Need Help!- G71 taper turning - why alarming out?

[bullandbladder]

System is OT, will allow taper to get bigger towards the chuck (ie Z- direction), when turning o/d with G71, but will not allow a minus taper. This works in the opposite way when boring. Alarm shown is 064, "shape program not monotonously". Now I know I've been able to do this on machines I've worked in the past, but this one doesn't seem to like it. I'm guessing this is a kind of interference check, set by a parameter - any ideas, anyone?

[Geof]

You want Type II roughing, on some machines it depends whether your P line has a single axis move or two axes to select between Type I and Type II roughing. If you are already moving both X and Z on the P line then I don't have any other suggestions.

[newc]

The only way I can see you doing this is to start your cut at the chuck, and work out. The only problem is that each plunging cut at the chuck end will be at roughing speed.
Have you thought about using G73 (pattern repeat)?

[SanDiegoCNC]

Originally Posted by bullandbladder System is OT, will allow taper to get bigger towards the chuck (ie Z- direction), when turning o/d with G71, but will not allow a minus taper. This works in the opposite way when boring. Alarm shown is 064, "shape program not monotonously". Now I know I've been able to do this on machines I've worked in the past, but this one doesn't seem to like it. I'm guessing this is a kind of interference check, set by a parameter - any ideas, anyone?

Some machines don't like it when the lap cycle has a negative geometry in the part profile. Two ways to get around this problem; 1. keep the profile the same diameter and then make a separate pass outside the lap to cut the taper, or 2. adjust the program to allow it to taper in the positive direction. That means editing the program to make the first diameter smaller and then compensate for it in the offset page.