G52 confusion

[davek]

I am just starting to write a macro which will be used by others than myself. It uses G52 to shift my X zero, as I see many here use. How do you handle operator confusion about where zero is? Like, say, if the operator hits reset while the program is running. Zero could be set somewhere with no clue to the operator as to what is up. What cancels G52 other than G52 X0? Are all offsets effected, or just the one active when the G52 is used? I was thinking of putting a note in the documentation saying, "If you stop the program for any reason, MDI "G52 X0"".

In this macro, I am using G59 to enable the operator to shift X and Y. It engraves lettering and the operator can then shift for a new line, etc. I'm moving G55 to G59 with or without adding a local variable as in...

IF[#24NE#0]THEN#2506=[#2502+#24]
IF[#24EQ#0]THEN#2506=#2502
IF[#25NE#0]THEN#2606=[#2602+#25]
IF[#25EQ#0]THEN#2606=#2602
IF[#26NE#0]THEN#2706=[#2702+#26]
IF[#26EQ#0]THEN#2706=#2702

Would a better way to shift X zero be to use something like this? As in...

#2506=[#2506+.625]

instead of

G52 X.625

to avoid operator confusion about where X is.

[uperez]

may i ask on which fanuc control is this? i believe you are using system variables for geometry offsets, aren't you supposed to be using #5000s, for example #5041,#5042,#5043 for G55?

[gar]

070908-0728 EST USA

davek:

My reference is HAAS. So all comments below refer to a HAAS machine. Similarities should exist for Fanuc.

In HAAS you can set one of three modes on mills. These are HAAS, Fanuc, and Yasnac. With respect to G52 in Yasnac it is I believe just another G5x.

In a HAAS machine and in HAAS mode G52 is never reset. You must explicitly set it, and there are three ways. In Fanuc mode G52 is zeroed from many conditions. Some of these are power-up, program start, and others.

In HAAS mode you can manually go to the offset page and change the G52 values individually for each axis. Within the program you can load the appropriate variable with a desired value, such as,
#5201 = 0.150 to load G52 X with 0.1500 .Or you could do it in MDI.
And you can do
G52 X0.15 within the program or any other program or MDI and the X component of G52 will be changed.

See the HAAS on-line manual for mills p 85
#5201-#5205 Common offset (this is the set for G52)
#5221-#5225 G54 work offsets
#5241-#5245 G55 work offsets
....
#5321-#5325 G59 work offsets

Always remember in HAAS mode the last values set into G52 by whatever means remain until changed. No matter where or how they were changed. I suggest that you never use G92.

To your specific problem.

Into the beginning of your program put this line of code
G52 X0 Y0
In HAAS mode this leaves G52 Z free for you to make minor Z adjustments if you want. In Fanuc mode that won't work because all G52 components are zeroed at the start of the program automatically.

How you restart a program will determine if you want to even use G52.

I need a better idea of what you want to do within a single execution of your program.

.