Programming a long thread, methods to compensate for flex
Close
Login to Your Account
Results 1 to 20 of 20
  1. #1
    Join Date
    Jan 2003
    Location
    Pacific Northwest
    Posts
    1,266
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    66

    Default Programming a long thread, methods to compensate for flex

    When threading a high aspect ratio rod supported with the tailstock with a Haas threading cycle, is there a way to compensate for the flex in the middle?

    What about with Mastercam?

  2. #2
    Join Date
    Aug 2016
    Country
    UNITED KINGDOM
    Posts
    76
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    20

    Default

    What thread is it? How long is it?

  3. #3
    Join Date
    Nov 2017
    Country
    UNITED STATES
    State/Province
    California
    Posts
    27
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    7

    Default

    Quote Originally Posted by laminar-flow View Post
    When threading a high aspect ratio rod supported with the tailstock with a Haas threading cycle, is there a way to compensate for the flex in the middle?

    What about with Mastercam?
    A follow rest could eliminate that

  4. #4
    Join Date
    Jan 2003
    Location
    Pacific Northwest
    Posts
    1,266
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    66

    Default

    It will be a .375-10 and about 5.250 long in steel. I can't easily rig up a follow rest on the CNC Haas.

  5. #5
    Join Date
    Sep 2010
    Location
    india
    Posts
    988
    Post Thanks / Like
    Likes (Given)
    58
    Likes (Received)
    157

    Default

    A lower DOC would reduce flexing.

  6. Likes Kleinfeldt liked this post
  7. #6
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    688
    Post Thanks / Like
    Likes (Given)
    389
    Likes (Received)
    700

    Default

    I think I'd just give it a few free passes.

    Edit: Thought it was 3/4-10. Free passes won't do it.

  8. Likes Kleinfeldt liked this post
  9. #7
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    23,102
    Post Thanks / Like
    Likes (Given)
    3403
    Likes (Received)
    6392

    Default

    3/8-10 x 5.25?

    I think you're gunna need more than taper control!


    If it is on a 3/8" bar, and if your threader bar is on the back side looking down, you can doo these with fair results in a Swiss lathe.


    In your Haas I would turn it with a box tool and get with Fette for a special set of thread rolls and a high helix head.

    You could get by probably with a die head and some "100" series chasers too I guess... (depending on material)
    That's a LOT of helix tho....


    Unless going with the Swiss, my first call would be to Fette and/or Cleveland Tool (? - the makers of the 100 series chasers?) and see what they have to say about using their tools on that helix.



    I kan't imagine trying to fight this by single pointing on a Haas.



    That's not going to leave much uncut stock in the middle either.
    That is going to be a DEEP thread for the size of bar.

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

    Think Snow Eh!
    Ox

  10. Likes 706jim liked this post
  11. #8
    Join Date
    Jan 2005
    Country
    CANADA
    State/Province
    Saskatchewan
    Posts
    9,430
    Post Thanks / Like
    Likes (Given)
    1138
    Likes (Received)
    3173

    Default

    Quote Originally Posted by laminar-flow View Post
    It will be a .375-10 and about 5.250 long in steel. I can't easily rig up a follow rest on the CNC Haas.
    Surely not a V thread! You'd think Acme is bad until you cut a coarse V thread, then realize Acme is a piece of cake for coarse threads.

    I think you can write consecutive G33 (thread cycle) commands and run them end to end non stop and so create a multi-vector profile with a tapered thread lead in, maybe a short flat zone near the center, then the opposite taper on the way out. At least this is possible on a Mits controller, probably Haas can do it too.

  12. Likes yardbird liked this post
  13. #9
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,871
    Post Thanks / Like
    Likes (Given)
    4181
    Likes (Received)
    1443

    Default

    If I was you I'd try a infeed angle of 55deg instead of 60. Kinda get as much load off the training side as I could. See if it didn't cut a little bit more freely.

    Brent

  14. #10
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    2,842
    Post Thanks / Like
    Likes (Given)
    1014
    Likes (Received)
    965

    Default

    Quote Originally Posted by yardbird View Post
    If I was you I'd try a infeed angle of 55deg instead of 60. Kinda get as much load off the training side as I could. See if it didn't cut a little bit more freely.

    Brent
    Won't that increase the amount of material getting cut by the trailing edge?

    One of the major weaknesses of Fanuc's two line G76 is the lack of control over infeed angle. I'm not a Haas user, but don't they allow ANY infeed angle to programmed (like every other control in existence apart from Fanuc...)

  15. #11
    Join Date
    Dec 2002
    Location
    Pacific NW
    Posts
    4,988
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    783

    Default

    3/8-10.... that's a thread sometimes used on pool cue joints.

    I made tooling for a couple cue makers. For the 3/8-10 I sent the material to Superior thread Rolling in LA. They had dies for it.

  16. Likes Bobw liked this post
  17. #12
    Join Date
    Jan 2003
    Location
    Pacific Northwest
    Posts
    1,266
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    66

    Default

    The die head sounds interesting, but this is a lead screw for a Schaublin 102 swiss lathe. Yes, the diameter is metric, just under .375. But we can find a .375-10 tap and cut a V thread instead of a acme. We are just thinking about this right now and wanted to see if there was a way to make this happen. We have access to Mastercam and will look to see if there is a way if we can't program the Haas. It will only require a few .000 and in the past I snuck in a piece of wood and acted like a follower

  18. #13
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    16,900
    Post Thanks / Like
    Likes (Given)
    12542
    Likes (Received)
    12027

    Default

    I know it's not ''original'' - typical of the Swiss I expect it was 9.5mm OD, ......and those bloody Vee threads on lead screws do wear. ........Anyway I'd go with ACME or better yet stub ACME, at least then you can clean up with a tap and die. - if of course you need to

    That said I'd probably buy a piece of ACME rod off the shelf and graft it on to the rest of the works.

