[cSpampinato]

We have a 32i series and a 21i series CNC and are trying to access a macro designed to move the machine's tailstock. The program number is O9023. The problem is that I cannot access it on edit to change a Z move that it does not need. I know it can be done because the technician that originally installed the machine actually put the Z move there when he set the machine up for us. The problem is that we do not have access to that technician any more, and really do not need that Z move there. Any help will be greatly appreciated.

[machinetoolmad]

Turning parameter 3202 bit 4 (NE9) to 0 should let you view and edit the 9000programs...

[cSpampinato]

What a life saver! Removing that Z move saves us 3 sec from a ~ 5 min operation. The accumulated time saved will be huge! Thanks a lot. Now the only thing I changed was the unnecessary movement on Z, the rest of the macro I could hardly understand. Is there anything I could read up on to better understand macros and how to create them?

[machinetoolmad]

No problem.

There are numerous resources available that you can use to read up on macros - FANUC CNC Custom Macros by Peter Smid is a good book to use. If it will help, post the macro on here or PM me and I'll see if I can go through it and comment it for you

[cSpampinato]

Ok, here is a link to the macro that I altered yesterday.

http://s10.postimage.org/46980tovt/MACRO.jpg

Yesterday I found a pdf that explains macro programming. I think it came from a fanuc book. I'm reading through it now, but if you get a chance to look at this macro and help me understand it, I would appreciate it.

[machinetoolmad]

Here you go. Let me know if you need anything clarifying




IF[#1001 EQ 1] GOTO 10 (System Variable #1001 relates to a data input bit. This statement says if the value of this variable is EQUAL to 1 then GOTO or jump to line N10 of the program)

#1=#4001 (Assign local variable #1 the value of system variable #4001. #4001 is the modal G code for the G code group 1. So G00, G01 etc)

#2=#4006 (Assign local variable #2 the value of system variable #4006. #4006 is the modal G code for G code Group 6 so G20 or G21)

#3=#4010 (Assign local variable #3 the value of system variable #4010. #4010 is the modal G code for G code Group 10 so G98 or G99)

#4=#4109 (Assign local variable #4 the value of the current Feed rate)

IF[#1004 EQ 1] GOTO 5 (System Variable #1004 relates to a data input bit. This statement says if the value of this variable is EQUAL to 1 then GOTO or jump to line N5 of the program)

IF[#503 EQ #5022] GOTO 3 (If Common Variable #503 is EQUAL to #5022 which is the current coordinate in the 2nd machine axis, which in your case seems to be the Z axis then GOTO or jump to line N10 of the program)

IF[#1002 EQ 1] GOTO 2 (System Variable #1002 relates to a data input bit. This statement says if the value of this variable is EQUAL to 1 then GOTO or jump to line N2 of the program)

N1
G98 G00 W-.05
GOTO 3
N2
G98 G00 W.05
GOTO 3
N3
M84

#503=#5022 Assign Common Variable #503 the value of #5022 - the current Z position

N5
M84
G#1 G#2 G#3 G#3 F#4 (Reassign G codes to their original values as above)
N10
M99