[ReacerX427]

I'm trying to prep some stock for a job that I need to run on an Ikegai Genesis 1210 CNC lathe w/Fanuc 21i-T control. The stock is square and I want to make it round so I can grab it in the chuck. The part is too long for the machine so I need to enter the stock on a taper. But whatever I try, it either will not do it (alarm) or it will do the first pass and then go straight to finish numbers. Any insight would be greatly appreciated. The program is a follows:

G28 U0
G28 W0
T0101
G50 S1400
G96 S300 M03
G0 X3. Z.1 M08
G71 U.05 R.01
G71 P10 Q20 U.005 W0 F.02
N10 G42 G1 X2.85 Z.1
Z0
X1.6 Z-1.3403
Z-19.5
X1.7
N20 G40 G1 X1.75
G0 X3.0 Z.1
G70 P10 Q20 F.003
G0 X3.0 Z.1 M09
G28 U0
G28 W0
M30

[fordav11]

I suspect your problem is the G40 needs to be outside the cycle (specifically, it should go below the G70 line)
But if you are just roughing it round remove the G42/G40 altogether to simplify it.

[ReacerX427]

I tried that. Tried with X and Z on same line, X and W0, with cutter comp, no cutter comp. Still get the same error. Couldn't afford to waste anymore time so I had to go "old school" and wrote it point to point. More writing/typing, but I am finally making chips. I think that the problem lies within the controller itself. That option might not be turned on. It would be weird if it isn't, but I did have to get Fanuc out before to turn on some other options (Drill cycles). Will do a little more investigating come Monday and we'll see where it leads. Will post if I get an answer.

[fordav11]

the official description of the error is.....
065 ILLEGAL COMMAND IN G71–G73
(T series)
1. G00 or G01 is not commanded at the block with the sequence
number which is specified by address P in G71, G72, or G73
command.
2. Address Z(W) or X(U) was commanded in the block with a
sequence number which is specified by address P in G71 or G72,
respectively.

the #1 check is ok because you have a G1 on line N10
the #2 check fails because you have X and Z on line N10. meaning your machine can't use Type II cycles (its an option).
If you change line N10 G42 G1 X2.85 Z.1 to N10 G1 X2.85 it should work (omit the G42 for simplicity)
if it doesn't work then you possibly don't even have Type I cycles option.
in your previous post you said you tried X and Z then X and W. both of those are illegal if you dont have Type II cycles option.
Just use an X on line N10 and it'll work.

[ReacerX427]

Unfortunately it doesn't. I did try that and numerous other combinations. Nothing worked. So I believe that the machine doesn't have that option. Which really ticks me off. I will be call Fanuc today and hopefully they will be able to shed some light on the situation. Can't understand why this would be an option, but like I stated in an earlier post, Fanuc had to come out before and turn on other "options".

[ReacerX427]

Well the verdict is in................................................ ...........and the answer is that we DO NOT have that option in the control!!!! So we must buy that option or continue to "old school" it, with point to point programming. Not looking forward to doing that, since the next job is a little complicated and I need that option for that job. Can't wait to see what the cost will be either!! LOL LOL But you got to do what you go to do to make the job. Thanks again!!

[fordav11]

I'll send you a PM.....