CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Pointwise & Gridgen (http://www.cfd-online.com/Forums/pointwise/)
-   -   Connection B.C. Problem (http://www.cfd-online.com/Forums/pointwise/124446-connection-b-c-problem.html)

paraglider October 5, 2013 06:36

Connection B.C. Problem
 
2 Attachment(s)
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...

taxalian October 6, 2013 16:49

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.

cnsidero October 6, 2013 17:20

Quote:

Originally Posted by paraglider (Post 455184)
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

paraglider October 7, 2013 09:36

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...

taxalian October 7, 2013 10:27

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.

dgarlisch October 7, 2013 13:09

Quote:

Originally Posted by taxalian (Post 455511)
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 October 7, 2013 14:46

Hi David,
Thanks for your reply and useful hints.

paraglider October 8, 2013 10:12

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!


All times are GMT -4. The time now is 05:47.