inputing work offsets

[heeler]

Does anyone know of a way to input workoffset data with the rs232. We are starting up a pallet system and would like the set the values up from a cmm. Also would like to do this with the tool lengths and dia's. Any other ideas as to how to do this?

 

Thanks

Glenn

 

P.S. This is on a Fanuc 18m and 21i controls

 

[ 02-12-2003, 11:38 AM: Message edited by: heeler ]

[PE @ IHS]

Use the G10 data register command. With G10 you can replace work or tool offset data, or change it incrementally. The best thing to do is to look it up in your manual. If you can't find out how to do it, let me know and I will post some examples. This works equally well on mills and lathes, and on lathes you can even input TNR values and comp direction values (0 to 9)

 

Peter Eigler

 

[ 02-12-2003, 11:49 AM: Message edited by: Peter E ]

[McRae]

Heeler and PeterE,

 

I like the G10 for this application but I wonder if you could get an even more root level and input indise the machine at the parameter level. IE #50001=13.1222 etc... and then read this in as a parameter file rather than trying to invoke changes as a gcode program.

 

Just a thought.

[heeler]

Peter,

 

I see in the manual how to do the G10 for length and cutter dia. But not work offsets. Could you please let me know the format and I can try it.

[chris m]

Andrew

 

As you know, I'm sure, when you use the G10, the machine writes the data into the parameters itself; why load separately when you can use the program to do it? Also, many Fanuc parameters are impossible to write to directly, I don't know if work offsets are among these or not...

 

C

[Henk]

Glenn,

 

 

G10 G90 L2 P1 X100. Y100. Z100.(G54)

 

 

L2 = WCS (L1 = Tool offsets)

P1-P6 = G54 - G59

 

HTH

[PE @ IHS]

To add to Henk's post

 

G90 G10 L2 P2 X-6.55 Y-3.322 Z1.22

(REPLACE VALUES IN G55 to X -6.55 Y-3.322 Z1.22)

 

G91 G10 L2 P1 X-.115 Z-.05

(MODIFY G54 X value by -.115 and z by -.05)

 

There is far more detail on this in Peter Smid's

book, available at www.industrialpress.com

 

It is a FAR better resource than the Fanuc manuals written in Jinglish.

 

Peter Eigler

[heeler]

Thanks to all. I've been able to test this in the 21i control and it works great. As soon as they have an 18M control free I'll try it there.

 

Thanks again.

[McRae]

quote:

---

Andrew

 

As you know, I'm sure, when you use the G10, the machine writes the data into the parameters itself; why load separately when you can use the program to do it? Also, many Fanuc parameters are impossible to write to directly, I don't know if work offsets are among these or not...

---

Chris, Peter, and group...

 

The reason for my suggestion was that I am currently involved with a probing project that changes the actual parameter thru a variable assignment for locations rather that writing to it thru a gcode (G10). Every maintainence program should include a pdump from the machine and these should be catalogued and stored. A re-load of the new position parameters would be possible at this level rather than a G10 statement. User preference will dictuate which to use. Given the option though I recommend the G10 - Look much nicer and easier to document to an operator - as well there is a lower possibility to make a mistake using the G10 as the addresses are explicit!