CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   STAR-CCM+ (https://www.cfd-online.com/Forums/star-ccm/)
-   -   Error at Volume Meshing (Interface problem) (https://www.cfd-online.com/Forums/star-ccm/71216-error-volume-meshing-interface-problem.html)

Trofrensis December 20, 2009 07:34

Error at Volume Meshing (Interface problem)
 
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

jsm December 21, 2009 01:54

Hi,

I am not sure what may be cause. However delete the interface and create once again. Just try this.

SKK December 21, 2009 09:01

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.

Trofrensis December 21, 2009 15:09

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

SKK December 22, 2009 06:36

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.

Trofrensis December 23, 2009 05:25

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

SKK December 23, 2009 06:59

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.

Trofrensis December 27, 2009 16:54

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!


All times are GMT -4. The time now is 00:07.