Results 1 to 12 of 12
  1. #1
    DMitchell is offline Junior Member
    Join Date
    Apr 2004
    Location
    Daytona Beach, FL, USA
    Posts
    6

    Default

    I'm trying to learn to program a Okuma CNC Lathe and am having difficulty with a aspect of the program. I'm trying to use G85 to cut a bore but the machine wants to rapid into the part and feed out instead of doing just the opposite. Here is my code, please let me know when is wrong with it. I'm learning from the book and it just isn't helping me.

    N8 G0 X30. Z20.
    T080808 S1500 M4 M8
    G96 S1500 X2. Z.25
    NBORE G81
    G0 X2.025Z-1.3
    G1 X2.89 F.008
    Z-1.05
    X3.24 Z-.88
    X6.485
    Z-.05
    G2 X6.585 Z0 L.05
    G1 X8.725
    G80
    G85 NBORE D.25 F.01 U.02 W.005
    G0 Z.25
    X2.
    G87 NBORE
    G0 Z.25

  2. #2
    Cheenist is offline Hot Rolled
    Join Date
    Feb 2004
    Location
    Alexandria Va. USA
    Posts
    526

    Default

    DMitchell
    IF the face of your part is Z0 then any – value is going to take the tool into the part. G00 is a rapid move….G01 is a feed move. Your fifth line of code is a rapid move into the part, the tool is going to rapid –1.3 into the part and the next line of code is going to move the tool in the X to 2.89 dia. and the next line will feed the tool
    out of the part or at least to within .250 of the part face. I don’t have a lot of G code experience as I use GibbsCAM but I did spend a week at Hardinge learning G code.
    Good luck
    Carl


  3. #3
    doug925's Avatar
    doug925 is offline Titanium
    Join Date
    Nov 2002
    Location
    Houston, Texas
    Posts
    2,412

    Default

    DMitchel,
    Ditto what Cheenist said.
    IF the front of the bore is Z0. then you have programmed a rapd into the part face.
    The fifth line reads "G0 X2.025Z-1.3",
    is that right?

    N8 G0 X30. Z20.
    T080808 S1500 M4 M8
    G96 S1500 X2. Z.25
    NBORE G81
    G0 X2.025Z-1.3 (z-1.3 ???)
    G1 X2.89 F.008 (feed from x2.02 to 2.98 ??)
    Z-1.05 (then back outaway from the chuck to Z-1.05 ??)
    X3.24 Z-.88
    X6.485
    Z-.05
    G2 X6.585 Z0 L.05
    G1 X8.725
    G80


    Without know the geometry of your part I can't help you with the programming any more that what has been said.
    Email me or repost with any more questions.
    Doug


  4. #4
    spottiepop is offline Junior Member
    Join Date
    Mar 2004
    Location
    Lubbock, Texas, USA
    Posts
    5

    Default

    DMitchell,
    I'll try and help you out the best I can, it's been a while since I had the Okuma manuals out to study the G-Code so here goes. In the G81 command you are defining the geometry of your bore along the Zaxis of the machine, the G0 X Z after the G81 is the starting point of the bore you are trying to cut so if you have this as a negative Z value as you do in your code when you are defining NBORE that is where you are telling the tool to start cutting when you pick-up NBORE in the G85 command.
    This might explain why it is rapiding into the part and feeding out. Since I don't know exactly what it is you are trying to cut it would be hard for me to tell you how to correct the code you posted, hope this helps.

  5. #5
    DMitchell is offline Junior Member
    Join Date
    Apr 2004
    Location
    Daytona Beach, FL, USA
    Posts
    6

    Default

    This is a canned cycle. The X2. Z.25 Defines the starting point of the cycle, then the Nbore G81 line begins the description of the part face. The lines of code describe a finish pass. The G85 should rough it then the G87 finishes it. What the machine does is rapid to x2.025 z-1.3 then rapids to x2.275 (.25 diameter as defined on the G85 line) then feeds to x2.275 z.25, then proceeds to continue the same process rough the part from the inside, out. The next feed move is from x2.525 z-1.3 to x2.525 z.25 The cycle is working in reverse of the way it should. spottiepop, the code defines the face of the part from a bar stock, the is already a 2" hole drilled in the part. Thanks for the replies any further help would be greatly appreciated.

