Type II G71 Stock Removal on Fanuc 0i-TB

[lowehardware]

I am turning 1.125" bar stock in to a 1" sphere with 270 degree arc swing. I keep getting an alarm 041 overcutting due to the tool nose radius compensation. Please help!!! The code is below: (This is using Type II G71 as you can tell by the repeated Z move in the startup block. Also, tool nose radius is .0312 in the 3 imaginary tool nose)

G0T0404(TURNING TOOL)
G96S650M03
G0X1.145Z0.
G1X-0.05F.004M08
G0X1.125 Z0.05
G71U.06R.02
G71P101Q201U.01W0F.006
N101G0G42X0.Z.05
G1Z0.F.003
G03 X0.7071 Z-0.8536 R0.5
G01 X1.125
N201G0G40Z0.05
G70P101Q201
G80M09

[SeymourDumore]

Without going deeper into the code and geometric accuracy, I think your Q block is incorrectly placed.

G00 T404 (TURNING TOOL)
G96 S650 M03
G00 X1.145Z0.
G01 X-0.05 F.004 M08
G00 X1.125 Z0.05
G71 U.06 R.02
G71 P101 Q201 U.01 W0 F.006
N101 G00 G42 X0. Z.05
G01 Z0. F.003
G03 X0.7071 Z-0.8536 R0.5
N201 G01 G40 X1.125 <---- N201 moved to here.
G00 Z0.05
G70 P101 Q201
G80 M09

Actually sort of surprized that you're not getting a "Non Monotonous" error.
In TypeII roughing your X may vary in the + or - direction, but your Z must still be monotonous either + or - direction. That N201 sent it back to Z.05 withing the cycle.
Now, depending on the control itself, you may still get an overcut at the back. Note that your G03 ends at Z-.8536, and then you move only up in X.
The way I've changed your code would probably overcut on the Haas, because in this block:
G01 G40 X1.125 would move the tool in the Z direction by +.0312 as well.
I'm pretty sure Fanuc does the same thing, or perhaps worse by moving by 2X tool R in the +Z direction.
So, the way I'd do this cycle is to make a clearance move at the back of the radius, perhaps a little more than your tool R.

G00 T404 (TURNING TOOL)
G96 S650 M03
G00 X1.145Z0.
G01 X-0.05 F.004 M08
G00 G42 X1.125 Z0.05 <--- Note the comp-on BEFORE the cycle
G71 U.06 R.02
G71 P101 Q201 U.01 W0 F.006
N101 G00 X0. Z.05
G01 Z0. F.003
G03 X0.7071 Z-0.8536 R0.5
G01 Z-.8856
N201 G01 X1.125
G70 P101 Q201
G00 G40 X1.125 Z.05 <--- Ramp-off move here.
G80 M09

Please note that the code may not be all kosher. I never use G70 due to all the minor radiuses and edgebreaks during the finish pass, but with G71 or G72 I always comp-on prior to, and comp-off after the cycle. Better control over exact tool position at each step.