[Michael82]

We just bought a Hwacheon hi-tech 200 B it has a Fanuc oi-TD series control, this is the 1st time this machine has cut any single point thread, while it has done some tapping as a matter of fact that is all this machine has even done is face, drill, bore, and tap. We are trying to cut a 1/2" -14 npt internal thread using G76 canned threading cycle , we brought over a program that has been proven on a Doosan Puma 300 and loaded it into the Hi-tech 200 and we keep getting alarm PS0317 ( Illegal thread command is in the thread cutting cycle ) when it reads the 2nd G76 line, I have changed every single variable in both G76 lines with no success and like I said this is a proven program from another machine that is running Fanuc i-series controls. I listed the program below, but I am thinking there is maybe a parameter that has not been setup and it is making this alarm. Does anyone have the parameter list that is associated with G76 threading, I have all the parameters, but I need to know what parameters the G76 canned cycle uses so I can check them to make sure they are set right?

n2 (SIR 0500 M16B threading bar with 16IR AG 60 IC250 insert )

G0 T0606

G97 S300 M3

G0 G54 X.5721 Z.2253

G76 P010029 Q20 R20

G76 X.8412 Z-.88 P571 Q100 R.0336 F.07143

G0 Z.2253

G28 U0. W0. M5

T0600

M1

[memoryman]

The control may not have that option enabled.

[Michael82]

I found the problem the difference from this series fanuc and the doosan is the on the 1st g76 line the r value needed a . So ( R.002 ) rather than R20

[Kassit]

Thank you. Solved my problem too. Started having this issue when they disabled the need for. For measurements. So in the g76 the second g76 line doesn't want. On the p or q but on the 1st g76 line the r value wants it.

Tldr if your machine doesn't need (.) the 1st line r needs it to function.