Help me improve this custom macro, also freebie chip breaker macro for lathes

Hello,
This custom macro was set up by the factory on a couple of our swiss machines to help control chips. It works awesome so feel free to use it if you have some unruly chips.

As the program exists you can only turn in Z. This works fine most of the time but I would like to be able to program in some taper in X. Could you guys tell me if this would be possible?

All it does is turn/dwell/turn/dwell ect.

Z=end
Q=turn distance before dwell
D=Dwell in seconds
F=Feed

Here is the existing program:

O0061(G1 MACRO: SET PARAMETER 6050 TO 61)
(CHANGE TO O9010 WHEN INSTALLED)
IF[#7LE0]GOTO5
IF[#9LE0]GOTO6
IF[#17LE0]GOTO7
IF[#26LE0]GOTO8
#501=#5042
IF[#501GT#26]GOTO10

WHILE[#501LT#26]DO1
N1G01Z#501F#9
G04X#7
#501=#501+#17
END1
G01Z#26F#9
M99

(CUTTING Z+ TO Z-)
N10
#501=#5042
WHILE[#501GT#26]DO1
N1G01Z#501F#9
M99

N5#3000=1(D MISSING)
N6#3000=2(F MISSING)
N7#3000=3(Q MISSING)
N8#3000=4(Z MISSING)

__________________________________________________ _____________

So, here's my (uneducated) thinking on how to improve this

#501=#5042---------------------- (#501=current Z position)
#502=[[#26-#5042]/#17] ---- [turn length/peck distance] (formula to get # of "pecks")
#10=#503------------------------- (didnt look up what # U actually is so its 10 for this example)
#503=[#503/#502 ] -------------(per peck U move)

WHILE[#501LT#26]DO1
N1
G1 Z#501 U#503 F#9
G4 X#7
#501=#501+#17
END1
G1 Z#26 U#503 F#9
M99

Could this work? thoughts? thanks!
__________________

#501=#5042---------------------- (#501=current Z position)
#502=[[#26-#5042]/#17] ---- [turn length/peck distance] (formula to get # of "pecks")
#10=#503------------------------- (didnt look up what # U actually is so its 10 for this example)
If you're passing U as an argument its #21. Also your assignment should be the inverse of the above, #503=#21 (#10 in your example). Or you could change #503 in your program to #21. Also, you would have to calculate what the total Incremental move in X is if you're not pre-calculating and passing it as the U argument.

#503=[#503/#502 ] -------------(per peck U move)
The above block would become
#21=[#21/#502]
and
U#503 would become U#21

WHILE[#501LT#26]DO1 This will only work if feeding in a Z- to Z+ direction
N1
G1 Z#501 U#503 F#9 In the 1st execution of this WHILE Loop, only an X move will result. The tool is already at Z#501. You need to execute #501=#501+#17 prior to starting the WHILE Loop
G4 X#7
#501=#501+#17 If #17 is a + value, this will also facilitate a movement in a Z- to Z+ direction.
END1
G1 Z#26 U#503 F#9
M99

Regards,

Bill

a previous post of yours provided a solution to this same problem. A least the pecking in Z part. Your re-worked program is completely different and not based on something that was proven.
http://www.cnczone.com/forums/fanuc/...er_custom.html

Ill give that a try angel. Thats a good point about the first time through it will just move up. Ill add what you suggested and see if it works. Thanks!

ford -The program at the top of my post is a working macro. the one you linked was me trying to remember the one I posted before I was able to get it back. Im using the posted macro on a job as i type this. It was made by a factory installer, so its plenty proven and works great. so the old one is irrelevant...