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

icem cfd tetra meshing error

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 22, 2011, 21:43
Default icem cfd tetra meshing error
  #1
Member
 
joegi
Join Date: Nov 2009
Location: genoa
Posts: 67
Rep Power: 7
joegi.geo is on a distinguished road
hi,

I am tryiing to mesh a quite complex geometry uisng tetra meshing (delaunay), but in the status window I get this message:

Initialization failed

Then the meshing crash/fail. I wonder what does it means this initialization failed message and how can i avoid this error. I am starting the volume mesh from a surface.

Regards,

Joel
joegi.geo is offline   Reply With Quote

Old   July 23, 2011, 13:48
Default
  #2
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
Delaunay requires an initialization before the volume filling can begin.

During this phase, it checks for single edges (holes), overlapping elements and other problems.

You should do these checks before hand and make sure your mesh is a water tight volume. Once you sort out your surface mesh problems, the volume mesh will generate.

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   July 23, 2011, 14:48
Default
  #3
Member
 
joegi
Join Date: Nov 2009
Location: genoa
Posts: 67
Rep Power: 7
joegi.geo is on a distinguished road
Hi Simon,


Thanks a lot for your reply. So at this point what should I do with these erros? I have uncovered faces, missing internal faces, penetrating elements, multiple edges, single edges and overlapping elements. Should I fix then automatically, erase them, groud them????????????


joel
joegi.geo is offline   Reply With Quote

Old   July 24, 2011, 00:17
Default
  #4
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
Create subsets for each one... I only use autofix for the last one (disconnected nodes or what ever it is called).

Then right click on each subset in the tree and add layers... This is just to give you an idea of what is actually going on there...

For instance, single edges just means shell elements that have an edge not connected to anything... The auto fix just deletes the elements, which is fine if they are just a junk tab (like a hanging chad from 2000), but if they are the edge of a hole or baffle, you don't want those deleted, you will just have a growing single edge problem. Instead create the subset and then add a few layers so you can diagnose properly... If it is the edge of a baffle (intentional and not a problem), you can just remove that clump of cells from the subset and look for other problems... If it is a hole in the surface, you can consider repairing the geometry and meshing again, or perhaps it would be easier to mesh edit your way out (Edit mesh => repair => Mesh from edges)...

And so on... Problem by problem.

If you have too many problems, you may want to go and think about your initial geometry. If you brought in in from an IGES file, consider other CAD formats... Pretty much anything is better than IGES. ACIS comes in very clean and could save you a ton of work.

If the geometry is hopeless, then perhaps a patch dependent method is not the best to start with. Try switching you shell meshing method to something that can tolerate the slop you are feeding it. You will find that Patch independent surface mesh works well with the sizing function and is a good starting point for delaunay volume mesh...
__________________
-----------------------------------------
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   July 25, 2011, 10:24
Default
  #5
Member
 
joegi
Join Date: Nov 2009
Location: genoa
Posts: 67
Rep Power: 7
joegi.geo is on a distinguished road
Hi simon,

Thanks a lot for the tips, I am continuously learning new stuff in icemcfd. I wonder if you can take a look at the geo and give me some ideas of what could be the problem. Pretty much I think the geometry is watertight but when I try to use local refinement the meshing is always failing. I get a mesh when I use coarse parameters.

Regards,

joel
joegi.geo is offline   Reply With Quote

Old   July 26, 2011, 08:34
Default
  #6
Member
 
joegi
Join Date: Nov 2009
Location: genoa
Posts: 67
Rep Power: 7
joegi.geo is on a distinguished road
Hi Simon,

I wonder what is the meaning of this message. SHould I worry about it?


rounding points to prescribed points
cannot round any tvertex to prescribed point PART_2_EDGE.709
joegi.geo is offline   Reply With Quote

Old   July 29, 2011, 11:00
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
The message just means it couldn't place a vertex on that point... It can happen if you have too many points in an area and the mesh is not fine enough to resolve all of them.

From a side conversation, I heard that your leakage problems were because you had not placed material points in the solids... That shouldn't cause this problem (it should automatically assume those are ORFN), but I am glad you are able to move on.
__________________
-----------------------------------------
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

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
Native ParaView Reader Bugs tj22 OpenFOAM Paraview & paraFoam 267 July 20, 2015 22:29
polynomial thermophysical properties II sebastian OpenFOAM Running, Solving & CFD 53 April 10, 2014 05:45
Help: "dbm_dealloc_arr" error in CFD ACE xonix Main CFD Forum 2 January 18, 2012 14:13
UDF: DEFINE_CG_MOTION for vertical jump motion of an electrode! alban Fluent UDF and Scheme Programming 2 June 8, 2010 18:54
POSDAT problem piotka STAR-CD 4 June 12, 2009 08:43


All times are GMT -4. The time now is 09:38.