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

Icem 12 cfd leakage through solid

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 18, 2010, 12:21
Default Icem 12 cfd leakage through solid
  #1
Member
 
Join Date: May 2010
Posts: 57
Rep Power: 7
Catthan is on a distinguished road
Hi fellow ansys users,

I am a new icem user and i need to mesh a burner for a stirling engine.
I import the SW09 CAD file through workbench readers and i am trying to run a tetra mesh to make sure that i don't have any leakage or other problems before i start blocking.
Unfortunately either (or both) of these 2 problems.
1: the mesh goes through solid surfaces
2: the mesh develops outside the volume because (apparently) of a hole which i cannot see and fix ..

I have tried different topo tolerances according to the guideline, different translation methods from SW09 and several ways to get rid of the yellow lines after build diagnostic topo,,
I know i am not too specific, unfortunately i am forbiden by the engine manufacturer to discuss-display any details.
Are there any general guidelines to avoid such problems?

Thank you very much.
Kind regards,
Thanos
Catthan is offline   Reply With Quote

Old   May 19, 2010, 11:52
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
Tough to help here. Have you tried the tutorials?

Have you run build topology? it should help you find holes.

When you run tetra, it will tell you about leakage and show you a line from the material point to the outside thru the hole... have you seen that?

In the end, Hexa is patch independent and doesn't "leak". So you can probably just move right on to Hexa and skip tetra completely.

Simon
PSYMN is offline   Reply With Quote

Old   May 19, 2010, 12:50
Default
  #3
Member
 
Join Date: May 2010
Posts: 57
Rep Power: 7
Catthan is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
Tough to help here. Have you tried the tutorials?

Have you run build topology? it should help you find holes.

When you run tetra, it will tell you about leakage and show you a line from the material point to the outside thru the hole... have you seen that?

In the end, Hexa is patch independent and doesn't "leak". So you can probably just move right on to Hexa and skip tetra completely.

Simon
Thanks a lot for your reply Simon.
Yes, I have tried the tutorials and I keep refering back to them every time i have a problem.
To be honest, when i run diagnostic topology with the proposed tolerance i get many yellow lines (part geom).
This proposed tolerance is smth around 0,0000004.
The guide says to use a tolerance about 1/10 of the smalest size which for me is 0.0001..when i use the latter tolerance i don't get any yellow lines.
Whatever the tolerance though, there 's not yellow curve at the spot where the mesh leaks so i couldn't identify it.
I will take a closer look however since you re recomending it.

Another problem is that, inside the geometry, the mesh goes thru the internal walls (layers and gas paths of the burner) no matter if i set them as internal walls etc.

Regarding hexa, i just started blocking today and apparently the model is too complex for a beginner,,
It seems i ll be posting questions about it soon so i ll try to get permission to at least provide a section view of the sw file to make it clearer.

Thanks for your time Simon,
Thanos
Catthan is offline   Reply With Quote

Old   May 19, 2010, 16:02
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
It could be that you have a poorly defined surface... Look at the surfaces in the leak area with "Solid wire / Full" display. You may see a hole without any edges.

To solve the problem of mesh leaking into internal voids, put a VORFN or Solid material point in those voids and you will be able to use the leakage detection tool to track where the hole is.

Simon
PSYMN is offline   Reply With Quote

Old   May 24, 2010, 09:48
Default
  #5
Member
 
Join Date: May 2010
Posts: 57
Rep Power: 7
Catthan is on a distinguished road
Hi there again.

So, I edited the geometry a bit but I still have the same problem.

What happens is that a few tetrahedra form outside the volume.
I tracked the lines and they all seem to intersect to one point inside the volume.
Attached are 2 pics to show this.
I keep looking and cannot find anything wrong with the particular geometry feature.
The input file is my solidworks model saved as parasolid text which has been the most succesful translation into icem compared to other formats, even directly importing sw file thru workbench readers, but i am starting to lose confidence about this.

If you could please have a look and post some opinions..

Thanks a lot,
Thanos
Attached Images
File Type: jpg Base Leakage wrfr.jpg.jpg (87.6 KB, 23 views)
File Type: jpg Base Leakage.jpg.jpg (60.1 KB, 24 views)
Catthan is offline   Reply With Quote

Old   May 24, 2010, 11:00
Default Material point placement?
  #6
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
Leakage just means that a flood fill from one material point can reach another.

When applied correctly, this means that there is probably a hole in the geometry, but since we have a lot of confidence in your geometry, perhaps we should look into where your material points are. You should have one material point clearly within each volume.

Occasionally, a new user will put the material point outside the volume or on the surface. This will lead to leakage because the material point is not within the correct volume.

Thanks for attaching these pics, but could you attach a pic showing the material points and perhaps the leakage path? That is what will show you the problem.

If ICEM CFD seems complicated now, keep in mind that it is just a few simple rules. As you gain experience, you will find that it is really a very logical and predictable tool set.
PSYMN is offline   Reply With Quote

Old   May 24, 2010, 11:57
Default
  #7
Member
 
Join Date: May 2010
Posts: 57
Rep Power: 7
Catthan is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
Leakage just means that a flood fill from one material point can reach another.

