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

[ICEM] material point found problem

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

Like Tree1Likes
  • 1 Post By Jeremie84

Reply
 
LinkBack Thread Tools Display Modes
Old   October 19, 2011, 03:42
Default material point found problem
  #1
New Member
 
Neal
Join Date: Oct 2011
Posts: 2
Rep Power: 0
mobiuss is on a distinguished road
Hello,
I have a problem in delaunay volume mesh.
I defined 2 material point, fluid1 and fluid2 and I successed the octree mesh,
but I found the below message at delaunay volume mesh and fail to flood fill in fluid2.
"element containing material point fluid2.1 was not found"
I used default option in volume meshing parameters and coumpute mesh(inherited volume part name) option.

Can you give me a help to solve this problem? I would like to finish delaunay volume mesh in fluid1 and fluid2.

Thnaks in Advance,
Neal
Attached Images
File Type: jpg octree.jpg (83.5 KB, 76 views)
File Type: jpg delaunay_error.jpg (86.6 KB, 67 views)

Last edited by mobiuss; October 19, 2011 at 06:29.
mobiuss is offline   Reply With Quote

Old   October 20, 2011, 04:35
Default
  #2
Member
 
Join Date: Apr 2009
Location: Pune
Posts: 37
Rep Power: 7
Sushilkumar is on a distinguished road
I tried the same case. Two concentric spheres of different diameters. you get octree mesh but when try to mesh with delaunay the second material point is not found.

I can suggest you to generate and export these two meshes separately and import into solver. I hope this workaround could help you.
Sushilkumar is offline   Reply With Quote

Old   October 20, 2011, 04:48
Default
  #3
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
With the Delaunay mesh option, you have to choose which material point you want to mesh.
I have never meshed two separated volumes with the Delaunay method, but maybe you could try to mesh your 1st volume, and then mesh the 2nd volume ?
BrolY is offline   Reply With Quote

Old   October 21, 2011, 10:13
Default Mesh Internal Domains
  #4
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,651
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
No, it is just a simple setting...

Under the Mesh tab => Global mesh Setup => Volume Meshing Parameters => Tetra/Mixed => Quick (Delaunay) you will find an option for "mesh internal domains".

Turn that on and it will mesh volumes that do not touch the outer surface.

When it meshes your internal region, you will have an element where your material point is and it will all be fine...

Actually, while you are in there, you can turn on the option for "Flood fill after completion" and it will check for the material points automatically.

Have fun.
__________________
-----------------------------------------
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   October 23, 2011, 22:59
Default Mesh Internal Domains
  #5
New Member
 
Neal
Join Date: Oct 2011
Posts: 2
Rep Power: 0
mobiuss is on a distinguished road
Hi, thank you your reply.

I turned on the "mesh internal domains", but this option meshed every internal domains. So the inside of propeller was also meshed.
Is it possible to delete only inside of propeller after delaunay mesh?


And I also turned on the "Flood fill after completion" option,
but it was same not to find the 2nd material point automatically.

Could you explain what I missed something?
mobiuss is offline   Reply With Quote

Old   October 24, 2011, 00:50
Default
  #6
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,651
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
The mesh in the propeller is in one of the parts (maybe "CREATED_MATERIAL_#").

Find out which one it is, right click on the part in the tree and delete. Hit "Yes" to confirm the delete. Another option would be to create a material called "ORFN" and put it inside the propeller. I think Flood fill will delete elements in the ORFN part.

I am not sure that I understood your second comment. Are you saying it didn't run flood-fill? I think there was a bug about that a number of versions ago. You can go into "Edit Mesh => Repair" and run the flood fill option manually.


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   April 16, 2012, 13:16
Default
  #7
New Member
 
Vincenzo
Join Date: Apr 2012
Posts: 1
Rep Power: 0
vincyc is on a distinguished road
HI PSYMN, to me seems that this option doesn't work at all. I tried many times but nothing. I will attach an image.
As probably you can see the volume mesh is applied only to the surface attache to the outer one. I started with a surface mesh and then applied a volume one trough Quick (Delaunay). Do you have any suggestion?

Quote:
Originally Posted by PSYMN View Post
No, it is just a simple setting...

