CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > STAR-CCM+

Error at Volume Meshing (Interface problem)

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 20, 2009, 07:34
Default Error at Volume Meshing (Interface problem)
  #1
New Member
 
Francesco
Join Date: Nov 2009
Posts: 9
Rep Power: 7
Trofrensis is on a distinguished road
Hi people!

I'm tring to generate volume mesh in my pipe model , the surface mesh it's ok , but when I start the volume ones , volume meshing end with this error:

Error: Invalid connectivity in Regions Fluid and Solid
{Command=GenerateVolumeMesh, command=CommandComplete, Processor=0, In=[Machine::main, VolumeMeshingModel::execute], CompletedCommand=GenerateVolumeMesh}


I've have no idea what kind of error is , becouse I think the model is ok : I have 2 regions ,a solid(heat shield) and fluid one and i used contact interfaces beetwen them. The surface diagnostic doesn't give me any error!
I noticed that after surface mesh ,all the interfaces boundaries of both regions have a faces number equal to zero and the relative icons are darken .

Maybe the error dipends of this? What can I do?

Anyone can help me?

Thank you people!

Francesco
Trofrensis is offline   Reply With Quote

Old   December 21, 2009, 01:54
Default
  #2
jsm
Senior Member
 
JSM
Join Date: Mar 2009
Location: India
Posts: 155
Rep Power: 11
jsm is on a distinguished road
Hi,

I am not sure what may be cause. However delete the interface and create once again. Just try this.
__________________
With regards,
JSM
jsm is offline   Reply With Quote

Old   December 21, 2009, 09:01
Default
  #3
SKK
Member
 
Join Date: Mar 2009
Posts: 55
Rep Power: 8
SKK is on a distinguished road
For the interfaces, the cells will be zero but the boundary names with [] at the end (ie the interface) should be non-zero. If you have conformal mesh, the cell numbers in the interfaces ideally should be equal to the number of cells in the original/parent boundary.

Have you checked your remeshed surface for errors? Check each regions separately and fix the errors before volume meshing.
SKK is offline   Reply With Quote

Old   December 21, 2009, 15:09
Default
  #4
New Member
 
Francesco
Join Date: Nov 2009
Posts: 9
Rep Power: 7
Trofrensis is on a distinguished road
Hi

I can see that both in the imported geometry , and remeshed surface , all the boundary ending with [] havo 0 faces , while the origin boundary and the copy have the same faces .its really strange . I CHECKED my geometry raising the accuracy level to 0,5 for surface proximity and 0,1 for faces surface quality i have only 10 surface proximity, but i don't think that they can generate that kind of error, maybe I wrong?

Thank you!!!!

Francesco
Trofrensis is offline   Reply With Quote

Old   December 22, 2009, 06:36
Default
  #5
SKK
Member
 
Join Date: Mar 2009
Posts: 55
Rep Power: 8
SKK is on a distinguished road
Interfaces should be created after volume meshing, so that's not a problem. Did you check the regions one by one? If there are no pierced faces, free edges,non-manifold edges and non-manifold vertices when you used 'surface repair' on region by region, conduct a diagnosis on all regions together. You will most possibly see non-manifold edges/vertices when you do that. Repair those and you should be able to volume mesh.
SKK is offline   Reply With Quote

Old   December 23, 2009, 05:25
Default
  #6
New Member
 
Francesco
Join Date: Nov 2009
Posts: 9
Rep Power: 7
Trofrensis is on a distinguished road
Thank you skk

I have tried again , the geometry is ok ! When i combine my regions (solid, fluid) in a fluid one ,I have no error and the volume mesh has succesful , but if a have two regions separated (even of the same continuum ), I get the "connectivity error"!

At this point what kind of problem could be?

maybe i must set somthing in the continuum?

Thank you
Trofrensis is offline   Reply With Quote

Old   December 23, 2009, 06:59
Default
  #7
SKK
Member
 
Join Date: Mar 2009
Posts: 55
Rep Power: 8
SKK is on a distinguished road
Firstly, how did you check for errors? Did you use surface repair tool? Represetation>Remeshed Surface>(right click mouse)Repair Surface
I had similar problem with my models a while ago. And the cause for this was due to non-manifold edges/vertices when all three regions were checked together in surface repair tool (no error when checked individually). This was because some cells where 'tresspassing' between different regions and these needed to be fixed manually. I was then able to volume mesh. If this is not the case for you, I suggest you contact CD ADAPCO support with a screenshot.
SKK is offline   Reply With Quote

Old   December 27, 2009, 16:54
Default
  #8
New Member
 
Francesco
Join Date: Nov 2009
Posts: 9
Rep Power: 7
Trofrensis is on a distinguished road
Thank you skk!

The problem was right there, rising the accuracy to 0.5 for quality cell and proximity in the surface ripair i found some errors ,now it works!

thank you!
Trofrensis 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
interFoam - stratified flow - problem with shear stress at interface AnjaMiehe OpenFOAM Running, Solving & CFD 8 June 14, 2010 06:49
Interface problem Shahriar FLUENT 10 December 10, 2008 11:44
Having problem in creating a volume mech in GAMBIT Jake FLUENT 1 April 25, 2008 05:01
Volume Meshing & Face Meshing? singularity of grid ken FLUENT 0 September 4, 2003 11:08
GAMBIT meshing problem Gauthier Lambert Main CFD Forum 1 August 3, 2000 09:22


All times are GMT -4. The time now is 05:04.