When applied correctly, this means that there is probably a hole in the geometry, but since we have a lot of confidence in your geometry, perhaps we should look into where your material points are. You should have one material point clearly within each volume.

Occasionally, a new user will put the material point outside the volume or on the surface. This will lead to leakage because the material point is not within the correct volume.

Thanks for attaching these pics, but could you attach a pic showing the material points and perhaps the leakage path? That is what will show you the problem.

If ICEM CFD seems complicated now, keep in mind that it is just a few simple rules. As you gain experience, you will find that it is really a very logical and predictable tool set.

Thanks

I have attached a picture where you can see the material point and an other one which is a zoom out to see the orfn point.

There are a few volumes in the geometry but all communicate thru certain paths and cavities. This is why i assigned only one material point. I hope this is ok..

Again, thanks a lot for your help
Attached Images
File Type: jpg material point.jpg (99.1 KB, 25 views)
File Type: jpg orfn.jpg (41.2 KB, 15 views)
Catthan is offline   Reply With Quote

Old   May 24, 2010, 17:53
Default
  #8
Senior Member
 
Charles
Join Date: Apr 2009
Posts: 179
Rep Power: 9
CapSizer is on a distinguished road
Simon, there is a problem that got introduced into the code somewhere after version 10. We've also wrestled with this, and sometimes the simple answer (when needing a robust octree type of tet mesh) is to revert to version 10 or 10.0.1. I would like to send you a geometry that demonstrates this behaviour, but like Thanos we also have confidentiality problems. I have taken a troublesome geometry, and morphed it into something that is certainly not confidential, but unfortunately it does not reproduce this problem! Nevertheless, the problem definitely exists, and it has been there since version 11. Basically, a good CAD model arrives in Icem, builds a perfect topology, but leaks. Save it as a Version 10 file, and it meshes quickly and with no issues in Version 10. If I can produce a non-confidential geometry that does demonstrate this problem, you will find it in your inbox!
CapSizer is offline   Reply With Quote

Old   May 24, 2010, 17:58
Default
  #9
Senior Member
 
Charles
Join Date: Apr 2009
Posts: 179
Rep Power: 9
CapSizer is on a distinguished road
Thanos, try to experiment with these options. Sometimes they make the problem go away: under surface mesh options, set the "Ignore size" to something sensible. Under volume meshing options, make sure that "Close gaps" and "Fix holes" are both turned on. The other thing to try is that I have found the step file to be a better import.
CapSizer is offline   Reply With Quote

Old   May 27, 2010, 09:05
Default
  #10
Member
 
Join Date: May 2010
Posts: 57
Rep Power: 7
Catthan is on a distinguished road
Thank you very much CapSizer for your suggestions.
Unfortunately they didn't work. It was very relieving though that sb else have had similar issues.
I would like to install icem 10 and try again but here in the Uni the IT guys who handle the licences are not very flexible.
I started to mesh the model with Hexa and I will post some questions soon in another thread.
Many thanks to Simon too.

Regards,
Thanos
Catthan is offline   Reply With Quote

Old   May 27, 2010, 09:40
Default
  #11
Senior Member
 
Charles
Join Date: Apr 2009
Posts: 179
Rep Power: 9
CapSizer is on a distinguished road
Here is something else you can try. Put a body point (different family name, something like RUBBISH) inside the internal region. When you now create the mesh, it will fill the inside with tetras belonging to this family. Afterwards, just delete the tetras in that family. Now, if there really was a leak, and you run the mesh checks, it should report uncovered faces. In my experience though, everything checks out OK if you do this, and you end up with a valid mesh.
CapSizer is offline   Reply With Quote

Old   June 2, 2010, 08:40
Default
  #12
Member
 
Join Date: May 2010
Posts: 57
Rep Power: 7
Catthan is on a distinguished road
Dear PSYMN and CapSizer,

I apologise to both for my lack of knowledge and experience.
I made one more attemt to mesh my burner with tetra, during my break from blocking for hexa.
What appeared as leakage was simply the huge tetra elements developing towards the exterior of the geometry, because i had set mesh sizes following blindly the tutorial, without accounting for my original model dimensions.
The resulting mesh is now fully contained within the volume, without entering through inner solids.
i am sorry i did not notice that earlier and kept bothering you with leakage etc.

Thanks again.
Regards,
Thanos
Catthan is offline   Reply With Quote

Old   June 2, 2010, 10:14
Default No problem.
  #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
Glad you sorted it out on your own. It is a learning process.

Simon
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
Need help icem cfd kakhtar ANSYS Meshing & Geometry 24 March 24, 2014 14:04
Learn ANSYS ICEM CFD easy_astronaut ANSYS 2 December 15, 2013 16:34
[ICEM] Export unstructured periodic mesh from ICEM CFD to Fluent ivanddd ANSYS Meshing & Geometry 1 February 3, 2011 01:51
ICEM CFD in Workbench marek CFX 1 February 15, 2008 11:35
Where do we go from here? CFD in 2001 John C. Chien Main CFD Forum 36 January 24, 2001 22:10


All times are GMT -4. The time now is 04:24.