CFD Online URL
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ICEM] Fixing tetra Surface Orientations after prism generation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 10, 2010, 07:09
Default Fixing tetra Surface Orientations after prism generation
  #1
siw
Senior Member
 
Join Date: Jul 2009
Posts: 436
Rep Power: 12
siw is on a distinguished road
Hi,

I need some help with the fixing some bad tetra elements which occur when the prism elements are generated for an external flow simulation (see 1st image). Before making the prisms I check and smooth the surface tri and volume tetra elements to get as good a mesh as possible. The node quanity after prism generation is about what I'm needing for the study.

Firstly, near the end of the prism generation process the following is shown in ICEM:

"I shouldn't be disconnecting stuck_triangles"

What does this mean?

Also, an error_log file is written and contains the following sample repeated many times but with different numbers:

{cells near 1792.661754 967.770023 235.080261 occupy the same volume
} {cells 53470 and 724239
} {face node numbers 152809 254038 316061
} {opposite vertices 338344 226282

When I check the mesh, after prism generation, a dialogue box appears saying:

21 problem elements were found. You can put them in a new subset "Surface orientations", or ignore.

So I select Create Subset and three clumps of elements are shown (images 2,3,4) and all are near the trailing edges (image 5).

It looks like ICEM has made some elements over lap each other. So I have tried editing these bad elements by deleteing them and using Repair Mesh -> Find/Close Holes In Mesh or Repair Mesh -> Remesh Elements but these don't fix the issue.

How can they be made into good quality elements?

I have used the prism settings shown in image 6. You can see that I have specified a 1st layer height and not let the prisms float but I have set a Max Height Over Base so that ICEM will keep adding prims until the transition to tetras a fairly smooth.

This was on purpose because I find that if I select (let's say) 7 prism layers and let them float I would then need to split and redistribute these 7. But beause I have a large variation in tri/tetra sizes on the surfaces (e.g. small elements on leading/trailing edges but larger elements in the middle of the wing) when I come to split the prisms by specifiying a 1st layer height (based on required y+ and Reynolds number) and number of layers I would either get too great a growth rate in the middle of the wing or too many layers at the small elements. Also I would need more layers on the wing middle to go from the specied 1st layer height to a smooth transition to the tetras at a sensible growth rate, but split/redistribute would mean the number of layers is the same all around the wing and either the groth rate or 1sy layer height not ideal (depending on which one I specify). If I split and redistibuted on that basis there would be far too many prisms near the leading/trailing edges not at a sensible growth rate. Which is why I use the Max Height To Base and more layer than I think is needed to ICEM stops making them to transition smoothly.

I hope that last paragraph gets my meaning across clearly.

Thanks.
Attached Images
File Type: jpg 1.JPG (57.3 KB, 223 views)
File Type: jpg 2.JPG (42.6 KB, 159 views)
File Type: jpg 3.JPG (44.2 KB, 141 views)
File Type: jpg 4.JPG (43.9 KB, 138 views)
File Type: jpg 5.JPG (51.0 KB, 154 views)
siw is offline   Reply With Quote

Old   October 10, 2010, 07:10
Default
  #2
siw
Senior Member
 
Join Date: Jul 2009
Posts: 436
Rep Power: 12
siw is on a distinguished road
Adding image 6 as only post 5 images per post.
Attached Images
File Type: jpg 6.JPG (33.9 KB, 137 views)
siw is offline   Reply With Quote

Old   October 16, 2010, 11:06
Default
  #3
siw
Senior Member
 
Join Date: Jul 2009
Posts: 436
Rep Power: 12
siw is on a distinguished road
I still cannot fix this.

Can anyone help?
siw is offline   Reply With Quote

Old   October 18, 2010, 03:37
Default Sorry, known bug
  #4
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Sorry I missed this post earlier, I have been traveling around for user group meetings. I will be at the Belgian meeting on Wednesday and the Italian conference on Thursday and Friday and then it is back home to normal life.

Sorry also for this bug. It showed up (in some specific models) in 11.0 when we improved some prism performance and was fixed partially for 12.0 and the rest of the way for 12.1.

In the mean time, we added an option under 12.0 advanced user settings to use PrismV10... (it is noted as a remedy to this error in the 12.0 release docs and tech support would have also been able to help you quickly) If you generate prism again with this older executable, you will sacrifice a bit of performance, but at least you won't get these strange self intersecting prisms when ever it deals with stuck elements...

I also recommend you upgrade to V13 due out in November (no additional charge if your license is current). Then you will have our most robust (lowest bug count, most stable) and most efficient (improved speed, lower memory and multi-threaded (SMP)) version of ICEM CFD ever...
PSYMN is offline   Reply With Quote

Old   October 18, 2010, 03:50
Default
  #5
siw
Senior Member
 
Join Date: Jul 2009
Posts: 436
Rep Power: 12
siw is on a distinguished road
PSYMN, you should visit England whilst you're in Europe. We've got a spare desk in the office and you could help out directly with these ICEM issues I've been having .

