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

[ICEM] How to avoid single edges at boundaries in 2D models?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 19, 2012, 06:33
Default How to avoid single edges at boundaries in 2D models?
  #1
New Member
 
Ivan Fernandez
Join Date: Aug 2011
Posts: 7
Rep Power: 5
Gandin is on a distinguished road
Hello everybody. I am new in ICEM CFD meshing. I have done some tutorials about hexa meshing, and I now I am trying to simulate in Fluent the movement of a fluid in a kind of ring by natural convection (like a thermosiphon).

I have made a 2D model and I have meshed it, by blocking strategy, pre-meshing and conversion to unstructured mesh. The quality of the resulting mesh is good, but I have found a big problem: when I check the mesh to find errors and possible problems, single edges reveal in all the elements of the domain boundary.

After this, I have tried meshing simple 2D shapes, as a square. I have created the geometry (4 points, 4 curves and a surface) and I have meshed by using different methods (blocking; surface meshing by Mesh>Compute mesh>Surface mesh only) but the problem of single edges at boundary always returns.

How can I avoid it? Thank you very much in advance!
Gandin is offline   Reply With Quote

Old   January 19, 2012, 08:41
Default
  #2
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
attach tin and blocking file
Far is offline   Reply With Quote

Old   January 19, 2012, 09:40
Default
  #3
New Member
 
Ivan Fernandez
Join Date: Aug 2011
Posts: 7
Rep Power: 5
Gandin is on a distinguished road
Far, the files are now attached. Thanks.
Attached Files
File Type: zip 2Dcut46.zip (10.0 KB, 14 views)
Gandin is offline   Reply With Quote

Old   January 19, 2012, 10:11
Lightbulb hi
  #4
Member
 
kiran Ambilpur
Join Date: Jun 2010
Posts: 34
Rep Power: 7
kiran is on a distinguished road
Send a message via Skype™ to kiran
Hi

you don't need to worry about the single edges this isn't a problem.

you can continue with the analysis.

Thanks
Kiran
kiran is offline   Reply With Quote

Old   January 19, 2012, 10:14
Default
  #5
New Member
 
Ivan Fernandez
Join Date: Aug 2011
Posts: 7
Rep Power: 5
Gandin is on a distinguished road
Thanks, Kiran.
Gandin is offline   Reply With Quote

Old   January 19, 2012, 10:41
Default
  #6
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Today I check one of my mesh on 32 and 64 bit systems. On 64 bit system I dont get this problem whereas on32 bit I am getting this problem. I guess this is due to round off error since meshing spacing is smaller than computer round off error.

Last edited by Far; January 19, 2012 at 11:42.
Far is offline   Reply With Quote

Old   January 19, 2012, 11:04
Default
  #7
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
When opened your files, I am not getting any error or warning message. Strange !!!!
Far is offline   Reply With Quote

Old   January 19, 2012, 11:11
Default
  #8
New Member
 
Ivan Fernandez
Join Date: Aug 2011
Posts: 7
Rep Power: 5
Gandin is on a distinguished road
Far, I have imported the mesh to Fluent, as Kiran said, and solved a case. Non error or warning message has been shown, and the solution seems valid.

Thank you both.
Gandin is offline   Reply With Quote

Old   January 20, 2012, 17:18
Default
  #9
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
For a little more explanation...

Single edges is on the list of "Possible Problems". If you were doing a 3D analysis and didn't have any baffles, then single edges would be a concern.

But you should expect single edges along all your boundaries for 2D analysis. You should also expect single edges along the edges of baffles in 3D, etc.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   January 21, 2012, 00:17
Default
  #10
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
What does single edges imply in the mesh? Like we know that skewness shows the distorted cell in the mesh.
Far is offline   Reply With Quote

Old   January 21, 2012, 13:14
Default Single - double - multiple...
  #11
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
A double edge of a shell element is an edge shared by two shells (normal situation). A triple edge is an edge shared by three shells (like a T-connection), which could be normal if you expected a T-connection or could suggest a problem. Rather than have a special diagnosis for "triple edge", we just have one for "multiple edge", which could be three or more shells meeting at an edge...

By the same logic, a single edge is an edge connected to only a single shell... In practice, it is the perimeter of a 2D or zero thickness shell model. Perfectly acceptable in those circumstances, but potentially a problem if you were trying to form a closed volume so you could fill with delaunay or hexa dominant fills...

When the mesh check tells me I have one of these situations, even if I am expecting it, I just ask for the subset. Then I add one or two layers to the subset so I can get an idea of what is going on. You can also right click on shells to have it highlight these single or multiple edges. Either way, don't decide if it is a problem or what to do until you have seen it in context.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   February 18, 2013, 16:54
Default
  #12
Member
 
Join Date: Jun 2011
Posts: 65
Rep Power: 6
maalan is on a distinguished road
Hi, Simon!!

Just a simple question... I am trying to mesh a 2D circular cylinder, so you can imagine which my problem is: single edes! also you told single edges is not always a problem (above all in 2D meshes), if I export my bidimensional mesh to fluent without checking, I found an error from fluent when reading. So, could you tell me how to face this problem?? I am sure it has to do a very easy solution as I was getting excellent results from 3D hexa meshes...

Best,
Antonio
maalan is offline   Reply With Quote

Old   October 16, 2014, 06:00
Default
  #13
New Member
 
Join Date: Oct 2014
Posts: 1
Rep Power: 0
gg33 is on a distinguished road
Hello everybody,
i am using icem cfd for 1 year and i am creating my first 3D mesh.
My cfd calculation give me an error with that mesh only on some elements.
Mesh quality is good for icem but there is a problem with some single edges,
these edges and faces are precisely the elements making problems during the
computation.
I dont' know how to deal with that problem, would you know what to do ?
Thanks
Jérôme
gg33 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
Incompressible Turbulence models achinta OpenFOAM 4 May 27, 2010 10:35
Two-fluid models vs mixture models for bubbly flows Hansong Tang Main CFD Forum 6 December 8, 2009 04:21
Single Bubble Gerrit Senger CFX 4 March 12, 2007 17:29
Different models in a single domain RANA FLUENT 2 February 15, 2007 10:23
P4 1.5 or Dual P3 800EB on Gibabyte board Danial FLUENT 4 September 12, 2001 11:44


All times are GMT -4. The time now is 11:34.