Haas Fanuc-style G71 - G76 cycles...

[dcoupar]

Anyone ever used 2-line Fanuc-style multiple repetitive cycles (G71 - G76) on a Haas lathe? I've run into a customer who swears up and down they work, and what's more, he uses 2-line and 1-line cycles in the same program! I'm wondering if this is a common practice???

G72 Unnnn Rnnnn
G72 P101 Q102 Unnnn Wnnnn Fnnnn Snnnn
N101
...
...
...
N102
G71 P103 Q104 Unnnn Wnnnn Dnnnn Fnnnn Snnnn
N103
...
...
...
N104
M30

[rossmkly]

note the skip lines in the first example ... when program is ran with skip off ir will run the g71 cycle ... with skip (block delete) on it will only run the finish pass ... this is a big time saver when setting up. Method would be to offset x up double the finish allowance (.05X2=.100) run once with skip off, then program out the taper ... run the second time with skip on checking for taper correction. If the there is no taper offset down to make the tool cut to the correct print dimention ... if the tool setting was correct this will be another .05 or so depending on tool pressure. Run the cycle for the third time again with skip on and you should have a correct part. Note again thet the second and third time the cycle is ran it only takes a finish pass exactly like it would in the G70 line.

(80 DEG)

N100
T303
G00G40
G50S2800M08
G96S280M03
G00X0.75Z1.
G41Z0.
G01X-0.06F0.005
Z0.05
G00G40X0.715Z0.15
/G71U0.06R0.03
/G71P101Q102U0.05W0.002S280F0.008
N101G00X0.21
G42Z0.1
G01X0.52Z-0.06F0.006
X0.53Z-0.41
Z-0.495
N102X0.8
/G70P101Q102
G00G40Z5.M09
T300
M01
M31
(80 DEG. O.D. TOOL)
N100
T303
G00G40
G50S1200M08
G96S600M03
G00X6.65Z1.
Z0.16
/G72W0.04R0.03
/G72P101Q102U0.W0.04S600F0.01
N101G00G41Z0S900
G01X1.F0.006
N102Z0.16
/G70P101Q102
G00G40X6.65Z0.15
/G71U0.1R0.03
/G71P103Q104U0.1W0.002S900F0.01
N103G00X5.899S900
G42Z0.1
G01Z0.F0.006
G03X5.999Z-0.05R0.05
G01Z-0.95
N104X6.65
/G70P103Q104
G00G40Z1.M09
G00Z10.
T300
M01


single line format type II

(ROUGH GROOVE WAM.015R STRIGHT TOOL)
N300
G28 U0
T505
G54 G50 S1000
G97 M03 S500
G96 S400
/ M08
G00 X1.66 Z-0.19
G71 P301 Q302 D0.01 U0.005 W0.002 F0.002
N301 G01 G42 Z-0.2049 X1.5748 F0.009
X1.545 Z-0.2285 F0.002
G02 X1.4355 Z-0.31 R0.088
G02 X1.545 Z-0.3915 R0.088
G01 X1.5748 Z-0.4151
X1.65
N302 G40 X1.75 F0.02
G00 Z3. X3.
G28 U0
T500 M01


N101 (ROUGH O.D.)
N102 G28 (Return to Machine Home reference point)
N103 T101 (55 Deg. O.D. TOOL x .0312 TNR)(Select tool 1, offset 1)
N104 G50 S2500
N105 G97 S591 M03
N106 G54 G00 X2.1 Z0.1 M08 (Rapid to start point)
N107 G96 S325
N108 Z0.005
N109 G01 X-0.063 F0.01
N110 G00 X2.1 Z0.1
N111 G71 P112 Q124 U0.02 W0.005 D0.1 F0.012 (Rough P to Q using G71 and TNC)
(Define part path PQ sequence)
N112 G42 G00 X0.55 Z0.1 (P) (G71 Type II, TNC approach)
N113 G01 Z0. F0.004
N114 X0.65
N115 X0.75 Z-0.05
N116 Z-0.75
N117 G02 X1.25 Z-1. R0.25
N118 G01 Z-1.5
N119 Z-1.72 X1. F0.006
N120 G01 Z-2.5
N121 G02 X1.25 Z-2.625 R0.125
N122 G01 Z-3.5 F0.004
N123 X2. Z-3.75 F0.008
N124 G40 G00 X2.1 (Cancel TNC Departure move)
N125 G97 S591
N126 M09
N127 G28 (Return to Machine Home reference point)
N128 M01

[dcoupar]

So... your're saying you DO run single-line and double-line roughing cycles in the same program?