CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ICEM] Hex-Core disconected

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

Like Tree1Likes
  • 1 Post By PSYMN

Reply
 
LinkBack Thread Tools Display Modes
Old   December 15, 2011, 13:18
Default Hex-Core disconected
  #1
Member
 
Max
Join Date: Apr 2011
Posts: 46
Rep Power: 6
max3.2 is on a distinguished road
Hey Guys,

I'm trying to mesh a duct flow with tets, prisms and hexa core. Everytime I try to do so, the hexa-core seems to be disconnected from the outside prisms. Theres's just a free space in the cut plane and the hexa elements are way to big. Mesh checks confirms unconnected faces.
I can't find any way around it, anyone knows what could possibly be wrong?

Cheers
Max
max3.2 is offline   Reply With Quote

Old   December 15, 2011, 13:45
Default
  #2
Member
 
Max
Join Date: Apr 2011
Posts: 46
Rep Power: 6
max3.2 is on a distinguished road
little update: if i do the hex first, prism wont work but hex does. other way around its prisms but no hex
max3.2 is offline   Reply With Quote

Old   December 19, 2011, 12:37
Default Recommend Change Mesh Type => 12 Tetra to 1 Hexa instead.
  #3
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Hex core works by deleting the prisms, meshing the region with a cartesian fill, then deleting the hexas that intersect the surrounding elements and then filling the gap with a delaunay tetra fill (gives you pyramids where needed).

The size of the Cartesian mesh is set by the size on the volume part (this is one of the few times that size on a volume part is used). If your hexas are too large, you could reduce this size.

The delaunay fill can fail for several reasons including too much of a size jump between the hexas and the surrounding elements or due to hanging nodes on the external surface of the hexa core block.

Personally, I avoid use of hexa core. I do not find it to be robust.

Instead, I suggest you use Octree Tetra. Then run an editing step to change mesh type and convert 12 tetras to 1 hexa. This will give you what you are really looking for.

Note: Prism is insterted post tetra and can only move tetras out of the way. It must be run before either Hexa Core or Tet to Hex conversion...
MDB likes this.
__________________
-----------------------------------------
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

Old   December 25, 2011, 15:42
Default
  #4
Member
 
Max
Join Date: Apr 2011
Posts: 46
Rep Power: 6
max3.2 is on a distinguished road
Hey,
Thank you that works fine now. Is the he a size only determined by the gets or is there a way to change them once they are created?
max3.2 is offline   Reply With Quote

Old   January 3, 2012, 17:01
Default
  #5
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
When you are converting tet to hex, the size of the hexas is determined by the size of the tetras...
__________________
-----------------------------------------
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

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
solving a conduction problem in FLUENT using UDF Avin2407 Fluent UDF and Scheme Programming 1 March 13, 2015 03:02
Superlinear speedup in OpenFOAM 13 msrinath80 OpenFOAM Running, Solving & CFD 18 March 3, 2015 06:36
BlockMesh number internal faces and boundary ynos OpenFOAM Native Meshers: blockMesh 6 December 13, 2011 06:36
Blockmesh error - 2D scramjet - please help ishaninair OpenFOAM Native Meshers: blockMesh 7 March 18, 2011 01:14
CheckMeshbs errors ivanyao OpenFOAM Running, Solving & CFD 2 March 11, 2009 03:34


All times are GMT -4. The time now is 04:27.