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

[ICEM] Hex-tet merge

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 29, 2011, 05:16
Default Hex-tet merge
  #1
New Member
 
Join Date: Oct 2009
Posts: 23
Rep Power: 7
doodek is on a distinguished road
Hello,
I have two blocks (cubes) adjoin one surface. Surface from tetra cube are in another part then surface from hexa cube. Geometry is only in hexa volume, because tet part is imported from separate file. Next, I use 'repair mesh -> associate with geom'. This way I associate tri surface elements to geometry. Tetra elements (2D) are moved to part with surface quad elements from hexa volume. When I want to merge two meshes surface (with both quad and tri elements in one part) is selected and hex volume as frozen volume.



Unfortunately there are many multiple edges (shown above). Maybe do you know how to deal with it?

Best regards,
doodek
doodek is offline   Reply With Quote

Old   November 1, 2011, 16:27
Default Not a problem...
  #2
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Multiple edges are only listed under "possible problems".

I would expect to see them around the perimeter after a merge. It just means that the elements along that edge are connected...

If you want the interface surface to remain (such as for CHT), then you are fine. Proceed to solver.

If you wanted the flow to be open between the hexa and tetra regions, you just need to delete the quads in that interface part...

Go to Edit Mesh and delete elements. For selecting the elements, use the select by part option from the tool bar and select the interface part...
__________________
-----------------------------------------
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   November 2, 2011, 08:16
Default
  #3
New Member
 
Join Date: Oct 2009
Posts: 23
Rep Power: 7
doodek is on a distinguished road
Yes, I want to calculate flow between hexa and tetra region, so this region should be open. If I delete quad elements on interface surface, the problem with 'missing internal faces' appears...

doodek is offline   Reply With Quote

Old   November 2, 2011, 09:56
Default
  #4
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Missing internal faces means that volume elements of different fluids are not properly separated by an interface (of shell elements). Your solver will want shells between elements of different zones.

If it is really one fluid, then just put elements on both sides into the same volume part.

Find out what the two parts are named. Lets say it was "FLUID" and "FLUID2".

In the model tree, right click on the one of them, "FLUID" and select "Add to Part". Then using the selection tool bar (pops up on the top right side of the display window), make sure it is in mesh selection mode (last toggle on the bar) and then select the option for "Select items by Part". When the part selection menu pops up, select FLUID2 and apply...

Now all your volume mesh is in one part and you won't get the uncovered faces error.

Another way to do this would be to create a new material (call it what ever you want), then when it asks you to select entities, toggle the selection toolbar to mesh selection mode and hit the option for select all volume elements... This will put all the volume elements into that one part and solve the problem that way. (Obviously don't do this if you have some volume elements that belong in another fluid or solid region).
__________________
-----------------------------------------
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   November 2, 2011, 10:09
Default
  #5
New Member
 
Join Date: Oct 2009
Posts: 23
Rep Power: 7
doodek is on a distinguished road
It works. Thanks a lot PSYMN.
doodek 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
Blockmesh error - 2D scramjet - please help ishaninair OpenFOAM Native Meshers: blockMesh 7 March 18, 2011 01:14
[ICEM] how can i create a consistent transitions between tet and hex? specifically my model? snailstb ANSYS Meshing & Geometry 3 March 15, 2010 21:26
Hex versus Tet Jade M CFX 1 March 12, 2010 00:41
CheckMeshbs errors ivanyao OpenFOAM Running, Solving & CFD 2 March 11, 2009 03:34
poly, hex dom, hex, tet azmir CD-adapco 0 October 31, 2007 20:24


All times are GMT -4. The time now is 03:22.