Need Help!- programming multiple parts from lathe bar

[metalmansteve]

I want to slice multiple rings from a tube. (face, chamfer, part-off) 5-10 per cycle using the counter on my lathe.

How do I program an incremental z-move after M99 that returns to it's origin after x many parts?


This should be easy!

?????

[BlueChip]

The best way .. IMHO ... would be to use sub-programming. Since you didn't mention the make of lathe nor control ... I'll assume it's a Fanuc ( 80%-90% ) of machines use it ... or "fanuc compatible".

Format is either :
M98 Pxxxx Lyy
where M98 is the call ... P is the O program to run and L is the number of times.
or M98 PxxxYYYY
where
xxx is the number of times and YYYY is the O program number to run.


So ........ you could do something like this :

Main Program :
O0001
M98 P1234 L5 ( run program O1234 ... 5 times )
G00 W( 5 x "cccc" dimension )
( any W move is an incremental move in the Z axis )
( any U is an incremental move in the X axis )
M30
%

Sub Program :
O1234
N0001
G96 S325 M03
G00 T0101
***********
make the part complete
***********
G00 W-cccc
( incremental move in the Z axis )
( the amount to move up for each cycle ... part length removed )
M99 ( return from sub to the main to the line after it left )
%

In the above ... the sub program will loop the L number of times and since their is an incremental move at the end ... each time it will move up that amount and start again.

Depending on how you have your work / geometry offset's set ... you may encounter other issues ....

.... but that's a whole nuther message.

Post your results and I'm sure someone will have some inputs.

Real World Machine Shop Software at
www.KentechInc.com

[HuFlungDung]

I used to do it similar to what Blue Chip described, except after the G0 W movement increment to the new start position, I'd use G92 Z.zzzz to reposition the Z work datum at this new location.

Knowing that G92 is anathema nowadays , one could also move the Z datum by using G10 to change the G54Z value on the fly. G10 can also be commanded incrementally.

[Geof]

As suggested make the part program a subprogram and call this subprogram multiple times, moving your work zero forward for each call. You can use G92 if you want to live dangerously, or you can use G52 to set a local work coordinate or you can use a series of G10 to set G55, G56, etc.

[HuFlungDung]

Oh, I should clarify that I tend to work in gcode system 3 (mill) so G92 crosses to G50 on some lathes.

I never understood the need for two different gcode systems and I've always stuck with "mill" type gcodes.

[metalmansteve]

Thank for the help gentlemen. I wish i had some good feedback but my operator just programmed 5 pieces 'long hand' and had the job running before I got back to him. I will use this next time....

thanks again.