osp5020m tool offset format?

[dmcdowell]

I need format info for an OSP5020M.
We are integrating a Tool Presetter into our network and plan on sending tool offset data from the presetter to a file on our network to be dumped into our CNC's.
I've gotten good results on our Fanuc controls but, have no clue on the Okuma controls.
What gcode syntax would I use to write a program that sets hgt. and dia. offsets?
Happy Friday!

[dcoupar]

Try outputting the offsets from the CNC to the PC. That should give you the format.

[broby]

Tool offsets are just another "System Variable" that can be both Read from and Written to.
To access the tool radius use VTOFD[x] where x represents the tool number.
To access the tool Length use VTOFH[x] where x also represents the tool number.
So a program might look like this (for 3 tools):
$TOOLDATA.MIN%
O1000
(SET TOOL 1 DATA)
VTOFH[1]=34.220
VTOFD[1]=10.010
(SET TOOL 4 DATA)
VTOFH[4]=-10.435
VTOFD[4]=0.000
(SET TOOL 15 DATA)
VTOFH[15]=156.012
VTOFD[15]=39.950
M2

Note in this example I am using Metric units, obviously the tool data will be in the correct unit for you anyway.
Once the presetter has the information formatted into a program as shown above, it should be a simple matter to load the program into your machine and run it.
The tool data will be updated instantly.
Hope this helps
Brian.

[dmcdowell]

Thanks everyone.
This should put me on the correct path.