Gweher's Avatar
 
Gwenael H.
Join Date: Mar 2011
Location: Switzerland
Posts: 87
Rep Power: 7
Gweher is on a distinguished road
If you could add your mesh file and .agdb geometry that I could have a look. But it may be related to your edge sizing or the way you created the sweep method. I don't know in which order you mesh your different subparts, or if you applied a automatic (default) or a manual "source and target" within the sweep method options.

Anyway, by looking at your pictures, i don't see any mapped face method, this will also improve your mesh quality. Again I don't have lot of information to help you out but if you share your .agdb file I can have a quick look.

Also you can relate to this topic regarding the mesh generation inside a U-bend (180 elbow)
Gweher is offline   Reply With Quote

Old   July 23, 2012, 08:05
Default
  #3
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,107
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
Try the advice I gave a few hours ago in a similar thread.

Quote:
Originally Posted by flotus1 View Post
First of all, you should apply a "structured mesh" to all the surfaces.
This will eliminate the unstructured mesh at the inlet faces.

In the second step, you could try to reset your mesh data (right-click on the mesh, choose "clear generated data")
This often helps when the Ansys mesher seems to ignore your input when
creating the mesh.
Additionally, you should deactivate the "use advanced size functions" option.
Afterwards, you can generate the mesh anew.

When applying sizing on edges, you should always choose "hard" as behaviour. Otherwise the ansys mesher does whatever it wants, but won't create the mesh you have in mind.

Hope this helps.

BTW: the biasing in wall-normal direction looks a bit hard. The volume jump is definitely too high.
famon likes this.
flotus1 is offline   Reply With Quote

Old   July 24, 2012, 01:32
Default
  #4
New Member
 
Anna
Join Date: Jun 2012
Location: Finland
Posts: 19
Rep Power: 5
Kirjain is on a distinguished road
Hi Gweher could you please give me your email address and I would be happy to send you my meshing and geometry files! I tried the mapped face method as well but it seems to amount to nothing! I'm confused with the generated mesh because only one side of the pipe shows abnormalities whilst meshing even though it is clearly a symmetrical case.
Kirjain is offline   Reply With Quote

Old   July 24, 2012, 03:36
Default
  #5
Member
 
Gweher's Avatar
 
Gwenael H.
Join Date: Mar 2011
Location: Switzerland
Posts: 87
Rep Power: 7
Gweher is on a distinguished road
For those who are curious, the problem was solved by selecting "manual source and target" under "sweep method" and specifying the source and target faces.
Attached Images
File Type: jpg ElbowPipe90.jpg (75.0 KB, 164 views)
John222 and atheresia like this.
Gweher is offline   Reply With Quote

Old   July 24, 2012, 06:05
Default Weird results in Fluent
  #6
New Member
 
Anna
Join Date: Jun 2012
Location: Finland
Posts: 19
Rep Power: 5
Kirjain is on a distinguished road
Thank-you, this really helped me. The problem went away after inserting a few face mappings as well, even though the orthogonal quality wasn't as good.

Could I still ask you for a tad more help with the results I get out of Fluent? I'm using the post-processing software in Workbench and the vector plots I obtain are well confusing..! I've attached a picture of both the vector plot for velocity in the pipe bend and the original mesh as a thumbnail for you to see. It seems as if the walls of the pipe weren't there as the velocity vectors happily go through them! Have I just missed something in the pre-calculation process? Is there a way to make the walls imprenetable? Or is this just a quirk in the post-processing programme? I do have all the wall surfaces defined as a named selection etc. so the problem doesn't derive from that.
Attached Images
File Type: jpg bend.jpg (95.9 KB, 105 views)
Kirjain is offline   Reply With Quote

Old   July 24, 2012, 06:39
Default
  #7
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,107
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
Normalize the vector size or make the vectors smaller, this will solve the confusing display type.
Since there are velocity vectors pointing towards the surfaces in cells which are a little bit away from the wall, the vectors seem to penetrate the wall if they are too long.
flotus1 is offline   Reply With Quote

Old   February 7, 2014, 10:30
Default
  #8
New Member
 
Anj
Join Date: Dec 2013
Posts: 8
Rep Power: 3
atheresia is on a distinguished road
Quote:
Originally Posted by Kirjain View Post
Hi Gweher could you please give me your email address and I would be happy to send you my meshing and geometry files! I tried the mapped face method as well but it seems to amount to nothing! I'm confused with the generated mesh because only one side of the pipe shows abnormalities whilst meshing even though it is clearly a symmetrical case.
Hi! Any chance you could send me the files as well? I am having similar problems.
Do let me know and I will inbox you my email address
Many thanks in advance!
atheresia is offline   Reply With Quote

Old   February 7, 2014, 11:05
Default
  #9
New Member
 
Anj
Join Date: Dec 2013
Posts: 8
Rep Power: 3
atheresia is on a distinguished road
Quote:
Originally Posted by Gweher View Post
For those who are curious, the problem was solved by selecting "manual source and target" under "sweep method" and specifying the source and target faces.
Hi!

Any chance you would be able to help me in meshing my geometry as below?
Many thanks in advance!
atheresia is offline   Reply With Quote

Reply

Tags
90 degree bend, elbow, meshing problem

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
Meshing problem Gambit-fluent ajay FLUENT 3 January 28, 2011 02:42
Structured Meshing Query Bennp2000 ANSYS Meshing & Geometry 0 December 9, 2010 21:47
[GAMBIT] Meshing a pipe vedravi ANSYS Meshing & Geometry 1 March 25, 2010 14:19
GAMBIT meshing problem Gauthier Lambert Main CFD Forum 1 August 3, 2000 09:22
fluid flow fundas ram Main CFD Forum 5 June 17, 2000 21:31


All times are GMT -4. The time now is 17:39.