production run issues w/ ST20-SSY

Hey all, banging my head against my machine over here trying to make multiple parts without have to re-enter a work offset every go around....pretty straight forward, right?

Essentially what I have going is one mill turn project on our live tooling lathe. all i've done is copy-pasted the lot of my program underneath of the original and changed the applicable work offsets from "G54" to "G55". im trying to run 4 parts without opening the door or pressing a button. I get my G54 by touching off, and I subtract my overall material to be taken and trickle it down "G55, 56, 57".

When I run the program it makes the first part, g28, tool change, rapids to where I need it too, and then it throws an error that says my G50 is conflicting with my G96/97. The error is "699 FPU OPERR ERROR":( (attached picture) Im far from an expert in the programming department but my spindle cap DOES NOT interfere with my surface speed.....in fact, i block deleted the G50 all together and still got this issue. If i reset and start from that offset manually then vuala! it runs. but i don't want to manually do that for every. single. part.

When i chase that down in my alarms page it prompts me to remedy the issue in DEBUG...which is way above my head and anybody else in the shop....


so basically, am i trying to mass produce this part incorrectly? is there a resource that explains making multiple parts from the same piece of stock without resetting of the work offset? any help is seriously appreciated
Attachment 264202

You want to make multiple parts from one length of stock before you stop the machine and pull the bar out further? That is what it sounds like.

If this is the case you need to read up on G52 and/or do a custom search here on cnczone for posts mentioning G52 and Haas.

G52 with a Z value simply shifts all your Z offsets that distance. For doing multiple parts from a length of stock you simply make your program into a subprogram and you have a 'main' program which simply sets the G52 value then calls the subprogram which makes the part; something like this:

G52 Z0.(The first part is not shifted)
M97 Pnnnn (nnnn is the line number for the start of the part program when it is a subprogram)
G52 Z-1. (Now G52 shifts evrything Z-1. or whatever your part length plus part off is)
M97 Pnnnn
G52 Z-2. (Shift two part lengths)
etc
etc

Of course I have omitted a lot of stuff but this is the basic concept.

Yes! hit the nail on the head! that answers my questions exactly. Thanks a lot:wave:

Or put your work offset in the main program and take the offset out of your sub.

G54
M97 Pnnnn
G55
M97 Pnnnn
etc.
etc.

I was looking for answers and saw this thread,so I'll share this...When switching from G18 to G17 or visa versa you must redesignate or you'll get the"FPU alarm"
turning =G18 Y axis =G17

I think you want M98 P(program # )L 1 =(loop 1 time)
MAIN PROGRAM M98 P1 L1
M30
O001
(MACHINE PART IN NC CODE)
USE PART PULL
M99

I believe you want G10. I have used it on a ST30-SSY successfully. This won't work on the HAAS Mills, the code is slightly different.


For Lathe:
G10 L2 P1 W-?

L2 - Is for G54 - G59
P1 - G54; P2 - G55; ect....
W = Z Axis Incremental; Z = Z axis Absolute.

G10 L2 P1 W-0.5 (Programmable Offset Setting, Work Origin for G54 - G59, References Work Coordinates for G54, Incremental Shift from current origin Z -0.5)

Haas CNC Lathe G10 Programmable Offset Setting G-Code - Helman CNC