Need Help!- Mori Seiki sl-1A lathe not work with G71

[torro]

My CNC lathe doesn't work with the G71 code. Is there anyone who was able to use the G71 code successfully on MORI SEIKI SL-1A WITH YASNAC LX-1 control or can someone fix my program
%
O1234(0161-0414AAA)
(DF.005R 11/23/2010, 7.30.32 PM)
(MORI LATHE G71/G72 cycles)
N10 G0 G40 G99 M08
G50 T5500 S1500
G97 S1500 M00
T505 M18
(BORE)
G0 X0.2
Z0.013
X0.1314
G71 P100 Q105 U0 W0.003 D0.05 F.005
N100 G94 G1 X-4.4828 Z0.003 F.005
G3 X-4.4376 Z-0.019 I0 K-0.0226
G1 X-4.423 Z-0.437
X-2.8938
G3 X-2.7826 Z-0.492 I0 K-0.0556
G1 X-2.7578 Z-1.202
X0.0312
N105 G0 X0.1314
Z0.013
G70 P100 Q105
G0 X0.2312 Z-1.202
Z0
X0
G0 Z2. M09
G51 M05
M30
%

[dcoupar]

In N100 you have a G94. That's a facing cycle and cannot be in the finish shape definition.

[torro]

I'll try tomorrow and I'll post the results later thanks for helping me.

[dcoupar]

If it's still not working please let us know any alarms, etc. that occur.

[torro]

So, I tried the program and the 93 alarm error went off and i was unable to run the program. The G71 didn't work. It jumped to the N105 and the alarm started.
If somebody was able to use the G71 on the Mori Secki lathe could you share a sample with me.Thanks

[dcoupar]

Originally Posted by torro So, I tried the program and the 93 alarm error went off and i was unable to run the program. The G71 didn't work. It jumped to the N105 and the alarm started. If somebody was able to use the G71 on the Mori Secki lathe could you share a sample with me.Thanks

Did you try it without the G94?

Alarm 093 is unusable G or M code in finish shape program (N100 to N105). As far as I can tell, there are NO M-codes, and only the G94 isn't "usable" in a Multiple Repetitive Cycle.

[torro]

I did try it without the G94 and was unsuccessful. The machine ignores the G71 cycle. It jumps to the N105 and the alarms shows up. We tried to find a sample from other users that way i can try their programs.

[dcoupar]

I'm not sure if this is your problem or not, but the manual states that the move in N100 must be parallel to X axis. You might try the following:

N100 G0 X-4.4828 F.005
G1 Z0.003
G3 X-4.4376 Z-0.019 I0 K-0.0226

[torro]

"I'm not sure if this is your problem or not, but the manual states that the move in N100 must be parallel to X axis. You might try the following:

N100 G0 X-4.4828 F.005
G1 Z0.003
G3 X-4.4376 Z-0.019 I0 K-0.0226"



I looked over the G71 code and saw that I had made a mistake and that you where right. Thanks for your help.

[Waynno]

A trick I have been using for many years on that control

Put a block skip "/" in front of the G71 and offset the tool back a safe distance

Turn on block skip on your panel, run the routine at a safe distance off your work piece

What this does, Will verify it the part program path works and take
the guess work out of Canned cycle vs Code error.

It only adds a few minutes to your set up time, but can save much time
scratching your head trying to figure out exactly where problems are
on new set ups

Lucky, that LX1 control gives you more clues to problems than earlier versions
on the alarm page

One of my favorite errors is forgetting to follow a G2 move with a G1,
After almost 30 years running these, I still sometimes forget to follow a radial move to a linear

Wayne