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

[ANSYS Meshing] About O-grid mesh for coil spring

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

Like Tree1Likes
  • 1 Post By Vidyanand Kesti

Reply
 
LinkBack Thread Tools Display Modes
Old   September 23, 2013, 05:00
Default About O-grid mesh for coil spring
  #1
C_O
New Member
 
Join Date: Sep 2013
Posts: 5
Rep Power: 3
C_O is on a distinguished road
Hello friends;

This is my first thread on this forum. Hi to yours all.

I am working at the automobile industry for design engineer. And working for AnSys analysis generally.

Nowadays, I am working different types of meshing operations. I am trying to reach o-grid type of mesh on the cylindrcal profile. But this is not the linear profile, it is circular, like coil spring (automobile front or rear spring)

Could you give me some help about this process?

All your thinkings will appreciate.

Best regards.
Attached Images
File Type: jpg o-grid.jpg (103.4 KB, 41 views)
C_O is offline   Reply With Quote

Old   September 24, 2013, 11:02
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: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
If you use the Ogrid tool (in ICEM CFD Hexa) or use Multizone with inflation in ANSYS Meshing (same underling ICEM CFD hexa Ogrid code), it will handle it for you.

In interactive blocking, you just block out the tube with a rectangular block wrapped from end to end... Add splits along the way and fit the rectangular cross section to the model... Then add an OGrid. Select all the blocks, add faces to the ends and hit apply... It will take care of the rest.

If you are using multizone, it does the blocking for you. You just need to set the method for that body as "Multizone" and put a named selection on the side of the spring (not the ends) so you can apply inflation. Then hit generate mesh. If the surface structure is not condusive to Multizone, you may be more successful by "splitting" the spring a number of times across its length... Either at the surface only or the bodies (but make it a single multibody part).
__________________
-----------------------------------------
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   September 24, 2013, 11:03
Default
  #3
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
If your spring has many turns, it may be good to use a sub model... Just block a single turn and then use blocking topology options to copy it up the rest of the way.
__________________
-----------------------------------------
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   September 25, 2013, 01:29
Default
  #4
Member
 
vidyanand
Join Date: Nov 2011
Location: bangalore,india
Posts: 66
Rep Power: 8
Vidyanand Kesti is on a distinguished road
If you are meshing ANSYS mesher best you can slice the model at each turn and at the end of the face you can slice the model to get the o-Grid,but its time consuming and its depend upon the number of turns
PSYMN likes this.
Vidyanand Kesti is offline   Reply With Quote

Old   September 26, 2013, 06:17
Default
  #5
C_O
New Member
 
Join Date: Sep 2013
Posts: 5
Rep Power: 3
C_O is on a distinguished road
Thank you friends. I think, I will handle it with your opinios. I will back to you after my works on it.

Thanx again.
C_O is offline   Reply With Quote

Old   September 27, 2013, 01:53
Default
  #6
C_O
New Member
 
Join Date: Sep 2013
Posts: 5
Rep Power: 3
C_O is on a distinguished road
Hello friends, I hope you are doing fantastic.

I am working on my model for meshing with o-grid type. Actually I made some steps.

You can follow the attachments like 1 and 2.

3 is my full-model.

I think I have done it about %70.. But problem is not sweeping mesh with all bodies. For example, you can see in 1.jpg, all plane meshs are same. but in the other parts of model are not. you can see in 2.jpg. Right side different, left side different.

I sliced my model as you suggest. you can follow it on 3.jpg and applied all parts multizone by one by. of course with named selection.

Could you help me for this problem...

Thank you by now.
Attached Images
File Type: jpg 1.JPG (59.2 KB, 35 views)
File Type: jpg 2.JPG (54.1 KB, 34 views)
File Type: jpg 3.JPG (61.0 KB, 36 views)
C_O is offline   Reply With Quote

Old   October 11, 2013, 01:42
Default
  #7
C_O
New Member
 
Join Date: Sep 2013
Posts: 5
Rep Power: 3
C_O is on a distinguished road
There is no opinion for this? I really need your suggestions..

Thank you very much and have nice day.
C_O is offline   Reply With Quote

Old   October 11, 2013, 02:21
Default
  #8
Senior Member
 
Josef Runsten
Join Date: Jul 2010
Location: Gothenburg, Sweden
Posts: 185
Rep Power: 14
jrunsten will become famous soon enough
Send a message via MSN to jrunsten
Did you use "Multizone" as your mesh method in Ansys meshing? Or just Sweep?

On the other hand.. Have you created a single Part from your bodies in DesignModeler?
jrunsten is offline   Reply With Quote

Old   October 11, 2013, 09:04
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: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Quote:
Originally Posted by jrunsten View Post
Have you created a single Part from your bodies in DesignModeler?
Yea, I think the issue is that you have separate parts instead of a multi-body part.

You should select all your parts in DM and right click to form a new part... The mesher will then know to give you a conformal mesh on the multi-body part.
__________________
-----------------------------------------
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
Star CCM Overset Mesh Error (Rotating Turbine) thezack CD-adapco 3 December 11, 2013 04:09
Spring deformation return a torsional mesh momo_sjx SU2 6 May 28, 2013 12:03
[ICEM] Unstructure Meshing Around Imported Plot3D Structured Mesh ICEM kawamatt2 ANSYS Meshing & Geometry 17 December 20, 2011 12:45
2d irregular grid Remy Main CFD Forum 1 December 22, 2008 05:49
Gambit problems Althea FLUENT 21 February 6, 2001 08:05


All times are GMT -4. The time now is 18:11.