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

[ICEM] Just started unstructured mesh !

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

Like Tree6Likes
  • 1 Post By diamondx
  • 1 Post By Far
  • 1 Post By diamondx
  • 3 Post By BrolY

Reply
 
LinkBack Thread Tools Display Modes
Old   August 28, 2012, 18:18
Default Just started unstructured mesh !
  #1
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,291
Blog Entries: 23
Rep Power: 20
diamondx will become famous soon enough
hello everyone,
Until now, i never tried an unstructured mesh, i got my feet wet today and it's giving me hard time !!! i'm trying to understand the logic behind it. I will try to explain my problem using a very simple geomtry as below, it's a heat exchanger.



So I created two materials, Hot_fluid and cold_fluid. After doing the training material and reading a lot in the forum. i found that there is a lot of method to mesh this some start by creating a surface mesh, then they use a quick (delauney) to fill the volume mesh ? is it the best way possible ? Why not generating a volume mesh directly ?

How to deal with the heat exchanger below ? i tried a volume mesh, checked hot_fluid as visible, then i succeeded in creating element inside the hot fluid ONLY. But how do i mesh the cold fluid now ? when i hide everything and i keep only the cold_fluid, it doesn't work. when i try the "by part" option and i only select "COLD_FLUID", it's telling "no parts containing surface found"



So my question:
- Using surface mesh, then volume mesh i noticed that i could only use it with delaunay otherwise i have to replace or merge, am i right ?
- that what we call the flood fill option ? is it a trick to get a better quality like adding an (o-grid) ?
- Can we mesh the Hot_fluid and Cold_fluid separatly ? if yes , do we have to merge then ?
- if i do i surface mesh on hot_fluid, then a volume mesh for the hot fluid, the volume mesh for the cold_fluid had to be conformal (sharing same element) with the surface of the hot fluid ? will this be automatically ?
- if i set a very refine and small size elements for a surface , and i take a curve belonging to that surface, set the parameter to coarse element, Which one ICEM will follow ?

I know it's too much question ! sorry about that. Thanks a lot in advance.
Far likes this.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   August 29, 2012, 06:27
Default
  #2
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,916
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
good thread.
BrolY likes this.
Far is offline   Reply With Quote

Old   August 29, 2012, 09:09
Default
  #3
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,291
Blog Entries: 23
Rep Power: 20
diamondx will become famous soon enough
thank you for the word of support
BrolY likes this.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   September 3, 2012, 04:16
Default
  #4
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
1) You have two ways of meshing : do only volume mesh, or do surface mesh then volume mesh. It won't change anything about your mesh at the end.

It's faster to do only volume mesh. The delauney volume mesh is better than the octree mesh. But, for surface meshing, if the quality of your geometry is not very good, the surface mesh generated by the octree method (known as patch independent method in the surface mesh option) would work better.
It's better to use the patch dependent method for surface meshing, but patch independent method works in more cases.
But if the quality of your geometry is good, you can create patch dependent surface mesh, then delauney volume mesh. It's up to you !

2) About your geometry, you need to specify the interface surface as internal part (in the part mesh setup). Because it's a 2D surface between two volume. So if you don't specify it as internal part, ICEM would think it's useless.

3) If you specify the min element size on a surface, and then change the number of nodes on the curve belonging to this surface, it's the curve which "wins".

4) I don't understand why you want to create two separate meshes for each fluid, but a way could be to create two separate projects with only one material point for each other. if you want to merge then, keep the exact same element size everywhere on the interface, and that should work.

I hope my explanations are clear, don't hesitate to ask more information
Far, stuart23 and diamondx like this.
BrolY is offline   Reply With Quote

Old   September 4, 2012, 12:27
Default
  #5
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,291
Blog Entries: 23
Rep Power: 20
diamondx will become famous soon enough
Thanks a lot Broly, that did help me to understand. one more...
Quote:
I don't understand why you want to create two separate meshes for each fluid
what if i wanna use a structured mesh inside the cylinder, and tetra outside. What will happens to the wall of the cylinder. what comes to my mind is making those wall interface in ICEM, then i will merge the two meshes. and in fluent when using the conformal mesh, i will select them as "coupled wall". will you do that to ?
Can i still select thickness and material of the coupled wall in Fluent ?

Thanks a lot for the answers
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   September 5, 2012, 05:18
Default
  #6
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
I know you can create a conformal interface between a tetra and an hexa mesh, but I don't know how. I've already seen some thread about it on this forum. Maybe with an "unstructured" structured mesh (aka not with blocking but automatic hexa mesh).
BrolY is offline   Reply With Quote

Old   September 5, 2012, 07:15
Default
  #7
Senior Member
 
Stuart Buckingham
Join Date: May 2010
Location: United Kingdom
Posts: 267
Rep Power: 16
stuart23 will become famous soon enough
If your interface has a surface mesh on it (ie from converting structured mesh to unstructured, or volume meshing one domain, or just by creating standalone surface mesh) you can fill the adjacent volume with mesh that is conformal to this surface mesh. The bottom up algorithms (Delauney, AF, TGrid) will all use this surface mesh to generate a conformal volume mesh. The top down algorithm (Octree) will first create its own mesh and then realign the surface mesh to the existing mesh. In my experience, the Octree mesh takes lots of smoothing to make it nice after it has made itself conformal. Octree also should not be your first preference algorithm unless you have dirty CAD.

I have never used surface quads to build a tet mesh. I'm not sure whether or not it will make pyramids at the interface, can someone else maybe clear this up?

Also, make sure you have put two separate material points in your two separate volumes. These "parts" will contain the mesh elements once created.


Good Luck

Stu
__________________
http://bc247.wordpress.com
stuart23 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
[ICEM] Generating Mesh for STL Car in Windtunnel Simulation tommymoose ANSYS Meshing & Geometry 48 April 15, 2013 04:24
2D unstructured mesh majidhojjat OpenFOAM Meshing & Mesh Conversion 1 May 14, 2009 17:09
Structured and Unstructured mesh Jingwei FLUENT 0 March 2, 2009 22:29
Unstructured hex mesh lr103476 OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 12 November 24, 2006 06:56
2D Modelling using unstructured mesh Yingchun CFX 8 December 12, 2005 07:05


All times are GMT -4. The time now is 00:22.