# [ICEM] how to mesh an edge use a group of points(points coordinate file)

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

 November 9, 2009, 04:08 how to mesh an edge use a group of points(points coordinate file) #1 Senior Member   Jiang Join Date: Oct 2009 Location: Japan Posts: 186 Rep Power: 9 Dear all: I use ICEM_CFD, I want to mesh an edge using a group of points which are in this edge. I have these points coordinate ,I want the meshing is the same with the distribution of these points, how can I do this ? Is ICEM can do this ? Thank you very much.

 November 9, 2009, 21:06 #2 Senior Member   Jiang Join Date: Oct 2009 Location: Japan Posts: 186 Rep Power: 9 Nobody knows this ? Because I have structure mesh generated by other soft ware using three direction coordinate. I want to compare, so I must use the same mesh. I thought if I can use these coordinae to mesh the edge in ICEM, then it can realize. but it seems to difficult to do this. I can't find this mesh law in ICEM or gambit. thanks.

 November 12, 2009, 13:07 Yes. #3 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,660 Blog Entries: 1 Rep Power: 38 Yes, ICEM CFD can do this. You would first need to import the points or create them in ICEM CFD (interactively or with a script to read your coordinates). Then create a curve thru the points. You can use the mesh tab to assign a mesh distribution along the curve and then mesh it. This will give you line elements along the curve... is that all you want? Simon

November 12, 2009, 14:21
#4
Super Moderator

Ryne Whitehill
Join Date: Aug 2009
Posts: 313
Rep Power: 11
Quote:
 Originally Posted by PSYMN Yes, ICEM CFD can do this. You would first need to import the points or create them in ICEM CFD (interactively or with a script to read your coordinates). Then create a curve thru the points. You can use the mesh tab to assign a mesh distribution along the curve and then mesh it. This will give you line elements along the curve... is that all you want? Simon
Is there a tutorial or guide for doing this type of scripting?

thanks,

Ryne

 November 12, 2009, 17:53 Scripting Basics... #5 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,660 Blog Entries: 1 Rep Power: 38 Yes there is, sort of. But I don't think I can hand it out on CFD-Online. To see the commands, just try it manually and record it with a replay script. I created a few points, then drew a line thru them to get this. 1. ic_point {} GEOM pnt.00 0,0,0 2. ic_point {} GEOM pnt.01 100,0,0 3. ic_point {} GEOM pnt.02 10,10,0 4. ic_point {} GEOM pnt.04 20,8,0 5. ic_point {} GEOM pnt.05 40,5,0 8. ic_curve point GEOM crv.00 {pnt.00 pnt.02 pnt.05 pnt.01} Then I would take that replay snipit and find out more about these commands (ic_curve for instance) and their usage in the programmers guide built into the software. Then I would create a script that reads thru a list of points from a file or might use an array to create the points from an external executable, etc. Contact Matt Middleton in Tech support for some good help. He can help you get to something like this... (\$ indicates a variable being used) proc ic_geo_create_naca4_curves {prt cam campos thick points zoom x y} { global env set data [exec \$env(ICEM_ACN)/bin/naca4 -camber \$cam -maxcamberpos \ \$campos -thickness \$thick -numpoints \$points -scale \$zoom \ -xoffset \$x -yoffset \$y] set data [split \$data \n] set i 0 for {set crv 1} {\$crv < 3} {incrcrv} { set pnts {} while 1 { set xy [lindex \$data \$i] incri if {\$xy == ""} break lappendpnts "\$xy 0" } set name [ic_geo_new_name curve crv.0] ic_curve point \$prt \$name \$pnts } }

 November 12, 2009, 18:00 Original question... #6 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,660 Blog Entries: 1 Rep Power: 38 Oops, back to the original question... If you then wanted to script the setting of mesh sizes on the curve and then creating the line elements... Just do it interactivly and then look at the replay script. 11. ic_set_meshing_params curve crv.00 emax 8 emin 0 ehgt 0 edev 0 hrat 0 ewid 0 nlay 0 14. ic_quad2 what curves_only entities crv.00 15. ic_uns_update_family_type visible {GEOM ORFN} {!NODE LINE_2} update 0 The first line (11) shows setting the meshing params for the curve to max size 8. Nothing else set, but you can see deviation, min size, etc. are all set to "0" (which means nothing set). Then Line 14 is actually meshing that curve (crv.00). You could just as easily mesh surfaces or volumes. The last line (15) isn't needed for a batch script, but it displays the new mesh, at least the line elements that were created.

 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 gschaider OpenFOAM 300 October 29, 2014 19:00 hardy OpenFOAM Paraview & paraFoam 7 September 18, 2008 04:59 matteo_gautero OpenFOAM Running, Solving & CFD 0 February 28, 2008 07:51 jens_klostermann OpenFOAM Bugs 11 June 28, 2007 17:51 Althea FLUENT 21 February 6, 2001 08:05

All times are GMT -4. The time now is 14:37.