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

[ICEM] Error in mesh writing

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

Like Tree3Likes
  • 1 Post By stuart23
  • 2 Post By diamondx

Reply
 
LinkBack Thread Tools Display Modes
Old   March 4, 2013, 07:31
Default Error in mesh writing
  #1
New Member
 
Join Date: Mar 2011
Posts: 20
Rep Power: 6
helios is on a distinguished road
Hi at all, i have a problem with mesh output writing...this is what happens: i choose the solver (fluent v6), then i save my project then the mesh ( uns format) and when i try to configure the fluent menu parameters the following error appears me:

"ERROR

running fluent v6 interface vers 14.5.12

ERROR

the interface cannot handle quadratic elements. child process exited abnormally"

and this is what i see in dialog box:

"WARNING:mesh has uncovered edges. fluent needs a complete boundary( lines in 2d)
or it will give a variety of errors and not read in the mesh. if this was 2D Hexa, perhaps your edges are not associated with perimeter curves".

So how can i see kind of error is?? i guess i have associated all geometry but i have no idea what i have to do to solve the problem. Please help me.

thanks at all
helios is offline   Reply With Quote

Old   March 4, 2013, 21:34
Default
  #2
Senior Member
 
Stuart Buckingham
Join Date: May 2010
Location: United Kingdom
Posts: 267
Rep Power: 16
stuart23 will become famous soon enough
Problems with export 2D mesh from ICEM to FLUENT

*Search first
BrolY likes this.
__________________
http://bc247.wordpress.com
stuart23 is offline   Reply With Quote

Old   March 5, 2013, 07:37
Default
  #3
New Member
 
Join Date: Mar 2011
Posts: 20
Rep Power: 6
helios is on a distinguished road
thanks a lot Stuart i'll try and i'll inform you.thanks again
helios is offline   Reply With Quote

Old   March 7, 2013, 04:31
Default
  #4
New Member
 
Join Date: Mar 2011
Posts: 20
Rep Power: 6
helios is on a distinguished road
Hi Stuart i've followed advices into post you've been saw me but now i'm still in troui explain you...this is what i've done:

"Turn on all your parts and turn on line elements but turn off shells...
You should have line elements around the perimeter and between any two shell parts...
If not, then that is your problem. The uncovered faces check should also find these.
The fix, if using ICEM CFD Hexa, is to go back and associate edges to curves...
When an edge is associated to a curve, line elements form in the part name of the curve...
No association, no line elements, no boundaries for fluent..." ( FROM SIMON REPLY)

1)i think i have associated all edges to each curve but several errors has been found..
1)all uncovered edges (pict.1)...i'have thought to add that uncovered edges to fluid
(it seems the better solution,doesn't it?)....
2)then the program ask me to choose the surface which contain the periodic faces...
but i don't understand which periodic surfaces it refers(pict2)....
3)icem found many single edge elements located round the airfoil and attached to domain's boundary..
what have i do to fix them?delete them?create a subset and do anything else?(pict3)
4)same question for last problem (pict 4) when icem found standalone elements?
what i have to do to fix them?(pict 4).

I attach pictures and if you can see them i can send you my files...

thanks a lot

1_EPPLER 61_PRIMO MESSAGGIO ERRORE.jpg

2_EPPLER 61_TRA PRIMO E SECONDO MESSAGGIO ERRORE.jpg

3_EPPLER 61_SECONDO MESSAGGIO ERRORE.jpg

4_EPPLER 61_TERZO MESSAGGIO ERRORE.jpg
helios is offline   Reply With Quote

Old   March 8, 2013, 11:38
Default
  #5
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
Wow, so much wrong here ;^)

Quadratic elements are elements with mid side nodes. They would be appropriate for FEA analysis in ANSYS or Nastran, but not for CFD codes which require linear elements (no mid side nodes).

ICEM CFD generates linear elements by default, so I am guessing you added mid side nodes at some point... Don't do that.

Your model is not periodic, so no need for the periodic check.

Single edge elements are expected around the perimeter of a 2D model. Just run the check to confirm they are all on the edges (around the far field and around the airfoil) and then be happy. If they are elsewhere, then you have a problem that needs some adjustment.

The other error messages are also not worth worrying about...

If you generated this model with Hexa, just unload your unstructured mesh... Go back to the hexa blocking and confirm that ALL the peirmeter edges are associated with curves. Then convert the premesh to uns mesh again. Smooth again. Run your checks, but don't do anything drastic ;^) Output to the solver...

Best regards,

Simon
__________________
-----------------------------------------
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   March 8, 2013, 11:48
Default
  #6
New Member
 
Join Date: Mar 2011
Posts: 20
Rep Power: 6
helios is on a distinguished road
thanks Simon but if i use quadratic elements without mid side nodes i lose definition around the arfoils...linear elements enter into it and i won't it...how can i do??
helios is offline   Reply With Quote

Old   March 8, 2013, 12:35
Default
  #7
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
Fluid solvers only use linear elements (with a few small exceptions). You just have to accept some faceting. The standard solution is a finer mesh in areas of higher curvature so that the facets are smaller and have a smaller max deviation.
__________________
-----------------------------------------
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   March 8, 2013, 12:46
Default
  #8
New Member
 
Join Date: Mar 2011
Posts: 20
Rep Power: 6
helios is on a distinguished road
mmm i see....Simon i appreciate too much your help but i haven't finished to stress you i have anothe question: when i use the split edge with autmatic linear option it doesn't work...i have always to use linear option to spread the edge on my curve...why?? and thanks again
helios is offline   Reply With Quote

Old   March 8, 2013, 13:05
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
The interactive blocking edge split controls ask you to provide the split vertex. The Automatic Linear option extracts point vertices based on the edge distribution. My guess is that you don't have many nodes along the edge you are trying to split. With no extra nodes for "Automatic Linear" to move, it doesn't appear to do anything. Increase your count on that edge and try again, but be aware that increasing the node count will cause it to propagate out to the model extents.