I'll give the PrismV10 option a try now and see how that goes. Unfortunately, due to the staggered release in ANSYS out of the customer portal I don't think I'll be getting v13 until December/January.
siw is offline   Reply With Quote

Old   October 21, 2010, 03:37
Default
  #6
siw
Senior Member
 
Join Date: Jul 2009
Posts: 436
Rep Power: 12
siw is on a distinguished road
ICEM will not run with PrismV10 activated. It displays a licencing error message than even ANSYS tech support could not fix.
siw is offline   Reply With Quote

Old   November 17, 2010, 01:58
Default
  #7
New Member
 
Join Date: Nov 2010
Location: Edinburgh
Posts: 2
Rep Power: 0
gmach is on a distinguished road
For ICEM 12.1 select "Do checks" and "Do not allow sticking" at the Advanced prism meshing parameters window (Mesh>Global mesh setup>Advanced prism meshing parameters) and recompute prism mesh. It worked for me.
gmach is offline   Reply With Quote

Old   November 17, 2010, 08:54
Thumbs up
  #8
siw
Senior Member
 
Join Date: Jul 2009
Posts: 436
Rep Power: 12
siw is on a distinguished road
Very big thanks gmach.

All this time and that has fixed the issue.
siw is offline   Reply With Quote

Old   November 17, 2010, 12:20
Default
  #9
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Thanks GMACH...

I was not aware of that fix either...

Best regards,

Simon
PSYMN is offline   Reply With Quote

Old   March 31, 2012, 15:30
Default Does not solve my error output
  #10
New Member
 
Eirikur Jonsson
Join Date: Aug 2011
Posts: 5
Rep Power: 5
eirikurjon07 is on a distinguished road
Hi Simon
It seems that the "Do checks" and "Do not allow sticking" are not doing their magic for my geometry and prism. I have a simple wing geometry (only the wing, without the fusalage) and I am trying to follow the bottom-up wingbody tutorial where the shell mesh is generated first, then prisms are extruded from the wing and finally the volume mesh is grown from the prism mesh and flooded with tri.

I am doing it slightly different that in the tutorial, where instead of growing 5 or 20 layers as in the tutorial I grow only 1 and split it manually later to speed up the process. However both fail.

The problem is that at the wing tip and trailing edge (sharp) the prism mesher merges the prisms together or fails to grow them properly. The figure show where one prism layer has been grown.

Performing mesh check reveals "volume orientation" problems which can be fixed but the prims are merged into larger elements which results in y+ beeing huge at that location compared to around 1 where the prisms are fine.

The strange thing is that if I double the node count, streamwise and spanwise then sometimes the prism process covers the wing properly but is still pumpes out the error "I shouldn't be disconnecting stuck_triangles"
just more lines than earlier. Now the mesh that covers the wing properly reports no errors in "check mesh" but it has way to many elements for my application and is then not an option. I would like to get as coarse mesh as possible.



Any idea what might be happening and why ICEM is pumping out this error even if it seems to cover the surface properly ?
eirikurjon07 is offline   Reply With Quote

Old   March 31, 2012, 15:31
Default
  #11
New Member
 
Eirikur Jonsson
Join Date: Aug 2011
Posts: 5
Rep Power: 5
eirikurjon07 is on a distinguished road
Ahh forgot one vital information. I am using the latest release of ANSYS ICEM 14.0
eirikurjon07 is offline   Reply With Quote

Old   July 3, 2012, 20:54
Default Anyone ?
  #12
New Member
 
Eirikur Jonsson
Join Date: Aug 2011
Posts: 5
Rep Power: 5
eirikurjon07 is on a distinguished road
I still cannot fix this.

Can anyone help?
eirikurjon07 is offline   Reply With Quote

Old   July 4, 2012, 10:21
Default
  #13
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Sorry, I don't know what the problem is... I don't use that bottom up method very often.

One thing I do often do with wings like this is create a trailing edge surface that extends for some distance behind the wing (some times all the way to the outlet). This prevents any trailing edge problems by splitting up the nearly 360 degree angle into two nearly 180 degree angles which are much easier for prism to handle...

When you are done meshing, just delete the surface elements on this trailing edge surface... Or set the right boco... depending on your solver.
__________________
-----------------------------------------
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 4, 2012, 15:41
Default
  #14
New Member
 
Eirikur Jonsson
Join Date: Aug 2011
Posts: 5
Rep Power: 5
eirikurjon07 is on a distinguished road
Thanks for your reply Simon
I have used similar technique in 2D but with a line. I have also tried the top down method (using patch independent) but then I am unable to use bunching functions which I need to capture the pressure rise at LE and separation at the TE as well as shocks on the upper surface. Maybe I am doing something wrong here.

My goal here is to mesh a 3D wing with inflation layer and density region aft of the wing. If not bottom-up approch what meshing strategy would you use ? I would prefer to use unstructured mesh.

Regards eiki
eirikurjon07 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
Problem with Gmsh nishant_hull Open Source Meshers: Gmsh, Netgen, CGNS, ... 17 December 7, 2007 02:33
ICEM CFD 5.0 (Tetra) - Internal Wall/Thin Surface James Date CFX 3 December 24, 2004 08:41
Surface Grid generation Von Main CFD Forum 0 March 4, 2002 18:03
surface mesh generation Jongtae Kim Main CFD Forum 0 April 11, 1999 21:56
Latest news in mesh generation Robert Schneiders Main CFD Forum 0 March 2, 1999 05:07


All times are GMT -4. The time now is 10:30.