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

[ICEM] Some 2D Mesh come out in my 3D model,anyone can help me?

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

Like Tree1Likes
  • 1 Post By PSYMN

Reply
 
LinkBack Thread Tools Display Modes
Old   May 14, 2012, 11:12
Default Some 2D Mesh come out in my 3D model,anyone can help me?
  #1
New Member
 
Zhonghai Xu(xuzhonghai@sjtu.edu.cn)
Join Date: Apr 2012
Location: Shanghai,CHINA
Posts: 17
Rep Power: 4
realstoneman is on a distinguished road
Hello,
everybody,as my title,my model is 3D,but when I created mesh by ICEM CFD,there exists some 2D mesh,which you can see from the attachments.
Thanks a lot in advance~Please explain the weird phenomenon in detail,I make the same mistake many times!
Attached Images
File Type: jpg 20120514231111.jpg (29.4 KB, 11 views)
File Type: jpg 20120514231159.jpg (53.6 KB, 9 views)
realstoneman is offline   Reply With Quote

Old   May 14, 2012, 11:20
Default
  #2
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,743
Blog Entries: 6
Rep Power: 36
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
attach model
Far is offline   Reply With Quote

Old   May 14, 2012, 11:22
Default
  #3
New Member
 
Zhonghai Xu(xuzhonghai@sjtu.edu.cn)
Join Date: Apr 2012
Location: Shanghai,CHINA
Posts: 17
Rep Power: 4
realstoneman is on a distinguished road
I will send a email to you,attachment is 300K,beyonds the limit
realstoneman is offline   Reply With Quote

Old   May 15, 2012, 10:02
Default
  #4
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,650
Blog Entries: 1
Rep Power: 33
PSYMN will become famous soon enoughPSYMN will become famous soon enough
Why do you think those are 2D elements? They look like very squished 3D elements to me.

However, your image doesn't provide enough info for me to diagnose more than that.
__________________
-----------------------------------------
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   May 15, 2012, 10:16
Default
  #5
New Member
 
Zhonghai Xu(xuzhonghai@sjtu.edu.cn)
Join Date: Apr 2012
Location: Shanghai,CHINA
Posts: 17
Rep Power: 4
realstoneman is on a distinguished road
Dear PSYMN,
Thanks for your reply.May I have your email?I will send you my model.
Mine:xuzhonghai@sjtu.edu.cn
realstoneman is offline   Reply With Quote

Old   May 21, 2012, 16:27
Default
  #6
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,650
Blog Entries: 1
Rep Power: 33
PSYMN will become famous soon enoughPSYMN will become famous soon enough
Hey Stone Man,

I finally took a look at this. The only issues I found using "Check Mesh" were single edges and multiple edges. These were both the result of your construction surfaces and are not causing you any troubles as long as you set up those construction parts properly in the solver (or delete the shells before sending them tot he solver).

The single edges are because a particular face was not actually associated to the Fuzhuwai part... You probably just missed it... You can fix it or not depending on how you plan to use that surface in post processing...

The multiple edges were just where these construction surfaces met the Outlet.

Next, I looked at quality and found the elements you were concerned about... Looking closer I could see that they were hexa elements, just very squished thin... On one side, they were almost zero thickness (pretty much like a very thin wedge). The edge parameters didn't explain this, so I thought maybe there was a geometry issue or something like that (sorry, I didn't take the time to really figure out what was wrong with the model).

The easiest way to walk over geometry issues at this scale is to go into Settings => Meshing Options => Hexa Mixed => Projection Limit.

The initial spacing there was about 0.02, so I set the projection limit to 0.05... This basically allows nodes within that distance of an edge to be linearly interpolated instead of projected...

That solved the problem immediately and brought min quality up to >0.25. The remaining elements have more standard problems, but your solver can probably handle the hexa mesh at that quality.
Attached Images
File Type: jpg StoneMan.jpg (103.1 KB, 9 views)
Far likes this.
__________________
-----------------------------------------
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   May 21, 2012, 22:13
Default
  #7
New Member
 
Zhonghai Xu(xuzhonghai@sjtu.edu.cn)
Join Date: Apr 2012
Location: Shanghai,CHINA
Posts: 17
Rep Power: 4
realstoneman is on a distinguished road
Dear PSYMN,
Thank you very much,
you explain it clearly.and I should be more patiently in associating the edges and surfaces. the fatal error comes from the edge and surface association,actually,I find out some edge and surface which I missed,as you said.it's really appreciate and thanks a lot.
realstoneman 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
[ICEM] surface mesh merging problem everest ANSYS Meshing & Geometry 39 June 5, 2013 19:02
[ICEM] Problem making structural mesh on a surface froztbear ANSYS Meshing & Geometry 1 November 10, 2011 08:52
snappyHexMesh won't work - zeros everywhere! sc298 OpenFOAM Native Meshers: snappyHexMesh and Others 2 March 27, 2011 21:11
Meshing aifoil in ICEM student123a ANSYS Meshing & Geometry 13 December 8, 2010 10:40
2d irregular grid Remy Main CFD Forum 1 December 22, 2008 04:49


All times are GMT -4. The time now is 11:42.