CFD Online Logo CFD Online URL
Home > Forums > ANSYS Meshing & Geometry

[ICEM] sub-domain mesh not generated?

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

LinkBack Thread Tools Display Modes
Old   February 8, 2012, 22:40
Default sub-domain mesh not generated?
Join Date: Sep 2011
Location: United Kigdom
Posts: 51
Rep Power: 8
federvo.mala is on a distinguished road
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?

federvo.mala is offline   Reply With Quote

Old   February 9, 2012, 10:14
Default Subdomain?
New Member
Mingyao Gu
Join Date: Jan 2012
Posts: 5
Rep Power: 7
mgu is on a distinguished road
Are you creating a subdomain to model the wind turbine or is the turbine geometry resolved?
mgu is offline   Reply With Quote

Old   February 9, 2012, 12:39
Retired from CFD Online
PSYMN's Avatar
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,665
Blog Entries: 1
Rep Power: 39
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
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...
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote


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
Domain Imbalance HMR CFX 5 October 10, 2016 05:57
2D Mesh Generation Tutorial for GMSH aeroslacker Open Source Meshers: Gmsh, Netgen, CGNS, ... 12 January 19, 2012 04:52
Problem in clearing generated mesh siara817 STAR-CCM+ 3 April 4, 2011 08:44
snappyHexMesh won't work - zeros everywhere! sc298 OpenFOAM Native Meshers: snappyHexMesh and Others 2 March 27, 2011 21:11
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 05:05

All times are GMT -4. The time now is 19:00.