Best regards,

Simon
__________________
-----------------------------------------
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   March 14, 2013, 10:54
Default
  #10
New Member
 
Join Date: Mar 2011
Posts: 20
Rep Power: 6
helios is on a distinguished road
Hi Simon...have you received my last message??please answer me because i have always the same problem....thanks

Best regards,

Helios
helios is offline   Reply With Quote

Old   March 14, 2013, 11:23
Default
  #11
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,291
Blog Entries: 23
Rep Power: 20
diamondx will become famous soon enough
before using split edge with automatic linear, you need to specify number of nodes on that edge. try it.
PSYMN and cesarcg like this.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   March 14, 2013, 11:37
Default
  #12
New Member
 
Join Date: Mar 2011
Posts: 20
Rep Power: 6
helios is on a distinguished road
thanks a lot diamond...i'll try immediately
helios is offline   Reply With Quote

Old   March 14, 2013, 11:44
Default
  #13
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
Quote:
Originally Posted by helios View Post
Hi Simon...have you received my last message??please answer me because i have always the same problem....thanks

Best regards,

Helios
Yes, I replied on the 8th.
__________________
-----------------------------------------
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   March 14, 2013, 11:48
Default
  #14
New Member
 
Join Date: Mar 2011
Posts: 20
Rep Power: 6
helios is on a distinguished road
Sorry Simon i referred to the next message i sent you about an icem's internal error message?? haven't you received it??
helios is offline   Reply With Quote

Old   September 3, 2013, 03:51
Default
  #15
New Member
 
Michael Bausas
Join Date: May 2013
Posts: 10
Rep Power: 4
mikebausas is on a distinguished road
Hello,

i am working with my thesis where i am trying to simulate the performance of a VAWT with NACA0025 airfoil. I made my mesh in ICEM CFD and successfully imported it to fluent. However, when i am trying to set up my mesh for simulation, the Mesh Interface is grayed out.

Can anyone please help me understand what specifically is the problem and how to fix it. Pls help.. THank you so much in advance.
mikebausas is offline   Reply With Quote

Old   September 3, 2013, 08:33
Default
  #16
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
Hey Mike, this looks like a new thread to me. Also, try to be more clear about if you have generated the mesh or not. I thought it was a bit confusing.
__________________
-----------------------------------------
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   April 6, 2014, 06:25
Default Error in ICEM CFD
  #17
New Member
 
Karan Gadani
Join Date: Apr 2014
Posts: 1
Rep Power: 0
karangadani is on a distinguished road
Error:
Running FLUENT V6 Interface Vers. 15.0.5

Creating a Fluent 2D mesh.
Computing connectivity for 67657 cells.
Error : face (near node 725) is attached to more than 2 cells.
Error : face (near node 739) is attached to more than 2 cells.
Error : face (near node 753) is attached to more than 2 cells.
Error : face (near node 126) is attached to more than 2 cells.
Error : face (near node 101) is attached to more than 2 cells.
Error : face (near node 702) is attached to more than 2 cells.
Error : face (near node 725) is attached to more than 2 cells.
Error : face (near node 753) is attached to more than 2 cells.
Error : face (near node 749) is attached to more than 2 cells.
Error : face (near node 739) is attached to more than 2 cells.
Error : face (near node 730) is attached to more than 2 cells.
Error : face (near node 726) is attached to more than 2 cells.
Error : face (near node 127) is attached to more than 2 cells.
Error : face (near node 690) is attached to more than 2 cells.
Error : face (near node 55) is attached to more than 2 cells.
Error : face (near node 706) is attached to more than 2 cells.
Error : face (near node 706) is attached to more than 2 cells.
Error : face (near node 84) is attached to more than 2 cells.
Error : face (near node 699) is attached to more than 2 cells.
Error : face (near node 698) is attached to more than 2 cells.
Error : face (near node 4810) is attached to more than 2 cells.
Error : face (near node 4810) is attached to more than 2 cells.
Error : face (near node 789) is attached to more than 2 cells.
Error : face (near node 688) is attached to more than 2 cells.
Error : face (near node 699) is attached to more than 2 cells.
Error : face (near node 84) is attached to more than 2 cells.
Error : face (near node 726) is attached to more than 2 cells.
Error : face (near node 654) is attached to more than 2 cells.
Error : face (near node 1274) is attached to more than 2 cells.
Error : face (near node 1274) is attached to more than 2 cells.
Error : face (near node 537) is attached to more than 2 cells.
Error : face (near node 537) is attached to more than 2 cells.
Error : face (near node 4810) is attached to more than 2 cells.
Error : face (near node 101) is attached to more than 2 cells.
Error : face (near node 789) is attached to more than 2 cells.
Error : face (near node 789) is attached to more than 2 cells.
Error in computing cell connectivity.
child process exited abnormally


WARNING: Mesh has uncovered edges. ANSYS Fluent needs a complete boundary (lines in 2D) or it will give a variety of errors and not read in the mesh! If this was 2D Hexa, perhaps your edges are not associated with perimeter curves

can you please help me out how to solve this problem???
karangadani 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
Cht tutorial in 15 braennstroem OpenFOAM Running, Solving & CFD 197 June 10, 2015 03:02
3D Hybrid Mesh Errors DarrenC ANSYS Meshing & Geometry 11 August 5, 2013 06:42
engrid -> save as .stl with boundarie codes Zymon enGrid 31 August 29, 2011 13:40
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
basic of mesh refinement arya CFX 4 June 19, 2007 12:21


All times are GMT -4. The time now is 18:42.