Results 1 to 12 of 12
Like Tree1Likes
  • 1 Post By pal's machining

Thread: HIGBEE THREAD CUT CYCLE

  1. #1
    Join Date
    Oct 2002
    Location
    owatonna mn. 55060
    Posts
    56

    Default

    Would anybody like to know how to make a National Standard Fire Hose Coupling and deburr the first thread so that that first fin is gone and the possibility of cross threading is gone?
    "Higbee Cut" is a true process and is in the machinist handbook in the National Standard Fire-Hose Coupling Screw Thread.
    If you are making a high priced part and you want to impress the customer this will do it!

    Pat.

  2. #2
    Pazuzu71's Avatar
    Pazuzu71 is offline Hot Rolled
    Join Date
    Dec 2001
    Location
    Live Oak, Texas
    Posts
    800

    Default

    My boss always makes me 'Higbee' the first thread, no matter what we're making.

  3. #3
    sasbenson is offline Member
    Join Date
    Sep 2002
    Location
    Tumwater Wa
    Posts
    63

    Default

    Pal, Im all ears & eyeballs and I bet there's more where I came from. Please give us a demo!! Thanks,

    sas

  4. #4
    Join Date
    Oct 2002
    Location
    owatonna mn. 55060
    Posts
    56

    Default

    I will try my best to explain how it is cut.
    First what you want to acheive is to remove the part of the thread which is usually a small fin on the turned 45 degree angle portion of the part blank up to where it is a full profile 60 degree thread form.
    To do this you use a grooving tool after you are done with the threading cycle. First off you must calibrate your threading and grooving tools to the face of the part (or zero.This is where an important trick lies hidden. The center or tip of the threading tip has to be calibrated so it is equal to the leading edge of the groove tool and the groove insert must be as wide or wider than the base of the thread form (an 1/8" wide insert will work up to 8 pitch. etc) Lets say you are doing 10 pitch threads 1" thread length. Now with your regular threading cycle when you program your length you will get 1 full inch of thread and your first full thread length will be z-.100" (a starting length to be deburred) Now program your grooving tool(also in the same threading cycle as used to thread with) to a depth of z-.100" and you are starting to get a deburred thread. You will only need a couple of deburring passes to remove the burr (so play with the starting x value). But there is more to explain !! Spindle rpm and the machines rapid traverse rate will determine the amount of angle of ramp on the deburred thread. The machines rapid rate will stay constant so for a squarer ramp run slower rpms and a tapered ramp more rpms. Only one more tip if after calibrating the tools you have to adjust the z length of cut you must offset the z length equally on both tools.

    Please rate me on this I would like to know how many people I just trained and if I'm any good at it!!(make this a hot site)
    Pat
    FredC likes this.

  5. #5
    sasbenson is offline Member
    Join Date
    Sep 2002
    Location
    Tumwater Wa
    Posts
    63

    Default

    Pat, thanks for the good info,not an easy operation to describe with just words and no pictures.We normally leave a 45 plus a little bit of the minor diameter to the + side of the start thread but the higbee cut looks WAY better. might be a tricky deal on a manual lathe with no stop mechanism but Looks like cake on cnc. I looked around the shop and found a coupler that shows exactly what it should look like.Now ..... if I can just make this link work!! http://photos.msn.com/myfiles/folderview.aspx?Folder=4gPozhciq6ZTdypEPFXEQi ctJ*RhGuXgXweAIQIykiw%24

    [This message has been edited by sasbenson (edited 12-15-2002).]

  6. #6
    ufscrap Guest

    Default

    I have found the G32 threading cycle to be perfect for stuff like this. G32 allows you to control the tool anyway you want to under a threading feed. In the manual for my Haas SL-30 the example is a continuous thread that goes from straight to tapered, then back to straight (I'd be interested to see the nut for this screw). With G32 you can change the vary the pitch while threading. I can't think of an application for this, but it might come in handy sometime. We use this cycle all the time for higby ends, and for taking the spring out of long threaded parts. In other words, you can program a thread that moves the tool into the piece at a variable taper rate to compensate for deflection.

    Your method was described well, and I am sure it works well. The only problem I have is my operators often override the rapid speeds on new jobs, and that would make for a bad end.

  7. #7
    Jeff is offline Hot Rolled
    Join Date
    Jun 2001
    Location
    WI
    Posts
    656

    Default

    ufscrap...there are different types of "augers" where the lead of the "flights" (probably not the right term) changes. Also, have seen types of feed rollers, I don't know what for, that had spiral grooves in the O.D. that increase/decrease in pitch along the length of the roll. Not sure how these were made, but maybe the G32 would work??? Some of them are obviously milled.

  8. #8
    Jcha is offline Junior Member
    Join Date
    May 2006
    Location
    Greencastle Pa
    Posts
    1

    Post

    In regards to the Higbee Cut on fire hose couplings it should be noted that the first thd is completely removed and the Higbee Cut starts on the second thd.

  9. #9
    mrainey's Avatar
    mrainey is offline Stainless
    Join Date
    Jul 2004
    Location
    Spartanburg, South Carolina
    Posts
    1,485

    Post

    At one time I could really have used a method for getting a Higbee on a lathe. We milled thousands of them on a CNC Bridgeport - not the fastest of all possible methods.

  10. #10
    alphonso is offline Stainless
    Join Date
    Feb 2006
    Location
    Republic of Texas
    Posts
    1,489

    Post

    Please rate me on this.
    Excellent explanation. My newest guy read it, tried it, says, "Wow! that's slicker'n snot on a doorknob!" Now he wants to add Higbee to all our threaded parts.

  11. #11
    Join Date
    Nov 2004
    Location
    McDonald, Pennsylvania
    Posts
    1,575

    Post

    I will try to get you a picture of it, they work great. With all the numb nuts that are in my fire department, it is very, very, extremely rare that anything gets cross threaded.
    They actually have a mark on them too where the thread starts engaging. Pretty neat.

  12. #12
    Cutter2 is offline Plastic
    Join Date
    Jun 2009
    Location
    Texas
    Posts
    19

    Default

    Quote Originally Posted by Jeff View Post
    ufscrap...there are different types of "augers" where the lead of the "flights" (probably not the right term) changes. Also, have seen types of feed rollers, I don't know what for, that had spiral grooves in the O.D. that increase/decrease in pitch along the length of the roll. Not sure how these were made, but maybe the G32 would work??? Some of them are obviously milled.
    "Flites" is the term I've always heard used for augers, so I think your correct there. Varying the pitch of the flite on the augers in a plastic injection mold's auger seems to be fairly common. Most shops build those augers with a mill and 4th axis, but it could be done on a lathe. Probably faster, especially if you were building several augers all the same.

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
  •