  19. #14
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,871
    Post Thanks / Like
    Likes (Given)
    4181
    Likes (Received)
    1443

    Default

    Quote Originally Posted by gregormarwick View Post
    Won't that increase the amount of material getting cut by the trailing edge?
    I thought it decreased it by 5deg?

    One of the major weaknesses of Fanuc's two line G76 is the lack of control over infeed angle. I'm not a Haas user, but don't they allow ANY infeed angle to programmed (like every other control in existence apart from Fanuc...)
    When I cut some of the larger pitch threads I set my first line P in the 2 line G76 cycle like this P020555. Doesn't that give you a indeed angle 55deg?

    I believe if you set your control to use the 1 line G76 cycle you have more angles to use but I agree with what you're saying it does seem like a downgrade for the 2 line cycle.

    My bitch is the way you have to do multiple lead threads by shifting the Z start instead just a freaking variable. Lol....

    Brent

  20. #15
    Join Date
    Mar 2007
    Location
    Milwaukee
    Posts
    339
    Post Thanks / Like
    Likes (Given)
    261
    Likes (Received)
    159

    Default

    Quote Originally Posted by laminar-flow View Post
    The die head sounds interesting, but this is a lead screw for a Schaublin 102 swiss lathe. Yes, the diameter is metric, just under .375. But we can find a .375-10 tap and cut a V thread instead of a acme. We are just thinking about this right now and wanted to see if there was a way to make this happen. We have access to Mastercam and will look to see if there is a way if we can't program the Haas. It will only require a few .000 and in the past I snuck in a piece of wood and acted like a follower


    I would have that ground from a solid, the original was.

    Have also used the wooden stick method before, not easy to hold size for a lead screw.

  21. #16
    Join Date
    Mar 2011
    Location
    MASS
    Posts
    709
    Post Thanks / Like
    Likes (Given)
    313
    Likes (Received)
    246

    Default

    geometric die head

  22. #17
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    23,102
    Post Thanks / Like
    Likes (Given)
    3403
    Likes (Received)
    6392

    Default

    Quote Originally Posted by laminar-flow View Post
    The die head sounds interesting, but this is a lead screw for a Schaublin 102 swiss lathe. Yes, the diameter is metric, just under .375. But we can find a .375-10 tap and cut a V thread instead of a acme. We are just thinking about this right now and wanted to see if there was a way to make this happen. We have access to Mastercam and will look to see if there is a way if we can't program the Haas. It will only require a few .000 and in the past I snuck in a piece of wood and acted like a follower

    Good grief - if you only need 1 pc, you better find something that you can modify to be what you want.
    Way too much of an uphill fight to make one yourself.


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

    Think Snow Eh!
    Ox

  23. #18
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,066
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1204

    Default

    Quote Originally Posted by yardbird View Post
    I thought it decreased it by 5deg?



    When I cut some of the larger pitch threads I set my first line P in the 2 line G76 cycle like this P020555. Doesn't that give you a indeed angle 55deg?

    I believe if you set your control to use the 1 line G76 cycle you have more angles to use but I agree with what you're saying it does seem like a downgrade for the 2 line cycle.

    My bitch is the way you have to do multiple lead threads by shifting the Z start instead just a freaking variable. Lol....

    Brent
    Hello Brent,
    By specifying an angle less than the included angle of the Threading Insert, material on the trailing flank of the Thread will be cut. For example, A0 will take an equal amount on the Leading and Trailing flank.

    On controls that use FS16 Standard Format (two Block Format), FS15 Format (one Block Format) can be selected via parameter. One Block Format allows the angle in the G76 cycle to be specified in 1deg increments for 0 to 120degs.

    To the OP
    I agree with OX, a thread of the diameter and length you specified will give you grief threading with a single point tool. However, from a programming point of view and although HAAS make no mention of it in their manual, you may be able to compensate for the flex by using the Continuous Threading function using G32. This is a function available on Fanuc Controls and as the HAAS mimic most of the Fanuc function, this also may be available with the HAAS.

    If the function is available, I would rough the thread using the G76 cycle and then finish using the G32 Continuous Threading function.

    Regards,

    Bill

  24. #19
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    2,842
    Post Thanks / Like
    Likes (Given)
    1014
    Likes (Received)
    965

    Default

    Quote Originally Posted by yardbird View Post
    I thought it decreased it by 5deg?



    When I cut some of the larger pitch threads I set my first line P in the 2 line G76 cycle like this P020555. Doesn't that give you a indeed angle 55deg?

    I believe if you set your control to use the 1 line G76 cycle you have more angles to use but I agree with what you're saying it does seem like a downgrade for the 2 line cycle.

    My bitch is the way you have to do multiple lead threads by shifting the Z start instead just a freaking variable. Lol....

    Brent
    Using a 55deg infeed with a 60deg insert causes the trailing edge to cut a little bit on each pass. For clarity, 0deg infeed is straight plunge in where it cuts equally on both edges of the insert.

    I think...

    Ah, Bill got in first while I was AFK

  25. #20
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,871
    Post Thanks / Like
    Likes (Given)
    4181
    Likes (Received)
    1443

    Default

    Well Shit!

    All this time I thought I was trying to make things better but in reality making things worse.

    Thanks Fellas!

    Brent


Tags for this Thread

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
  •