Results 1 to 7 of 7

Thread: G71 Threading for Okuma Lathe

  1. #1
    Registered
    Join Date
    Nov 2006
    Location
    us
    Posts
    4
    Downloads
    0
    Uploads
    0

    Default G71 Threading for Okuma Lathe

    I am having a problem threading a 1"-8 2A thread on an Okuma lathe. The code I have right now reads:

    G71 X.915 Z-2.35 D.008H.1482 U.005 F1 J8 I-.0010 M33M73


    The threads are not being cut deep enough. I believe it has to do with the H value, but I am not familiar at all with coding for an Okuma. Any help would be greatly appreciated. Thanks.

    Similar Threads:


  2. #2
    Community Moderator Al_The_Man's Avatar
    Join Date
    Dec 2003
    Location
    Canada
    Posts
    20577
    Downloads
    0
    Uploads
    0

    Default

    What control? Some okuma's had Fanuc's of different vintages.
    Al.

    CNC, Mechatronics Integration and Custom Machine Design (Skype Avail).

    Logic will get you from A to B. Imagination will take you everywhere.
    Albert E.


  3. #3
    Registered
    Join Date
    Nov 2006
    Location
    us
    Posts
    4
    Downloads
    0
    Uploads
    0

    Default

    It has an Okuma control. The number on the bottom left of the controls reads: "OSP5020L". Is that what you are looking for? If not, how would I find what you need.

    Thanks for you help.



  4. #4
    Registered broby's Avatar
    Join Date
    Apr 2006
    Location
    Australia
    Posts
    677
    Downloads
    0
    Uploads
    0

    Default

    Hi pedgette,
    In your threading program of:

    G71 X.915 Z-2.35 D.008H.1482 U.005 F1 J8 I-.0010 M33M73

    The X word is the final diameter that the tool will cut to (minor diameter for external threads, Major diameter for internal threads)
    Z word is the finish point on Z for the threading cycle.
    D word is the depth of cut (can't remember of the top of my head if it's Diameter Or Radius... not at work)
    H word is the Height from the X word to the first cut, so if you are screwcutting something soft you can specify a small H value and the first cut will be deep...
    U word is the depth of cut for the last pass... once again can't remember Diam or Rad...
    F is the Pitch of the thread, in your case 1 inch
    J is the number of divisions per F. in your example 8 pitches per inch
    (you could have programmed only the F word as F0.125)
    this is used when programming odd thread pitches such as 11.5 threads per inch... as F2 J23 which equals 23 pitches for every 2 inches of thread ie 11.5TPI.
    I word is the incremental change in radius along the length of the thread. i.e. use this to get taper out (or into) your thread. Measure the pitch diameter at each end of the thread, divide the difference by 2 and use the answer in the I word - values make the tool cut -, + values are + direction.
    M33 is a Zig-Zag infeed pattern, where the tool will move from side to side as it moves down the flank. You really need the B word specified also to get this to work well.
    B word is the included angle of the thread i.e. B60 for a UN or metric thread, B55 for a BSW thread etc...
    M73 specifies the infeed pattern but as I am not at work at the moment I can not tell you the exact infeed pattern that it is. However it is the most common infeed pattern that we use.

    Therefore if you are not getting a deep enough thread you probably need to check your X value 1st, tool offset on X 2nd or finally the threading insert itself (if you are using full form inserts).

    If you want I can scan in the infeed patterns and post them for you. Let me know.
    Hope this helps
    Regards
    Brian.



  5. #5
    Registered
    Join Date
    Nov 2006
    Location
    us
    Posts
    4
    Downloads
    0
    Uploads
    0

    Default

    Thanks for the reply. We ended up using an offset to get the threads to look good at the end of the day. After checking the major dia. and using a pitch mic they are within spec; we are just waiting for thread gauges to come in on monday to make sure. Thanks for the reply. I'll let you guys know on monday how it checks out.



  6. #6
    Registered broby's Avatar
    Join Date
    Apr 2006
    Location
    Australia
    Posts
    677
    Downloads
    0
    Uploads
    0

    Default

    Have scanned in the manual referring to the G71 cycle.
    See attachment, if I have done it correctly that is!
    Brian.

    Attached Files Attached Files


  7. #7
    Registered broby's Avatar
    Join Date
    Apr 2006
    Location
    Australia
    Posts
    677
    Downloads
    0
    Uploads
    0

    Wink

    Hi Pedgette,
    How did the threads turn out?

    I looked up the thread specs for a 1"-8UN 2A thread out of curiosity and have realised what your problem was!
    You have programmed to the Pitch Diameter of the thread rather than the Minor Diameter of the thread!

    The specs for your thread are:
    1"-8UN Class 2A
    Major 0.9980" -> 0.9830"
    Pitch 0.9168" -> 0.9100"
    Minor 0.8446" -> 0.8288"

    Thus you should have programmed an X value of between 0.8446 and 0.8288


    Brian.



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 from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!

Follow us on

Facebook Dribbble RSS Feed