584,846 active members*
3,782 visitors online*
Register for free
Login
IndustryArena Forum > Machine Controllers Software and Solutions > Fanuc > I.D. threading Fanuc 18t Hardinge T42
Results 1 to 4 of 4
  1. #1
    Join Date
    Oct 2009
    Posts
    16

    I.D. threading Fanuc 18t Hardinge T42

    I was wondering if someone could give me some info on how to thread an internal thread on my Hardinge T42 with Funuc 18t
    Heres how I would thread an O.D.thread

    (THREADING 25mm X 1.5p O.D.Thread)
    N1
    G97 S650 M13
    T101
    G0 X1.0506 Z.25
    S650
    G4 U.6
    G76 P030029 Q0025 R.0
    G76 X.9054 Z-.500 P0363 Q0040 F.059055
    G0 X1.250
    Z6.0
    M01

    What would I change to do the same thread internally?
    Thanks
    Brian

  2. #2
    Join Date
    Sep 2010
    Posts
    1230
    Quote Originally Posted by rwpbrian View Post
    I was wondering if someone could give me some info on how to thread an internal thread on my Hardinge T42 with Funuc 18t
    Heres how I would thread an O.D.thread

    (THREADING 25mm X 1.5p O.D.Thread)
    N1
    G97 S650 M13
    T101
    G0 X1.0506 Z.25
    S650
    G4 U.6
    G76 P030029 Q0025 R.0
    G76 X.9054 Z-.500 P0363 Q0040 F.059055
    G0 X1.250
    Z6.0
    M01

    What would I change to do the same thread internally?
    Thanks
    Brian
    Hi Brian,
    G0 X1.0506 Z.25 - Specify an X value that is smaller than the Minor Diameter of the thread.
    S650 - This is not required, you've already started the spindle
    G4 U.6 - Why the Dwell here?
    G76 P030029 Q0025 R.0
    G76 X.9054 Z-.500 P0363 Q0040 F.059055 - Specify an X value equal to the Major Diameter of the internal thread.


    G76 P030029 Q0025 R.0

    With regards to the argument shown in Red above, this is generally set to the included angle (Tip Angle) of the thread. Either:
    1. the thread angle is 29 degrees,
    2. you inadvertently specified 29 degrees when the thread angle is 60 degrees,
    or
    3. you purposely specified 29 degrees when the thread angle is 60 degrees.

    If 3, that's not an altogether bad thing. It just means that more work is being done by the leading edge of the tool, and some by the trailing edge. I often do this but use 55 instead of 60, so that most of the work is being done by the leading edge.


    Regards,

    Bill

  3. #3
    Join Date
    Oct 2009
    Posts
    16
    Thanks Bill works great!

    Also I was wondering if you had any knowledge of programming live tooling with the Fanuc 18t maybe i can run a couple things past you if you dont mind?

    Thanks Brian

  4. #4
    Join Date
    Sep 2010
    Posts
    1230
    Quote Originally Posted by rwpbrian View Post
    Thanks Bill works great!

    Also I was wondering if you had any knowledge of programming live tooling with the Fanuc 18t maybe i can run a couple things past you if you dont mind?

    Thanks Brian
    Hi Brian,

    Thanks for the feed back. I'm sure there are others that follow the Threads, excuse the pun, and gain by knowing that the answer to the question worked, or just as importantly, didn't work.

    I'm sure I, or many other Forum members will be able to help you with other questions regarding live tooling. However, start another Thread with a title that relates to the question.

    Regards,

    Bill

Similar Threads

  1. Hardinge Cobra42 w/ Fanuc 21-T
    By danohpsp in forum Fanuc
    Replies: 3
    Last Post: 03-30-2013, 09:34 PM
  2. Help on Fanuc 18m for Hardinge Conquest VMC 700
    By chuckblowers in forum Fanuc
    Replies: 3
    Last Post: 02-20-2012, 10:24 AM
  3. G73 Cycle on Hardinge GT-27 / Fanuc-18T
    By jdr1961 in forum Hardinge Lathes
    Replies: 1
    Last Post: 01-06-2010, 10:33 PM
  4. Hardinge threading code
    By Pontiff51 in forum MetalWork Discussion
    Replies: 3
    Last Post: 03-16-2009, 05:37 PM
  5. Hardinge TT-65 w/ Fanuc 18i-T
    By Jeff_Mezzo in forum Hardinge Lathes
    Replies: 3
    Last Post: 01-29-2009, 03:24 AM

Posting Permissions

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