Under the Mesh tab => Global mesh Setup => Volume Meshing Parameters => Tetra/Mixed => Quick (Delaunay) you will find an option for "mesh internal domains".

Turn that on and it will mesh volumes that do not touch the outer surface.

When it meshes your internal region, you will have an element where your material point is and it will all be fine...

Actually, while you are in there, you can turn on the option for "Flood fill after completion" and it will check for the material points automatically.

Have fun.
Attached Images
File Type: jpg Internal mesh.jpg (97.0 KB, 45 views)
vincyc is offline   Reply With Quote

Old   April 17, 2012, 10:16
Default
  #8
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,651
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
I know it has worked for others... Turn on both the Mesh internal volumes and the Flood fill option and it should work.

If not, and you are willing to share the model privately, I can test it for you.

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   November 27, 2012, 17:52
Default
  #9
Member
 
Join Date: Mar 2011
Location: Canada
Posts: 35
Rep Power: 5
Jeremie84 is on a distinguished road
Hi,

I am facing the same problem. I am using ICEM CFD 12.1 for meshing a VAWT. I have 2 material points (one for the rotor region, one for the stator region). I first generate an octree mesh, then delete the volume mesh, and then generate the volume mesh with the Delaunay mesher (TGlib, Use AF). I check "Mesh internal domains" and "Flood fill after completion". But I keep having the same message :
element containing material point ROTATION.1 was not found

Only the external region is meshed, but the internal region (ROTATION) is not meshed.
Am I missing something ? With the octree method, the 2 domains are meshed...

Thank you very much

Jeremie
Jeremie84 is offline   Reply With Quote

Old   November 28, 2012, 10:34
Default
  #10
Member
 
Join Date: Mar 2011
Location: Canada
Posts: 35
Rep Power: 5
Jeremie84 is on a distinguished road
I have attached some screen captures of the Global Mesh Setup, and the messages I get during the Delaunay meshing.
As I said, the 2 domains are meshed with the Octree method, but when I try to mesh with the Delaunay method, based on the surface mesh obtained with Octree, I keep having this problem...

Thank you

Jeremie
Attached Images
File Type: jpg Global Mesh Setup.jpg (58.6 KB, 22 views)
File Type: jpg material not found.jpg (68.7 KB, 19 views)
Jeremie84 is offline   Reply With Quote

Old   June 27, 2013, 06:08
Default
  #11
Member
 
Tarantino
Join Date: Feb 2013
Posts: 34
Rep Power: 3
Tarantino is on a distinguished road
Hello

I have the same issue.
I want to generate a multi-zone mesh. I creat material point, and I turned on the "mesh internal domains" and "Flood fill after completion". the mesh generated for all the volumes, but only on one material. I can not have them in different materials which I define already.
Can anyone assist me?
thanks.
Tarantino is offline   Reply With Quote

Old   June 27, 2013, 15:22
Default
  #12
Member
 
Join Date: Mar 2011
Location: Canada
Posts: 35
Rep Power: 5
Jeremie84 is on a distinguished road
Hello Tarantino,
I had the same problem. Here is the answer from the ANSYS support I got:

"Hi Jérémie,
I tried your case and found that ICEM12.1 doesn't work and ICEM 13 and ICEM 14 work.Please update your ICEM. "

I tried the same case with ANSYS 14.5, and it worked. So, it seems to be a bug of the 12.1 release. That's all I can say.

Regards,

Jeremie
Tarantino likes this.
Jeremie84 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
OpenFOAM 1.7.1 installation problem on OpenSUSE 11.3 flakid OpenFOAM Installation 16 December 28, 2010 09:48
OF 1.7 installation problem "command not found error" maysmech OpenFOAM Installation 23 December 11, 2010 08:07
OpenFOAM15 paraFoam bug koen OpenFOAM Bugs 19 June 30, 2009 11:46
two material propoery for Heat exchange problem. JUN CFX 2 January 12, 2009 20:37
OpenFOAM15 installables are incomplete problem with paraFoam tryingof OpenFOAM Bugs 17 December 7, 2008 05:41


All times are GMT -4. The time now is 01:15.