[smegma]

I'm starting to experiment with programming multiple work offsets using the M97 on my Haas OM2 and I keep getting stuck on my first sub program. It's probably just a matter of my syntax being slightly off:

O10001(Base modification)
G20 G90 G40
T01 M06 (0.03" EM)
G54
S10000 M3
G0 X0.2889 Y-0.1071
G43 H01 Z1.
M97 P12000
/G55
/M97 P12000
/G56
/M97 P12000
/G57
/M97 P12000
/G58
/M97 P12000
/G59
Z1.

N12000
... (insert sub here)
G0 Z1.
M99

G28 Z0 M5
M9
M01

T02 M06 (0.01" EM)
...
(N13000 on 6 locations to follow with 2nd tool)

I think my problem lies in the placement of the M99, but I've tried switching it with an M02, and moving it within and outside of the sub. and it doesn't seem to make any difference. The machine just keeps looping back to G54 indefinitely.

Any suggestions how I can continue to the G28 block would be much appreciated

[Fletch_CNC]

/G59
Z1.

N12000
... (insert sub here)
G0 Z1.
M99

G28 Z0 M5
M9
M01

T02 M06 (0.01" EM)
...
(N13000 on 6 locations to follow with 2nd tool)

Unless you edited this to shorten the post, you need something like an M30 or a GOTO between the the Z1. line and the N12000 line, or it is just going to keep running the "subprogram" as an inline part of the main program. Since in that instance the M99 is not returning anywhere (as it would if there was an M97 or G65 call that sent the program to a subprogram), it will just jump to the head of the program (and loop endlessly).

[rcs60]

Fletch said it above




O10001(Base modification)
G20 G90 G40
T01 M06 (0.03" EM)
G54
S10000 M3
G0 X0.2889 Y-0.1071
G43 H01 Z1.
M97 P12000
/G55
/M97 P12000
/G56
/M97 P12000
/G57
/M97 P12000
/G58
/M97 P12000
/G59
Z1.
G28 Z0 M5
M9
M01

T02 M06 (0.01" EM)


(end of tool call outs)
M30(Place the m30 between tool call outs and sub routines)
Your example above says to goto n12000 return to just after first m97 call then with the block deletes active it runs N12000 and return to the beginning of the program and start again


N12000
... (insert sub here)
G0 Z1.
M99
%