554,328 active members*
3,044 visitors online*
Register for free
Login
IndustryArena Forum > Machine Controllers Software and Solutions > G-Code Programing > Thread milling with G92 using subroutine on X0Y0
Results 1 to 4 of 4
  1. #1
    Registered
    Join Date
    Aug 2005
    Posts
    120

    Thread milling with G92 using subroutine on X0Y0

    Hi. Weve been using thread mills on stainless happily. We use the subroutines generated by the manufacturer's website. Their subroutines are created with X0Y0 being the hole location with absolute depths and circular G91 moves.

    So, in the "office programming system" we just move to a point over the hole and put in a "manual entry" to call the manufacturer's subroutine to thread the hole. This worked great on older Mazak machines (M2) but not on the newer Mazak (M-Plus). On the old machine G54 CANCELLED G92, allowing us to move to the next hole and repeat the process, but on the newer one the G92 stays active, as other posts here have said, despite the G54 being there.

    Thoughts? I'd really just like a way to program (from the office) to position to a hole and run the thread sub. If all else fails we're going to make the depth moves G91s also and eliminate the G92.

    OLD CODE
    G54
    (hole 1)
    G90 G0 X5.0 Y3.0
    G92 X0 Y0
    G65 P1420 (sub threads on x0y0)
    G54
    (hole 2)
    G90 G0 X7.0 Y3.0
    G92 X0 Y0
    G65 P1420 (sub threads on x0y0)
    G54

  2. #2
    Member
    Join Date
    Jan 2005
    Posts
    14310

    Re: Thread milling with G92 using subroutine on X0Y0

    Quote Originally Posted by underdog View Post
    Hi. Weve been using thread mills on stainless happily. We use the subroutines generated by the manufacturer's website. Their subroutines are created with X0Y0 being the hole location with absolute depths and circular G91 moves.

    So, in the "office programming system" we just move to a point over the hole and put in a "manual entry" to call the manufacturer's subroutine to thread the hole. This worked great on older Mazak machines (M2) but not on the newer Mazak (M-Plus). On the old machine G54 CANCELLED G92, allowing us to move to the next hole and repeat the process, but on the newer one the G92 stays active, as other posts here have said, despite the G54 being there.

    Thoughts? I'd really just like a way to program (from the office) to position to a hole and run the thread sub. If all else fails we're going to make the depth moves G91s also and eliminate the G92.

    OLD CODE
    G54
    (hole 1)
    G90 G0 X5.0 Y3.0
    G92 X0 Y0 (Remove if not needed)
    G65 P1420 (sub threads on x0y0)
    G54
    (hole 2)
    G90 G0 X7.0 Y3.0
    G92 X0 Y0 (Remove if not needed)
    G65 P1420 (sub threads on x0y0)
    G54
    Why are you using the G92 X0Y0

    Is the G0 X5.0Y3.0 move to the center of the hole, if so then G92X0Y0 on each line is not needed

    A G54 does not cancel anything, you only need the G54 at the start of the program
    Mactec54

  3. #3

    Re: Thread milling with G92 using subroutine on X0Y0

    Yes... why G92? Below is a visual representation of what I and Mactec are saying

    This is all the code you need to thread mill your holes on about any machine. Once again we witness a post processor putting out junk.

    As I understand it, your sub uses absolute Z moves to start and stop and incremental moves while machining the thread. Sounds perfect.

    G54G90
    (hole 1)
    G0 X5.0 Y3.0
    G65 P1420
    (hole 2)
    G0 X7.0 Y3.0 (If your sub ends with a G0 retract to clearance plane, you do even need the G0 here)
    G65 P1420

  4. #4
    Registered
    Join Date
    Aug 2005
    Posts
    120

    Re: Thread milling with G92 using subroutine on X0Y0

    Mactec54 and The_Gentlegiant,

    I do see your point now that the G92 is not needed. I guess I was just trying to zero the coordinate system so the sub wouldn't run away on me, but the XY moves are incremental.

    Good observations. Thanks! (I may edit the sub a bit more since the absolute z moves in the sub mean you can only thread mill if the hole is on z zero.)

    Sorry for the late reply. Just got thru that job back in March and now we're back on thread milling again!

Similar Threads

  1. G92 Taper Thread I or R ?
    By ashisroy in forum G-Code Programing
    Replies: 1
    Last Post: 05-10-2017, 05:04 AM
  2. G92 thread cycle
    By AE81 in forum CNC Swiss Screw Machines
    Replies: 2
    Last Post: 02-22-2017, 07:16 PM
  3. cnc pocket milling subroutine problem
    By RTC_CNC_STUDENT in forum Fadal
    Replies: 1
    Last Post: 10-14-2014, 10:58 PM
  4. How to change thread indexing with G92
    By daz59 in forum G-Code Programing
    Replies: 16
    Last Post: 11-19-2012, 09:17 AM
  5. Found in archives - A2100 thread mill subroutine
    By Ron P in forum Cincinnati CNC
    Replies: 2
    Last Post: 05-17-2011, 02:38 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
  •