532,233 active members*
3,882 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking Machines > Okuma > Drilling G83 help please!
Results 1 to 9 of 9
  1. #1

    Drilling G83 help please!

    Hi Guys,

    I am trying to run a test part with a drill followed by inside bore, the drill cycle gets the bit to the front face of the piece, then skips to the end of the cycle,
    it then skips the boring cycle, and goes straight to the next cycle.

    Anyone see what i'm doing wrong?#

    (Okuma OSP U10L)

    (DRILL3)
    N103 M1
    N104 T080808
    N105 M8
    N106 G94
    N107 G97 S3000 M3 M42
    N108 G0 X0. Z15.
    N109 Z5.
    N110 G83 X0. Z-38. R0. Q1. P300. F300. L38.
    N111 Z15.
    N112 G97 S3000 M3 M42
    N114 M9
    N115 X200.
    N116 G0 Z200.

    (PROFILE ROUGHING3)
    N117 M1
    N118 T060606
    N119 M8
    N120 G95
    N121 G97 S3000 M3 M41
    N122 G0 X0. Z5.
    N123 G50 S3000
    N124 G96 S200 M3 M41
    N125 G0 Z-1.5
    N126 X13.
    N127 G85 NAT4 D1. U-0.2 W0.1 F0.5
    NAT4 G81
    N128 G0 X23. Z-1.5
    N129 G1 Z-2.
    N130 X22. Z-2.5
    N131 Z-9.
    N132 X14.
    N133 G80
    N134 G0 X0. Z-1.5
    N135 Z5.
    N137 G97 S3000 M3 M41
    N138 M9
    N139 X200.
    N140 G0 Z200.

  2. #2
    Registered
    Join Date
    Nov 2009
    Posts
    11

    Re: Drilling G83 help please!

    Maybe you should try g80 after drilling cycle. But not sure, not much of a okuma-guy

  3. #3

    Re: Drilling G83 help please!

    Thanks for that - G80 got it to go to the IB cycle after, so one prob solved.
    Still not actually running the drilling cycle past getting to X0 Z5

  4. #4
    Member
    Join Date
    Jun 2015
    Posts
    3224

    Re: Drilling G83 help please!

    hy joe, if you wish to customize your post, you need good working codes, so to use them as a reference

    if you wish, i will provide you samples for drilling, id boring and id finishing, and whatever else, general, or on a specific part pls follow this link for the programming manual ( https://we.tl/t-gQmeES0Z25 ), but i recomand you to build your post from a good code, that i will gladly share, then searching portions of code through the manuals, which is time consuming

    it's easier to build from a good code, than sharing and hoping that someone will spot an error; debugging a code is more mind demanding than rewriting it

    in most cases when someone complains about a machine not performing as expected, i always re-write the code / kindly
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  5. #5

    Re: Drilling G83 help please!

    That would be amazing! Im struggling with the Okuma turning post in Fusion spitting out crap code TBH, i have to re-write sections on every program.
    Happy to pay for a re-write too :-)

  6. #6
    Member
    Join Date
    Jun 2015
    Posts
    3224

    Re: Drilling G83 help please!

    ok, tomorrow morning, i will send you some igf generated codes, that are really close to what okuma official codes looks like

    until then, think what you need, maybe share a drawing, demand whatever operations, etc / kindly
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  7. #7
    Member
    Join Date
    Jun 2015
    Posts
    3224

    Re: Drilling G83 help please!

    hy , pls check attached

    there may be required some minimal modifications, since the code is for a newer machine

    really, should be minimal, since okuma codes are tough build, with almost none timeline changes
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  8. #8
    Registered
    Join Date
    Apr 2006
    Posts
    773

    Re: Drilling G83 help please!

    Quote Originally Posted by JoeTall69 View Post
    Hi Guys,

    I am trying to run a test part with a drill followed by inside bore, the drill cycle gets the bit to the front face of the piece, then skips to the end of the cycle,
    it then skips the boring cycle, and goes straight to the next cycle.

    Anyone see what i'm doing wrong?#

    (Okuma OSP U10L)

    (DRILL3)
    N103 M1
    N104 T080808
    N105 M8
    N106 G94
    N107 G97 S3000 M3 M42
    N108 G0 X0. Z15.
    N109 Z5.
    N110 G83 X0. Z-38. R0. Q1. P300. F300. L38.

    Need G0 or G80 here


    N111 Z15.
    N112 G97 S3000 M3 M42
    N114 M9
    N115 X200.
    N116 G0 Z200.

    (PROFILE ROUGHING3)
    N117 M1
    N118 T060606
    N119 M8
    N120 G95
    N121 G97 S3000 M3 M41

    The X value on this line (N122) needs to be your hole size, not the centre of the job.
    N122 G0 X0. Z5.
    N123 G50 S3000
    N124 G96 S200 M3 M41
    N125 G0 Z-1.5
    N126 X13.

    Finish allowances need to be Positive values, not negative values, even for ID operations.
    N127 G85 NAT4 D1. U-0.2 W0.1 F0.5

    NAT4 G81
    N128 G0 X23. Z-1.5
    N129 G1 Z-2.
    N130 X22. Z-2.5
    N131 Z-9.
    N132 X14.
    N133 G80

    X value on here should be the same as on N122,
    Machine will ALWAYS return to the start point on X and Z when ROUGHING, not when finishing though.
    So leaving the X0 here would make the machine return to the roughing start point and then rapid to X0, probably scaring the crap out of the operator.
    N134 G0 X0. Z-1.5
    N135 Z5.
    N137 G97 S3000 M3 M41
    N138 M9
    N139 X200.
    N140 G0 Z200.
    Hope these suggestions help.
    Brian.

  9. #9
    Registered
    Join Date
    Apr 2009
    Posts
    1102

    Re: Drilling G83 help please!

    It looks like the bulk of the post issues are that there is no " cancel commands" after an operation, ie; G00 or G80 when finished. Get the post fixed using the IGF code kitty sent as a reference and you'll save yourself a lot of time and effort.

    Broby did a nice job explaining where things went wrong for you. (he always does, so trust him...)

    Start points and reference points are very important to the Okuma control. They determine what direction a roughing cycle is going and where the depth of cut starts from, so pay attention when choosing them. Clearances are also determined by them inside a canned cycle, so you want to be sure they are in the right places. For example when turning an OD, your reference point should be > or = your start point in Z and definitely < in X. If the Z is = it will rapid down, but if it is not and is < then it will feed down.

    BTW you do not need to go to G94 for drilling (or live tooling) if you do not want to. The control can feed in IPR using the spindle or live tool rpm for the calculation.

    Best regards,
    Experience is what you get just after you needed it.

Similar Threads

  1. solidcam naming drilling geometry to drilling radius automatically
    By allenp in forum SolidCAM for SolidWorks and SolidCAM for Inventor
    Replies: 0
    Last Post: 09-07-2015, 07:04 AM
  2. Drilling using a Gun Drilling tool on HBM
    By SatishNaik in forum Videos
    Replies: 0
    Last Post: 06-02-2014, 11:23 AM
  3. G87 wrap drilling or cross drilling
    By Drake75 in forum G-Code Programing
    Replies: 2
    Last Post: 05-14-2013, 02:30 PM
  4. Spot Drilling/Center Drilling Steel 55 HRC
    By JWB_Machining in forum General MetalWork Discussion
    Replies: 7
    Last Post: 03-11-2009, 07:35 PM
  5. drilling and drilling cycles tutorial
    By wmorre in forum General MetalWork Discussion
    Replies: 0
    Last Post: 10-19-2006, 12:30 AM

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
  •