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

[ICEM] Delete wall between two regions

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

Like Tree1Likes
  • 1 Post By PSYMN

Reply
 
LinkBack Thread Tools Display Modes
Old   September 21, 2013, 19:35
Unhappy Delete wall between two regions
  #1
New Member
 
Carlo
Join Date: Apr 2013
Posts: 10
Rep Power: 4
cscalo is on a distinguished road
Hello ICEM crowd,

I need to create a hexa mesh with two different adjacent regions, say FLUID0 and FLUID1. I can do this easily by creating a "Part" for each region. ICEM CFD thinks that these two parts are two different materials. This wouldn't be a problem if only ICEM didn't create a wall in between them.

I read on this forum that is possible to setup the hexa mesh (in Global Mesh Parameters.. or something like that) so that it doesn't do this. I'm not sure how to do this.

I basically need one mesh with regions of it that have different labels ("FLUID0" and "FLUID1"). I need these labels in my solver in these specific regions to activate certain functionalities.

I would appreciate your help on this! Thanks!
cscalo is offline   Reply With Quote

Old   September 22, 2013, 21:24
Default
  #2
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
keep that wall and make it "interior" when setting the boundary condition in the output tab
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   September 22, 2013, 22:13
Default
  #3
New Member
 
Carlo
Join Date: Apr 2013
Posts: 10
Rep Power: 4
cscalo is on a distinguished road
Hi Diamondx - thanks for your reply. Unfortunately it didn't work. My solver tells me that some faces "are not associated" with the internal wall. Is there something deeper and non-Fluent dependent that I can do? Something in Global Mesh Setup for example? I simply want to leave the labels to the volume with no physical surface dividing them.

Thanks!
cscalo is offline   Reply With Quote

Old   September 22, 2013, 23:29
Default
  #4
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,910
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by cscalo View Post
Hello ICEM crowd,

I need to create a hexa mesh with two different adjacent regions, say FLUID0 and FLUID1. I can do this easily by creating a "Part" for each region. ICEM CFD thinks that these two parts are two different materials. This wouldn't be a problem if only ICEM didn't create a wall in between them.

I read on this forum that is possible to setup the hexa mesh (in Global Mesh Parameters.. or something like that) so that it doesn't do this. I'm not sure how to do this.

I basically need one mesh with regions of it that have different labels ("FLUID0" and "FLUID1"). I need these labels in my solver in these specific regions to activate certain functionalities.

I would appreciate your help on this! Thanks!
HEXA or TETRA ?
Far is offline   Reply With Quote

Old   September 22, 2013, 23:33
Default
  #5
New Member
 
Carlo
Join Date: Apr 2013
Posts: 10
Rep Power: 4
cscalo is on a distinguished road
Hi Far - My mesh is purely HEXA... I think it was you (in some post I read) who said that you can do this at the Global Mesh Setup level.. thanks for your help.
cscalo is offline   Reply With Quote

Old   September 23, 2013, 01:22
Default
  #6
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,910
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Are you associating face to part for the interface?
Far is offline   Reply With Quote

Old   September 23, 2013, 01:34
Default
  #7
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,910
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by diamondx View Post
keep that wall and make it "interior" when setting the boundary condition in the output tab
Yes exactly. Still you will see the boundary condition (interface or whatever name you choose) in fluent (as int_interface) but now it interiour. Means it will pass the flow as usual.
Far is offline   Reply With Quote

Old   September 23, 2013, 01:37
Default
  #8
New Member
 
Carlo
Join Date: Apr 2013
Posts: 10
Rep Power: 4
cscalo is on a distinguished road
yes.. I create a surface in between the two regions and that surface is added to a "PART" called, say, SHARED_WALL. This (surface) part is a boundary in between the two regions which have different labels (or part names). I would like this boundary to disappear before my mesh gets to the solver. If I define it as an internal face I feel like that would work for Fluent but for an in-house solver I think I need that wall to be removed before (at the connectivity level).

I will retry as you say -- labeling that surface as an "internal_surface" -- and see if I can have my solver accept it if that's the only way I can do such a thing with ICEM.

Thanks!
cscalo is offline   Reply With Quote

Old   September 23, 2013, 01:49
Default
  #9
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,910
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
I am not sure about the in-house solver. For this, Simon is the most appropriate person to answer or you can contact ANSYS support.
Far is offline   Reply With Quote

Old   September 23, 2013, 14:36
Default
  #10
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
Yes, of course there is an automatic way to turn that off that doesn't require creating any geometry, etc... The fact that ICEM CFD Hexa defaults to project a face between two materials to the nearest surface is meant as a convenience, not to cause trouble. ;^)

If you have two blocking materials, say FLUID1 and FLUID2, and you don't want to have default face to surface projection between blocks of these two materials (usually because you want these in different materials for selection or other "non-physics" reasons);
  • Blocking tab>Blocking Associations>Associate Face to Surface...
  • You will find a bunch of methods in there. One of them is "Shared Wall".
  • Switch the radio button to "Shared Wall" and Select all the volume parts that you wish to allow adjacent without surface projection between. The command is iterative, so cancel (or accept without selecting) after the ones you want disappear from the options.
  • Switch the Radio Button for "Shared surface elements" to "None", so that no surface projection will be the default between these materials.
  • Apply

Let us know if that is what you were looking for... Of course, this just changes the default. If you want to associate a face between these blocks to a surface, you can always do that manually.
manymen likes this.
__________________
-----------------------------------------
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
Enhanced Wall Treatment paduchev FLUENT 18 April 11, 2014 07:37
Radiation interface hinca CFX 15 January 26, 2014 18:11
Conjugate Heat Transfer: Wall Heat Flux at Coupled Walls? MaxHeat FLUENT 3 April 21, 2013 18:22
Wall functions? Pr Main CFD Forum 7 April 8, 2004 06:15
Quick Question - Wall Function D.Tandra Main CFD Forum 2 March 16, 2004 05:29


All times are GMT -4. The time now is 18:30.