Changing parameters in program?

[chucker]

Can anyone explane the programs below I know they are changing parameters and I relize that they are calling up the programs with a M code I just dont understand why they were doing it. I found them in a 2500SY Deawoo lathe with a FANUC 18i it has live tooling sub spindle Y axis C1 and C2 we bought it used

(5110 is C-Axis clamp M code in drilling canned cycle)
(5461 is Axis(rotary axis)specification for polar coordinate interpolation)
(1020 is setting name for each axis used in programming)
%
O9004(M291 SUB SPINDLE C2-AXIS)
#3003=1
G10L50
N1020P3R65
N1020P6R67
N5461R6
G11
#3003=0
M99
%
%
O9003(M290 MAIN SPINDLE C-AXIS)
#3003=1
G10L50
N1020P3R67
N1020P6R65
N5461R3
G11
#3003=0
M99
%
%
O9002(M389 5110=189)
#3003=1
G10L50
N5110R189
G11
#3003=0
M99
%
%
O9001(M289 5110=89)
#3003=1
G10L50
N5110R89
G11
#3003=0
M99
%
Thanks in advance

[dcoupar]

O9001 and O9002 change parameter 5110 to either 89 or 189 so the c-axis will clamp/unclamp during drill cycles. For main spindle operation (C1), M89 is the C-axis clamp command. For sub-spindle operation (C2), M189 is the clamp command.

O9003 and O9004 change the axis names C-axis. Normally, when commanding C1, it is assigned "C" and C2 is assigned "A". When you want to use C2, O9004 changes the axis name assignement so C2 is "C" and C1 is "A".

Hope this helps.

[chucker]

So mainly they were making changes to make the programming the same on the sub and main spindle. this makes more sence now thank you.