Need Help! Custom drilling cycle


Results 1 to 5 of 5

Thread: Custom drilling cycle

  1. #1
    Member
    Join Date
    Jan 2010
    Location
    Norway
    Posts
    171
    Downloads
    0
    Uploads
    0

    Default Custom drilling cycle

    Hi

    So i have created my own drilling cycle and instead of using G66 Pxxxx i want to use G810.
    My issue is that it wont excecute the cycle on the next hole.
    Example
    G810 x10y0 <-- this one works
    x20y0 <- no cycle here
    G80 <-- also not sure if G80 would work?

    What do i need to put in the sub program? And is this even possible?

    Similar Threads:


  2. #2
    Member dcoupar's Avatar
    Join Date
    Mar 2003
    Location
    USA
    Posts
    2932
    Downloads
    0
    Uploads
    0

    Default Re: Custom drilling cycle

    What model Fanuc is this for?

    According to the Fanuc Mill operator's manual (0i-B/C) macros called by G-codes are simple only (G65), not modal (G66). I assume this holds true throughout other models.



  3. #3
    Member
    Join Date
    Jan 2010
    Location
    Norway
    Posts
    171
    Downloads
    0
    Uploads
    0

    Default Re: Custom drilling cycle

    Quote Originally Posted by dcoupar View Post
    What model Fanuc is this for?

    According to the Fanuc Mill operator's manual (0i-B/C) macros called by G-codes are simple only (G65), not modal (G66). I assume this holds true throughout other models.
    This is for 31i, i was thinking of maybe putting G66 inside the macro? But i'm not sure if this will work.



  4. #4
    Member dcoupar's Avatar
    Join Date
    Mar 2003
    Location
    USA
    Posts
    2932
    Downloads
    0
    Uploads
    0

    Default Re: Custom drilling cycle

    It appears that Fanuc has included the ability to call modal macros from G-codes on the 31i (see attached)

    Attached Thumbnails Attached Thumbnails Custom drilling cycle-f31i-custom-macro-call-using-g-code  


  5. #5
    Member
    Join Date
    Jan 2010
    Location
    Norway
    Posts
    171
    Downloads
    0
    Uploads
    0

    Default Re: Custom drilling cycle

    Thank you that worked
    However it gave me another issue, when going to the next coordinate it doesn't remember the values, so i put them all in other variables and i will skip adding them again when moving to the next coordinate, but i if i wanna change depth of the next hole this doesn't really work. Any suggestions?
    In time i will add some pecking options to it


    O9810(LONGDRILL-CYCLE)
    (G810 R5 Z-150. E50 F230 S800)
    (R=SAFETY PLANE)
    (Z=DEPTH)
    (E=PREDRILL POINT)
    IF[#7 EQ 80]GOTO9999
    IF[#120 EQ 1]GOTO10
    #120=1(FIRST TIME CALL)
    #111=#5003(CURRENT Z)
    #110=#4119(CURRENT S)
    #100=#18(R)
    #101=#19(S)
    #102=#9(F)
    #103=#8(E)
    #104=#26(Z)
    IF[#8LT20]THEN#3000=1(-E-MUST-BE-BIGGER-THAN 20)
    IF[#110LT1]THEN#3000=1(NEED SOME SPEED WHILE ENGAGING)
    N10
    S#110M3
    G0Z#100
    G1Z[#100-#103+5]F500
    M88(COOLANT ON)
    G04X0.2
    S[#101/2]
    G1Z[#100-#103-10]F[#102/2]
    G1Z[#5003+0.2]
    S#101
    G4X0.5
    G1Z#104F#102
    G1Z[#5003+0.2]
    G4X0.5
    S#110M3
    M89(COOLANT OFF)
    Z#100F1000
    G0Z#111
    M99
    N9999
    #199=0
    G67
    %



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
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Custom drilling cycle

Custom drilling cycle