Results 1 to 9 of 9
  1. #1
    MikeJB is offline Aluminum
    Join Date
    Mar 2007
    Location
    Aylesbury, U.K.
    Posts
    232

    Question Thread milling with boring bar

    We were talking with a very experienced CNC machinist and he suggested using a lathe boring bar with a thread cutting insert to mill threads with our Haas VF0. Much cheaper than purpose made thread milling tools.

    Will this work OK? Anybody else doing this? Our visitor was absolutely confident that it would work.

    Regards,

    Mike.

  2. #2
    mrainey's Avatar
    mrainey is offline Stainless
    Join Date
    Jul 2004
    Location
    Spartanburg, South Carolina
    Posts
    1,500

    Default

    It works, but it's slow.

  3. #3
    Boris is offline Titanium
    Join Date
    Oct 2005
    Location
    England
    Posts
    3,015

    Default

    Can be done
    But its slow, but if you've got no other way of getting a thread in there... or its a one off part with a very odd thread.

    Heres an example program for a 20mm*2 thread 40 mm deep
    Have not put in any roughing cuts or anything

    O1001
    T1 S1500 M6
    G54 G0 X0 Y0
    G43 Z0 H1 M3 // tool height
    G1 G41 Y20 H21 F250 // move to tool out to thread dia with comp
    M98 P201002 // call the threading 20 times
    G1 G40 Y0 // cancel comp
    G0 Z25 M5
    M30

    O1002
    G2 J-20. Z-2. // spin the tool around once and down the thread pitch
    M99

    Boris

  4. #4
    Alum chips is offline Banned
    Join Date
    May 2005
    Location
    Out in the middle of nowhere
    Posts
    244

    Default

    Oh yea, do it all the time
    Gary

  5. #5
    706jim is offline Stainless
    Join Date
    Jun 2006
    Location
    Thunder Bay Canada
    Posts
    1,257

    Default THread milling with BB

    Quote Originally Posted by mrainey View Post
    It works, but it's slow.
    I did 4" of 2.75-12 thread in mild steel using a HSS tool and boring bar. Feed was 0.3ipm (BB centerline). Set up a subroutine (as above) and went for coffee. Perfect thread, but the tool has to survive for the whole process if its not an indexable insert.

  6. #6
    spock is offline Hot Rolled
    Join Date
    Dec 2006
    Location
    Central Ky
    Posts
    925

    Default

    If you guys are familiar with the triangle shaped thread inserts (for lathe IIRC), they have three cutting edges, you can mill a triangle pocket on the end of a piece of 3/4 rod, tap a hole and go. Very cheap, and you have three edges instead of one.

  7. #7
    MikeJB is offline Aluminum
    Join Date
    Mar 2007
    Location
    Aylesbury, U.K.
    Posts
    232

    Default

    Thanks guys for your advice; I guess that this technique is best for those one off or last minute jobs when buying the proper tool is not an option.

    Regards,

    Mike.

  8. #8
    crowellmachine is offline Plastic
    Join Date
    Nov 2006
    Location
    NC PA
    Posts
    17

    Default

    You can also make multiple start threads if you use your scaling and rotation..... KJC

  9. #9
    Boris is offline Titanium
    Join Date
    Oct 2005
    Location
    England
    Posts
    3,015

    Default

    Quote Originally Posted by crowellmachine View Post
    You can also make multiple start threads if you use your scaling and rotation..... KJC
    Eh?
    Not meaning to pour cold water on your idea but for a M40*2 2 start thread like the single start listed above:

    O1001
    T1 S1500 M6
    G54 G0 X0 Y0
    G43 Z0 H1 M3 // tool height
    G1 G41 Y20 H21 F250 // move to tool out to thread dia with comp
    M98 P101002 // call the threading 10 times
    G1 G40 Y0 // cancel comp
    G0 Z+2
    G1 G41 Y20 H21 F250
    M98 P101002
    G1 G40 Y0
    G0 Z25 M5
    M30

    O1002
    G2 J-20. Z-4. // spin the tool around once and down the thread pitch*number of starts
    M99

    Boris

    And hope the tool does'nt break

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
  •