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

[ICEM] Problems with export 2D mesh from ICEM to FLUENT

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

Like Tree16Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   December 12, 2012, 18:04
Default
  #21
Retired from CFD Online
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
It is usually better to split all the way rather than try to split only selected blocks... It keeps things less messy.

You can always merge blocks later if you need to clean it up.

For the checking options, there may be a tutorial, but you really just need to look in the help to see what each one does.
__________________
-----------------------------------------
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   December 12, 2012, 18:15
Default
  #22
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 271
Rep Power: 7
Bollonga is on a distinguished road
There's only something weird, when I'm connecting curves to edges, inlet and outlet curves seem to be somehow associated. I didn't care for that, but then in fluent I see that there's no inlet boundary, just to outlets! I've tried to fix that with no success... Any suggestions?
Bollonga is offline   Reply With Quote

Old   December 12, 2012, 18:52
Default
  #23
Retired from CFD Online
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
No idea, it worked properly for me.
__________________
-----------------------------------------
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   December 12, 2012, 18:55
Default
  #24
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Tokyo, Japan
Posts: 1,366
Blog Entries: 23
Rep Power: 21
diamondx will become famous soon enough
Quote:
Originally Posted by Bollonga View Post
There's only something weird, when I'm connecting curves to edges, inlet and outlet curves seem to be somehow associated. I didn't care for that, but then in fluent I see that there's no inlet boundary, just to outlets! I've tried to fix that with no success... Any suggestions?

i think this happens if you do association of multiple edge with multiple curve.

You need to UNGROUP the curve then you will be able to associate each one of them
PSYMN likes this.
__________________
Regards,
New to ICEM CFD, try this document --> https://goo.gl/NEbygB
Ali
diamondx is offline   Reply With Quote

Old   December 13, 2012, 03:49
Default
  #25
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 271
Rep Power: 7
Bollonga is on a distinguished road
I've managed to unrelate the curves and reassociate them. I've reassigned BC but in fluent Inlet boundary is still as outlet. I've also tried fixing the mesh again with no results. I can continue working with Simon's mesh, but I'd like to learn how to solve that issue. Anymore thing to try?

Thanks a lot guys!
Bollonga is offline   Reply With Quote

Old   December 13, 2012, 07:58
Default
  #26
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,314
Blog Entries: 6
Rep Power: 43
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
What are the issues with your mesh? did you solve them? I assume you are now working with Simon's blocking.
Far is offline   Reply With Quote

Old   December 13, 2012, 08:21
Default
  #27
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 271
Rep Power: 7
Bollonga is on a distinguished road
Well, I did all the steps Simon told me, and everything went fine untill I loaded the mesh in fluent. The problem is there is no inlet BC, just two outlet BCs. I checked it on Icem and everything was okay. That wasn't happening to Simon's mesh. I can upload the icem files in case you wanna check it out.

https://dl.dropbox.com/u/6986695/PS_12_12.rar
Bollonga is offline   Reply With Quote

Old   December 13, 2012, 12:48
Default Post # 10 & 12
  #28
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,314
Blog Entries: 6
Rep Power: 43
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
I am talking about the blocking issues at post # 10 and 12. Did you solve them or moved with new blocking as suggested by the Simon. Because I just took look on those files (post 12) and worked around half an hour and finally found the fault besides the blocking problems as described in detail by Simon. Wanna know the reason

PS: I have recorded all into one video clip too, where you can see my frustrution

Last edited by Far; December 13, 2012 at 13:13.
Far is offline   Reply With Quote

Old   December 13, 2012, 15:17
Default
  #29
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,314
Blog Entries: 6
Rep Power: 43
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by Bollonga View Post
Well, I did all the steps Simon told me, and everything went fine untill I loaded the mesh in fluent. The problem is there is no inlet BC, just two outlet BCs. I checked it on Icem and everything was okay. That wasn't happening to Simon's mesh. I can upload the icem files in case you wanna check it out.

https://dl.dropbox.com/u/6986695/PS_12_12.rar

There are lot of problems in the attached ICEM project as already mentioned by Simon. But i worked Ab_initio, I still got problem.........

In which blocking you have the inlet problem? can you attach that?
Far is offline   Reply With Quote

Old   December 13, 2012, 16:05
Default
  #30
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,314
Blog Entries: 6
Rep Power: 43
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Check this ....

https://dl.dropbox.com/u/68746918/ballogona.mp4

https://dl.dropbox.com/u/68746918/final.mp4
Attached Files
File Type: zip PS_2D_12_12_Far.zip (9.4 KB, 3 views)
Far is offline   Reply With Quote

Old   December 14, 2012, 04:46
Default
  #31
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 271
Rep Power: 7
Bollonga is on a distinguished road
All the problematic files are in the link I posted. I don't know which block was the one causing trouble. I'm sorry for your lost time.
Bollonga is offline   Reply With Quote

Old   December 14, 2012, 05:33
Default
  #32
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,314
Blog Entries: 6
Rep Power: 43
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
First, I noticed that you had the fluid part set to internal wall instead of fluid. You also had a part for internal wall, which you didn't need. (i just un-associated all those edges).
This was problem, which is solved by Simon already.


Then the blocking issues were solved by Simon's six steps

Quote:
To clean this up...

1) Reset index control
2) Split Block => Extend Split => All Edges (you will see the extra splits revealed)
3) Merge Vertices (turn on option to "propagate merge") select a pair of verts that need to be merged away...
4) Confirm "delete station" (this removes the unnecessary indices, you should see the I index Max decrease to "5")
5) fix any lost projections... (this is why you still had an uncovered face, the tiny edge may not have been properly associated).

