|
[Sponsors] |
[ICEM] Some 2D Mesh come out in my 3D model,anyone can help me? |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
May 14, 2012, 11:12 |
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: 14 |
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! |
|
May 14, 2012, 11:22 |
|
#3 |
New Member
Zhonghai Xu(xuzhonghai@sjtu.edu.cn)
Join Date: Apr 2012
Location: Shanghai,CHINA
Posts: 17
Rep Power: 14 |
I will send a email to you,attachment is 300K,beyonds the limit
|
|
May 15, 2012, 10:02 |
|
#4 |
Senior Member
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,663
Blog Entries: 1
Rep Power: 47 |
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 |
|
May 15, 2012, 10:16 |
|
#5 |
New Member
Zhonghai Xu(xuzhonghai@sjtu.edu.cn)
Join Date: Apr 2012
Location: Shanghai,CHINA
Posts: 17
Rep Power: 14 |
Dear PSYMN,
Thanks for your reply.May I have your email?I will send you my model. Mine:xuzhonghai@sjtu.edu.cn |
|
May 21, 2012, 16:27 |
|
#6 |
Senior Member
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,663
Blog Entries: 1
Rep Power: 47 |
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.
__________________
----------------------------------------- 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 |
|
May 21, 2012, 22:13 |
|
#7 |
New Member
Zhonghai Xu(xuzhonghai@sjtu.edu.cn)
Join Date: Apr 2012
Location: Shanghai,CHINA
Posts: 17
Rep Power: 14 |
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. |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[ICEM] surface mesh merging problem | everest | ANSYS Meshing & Geometry | 44 | April 14, 2016 06:41 |
[ICEM] Problem making structural mesh on a surface | froztbear | ANSYS Meshing & Geometry | 1 | November 10, 2011 08:52 |
[snappyHexMesh] snappyHexMesh won't work - zeros everywhere! | sc298 | OpenFOAM Meshing & Mesh Conversion | 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 |