CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] sub-domain mesh not generated? (http://www.cfd-online.com/Forums/ansys-meshing/97104-sub-domain-mesh-not-generated.html)

federvo.mala February 8, 2012 22:40

sub-domain mesh not generated?
 
Hello everybody,

I am sure this has already been asked but I could not find something useful.

On ICEM, I have wind turbine inside a cylindrical volume. I have done the geometry check and build diagnotic topology but sometimes, the blade mesh is not generated, i.e. i only have get a volume mesh without the turbine mesh.

I have noticed that this happens when I try to reduce the 'edge criterion' or/and 'max mesh size' for the blade. For example below 0.02 for edge criterion the blade mesh simply disappears.

Does anyone has any suggestions to help on this?

Thanks
Fred

mgu February 9, 2012 10:14

Subdomain?
 
Are you creating a subdomain to model the wind turbine or is the turbine geometry resolved?

PSYMN February 9, 2012 12:39

I assume you are using the octree tetra mesher...

In an effort to be robust and ignore small bits of geometry that you don't need, the algorithm checks for surface elements with the same volume material on either side. If it finds this situation, it deletes the element.

In your case, this is happening because you have a small hole or gap... When your mesh is large enough, it walks over this gap and you are fine. But when you adjust your settings, the finer mesh falls thru the gap and the solid volume fills with fluid, which then results in the removal of the surface mesh...

There are lots of ways to fix this... but here are two;

1) to find the leak, try putting a material point inside the solid region, then when it fills it will detect it as a leak and show you the path... Then you can fix the geometry to prevent leakage. In many cases, the problem may be due to a closely spaced pair of yellow curves... Often just building topology with a larger tolerance or even manually deleting one of the yellow curves will be enough to fix the problem. In other cases you may need to create a patch surface or something like that.

2) To proceed anyway (without fixing geometry), go into Mesh (tab) => Params by parts and check the box for "internal wall". This option is meant to allow for zero thickness baffles, but in this case you would simply be telling the mesher not to delete the surface mesh even though the inside fills up... Then I would go and delete the volume mesh... Then run a check for single edges, find the hole and repair it (mesh from edges, merge nodes, create elements, what ever). Then Run Delaunay to regenerate the volume mesh and continue on with your day...


All times are GMT -4. The time now is 12:45.