Program problems with my lathe....

[Josh-PTP]

Hey guys,

I am having a little problem with a tool nose radius program on my lathe. The tools radius is .031" Here is the part of the program that is giving me problems. Thanks for any help.......



N1
M98P1
T0101(80 DIAMOND)
G97S800M13
G00X1.55Z.1
G50S2500
G96S600
G42X1.45Z.05
G99
G71U.05R.015
G71P100Q200U.03W.01F.005
N100G0X0.
G01G99Z0.F.005
X1.191,R.03
X1.375Z-.875
Z-1.0
X1.4
N200G0X1.45
G70P100Q200
M98P1



Thanks for any help........

[Geof]

I think G71 will not use Tool Compensation. But I think the finish pass G70 does. Somewhere I read that you have to make U and W in the G71 a bit bigger than your tool nose radius so there will be something to clean up with the G70.

You can check it in graphics by stepping through.

Another thing that will give trouble is if you don't have the correct Tip # based on the tool position. There is a section in the manual explaining it.

[Wiseco]

You must put your G42 in the motion of the canned cycle.

Example
G71 P100 Q200 U0.062 W0.005 D.1 F.01
N100 G42 G0 X0. Z.05
G01 Z0. F.005
X1.191,R.03
X1.375Z-.875
Z-1.0
X1.4
N200 G40 G0 X1.45

Try this.

Oh and I think you have some error in your code. Here it should work :

N1
M98 P1
T0101(80 DIAMOND)
(Initialization)
G40 G20 G80 G99
G97 S800M03
G00 X1.55 Z.1
G50 S2500
G96 S600
X1.45 Z.05
(G71U.05R.015 = ?)
G71 P100 Q200 U0.062 W0.005 D.1 F.01
N100 G42 G0 X0. Z.05
G01 Z0. F.005
X1.191 R.03
X1.375 Z-.875
Z-1.0
X1.4
N200 G40 G0 X1.45
G96 S1200 (Raising speed for finish cycle)
G70 P100 Q200
M98 P1

[Geof]

He is using a Fanuc control. See this thread:

http://www.cnczone.com/forums/showthread.php?t=39809

[njhaasman]

If you're looking for a corner break on the front of your part, I believe that the R.03 value needs to be negative (R-.03).