[Jerseycnc]

Hello,
Just started a new job and working on a Leadwell with a Fanuc OM control.
Older control not sure the date.
Noticed on the control where the fixture offsets are you have your standard G54 to G59, when you page down I notice more - started as P1 G54 all the way as you page down to P48 G54. If these are more offsets how do I call them up in a program. I looked in their manual and has nothing on it. Can someone assist........THKs

Jerseycnc

[dcoupar]

Hello,
Just started a new job and working on a Leadwell with a Fanuc OM control.
Older control not sure the date.
Noticed on the control where the fixture offsets are you have your standard G54 to G59, when you page down I notice more - started as P1 G54 all the way as you page down to P48 G54. If these are more offsets how do I call them up in a program. I looked in their manual and has nothing on it. Can someone assist........THKs

Jerseycnc

G54 to G59 activates the standard (6) work coordinates.
G54 P1 to G54 P48 will activate the extended (48) work coordinates.

[Jerseycnc]

Thanks I guess its that simple. just adding the sequence of the P call from 1-48 after G54 will do it. I will try that this coming monday. Do appreciate the response.

Jerseycnc

[beege]

If what dcoupar wrote doesn't seem to work, try G54.1 P1 thru G54.1 P48 for each of the fixture offsets.

[Jerseycnc]

OK So in my line of code it would be something like this
Ex.
G17 G20 G40 G49 G80 G90
N1 T3
(TOOL_3 .500 DOWEL PIN TLO=H3)
(OPERATION_1 LOCATE PART)
M6
M5 S0
G00 G90 G54.1 P1 X-0.4387 Y-0.25 (only have to change P from 1-48)
G43 Z1. H3
M9
G01 X-0.4387 Y-0.25 Z-0.250 F15.
(SLIDE PART UP TO PIN_TIGHTEN VISE)
M0
Z1.
M9
G00 G28 G91 Z0 M5

Jerseycnc

[beege]

Looks about right to me, although it's been 12 or so years since I've had a machine with those extra fixture offset options turned on.

[John_B]

I have a 2006 machine with the 18im-b control which has the extended offsets. I use the "G54.1 P#" format to use it. I don't think just using "G54 P#" will work.

[maz43]

I use the "G54.1 P#" format to use it. I don't think just using "G54 P#" will work.

Ditto on the Fanuc 0IMB control.

[gbowne1]

From what I've been told 18iMA was initially set up to use the G5x.1 P fixture offsets when it was first installed.. but I've used them.

I'd have to see your operation but the programming looks about right to me.

[fordav11]

according to the manual both G54 Px and G54.1 Px are valid for enabling the additional workpiece coordinate systems.

see attached pages from Fanuc manual.

[dcoupar]

according to the manual both G54 Px and G54.1 Px are valid for enabling the additional workpiece coordinate systems.

see attached pages from Fanuc manual.

If I'm not mistaken, those pages are from the 21i manual. He said he has a 0M. The 0M-B/C manual makes no mention of G54.1.

[fordav11]

yes you're right. I missed that it was a 0M. so just G54 Pn works on 0M.
here's the relevant page from the 0-series manual.

[Jerseycnc]

Sorry for a late response _ want to thank everyones input and will address this at work tomorrow. Its nice to know theres help and with a great response.

jerseycnc