[cogsman1]

Your code was not too bad to start with but you are turning on comp with a move in the wrong direction. Try this.


G0T0404(TURNING TOOL)
G96S650M03
G0X1.145Z0.
G1X-0.05F.004M08
G0X1.125 Z0.1 (*********)
G71U.06R.02
G71P101Q201U.01W0F.006
N101G0X0 (*********)
Z.05 (*******)
G01G42Z0F.003 (********)
G03 X0.7071 Z-0.8536 R0.5
G01 X1.125
N201G0G40Z0.05
G70P101Q201
G80M09

[lowehardware]

is that even Type II? in the N101 line you have to specify Z0.1 (where the tool starts) Correct?

[SeymourDumore]

Actually it doesn't matter where you turn on that comp. IN fact I'd suppose that cogsman's method won't even work in this instance, as the toolR is .0312 and the move from Z.05 to Z0 is less than the .062 required, and would likely cause overcut on Fanuc OR "Tool too big" error on Haas.

lowehardware
The next time you get this or similar part where you're forming a sphere, see if you can re-define your tool to be Dir8 rather than Dir3.
The really cool thing about it is that it truly uses the tool as it was a ball forming a ball, and you can dial in OD and sphericity variations easily.
Also, your comp-on and off moves become easier to manage, as you can plunge-in and retract in a straight move in front and back of the ball.
You can use the same tool as right now, all you have to do is add -.0312 to your Z offset and change the tool definition to 8.
I do turn a decent amount of balls, and this method gives me straight plunges for roughing and finishing, AND I can dial in the part to be spherical within .0002.

[cogsman1]

I have used this format on both types and it works perfectly. You do NOT have to start twice the radius away that is a very old myth. The moves I have from the rapid (Z.1) before the N101 followed by the (Z.05) after entering the cann cycle will allow the machine to see which direction you are coming from and will work. I used to cut ball valves +/-.0003 and learned this method works no matter what machine(Lathe) I was using. Mori, Mazak, Nakamura, Tsugami, Citizen, Hitachi, and more. Some of these use different codes for their rough cycles but once in the cycle, this format is flawless. Some don't need the extra moves but all accept it.

[SeymourDumore]

Agreed on the comp-on move.
For some reason I was stuck on that you've ramped in the N101 block at Z.05 as Lowe's original code. That would in fact would have put the tool to Z-.012 after the N101 block.

Quote from original post:
"""
G0 X1.125 Z0.05
G71 U.06 R.02
G71 P101 Q201 U.01 W0F.006
N101 G0 G42 X0. Z.05
"""

Nonetheless, you've still got a return move inthe N102 block, which is not allowed even in Type II roughing. Your Z has changed fromZ-.8536 to Z.05, thereby changing direction from negative to positive.
Not happening on Fanuc Oi-Tc or on Haas.

[cogsman1]

I spent some time checking as many of my proven programs as I could for the different machines. The only difference I found was on a couple I had to cancel comp BEFORE the N102 ending line, but everyone always ends with the retract to the starting point off the face. I remember having an issue if I tried to retract to a position that was NOT the exact same as the starting position. This would be the position BEFORE the "G71" line.

[SeymourDumore]

Interesting.
Unfortunately I cannot copy/paste from teh Fanuc Oi-TC manual, so I'll just quote a segment from Page 145, which describes TypeII roughing:

"""
Note that, however, the profile must have monotone decrease or increase along the Z axis.
"""

This is word for word.

I know for a fact that the Haas would complain and not run with the return, but I'll check it out on the Mori sometime this weekend.
I do know that I never did send the tool back, as the cycle itself does that automatically in every case. In fact I don't even program a clearance move after the cycle and before a toolchange, knowing that the tool will be in the clear no matter what.