# [ICEM] let ICEM compute the number of nodes on an edge

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

 November 15, 2012, 13:57 let ICEM compute the number of nodes on an edge #1 New Member   motorbean Join Date: Nov 2011 Posts: 16 Rep Power: 8 Hello, everyone! I'm using ICEM for some time. But I have a problem: In Hexa meshing, is it possible to specify the bunching law (spacing 1, ratio1, spacing 2, ratio 2) and let ICEM to compute the number of nodes required on an edge? I'm using scripting to automatically generate hexa mesh for different geometry, and the edge length will change according to different geometry. Therefore, if I specify the constant number of nodes in the script file, it will produce very dense mesh for the short edges and sparse mesh for the long ones. This should be avoided in my case. Can anyone give some help for me? Any solutions, whether direct or indirect, as long as they shed some light on this problem, will be highly appreciated Thank you very much! Regards to all motorbean

November 15, 2012, 18:33
#2
Retired from CFD Online

Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,665
Blog Entries: 1
Rep Power: 39
I usually deal with this problem by setting a size on the surface and then initialize the blocking sizes from that... if the edge length is greater, it will be over more surface and a larger number of nodes will be assigned automatically... Then I adjust the initial spacing, etc. in my script.

Anyway, assuming that is not enough, I asked around and found some workarounds... Basically, there is no way to float the number of nodes, but you can script to get the length of the edge and then use a calculation to work out how many nodes you need...

Here are some snipits of the suggestions I got...

Quote:
 Try the following ic_hex function: set param [ic_hex_get_edge_param node1 node2 param] e.g. set edge_len [ic_hex_get_edge_param 14 17 len] which returns the length of edge 14 17. For more detials, look into file lib/med_batch/hex_funcs.tcl). But maybe it helps to set the number of nodes depending on the edge length. The options for this command: nodes (number of nodes) len (edge length) law (mesh law) max (max space) sp1a or sp2a (actual spacing 1 or 2) sp2r or sp2r (requested spacing 1 or 2) r1a or r2a (actual ratio 1 or 2) r1r or r2r (requested ratio 1 or 2)
__________________
-----------------------------------------

Public ANSYS ICEM CFD Users Survey

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

CFD Online Users Survey

 November 15, 2012, 18:34 #3 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,665 Blog Entries: 1 Rep Power: 39 Or you could use these older commands... set mparams [ic_hex_mesh_params 14 17] set edge_len [lindex \$mparams 5] __________________ ----------------------------------------- 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

November 15, 2012, 18:36
#4
Retired from CFD Online

Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,665
Blog Entries: 1
Rep Power: 39
One of the Tech support guys (Matt M.) agreed with my initial suggestion. He also suggested this more advanced way of doing things...

Quote:
 With the ic_hex_mesh_params, it should return requested as well as actual values, so he could have a loop that keeps upping the number of nodes and then checking the spacings and ratios actual values against requested values, and the loop would stop when they match. I don't know if setting the number of nodes as a scale factor of the edge length would get the exact number, but using this looping after the fact could pinpoint it, and using the scale factor at the beginning would reduce the number of loops needed.
Hopefully one of these approaches will get you going.
__________________
-----------------------------------------

Public ANSYS ICEM CFD Users Survey

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

CFD Online Users Survey

 November 16, 2012, 07:42 #5 New Member   motorbean Join Date: Nov 2011 Posts: 16 Rep Power: 8 Thank you so much for such an detail answer. The solutions are very inspiring. I will give a try. Regards, motorbean

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Rohit ANSYS Meshing & Geometry 0 August 20, 2012 11:38 Jasmine CFX 1 July 29, 2010 07:12 Karatix ANSYS Meshing & Geometry 6 March 31, 2010 09:40 strider Main CFD Forum 2 July 24, 2006 15:31 Rui CFX 3 April 11, 2005 20:46

All times are GMT -4. The time now is 21:15.