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

[ICEM] Extruded unstructured mesh association with boundaries, volumes, etc.

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 6, 2012, 15:39
Default Extruded unstructured mesh association with boundaries, volumes, etc.
  #1
Senior Member
 
François Grégoire
Join Date: Jan 2010
Location: Laval University, Canada
Posts: 366
Rep Power: 8
macfly is on a distinguished road
Hi all,

I'm just trying to extrude a 2D mesh of a duct with walls and a baffle and export the resulting the 3D mesh to fluent with appropriate bocos and volume definitions. In 2D, the inlet is a distinct curve, same for the outlet. The fluid and solid surfaces are in seperate parts, etc.

Without blocking:
It works well without blocking (right bocos and volume definitions), I manage to get everything right in 3D by playing with 'New volume/side/part name' of the Extrude mesh panel. The thing is that I'm not satisfied with the quad mesh that was generated in 2D by Icem.

With blocking:
When I use blocking, my problem is that when I extrude the mesh (after convert to unstruct mesh), the bocos are not respected as with the automatic meshing without blocking, all the elements are in the same part where I've put my blocks. How can I assign the right elements to inlet, outlet, fluid, solid after the 'Convert to unstruct mesh'? Is there a kind of 'Build topology' to assign the unstructured elements to the right parts?

Or, is there better way of extruding a 2D blocked mesh than converting it to unstructured mesh? I need to extrude my mesh with a growth ratio.

Many thanks in advance if you have some tips for me. Here are some pics describing my problem.
Attached Images
File Type: jpg 1.jpg (40.5 KB, 66 views)
File Type: jpg 2.jpg (66.3 KB, 49 views)
File Type: jpg 3.jpg (59.6 KB, 42 views)
File Type: jpg 4.jpg (89.3 KB, 52 views)

Last edited by macfly; August 6, 2012 at 21:32.
macfly is offline   Reply With Quote

Old   August 6, 2012, 16:04
Default
  #2
Member
 
Touré
Join Date: Aug 2010
Location: Montréal
Posts: 85
Rep Power: 6
Touré is on a distinguished road
I have the same kind of post and no answer. Why don't you just do the blocking in 3D ?
Touré is offline   Reply With Quote

Old   August 6, 2012, 16:12
Default
  #3
Senior Member
 
François Grégoire
Join Date: Jan 2010
Location: Laval University, Canada
Posts: 366
Rep Power: 8
macfly is on a distinguished road
Because in fact my duct is much more complex than that, with dozens of baffles and 90 degree turns. Just extruding a 2D blocking with a growth ratio is much more simple than having to play with dozens of 3D blocks (really mind-boggling, a maze for the eyes), associate many dozens of surface and having to apply edge parameters to hundreds of edges.

Last edited by macfly; August 6, 2012 at 21:54.
macfly is offline   Reply With Quote

Old   August 6, 2012, 23:34
Default
  #4
New Member
 
clocter
Join Date: Jan 2012
Posts: 7
Rep Power: 5
clocter is on a distinguished road
Make sure before you extrude, the points and lines are selected/ticked in the mesh section. So when you extrude the bocos comes through in the 3D mesh.

Cheers
clocter is offline   Reply With Quote

Old   August 7, 2012, 09:20
Default
  #5
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
That should work (works for me).

The most common mistake people make is to forget to associate edges to curves (no association means no line elements formed in the parts of the curves), but it looks like you have associated all your edges.

First check to make sure that your 2D model has everything in the right part names.

If that does, then I can only assume that you are not extruding correctly. Make sure the sides are "inherited" so the new shell elements will get their names from the line elements that are extruded.

You can also extrude the geometry (curves become surfaces of the same part) and then you could use "Edit Mesh => Repair Mesh => Associate Mesh" to associate elements with the geometry parts they are sitting 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

Old   August 7, 2012, 09:22
Default
  #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
One other thought... If it is really just an extruded duct, you may want to use a 2D mesh. Unless your flow is entering the duct at some angle to the plane...

The 2D mesh will solve more quickly and can accurately simulate an extruded 2D mesh if the boundary conditions are in the plane...
__________________
-----------------------------------------
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   August 7, 2012, 16:13
Default
  #7
Senior Member
 
François Grégoire
Join Date: Jan 2010
Location: Laval University, Canada
Posts: 366
Rep Power: 8
macfly is on a distinguished road
Nice, everything works now. You were right, my edge to curve associations were not well configured. I started over and did the edge to curve associations one edge at a time, instead of multiple selections at one time, then the 'convert to unstruct mesh' was perfect with the right line elements on the right parts.

Another twist that I had not performed the 1st time : I created 2 parts containing 'fluid' blocks and 'solid' blocks, this way when I extrude with New volume part name set to inherited, I get a fluid zone and a solid zone in Fluent.

The twist that I discovered in order to create geometry or block parts is that when you right click on Parts to Create Part, the Select bar is different depending if you are in the Geometry tab or in the Edit Mesh tab, you get a Select Geometry bar or a Select mesh elements bar respectively. I know it's logical, but you have to know it... probably written in the user's guide somewhere but not instinctive.

Psymn, I'm modeling turbulent combustion and there will be heat transfer towards the rear wall (the extruded wall), it's symmetric but I need 3D: I extrude up to the symmetry plane of the duct. There are solids adjacent to the duct (behind the rear wall) that are baking. I hope I'm clear... just for your information. The mesh in my 1st post is useless, it's just a simple case to make sure that I can perform all the meshing operations that I need for my ultimate geometry/mesh.

Thanks guys, it was very nice to just know that it's feasible and that I was not wasting my time.

François
macfly 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
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
Mesh motion with Translation & Rotation Doginal CFX 2 January 12, 2014 07:21
Gambit problems Althea FLUENT 21 February 6, 2001 08:05
Mesh Mignard FLUENT 2 March 22, 2000 06:12
unstructured vs. structured grids Frank Muldoon Main CFD Forum 1 January 5, 1999 11:09


All times are GMT -4. The time now is 23:46.