Results 1 to 13 of 13
  1. #1
    Tory is offline Plastic
    Join Date
    Jul 2011
    Location
    houston,texas
    Posts
    2

    Angry 3/4 npt external using G76 canned cycle

    I am looking to find someone that can help me with an external 3/4 npt thread using the G76 canned cycle the only thing is that I am cutting the thread the opposite direction from large diameter to small so in other words I am cutting the thread backwards. Anyone please help!!!!! The material being cut is alloy steel about 34 Hrc.

  2. #2
    Sean the Dog is offline Cast Iron
    Join Date
    May 2011
    Location
    Nova Scotia
    Posts
    299

    Default

    Are you using a left hand threading tool to cut a right hand thread?

    (Assuming you are

    This can be done, but you will end up with a groove at the start of the thread (unless there is already an undercut there). You will be plunging into the material, which will be hard on the tool.

    Also, because of lag time getting the threading feed up to speed and synchronized with the spindle speed, the big end of your thread may not be quite right.

    To do it, your start point will be a safe height over the big end at the distance you want to start at, and the finish point will be at the minor diameter off the small end (in space).

    I can't remember if the "i" value is positive or negative, but make sure to apply it over the ENTIRE length of travel, not just the length of thread.

  3. #3
    Tory is offline Plastic
    Join Date
    Jul 2011
    Location
    houston,texas
    Posts
    2

    Default 3/4 npt using G76 canned cycle

    Sean,
    Thanx for the response There is a releif at the end of the thread I use an R value instead of the I and no I am not using a left hand tool. I am very close to getting this solved but still working on it. I will give you an example of the threading cycle that I am using.

    G76 P011260 Q30 R60
    G76 x.___ Z-.___ P____ Q___ R+.___ F.0714285

  4. #4
    Ox's Avatar
    Ox
    Ox is offline Diamond
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    17,739

    Default

    1*47' per side for pipe taper,

    R value will depend on how much total Z travel you have.

    Pipe dimmenssions are in your Machinery Handbook, but can prolly be found quicker on Google.


    ----------------

    Think Snow Eh!
    Ox

  5. #5
    cncbrit is offline Hot Rolled
    Join Date
    Apr 2011
    Location
    California
    Posts
    518

    Default

    Make sure the holder doesn't hit the threads at the small end of travel.

  6. #6
    SeymourDumore is offline Diamond
    Join Date
    Aug 2005
    Location
    CT
    Posts
    6,261

    Default

    Quote Originally Posted by Tory View Post
    Sean,
    Thanx for the response There is a releif at the end of the thread I use an R value instead of the I and no I am not using a left hand tool. I am very close to getting this solved but still working on it. I will give you an example of the threading cycle that I am using.

    G76 P011260 Q30 R60
    G76 x.___ Z-.___ P____ Q___ R+.___ F.0714285
    That looks to be allright, tough I don't have the exact numbers to plunk in for X and Z. The Z would likely be a Z+ something if you're threading on the front but ....

    However, care to explain how you'd attempt to pull it off without a left hand tool???
    Unless I got my head wrapped around incorrectly, you'll either cut a left hand NPT or rub it off for a right hand one.

  7. #7
    sinha is offline Cast Iron
    Join Date
    Sep 2010
    Location
    india
    Posts
    278

    Default

    Yes, R in the second block would be positive for this application.
    The value would be total Z-travel divided by 32.
    The convention for sign is same as that in taper turning with G90.

  8. #8
    Sean the Dog is offline Cast Iron
    Join Date
    May 2011
    Location
    Nova Scotia
    Posts
    299

    Default

    "However, care to explain how you'd attempt to pull it off without a left hand tool???
    Unless I got my head wrapped around incorrectly, you'll either cut a left hand NPT or rub it off for a right hand one. " - SeymourDumore


    I'm guessing a top notch threading tool, not pitch matched, with LOTS of selective grinding on the holder, and workpiece geometry that doesn't interfere.

    Sorry I couldn't help more with the code; we always used one-line G76. Can't even remember how two-line works.

  9. #9
    SeymourDumore is offline Diamond
    Join Date
    Aug 2005
    Location
    CT
    Posts
    6,261

    Default

    Quote Originally Posted by Sean the Dog View Post

    I'm guessing a top notch threading tool, not pitch matched, with LOTS of selective grinding on the holder, and workpiece geometry that doesn't interfere.
    All that grinding to turn a perfectly good RH threading tool into an iffy left handed one?

    As far as I can see this, to single point a standard RH thread from back to the front, you need a left hand tool.

  10. #10
    Sean the Dog is offline Cast Iron
    Join Date
    May 2011
    Location
    Nova Scotia
    Posts
    299

    Default

    I may be looking at this wrong, but it appears from the code that the OP is cutting a right hand NPT thread that goes down toward the chuck...

    ...maybe last operation before parting to give a finished piece without a second setup to finish the other end. I've done similar things with studs, but with straight threads.

  11. #11
    Goulish is offline Plastic
    Join Date
    Dec 2010
    Location
    Nampa, Idaho
    Posts
    4

    Default

    this is for a RH thread for a 3/4-16 on a Fanuc OI-TC controller I didnt use any R value it always hangs on my machine.
    M03 S1000
    G99
    G0 G54 Z.2167
    X.75
    G76 P010029 Q0 R0
    G76 X.6733 Z-.8075 P383 Q97 F.0625
    for a LH thread on the O.D. all you need to do is start your Z on the opposit side and tell it to go positive while still spinning in M03 so
    M03 S1000
    G99
    G0 G54 Z.2167
    X.75
    G76 P010029 Q0 R0
    G76 X.6733 Z-.8075 P383 Q97 F.0625

    Hope this helps

  12. #12
    SeymourDumore is offline Diamond
    Join Date
    Aug 2005
    Location
    CT
    Posts
    6,261

    Default

    well, since the OP has not chimed in for a while....

    I am going under the assumption that he is cutting an NPT thread, so he needs an R. ( or I in case of a single line G76cycle)
    He is also stating that all he is doing differently is that he intends to cut it backwards, from chuck to end of part.
    That would mean he is cutting a RH thread.

    That thread in the reverse direction should be possible just fine, but he'll need a left hand tool, positive +R, and likely finish at somewhere in the +Z area.

    But until he clarifies things, the discussion is mute.

  13. #13
    CNCJockey is offline Plastic
    Join Date
    Mar 2011
    Location
    Southern USA
    Posts
    8

    Default

    I've cut pipe threads where I had to thread away from the chuck, I only did this because it was a barfeed job where the threads had to be on the rear and we didn't want to do a second op, I just used a regular thread tool and spin the chuck backwards, use three wires to measure the P.D. on the first part, biggest pain is getting the truncation of the threads correct without using a forming type insert.

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
  •