6) New premesh, new unstructured mesh, check mesh, output (2D), etc.
To undetstand the problem what i did is :

Case A: (https://dl.dropbox.com/u/68746918/ballogona.mp4)

1. Started the blocking from scratch that is I did not use the six steps by Simon. Instead I went o create block > 2d planner block

2. Deleted the unwanted geometric entities such as internal curves and points. Also deleted the symmetry curves and recreated them.

3. Made the splits according to geometry.

4. Associated the all edge to appopriate curves and points to vertices.

5. Edge mesh parameters (roughly specified)

6. Pre-mesh and then unstructured mesh .

7. Solver selection and boundary condition specification as usual.

8. Mesh output and read into Fluent

9. Bingo error. No matching of nodes. Zero nodes. Non positive volume

10. repeated again and again..................... every time failure.

11 Finally went to boundary condition panel and deleted boundary conditions for the Fluid and interior.

12. Got the mesh working.

Case B: (https://dl.dropbox.com/u/68746918/final.mp4)

1. Deleted boundary conditions, geometry parts and blocking.

2. recreated the some curves.

3. Initialized new blocking, made splits and associated

4. Edge mesh parameters, pre mesh and conversion to unstructured mesh.

5. solver selection, boundary conditions, and output mesh

6. Read in Fluent. Every thing went fine.


PS: Your case had multiple injuries
Attached Images
File Type: jpg a.jpg (73.7 KB, 18 views)
Far is offline   Reply With Quote

Old   December 14, 2012, 06:53
Default
  #33
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 271
Rep Power: 7
Bollonga is on a distinguished road
Wow! Thanks a lot Far, people like you make CFD less cryptic!
Bollonga is offline   Reply With Quote

Old   December 14, 2012, 07:32
Default Case 3 - same blocking and same geometry
  #34
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,314
Blog Entries: 6
Rep Power: 43
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Here is the case - Minimum changes from original geometry and blocking. (https://dl.dropbox.com/u/68746918/case3.mp4)

Steps:

1. Start ICEM CFD

2. Load first tin and then blocking.

3. edge mesh parameter on the lower symmetry centre edge were set. Just changed scheme to uniform from geometric.

4. Used extend split > all edges.

5. Delete internal curves. Disassociate (remove association) the corresponding edges.

5. recompute pre-mesh, convert to unstructured meshing, boundary conditions (if needed) and output 2d meshing.

6. Read mesh in Fluent.
Attached Files
File Type: zip Case3_Far.zip (6.8 KB, 2 views)
Far is offline   Reply With Quote

Old   December 19, 2012, 08:07
Default
  #35
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 271
Rep Power: 7
Bollonga is on a distinguished road
Hello again guys,

I've been trying a different mesh for the same case but I've encountered some trouble with my blocking edges.
It seems that when more than 4 edges arrive to a vertex there are some extra edges collapsed into the corners which I cannot erase, in the attached picture the edge count is displayed, and there are some extra numbers in the corners.The desired blocks are also shown in a picture.
I've tried to extend split and then merging nodes and erasing extra blocks but it didn't worked, and it messed everything up.

How can I avoid that "collapsed" edges?

Thanks!
Attached Images
File Type: jpg Edges_count.jpg (21.3 KB, 9 views)
File Type: png Blocks.png (18.9 KB, 9 views)
Bollonga is offline   Reply With Quote

Old   December 19, 2012, 08:37
Default
  #36
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 271
Rep Power: 7
Bollonga is on a distinguished road
I've also checked the faces of each blocks and there are some missing ones, I don't know why. In the picture blocks are pink and faces black.
Attached Images
File Type: png Blocks_faces.png (18.9 KB, 5 views)
Bollonga is offline   Reply With Quote

Old   December 19, 2012, 10:34
Default
  #37
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,314
Blog Entries: 6
Rep Power: 43
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
check out this ..........

http://www.youtube.com/watch?v=IuOCRmNyPQM

http://www.youtube.com/watch?v=3bAKfxSL6Es
Far is offline   Reply With Quote

Old   December 19, 2012, 17:05
Default
  #38
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 271
Rep Power: 7
Bollonga is on a distinguished road
Thanks Far, but I already did a mesh like the one in the videos. The problem isn't this specific mesh but how to solve this "collapsed" edges for any mesh.
Bollonga is offline   Reply With Quote

Old   December 19, 2012, 17:11
Default
  #39
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,314
Blog Entries: 6
Rep Power: 43
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
attach files so that I can take look of them......
Far is offline   Reply With Quote

Old   December 20, 2012, 04:06
Default
  #40
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 271
Rep Power: 7
Bollonga is on a distinguished road
Hi, vertex 61 is an example of the issue with the edge. I solved the case with a different blocking, but I'd like to know how to solve that. Thanks.

http://dl.dropbox.com/u/6986695/PS_2D_19_12.zip
Bollonga is offline   Reply With Quote

Reply

Tags
batch mode, flat plate, fluent, icem

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
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
Transport mesh from ICEM CFD, to Fluent, to Sysnoise Wieland FLUENT 2 April 15, 2012 06:28
[ICEM] Export refined mesh to fluent Heleen ANSYS Meshing & Geometry 8 March 26, 2012 08:33
Export mesh from ICEM to Fluent 6.3 (3D) bigbang ANSYS 0 June 7, 2010 23:05
ICEM - problems with prism mesh João Lourenço CFX 1 November 6, 2007 15:41


All times are GMT -4. The time now is 01:47.