  6. #6
    Cheenist is offline Hot Rolled
    Join Date
    Feb 2004
    Location
    Alexandria Va. USA
    Posts
    526

    Default


    DMitchell,
    I will give you a description of what each line of your code will do. Again this assumes the face of the part is Z0…and I understand the part has a hole already drilled.
    T080808 S1500 M4 M8
    G96 S1500 X2. Z.25
    NBORE G81 (this is a canned drill cycle)is this your problem??
    G0 X2.025Z-1.3(rapid move of the X to 2.025dia. and Z-1.3…hope the hole is big enough for these rapid moves)
    G1 X2.89 F.008(feed move of X to 2.89 dia. at a feed rate of .008
    Z-1.05(Z-1.05…Z is going feed AWAY from the chuck)
    X3.24 Z-.88(feed move of X to 3.24 dia. and Z to -.88…Z is now moving towards the chuck)
    X6.485(X is feeding to 6.485 dia.)
    Z-.05(Z is moving away from the chuck)
    G2 X6.585 Z0 L.05(clockwise interpolation move...X is feeding to 6.585 dia. Z is at 0 and L “usually” is how many times to repeat)
    G1 X8.725(feed move X to 8.725 dia.
    G80(canned cycle cancel)
    G85 NBORE D.25 F.01 U.02 W.005(G85 is a canned boring cycle…D,F,U,W...well I don’t know, but they should be described in the manual and most likely are depth of cut, feed, clearance)
    G0 Z.25(rapid Z to .25…tool moves to .25 in front of part)
    X2.(X rapids to 2.0 dia.
    G87 NBORE(bore/manual retract canned cycle)(this could be your problem)
    G0 Z.25(rapid move of Z to .25 in front of part.
    I hope this helps, but keep in mind that machine tool manufactures use the same G codes differently…like you really wanted to hear that. A G87 is a canned boring cycle but how each manufacture has you fill out the necessary info for the cycle to work can be very different. Without a drawing the above is a shot in the dark but don’t hesitate to ask any more questions, I was once right where your sitting…complete with a boss looking over my shoulder and a new lathe yet crashed.
    Good luck,
    Carl

  7. #7
    DMitchell is offline Junior Member
    Join Date
    Apr 2004
    Location
    Daytona Beach, FL, USA
    Posts
    6

    Default

    The canned cycle, Nbore, from the G81 to G80 is the description of the part shape. The G85 tells the machine to rough this part. The machine is roughing it from the inside out instead of the outside in. The part has a through hole of 2.89" and is 1.2" overall. The numbers in the canned cycle are finish numbers. The machine's movements are:

    Rapid to x2.025 z-1.3
    rapid to x2.275 z-1.3
    feed to x2.275 z.25
    rapid to x2.025 z.25
    rapid to x2.025 z-1.3
    rapid to x2.525 z-1.3
    feed to x2.525 z.25
    rapid to x2.275 z.25
    rapid to x2.275 z-1.3
    rapid to x2.775 z-1.3
    feed to x2.775 z.25
    rapid to x2.525 z.25
    rapid to x2.525 z-1.3
    rapid to x2.87 z-1.3 (it stays .02 from finish dimension in rough cycle because of u.02)
    feed to x2.87 z-1.045 (stays .005 from finish dimension in rough cycle because of w.005)
    then proceeds roughing the program. I hope this finally fully describes what the problem is. The finish cycle (g87) will then cut the final dimensions. Or at least should. Thanks again.


  8. #8
    DMitchell is offline Junior Member
    Join Date
    Apr 2004
    Location
    Daytona Beach, FL, USA
    Posts
    6

    Default

    the L code in the program denotes the radius similar to an R code would in a mill. I'm very familiar with milling G code. Too bad this isn't milling.

  9. #9
    Cheenist is offline Hot Rolled
    Join Date
    Feb 2004
    Location
    Alexandria Va. USA
    Posts
    526

    Default

    DMitchell,
    Maybe take a closer look at your canned cycle selection. Some feed in and rapid out, others rapid in and feed out and another feeds in and feeds out. The code in your last post does rapid in and then feed out.
    Carl

  10. #10
    DMitchell is offline Junior Member
    Join Date
    Apr 2004
    Location
    Daytona Beach, FL, USA
    Posts
    6

    Default

    I tried changing the first line of the canned cycle to a feed. All it did was on the first pass it fed in, every other pass was a rapid in. I'm going to try using a G83 which "should" define the dimensions of the stock.

  11. #11
    DMitchell is offline Junior Member
    Join Date
    Apr 2004
    Location
    Daytona Beach, FL, USA
    Posts
    6

    Default

    I finally figured this out. The key was to program it from the outside to the inside, but position the tool at the inside to begin. Here was the final code that worked. Thanks for all the help.

    GOX30.Z20.
    X1.5Z.25G96S1500M4T080808
    G85 NBORE U.02W.005D.25F.01
    NBORE G81
    GOX8.725Z.25
    G1Z0.F.008
    X6.545
    G02X6.485Z-.03L.03
    G1Z-.88
    X3.24
    X2.89Z-1.2
    Z-1.3
    X2.75
    G40
    G80
    G0Z.25
    G87 NBORE
    G0Z.25M9
    X30.Z20.

  12. #12
    Cheenist is offline Hot Rolled
    Join Date
    Feb 2004
    Location
    Alexandria Va. USA
    Posts
    526

    Default

    DMitchell,
    Thanks for letting us know you worked it out. So many post just leave us hanging. Programing a CNC lathe is not easy, there's a lot going on in a small space and tool/part clearance is always an issue, not to mention rapids approching 1000 IPM.
    Good luck,
    Carl

Bookmarks

Posting Permissions

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