CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Pointwise & Gridgen

Connection B.C. Problem

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

Like Tree5Likes
  • 1 Post By taxalian
  • 2 Post By cnsidero
  • 2 Post By dgarlisch

Reply
 
LinkBack Thread Tools Display Modes
Old   October 5, 2013, 06:36
Default Connection B.C. Problem
  #1
New Member
 
Join Date: Dec 2012
Posts: 6
Rep Power: 4
paraglider is on a distinguished road
Hi everyone

When I create 2 neighbour domain by meshes (in 2D), I everytime have a problem while loading it to FLUENT. It says "No face with given nodes". I searched and found it's about the "connection" in Boundary condition.

If you look at the picture in the attachment named "pic-1" you will see there is 2 mesh domain and a connection between them. I think this connection makes the problem.

Even if I made Pointwise 2D T-Rex mesging "Tutorial", I can load it to FLUENT but I can't even initialize it. It doesn't moves. There is a connector too. (as seen in the attachment "Mesh-2"). Pointwise or Fluent can not connect theese meshes.

What should I do with theese connections?

Thank you...
Attached Images
File Type: jpg Mesh-1.JPG (61.9 KB, 15 views)
File Type: jpg Mesh-2.jpg (73.7 KB, 21 views)
paraglider is offline   Reply With Quote

Old   October 6, 2013, 16:49
Default
  #2
Senior Member
 
Join Date: Nov 2010
Posts: 128
Rep Power: 6
taxalian is on a distinguished road
Hi,
I tried the similar tutorial as you mentioned, it didn't work in 2D. But if you choose the 3D mode and use a kine of 2D grid with one cell thickness for your finite volume in third dimension then it works fine with Fluent.
In Gridgen , the 2D meshes export for Fluent works by using the block command for both the structured and unstructured meshes i.e making separate block for different mesh shapes. Don't forget to have the similar orientation for structured meshes if you have more than one block.
If you have Gridgen then you should not get such problem as faced now in Pointwise. It seems to be a bug or we don't know the right option.
paraglider likes this.
taxalian is offline   Reply With Quote

Old   October 6, 2013, 17:20
Default
  #3
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 369
Rep Power: 12
cnsidero is on a distinguished road
Quote:
Originally Posted by paraglider View Post
Hi everyone

When I create 2 neighbour domain by meshes (in 2D), I everytime have a problem while loading it to FLUENT. It says "No face with given nodes". I searched and found it's about the "connection" in Boundary condition.

If you look at the picture in the attachment named "pic-1" you will see there is 2 mesh domain and a connection between them. I think this connection makes the problem.

Even if I made Pointwise 2D T-Rex mesging "Tutorial", I can load it to FLUENT but I can't even initialize it. It doesn't moves. There is a connector too. (as seen in the attachment "Mesh-2"). Pointwise or Fluent can not connect theese meshes.

What should I do with theese connections?

Thank you...
2 things you should check:

- domain orientations need to point in the +z direction
- domains in a single volume condition

-Chris
taxalian and paraglider like this.
cnsidero is offline   Reply With Quote

Old   October 7, 2013, 09:36
Default
  #4
New Member
 
Join Date: Dec 2012
Posts: 6
Rep Power: 4
paraglider is on a distinguished road
Thank you all. I made the tutorial again. In "assemble domain", I selected nodes "counterclockwise" (not in clockwise as tutorial says for CGNS solver), then it's oriantation gets in +z direction. And fluent solved it.

I have one more question. I can join 2 neighbour unstructured domain. Is it what you said "domains in a single volume condition" Chris? What can I do with structured and unstructured neighbour domains?
I can't make them complete 1 domain.

Thank You...
paraglider is offline   Reply With Quote

Old   October 7, 2013, 10:27
Default
  #5
Senior Member
 
Join Date: Nov 2010
Posts: 128
Rep Power: 6
taxalian is on a distinguished road
Hi Chris,
thanks a lot for this useful tip and i assume by single volume condition you mean single fluid volume boundary condition consists of several domains.
taxalian is offline   Reply With Quote

Old   October 7, 2013, 13:09
Default
  #6
Member
 
David Garlisch
Join Date: Jan 2013
Location: Pointwise HQ
Posts: 83
Rep Power: 4
dgarlisch is on a distinguished road
Quote:
Originally Posted by taxalian View Post
Hi Chris,
thanks a lot for this useful tip and i assume by single volume condition you mean single fluid volume boundary condition consists of several domains.
I believe Chris' answer would be yes.

In 2D grids, the Pointwise domains entities are the "volumes".

You can assign Volume conditions to the domains using the CAE/Set Volume Conditions... menu.

Fluent does NOT like connected volumes with differing VCs. It will make interesting changes to the grid conditions during import if it detects this.

So, you have at least three options:
  1. Leave all VCs set to Unspecified (the default for all newly created 2D domains).
  2. Create a single VC (of any type) and assign it to all 2D domain volumes.
  3. Use different VCs and deal with the changes made by Fluent during import.
taxalian and paraglider like this.
dgarlisch is offline   Reply With Quote

Old   October 7, 2013, 14:46
Default
  #7
Senior Member
 
Join Date: Nov 2010
Posts: 128
Rep Power: 6
taxalian is on a distinguished road
Hi David,
Thanks for your reply and useful hints.
taxalian is offline   Reply With Quote

Old   October 8, 2013, 10:12
Default
  #8
New Member
 
Join Date: Dec 2012
Posts: 6
Rep Power: 4
paraglider is on a distinguished road
Thank you very much taxalian, cnsidero and dgarlisch!

I corrected meshes orientation, than I connected all the mesh volumes in new VC. fluid so the problem solved!
paraglider is offline   Reply With Quote

Reply

Tags
connections, fluent 2d, pointwise

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
Paraview 3.98 - errors when saving geometry file pajot OpenFOAM Paraview & paraFoam 1 September 28, 2013 10:45
Radial Turbine Analysis B.C Problem yjs1027 FLUENT 0 April 18, 2013 03:06
Interior B.C. Problem Samaneh Zeighami FLUENT 6 September 8, 2012 05:06
Handling cyclic BC from gambit to openfoam for a cascade airfoil problem - OF 1.6 maverick OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 June 18, 2011 04:36
problem in giving b.c kiran FLUENT 0 August 10, 2004 04:21


All times are GMT -4. The time now is 04:43.