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

ICEM Internal wall structured mesh blocking

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 1, 2014, 14:28
Default ICEM Internal wall structured mesh blocking
  #1
New Member
 
diego
Join Date: Sep 2013
Posts: 14
Rep Power: 3
costy is on a distinguished road
I have a problem with ICEM CFD.
I have realized a structered mesh using blocking. Now how can I realize the internal wall?
I've posted an image of my mesh. There are two cubes. I want that the common face between the two cubes is interior. I've called that surface INTERNAL WALL.
When I run the mesh using Fluent, the following message appears: Cannot change int_internalwall to interior because
there is only one adjacent cell thread.

How can I resolve the problem?
Attached Images
File Type: jpg Cattura.JPG (43.6 KB, 31 views)
costy is offline   Reply With Quote

Old   March 1, 2014, 20:09
Default
  #2
Member
 
Tom-Robin Teschner
Join Date: Dec 2011
Location: Cranfield, UK
Posts: 64
Rep Power: 5
t.teschner is on a distinguished road
let me see if i get that one right, you are talking about the "outlet" of the smaller channel into the bigger one, right?

if so, then the first question would be, why you would put a wall there? do you want anything to flow from the smaller channel to the bigger channel? if so then i would just simply remove it.

if that is not what you are looking for and you want the wall to be there (and treat it as an interior), you will need to have two walls there, i.e. you would create a surface on both channels which then overlap, although i am not sure if fluent is "clever" enough to understand, that you have two faces of different size which are only connected through the smaller face of the small channel. in this case you might have to split the face of the bigger channel.

in fluent itself you would then need to specify that those two faces are actually interior walls, called interfaces in fluent. go to the boundary condition tab and specify both faces as "interface". then, just underneath the boundary condition tab there is something called "mesh interfaces". there you will have to click on create/edit to set up a new interface, you do that by selecting the interfaces in the two available lists. so for example, say you have created the two interfaces called "interface1" and "interface2" you will have to select interface1 in on of the lists and interface2 in the other one.
fluent knows now that those are interfaces and doesn't treat them as boundary conditions.
t.teschner is offline   Reply With Quote

Old   March 2, 2014, 05:37
Default
  #3
New Member
 
diego
Join Date: Sep 2013
Posts: 14
Rep Power: 3
costy is on a distinguished road
Thanks for your reply, you've been very kind.
I've tried to split the surface of the big channel and then I realized two interfaces. It seems to work.
But I wanted to put the boundary condition fan to the surface which linked the two channels.
I try to explain better, I' ve attacched the final mesh I should realize. Now the volume called pipe is linked to the one called air through two faces. One face should be interior, the other one should be fan.
How can I resolve the problem?
Attached Images
File Type: jpg Cattura.JPG (23.2 KB, 16 views)
costy is offline   Reply With Quote

Old   March 3, 2014, 13:45
Default
  #4
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,967
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
http://www.youtube.com/watch?v=Pe6DfdLUFZU

Large and small cylinder with inner wall
Far is online now   Reply With Quote

Old   March 3, 2014, 14:49
Default
  #5
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,967
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by costy View Post
Thanks for your reply, you've been very kind.
I've tried to split the surface of the big channel and then I realized two interfaces. It seems to work.
But I wanted to put the boundary condition fan to the surface which linked the two channels.
I try to explain better, I' ve attacched the final mesh I should realize. Now the volume called pipe is linked to the one called air through two faces. One face should be interior, the other one should be fan.
How can I resolve the problem?
Your question is not clear. you want internal wall or interior zone?
Far is online now   Reply With Quote

Old   March 4, 2014, 06:44
Default
  #6
New Member
 
diego
Join Date: Sep 2013
Posts: 14
Rep Power: 3
costy is on a distinguished road
Dear Sijal Ahmed Memon thanks a lot for you reply.
I have to realize two internal walls; One between the inlet side of pipe and air and the other one between the outlet side of pipe and air. In order that at the inlet side I can put the boundary condition fan, and at the outlet the boundary condition interior.
costy is offline   Reply With Quote

Old   March 4, 2014, 11:24
Default
  #7
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,967
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
if you want the wall inside the fluid domain, just follow the link given above.

