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

[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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 9, 2009, 03:08
Default 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: 6
panda60 is on a distinguished road
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.
panda60 is offline   Reply With Quote

Old   November 9, 2009, 20:06
Default
  #2
Senior Member
 
Jiang
Join Date: Oct 2009
Location: Japan
Posts: 186
Rep Power: 6
panda60 is on a distinguished road
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.
panda60 is offline   Reply With Quote

Old   November 12, 2009, 12:07
Default Yes.
  #3
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,650
Blog Entries: 1
Rep Power: 33
PSYMN will become famous soon enoughPSYMN will become famous soon enough
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
PSYMN is offline   Reply With Quote

Old   November 12, 2009, 13:21
Default
  #4
Super Moderator
 
Ryne Whitehill
Join Date: Aug 2009
Posts: 313
Rep Power: 8
rwryne is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
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
rwryne is offline   Reply With Quote

Old   November 12, 2009, 16:53
Default Scripting Basics...
  #5
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,650
Blog Entries: 1
Rep Power: 33
PSYMN will become famous soon enoughPSYMN will become famous soon enough
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
}
}
PSYMN is offline   Reply With Quote

Old   November 12, 2009, 17:00
Default Original question...
  #6
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,650
Blog Entries: 1
Rep Power: 33
PSYMN will become famous soon enoughPSYMN will become famous soon enough
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.
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
GroovyBC the dynamic cousin of funkySetFields that lives on the suburb of the mesh gschaider OpenFOAM 294 July 12, 2013 05:39
Paraview command not found hardy OpenFOAM Paraview & paraFoam 7 September 18, 2008 04:59
Problem with rhoSimpleFoam matteo_gautero OpenFOAM Running, Solving & CFD 0 February 28, 2008 06:51
DecomposePar links against liblamso0 with OpenMPI jens_klostermann OpenFOAM Bugs 11 June 28, 2007 17:51
Gambit problems Althea FLUENT 21 February 6, 2001 07:05


All times are GMT -4. The time now is 03:32.