Offsetting sub programs (Mitsu M50, Daewoo lathe)

[Chuck Reamer]

I have never used sub programs on a lathe before, and I want to use it on the lathe.

I am making a bunch of thin plastic seals out of a Teflon tube, I want to run 5 then dig them out of the chips.

The sub call up works perfectly, but just cuts air over the same spot. What code is best for offsetting my G54 z-.31 with each pass?

I have been looking at G10, but am not very familiar with it. I know a lot of you must be running subs and know a fix for my little problem.

I have never used a Mitsu before (fanuc about 6 years ago) and haven't done any lathe programing in about 16 months.

[cnc-king]

you can try G10 L2 P1 W-.31 after every part off, this should shift your G54 incrementaly -.31 after every part
At the end of your 5 pc run insert G10 L2 P1 W1.55 which sets your G54 Z coordinates to the original #
Or you can use G10 L2 P1 Z****** This Z value should be your original
G54 Z coordinate.

or the other format
M98P####
G10 L2 P1 W-.31
M98P####
G10 L2 P1 W-.31
M98P####
G10 L2 P1 W-.31
M98P####
G10 L2 P1 W-.31
M98P####
G10 L2 P1 W-.31
M98P####
G10 L2 P1 W1.55



lots of CNC machinist do not like to use G10's to set offset, they think it's evil, one of the main reason for that is understanding the concept, once G10's is understood it becomes a powerful too to register tool and work offsets.

my 2 cents

[Chuck Reamer]

Thanks for the help, I ended up putting G10 L2 P2 W-.310 on the second last line line of the sub program right before the M99.

Now depending on how much length I have left I just change the L value in the G98 to how ever many pieces that I have. It works like a charm.

Can I use a G10L2p1UXX.XX to change all the diameters and create a larger seal of the same profile without having to write a new program?

G10 is the best thing since solid carbide, as far as I am concerned.

[CNCRim]

Originally Posted by Chuck Reamer Can I use a G10L2p1UXX.XX to change all the diameters and create a larger seal of the same profile without having to write a new program?

I think you will have trouble with the drill....... it's not design to drill off center of rotation. You best bet is check see your machine has macro option. However, you can twist certain way, and it should work.


G10L2P1Uxxxx
M98P####
G10L2P1U-xxxx

[Chuck Reamer]

Originally Posted by newtexas2006 I think you will have trouble with the drill....... it's not design to drill off center of rotation. You best bet is check see your machine has macro option. However, you can twist certain way, and it should work. G10L2P1Uxxxx M98P#### G10L2P1U-xxxx

It is tube stock, there is no drill cycle. I will try to figure out if I have macros or not. Never even known anyone who uses them befor, but I am always up for a challange.