Here you should put the clear question that what you want from ICEM, applying the wall or fan condition is the task to be done in fluent/cfx (i.e. in solver).
Far is online now   Reply With Quote

Old   March 5, 2014, 15:46
Default
  #8
New Member
 
diego
Join Date: Sep 2013
Posts: 14
Rep Power: 3
costy is on a distinguished road
thanks For Your help. I Know that the condition interior or fan must be put in fluent but when I run fluent it changed the surface in wall because there are two adiacent zones
costy is offline   Reply With Quote

Old   March 6, 2014, 10:18
Default
  #9
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,967
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by costy View Post
thanks For Your help. I Know that the condition interior or fan must be put in fluent but when I run fluent it changed the surface in wall because there are two adiacent zones
Can you show some pics with annotation that where you want wall and where you want interiour. Using the same material point will get you the interiour cells
Far is online now   Reply With Quote

Old   March 7, 2014, 06:55
Default
  #10
New Member
 
diego
Join Date: Sep 2013
Posts: 14
Rep Power: 3
costy is on a distinguished road
Thanks for your help.
In the blue area I want the condition fan. In the red area I want interior and in the Yellow area I want wall.
The problem is that when I run fluent the following message appears:
Error: Cannot change int_internalwall1 to interior because
there is only one adjacent cell thread.
Attached Images
File Type: jpg Cattura.JPG (23.4 KB, 11 views)
costy is offline   Reply With Quote

Old   March 7, 2014, 08:47
Default
  #11
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,967
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
There are two fluid domains: 1) pipe and 2)fluid ?

If two fluids are not there then you cannot use interiour boundary condition there because at boundary you have inlet, outlet or wall boundary. Why you want interiour boundary there? ?

Last edited by Far; March 7, 2014 at 10:37.
Far is online now   Reply With Quote

Old   March 7, 2014, 13:16
Default
  #12
New Member
 
diego
Join Date: Sep 2013
Posts: 14
Rep Power: 3
costy is on a distinguished road
I have two volumes pipe and tunnel. But the fluid is the same for both the volumes.
The pipe has to simulate a fan pushing air into the gallery. In a side I put the condition fan with a pressure jump and in the other one interior.
costy is offline   Reply With Quote

Old   March 8, 2014, 13:48
Default
  #13
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,967
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
If the fluid is same then do the following procedure:

1. For interior boundary dont do any anything. You only need do the some association if you need this boundary in fluent for some post processsing purpose.

2. associate fan to surface for the fan and wall boundaries.

3. Recompute pre mesh and convert to unstructured mesh.

4. Set the boundary conditions for fan and walls

5. output mesh and read in fluent
Far is online now   Reply With Quote

Old   March 11, 2014, 03:45
Default
  #14
New Member
 
diego
Join Date: Sep 2013
Posts: 14
Rep Power: 3
costy is on a distinguished road
Dear Sijal Ahmed Memon
Thank you very much for your help, I managed to solve the problem.
costy is offline   Reply With Quote

Reply

Tags
blocking, cfd, icem, internal wall, structured

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
how buliding structured hexahedral mesh of wire wrapped using ICEM huisenanhai ANSYS Meshing & Geometry 0 December 25, 2013 04:21
[ICEM] Icem blocking mesh S73f490 ANSYS Meshing & Geometry 6 April 24, 2013 05:42
[ICEM] ICEM CFD internal Wall by using structured Grid challenger85 ANSYS Meshing & Geometry 16 January 19, 2012 11:59
2d irregular grid Remy Main CFD Forum 1 December 22, 2008 05:49
Multicomponent fluid Andrea CFX 2 October 11, 2004 05:12


All times are GMT -4. The time now is 10:50.