502,743 active members
4,799 visitors online
Register for free
IndustryArena Forum > MetalWorking Machines > Haas Lathes > production run issues w/ ST20-SSY
Results 1 to 7 of 7
  1. #1
    Join Date
    Oct 2014

    Exclamation 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

  2. #2
    Gold Member
    Join Date
    Jul 2005

    Re: production run issues w/ ST20-SSY

    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)

    Of course I have omitted a lot of stuff but this is the basic concept.
    An open mind is a virtue...so long as all the common sense has not leaked out.

  3. #3
    Join Date
    Oct 2014

    Re: production run issues w/ ST20-SSY

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

  4. #4
    Join Date
    May 2013

    Re: production run issues w/ ST20-SSY

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

    M97 Pnnnn
    M97 Pnnnn

  5. #5

    Re: production run issues w/ ST20-SSY

    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

  6. #6

    Re: production run issues w/ ST20-SSY

    I think you want M98 P(program # )L 1 =(loop 1 time)

  7. #7
    Join Date
    Aug 2015

    Re: production run issues w/ ST20-SSY

    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

Similar Threads

  1. ST20 rigid tapping
    By Snoopy_One in forum Haas Lathes
    Replies: 17
    Last Post: 12-11-2012, 12:40 AM
  2. Bar Feeder for ST20 SSY
    By manike in forum Haas Lathes
    Replies: 4
    Last Post: 11-20-2012, 03:46 PM
  3. views on the st20 please
    By daleman in forum Haas Lathes
    Replies: 2
    Last Post: 08-31-2012, 07:01 PM
  4. ST20 drills off offcenter
    By BryanDavid in forum Haas Lathes
    Replies: 4
    Last Post: 09-26-2011, 08:47 PM
  5. new ST20 any opinions??
    By gixxergary in forum Haas Lathes
    Replies: 8
    Last Post: 05-11-2011, 09:10 PM

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts