Results 1 to 9 of 9
  1. #1
    Madster67 is offline Plastic
    Join Date
    Aug 2008
    Location
    CHICAGO
    Posts
    2

    Default Higbee or Blunt Forced Tread

    Hello,

    If anyone here in the forum is familiar with what is known as an (Higbee/Blunt Srart Thread).

    I use this on a daily basis in lathe turning process to flatten the first thread(feathered sharp thread) of an acme thread both OD and ID.

    the programs are pre written by our engineering department BUT! each time i set up a certain job i always have to re adjust the starting and or ending points of the higbee to get it just right without hitting the secound thread and scraping my first part.
    I know this process has been used for years on fire hose couplings and so forth and it is described in serveral different issues of the machinist handbook but it does not describe a formula on how to calculate the begining and ending points to make a proper higbee.

    so what i'm looking for is just how to calculate the starting and ending points of the higbee/blunt start thread points. If anyone is familiar with this it would be most appriciated.

    Thank You

  2. #2
    Walter A's Avatar
    Walter A is offline Titanium
    Join Date
    Jul 2007
    Location
    Hampton, Virginia
    Posts
    2,242

    Default

    Ran into the Higbee cut all the time when working as a firefighter. Firehose couplings also have a mark on the lug aligned with the cut. That's called the Higbee indicator.

    Maybe someone from one of the firehose manufacturers could help you. If you can just get past the phone system and into engineering. I also remember the data being shown in one of the catalogs. (Too many years ago)

    I used them but never made them.

    Walter A.

  3. #3
    Troup is offline Titanium
    Join Date
    Jun 2007
    Location
    New Zealand
    Posts
    2,661

    Default

    I made one recently, on a hardened spindle for a small lathe, using an improvised toolpost grinder, per the photos, eyeballing the start and end point . The carriage was driven by the leadscrew, so the DTI in the photo was actually reading spindle angle as well as carriage position.

    With toolpost grinding you have fingertip control of the spindle angle, and all the time in the world, but of course that's no direct use to you.

    However a similar method would work, turning the thread normally then using a large end mill to make the Higbee cut, if your CNC lathe has live spindles in the turret.

    I can't actually see how it could be done neatly and repeatably by simple turning, without a trial-and-error approach such as you describe - seems to me the lathe would need to be set up for relieving, polygon turning or some such.

    Although obviously it's much more straightforward with an Acme thread than in the case of the V thread as pictured.
    Attached Thumbnails Attached Thumbnails grinding-spindle-nose-thread-higbee-cut-1.jpg   grinding-spindle-nose-thread-higbee-cut-2.jpg  

  4. #4
    Ox's Avatar
    Ox
    Ox is offline Diamond
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    18,063

    Default

    Programming it isn't really eny diff than prog the threaded part, other than you need to make sure that you ramp out as fast as possible and in turn (pun?) you need to keep spindle RPM down a bit to help keep the ramp out small.

    The only other thing then is to adjust your Z offset on your grooving toy to match - as you already have been dooing.


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

    Think Snow Eh!
    Ox

  5. #5
    mrainey's Avatar
    mrainey is offline Stainless
    Join Date
    Jul 2004
    Location
    Spartanburg, South Carolina
    Posts
    1,503

    Default

    Some good info here.


    HIGBEE THREAD CUT CYCLE

  6. #6
    i_r_machinist is offline Titanium
    Join Date
    Apr 2007
    Location
    Dublin Texas
    Posts
    2,264

    Default

    Alot of it depends on the machine travel rates. What tool are you useing? The old kennametal top locks were my favorite. Good beefy insert.
    have fun
    i_r_machinist

  7. #7
    SwissPro's Avatar
    SwissPro is offline Hot Rolled
    Join Date
    May 2006
    Location
    Illinois
    Posts
    958

    Default

    I don't know that there is a formula per se but I just calculate the start and end points based on the thread being machined. In the case of an Acme or Stub Acme you can usually just use the threading tool to blunt the start of the thread on a CNC lathe.

    You can calculate based on your start point in "Z" where your first full thread will be. You can also calculate where the first sliver of the thread will be. I use G32 to blunt the thread.

    If you move your start point by 1/2 the lead you will now be centered on the crest of the thread. The program would look something like this:

    G0 X#.#### (minor diameter of the thread plus all your passes but the first)
    G32 Z#.### F#.### (Feed to the very start of the thread in 'Z" at the normal thread pitch)
    G32 X#.### Z#.### F#.### (feed in "Z" to the point of the first full thread, "X" to the major diameter and feed at the thread lead. Some controls might require a slightly faster feed)

    Go X#.### (Clear the Part)
    Z#.### (Return to start point)
    Repeat for second pass.

    It's simpler than it sounds. Sit down and work out the numbers and you'll see what I mean.

    Good luck.

  8. #8
    Madster67 is offline Plastic
    Join Date
    Aug 2008
    Location
    CHICAGO
    Posts
    2

    Default

    Thanx alot for all of the good feedback on this issue.

    I wiil definatley bring up to my boss on using the threading insert to remove the feather of the acme thread and make the higbee.
    as of now how we do it is thread the part and then use a CNMG 433 insert to make the higbee. maybe this would solve my problem.
    Thanks alot everybody you have put some new ideas in my head and been a great deal of help

  9. #9
    badgerman is offline Plastic
    Join Date
    May 2014
    Location
    IL, USA
    Posts
    1

    Default

    Quote Originally Posted by SwissPro View Post
    I don't know that there is a formula per se but I just calculate the start and end points based on the thread being machined. In the case of an Acme or Stub Acme you can usually just use the threading tool to blunt the start of the thread on a CNC lathe.

    You can calculate based on your start point in "Z" where your first full thread will be. You can also calculate where the first sliver of the thread will be. I use G32 to blunt the thread.

    If you move your start point by 1/2 the lead you will now be centered on the crest of the thread. The program would look something like this:

    G0 X#.#### (minor diameter of the thread plus all your passes but the first)
    G32 Z#.### F#.### (Feed to the very start of the thread in 'Z" at the normal thread pitch)
    G32 X#.### Z#.### F#.### (feed in "Z" to the point of the first full thread, "X" to the major diameter and feed at the thread lead. Some controls might require a slightly faster feed)

    Go X#.### (Clear the Part)
    Z#.### (Return to start point)
    Repeat for second pass.

    It's simpler than it sounds. Sit down and work out the numbers and you'll see what I mean.

    Good luck.

    I am a little slow... for a 2 pitch ACME (.5 Lead):

    G0 X(major diameter - first depth of cut) Z(Start Z of my final 14.5 infeed pass plus .250)
    G32 Z0 F.5 (the thread starts at top face which is program zero)
    G32 X(major diameter) Z-.5 F.5 (depth of first full thread)

    I don't understand what I would do on a second pass. Please help a brother out.

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
  •