G10 to select coordinate system

[jorgehrr]

All my fixture offsets are full (G54, G55.....)

I know I can use G10 to input new offsets, my question is at the end of the program.... are the original numbers going to go back and what is the M/G code that does it.

I just want to make sure if the original fixture offsets will remain after I use G10.

Thank you in advance

George

[hoidahl]

Yes the offsets should remain. Here is an example of what we use.

G10L20P1X-9.9149Y-11.8528Z-22.419
G10L20P2X-1.9459Y-11.8528Z-29.771
G10L20P3X-17.8819Y-11.8528Z-29.771
G0G17G40G80
T5
M6
T6
G54.1P1
G0G90X0.Y1.375S1579M3
G43Z1.H5M8
G81G98X0.Y1.375Z-.1565R.1F9.47
Y-1.375
G0G80Z1.
G91G28Z0.
G54.1P2
G90G0X.75Y0.
G43Z1.H5
G81G98X.75Y0.Z-.0985R.1F9.47
G0G80Z1.
G91G28Z0.
G54.1P3
G90G0X-.75Y0.
G43Z1.H5
G81G98X-.75Y0.Z-.0985R.1F9.47
G0G80Z12.
M9
G91G30X0Y0Z0M67
M1

[jorgehrr]

Ohhh.

Do you see anything wrong with mine????

O6001
G80 G40
T01M06 (1/2 Drill)
G0 G90 G10 L2 P1 X-22.3837 Y-12.2827 Z-11.0387 M3 T2
G43 H01 Z0.1 M08
G54 P1 X1.0 Y1.0
G81 R0.1 Z-0.3 F5.0
G0 G80 Z1.0 M9
G91 G28 Z0 M19
M30

Thank you in advance

George

[hoidahl]

We just put the g10 lines at the beginning of the program so they can be located easily. Looks like it should work. Does it?

[Geof]

Originally Posted by jorgehrr All my fixture offsets are full (G54, G55.....) I know I can use G10 to input new offsets, my question is at the end of the program.... are the original numbers going to go back and what is the M/G code that does it. I just want to make sure if the original fixture offsets will remain after I use G10. Thank you in advance George

The G10 line will permanently change the offset values. The only way to get your original ones back is to have another G10 line that re-enters the original values.

Based on the little bit you have written I think you should do some reading about G52.

G52 gives you an offset shift and it does not change the G54, etc offset values. You can use many different G52 commands in a single program; in effect with G52 you have an unlimited number of offsets possible.

Depending on your machine the G52 values may be zeroed by M30 or RESET but you can always zero them by using G52 X0. Y0. Z0.

[hoidahl]

g54 isn't changed doing it this way its put into a p1(101)p2(102) etc. offset and g54 remains the same.

[jorgehrr]

Well.......

It changed mine. I was convince numbers will remain the same after the M99 code but Geof. is correct, the change stays.

In my machine I can not use G54.1 P? (machine alarms out)
It has to be only G54 P?

May be that is the reason.

Thank you guys. I'll find the way to get them back.

Cheers

George

[Geof]

Originally Posted by jorgehrr .... Thank you guys. I'll find the way to get them back. Cheers George

Like I said above...read up on G52, it will do what you want.

[aa8vs]

"my machine I can not use G54.1 P? (machine alarms out).."

You do not have the Extended offset option so the G54.1 P? will generate an alarm, there is a cost if you need that many offsets.

G54 G55, G56, etc. is standard on the controls, and it gives you six offests to play with. The extended offset option gives you those 6 plus 48 additional.

[tranbell]

G52 or G92 works good.

[Thrasher]

Our machines run several different programs and we change the work offset many, many times within a given program. I guess my question would be: Why not use the G10 as much as needed. With good programing discipline you can change as much as need to accomplish the programming needs.

[aa8vs]

These were production machines and machine operators did not adjust the offsets. That was process engineer function. We used a single G54 offset register but transfered in the offsets for specific table positions from the extended offset table. The B<value> selected the offsets to use automatically. Basically think of a dynamic offset that follows the table, but on a control that did not have the option. So we created a sub program that accomplished the task automatically.