Loading ...
Sorry, an error occurred while loading the content.

Re: threading

Expand Messages
  • Fred Smith
    ... do at ... pieces, ... female) ... For OD threads, you need to verify 2 things: 1) Thread form. Your threading tool must be ground within 59-60 degrees (
    Message 1 of 5 , Mar 1, 2006
    • 0 Attachment
      --- In SherlineCNC@yahoogroups.com, "baldysm" <baldysm@...> wrote:

      > Is there some formula or something that I can use to program
      > internal/external threads that mesh well? I don't know what else to
      do at
      > this point, other than everytime I need a thread, make several test
      pieces,
      > and use trial and error to come up with 2 programs (1 male and 1
      female)
      > with threads that mesh.

      For OD threads, you need to verify 2 things:

      1) Thread form. Your threading tool must be ground within 59-60
      degrees ( 59-59.5 would be even better), and oriented exactly 90
      degrees to the part diameter. If your threading tool has the wrong
      angle, or is not precisely aligned, your threads will never meet the
      specs, and will not be usable for interchangable parts. There is a
      threading gage used for measuring both the angle of the tip and the
      orientation to the part.

      2) Pitch diameter. Get some thread wires and a micrometer at a
      minimum, and if you are running production, get a set of thread pitch
      mics and a calibrating standard.

      There are pictures and some details of this information in the desktop
      threading writeup at this link
      http://www.cadcamcadcam.com/hobby

      If your thread is slightly oversize after running the program, make
      a .001( or whatever you need) adjustment in the tool position in X and
      reset the coordinates. If you are at .5000 and the thread pitch comes
      out .002 oversize ( .502), move the X axis to .500 and reset the X
      coordinate to .502. Now rerun the part and the thread will make a
      small cut on the last pass or so and it should be to size. A HSS tool
      will work better on a Sherline than Carbide tool.

      There is no cost effective gage for ID threads, except for an accurate
      male plug. Make a plug gage by using a pitch gage to assure that
      the "nut" you are making will fit other screws. Cut the ID thread
      slightly undersize, then make additional cuts, just slightly adjusting
      the tool position, similar to the method used for OD thread diameter
      adjustment.

      Fred Smith - IMService
      http://www.cadcamcadcam.com/hobby
    • Fred Smith
      ... By pitch gage I meant, by measuring with thread wires, or a pitch mic. ... adjusting ... Here I meant to say, until the plug gage can be screwed into the
      Message 2 of 5 , Mar 1, 2006
      • 0 Attachment
        --- In SherlineCNC@yahoogroups.com, "Fred Smith" <imserv@...> wrote:
        > Make a plug gage by using a pitch gage to assure that
        > the "nut" you are making will fit other screws.

        By pitch gage I meant, by measuring with thread wires, or a pitch mic.

        >Cut the ID thread
        > slightly undersize, then make additional cuts, just slightly
        adjusting
        > the tool position, similar to the method used for OD thread diameter
        > adjustment.

        Here I meant to say, until the plug gage can be screwed into the id of
        the "nut".

        Fred Smith - IMService
      • baldysm
        Makes sense so far. Can I test the thread, change my X0 as necessary, and then rerun the same program recutting the same thread? On a manual lathe, you can
        Message 3 of 5 , Mar 1, 2006
        • 0 Attachment
          Makes sense so far.

          Can I test the thread, change my X0 as necessary, and then rerun the same
          program recutting the same thread?

          On a manual lathe, you can take another threading pass as long as you engage
          the threading dial at the right location and keep going deeper until you get
          a proper fit. I cut threads all the time on a manual lathe.

          If you cut a thread on a CNC lathe, using IMService's servos, encoder, and
          DeskCNC, can you "make another pass"? Will DeskCNC remember (and adjust if
          the spindle moved while testing the thread) the relationship between the
          spindle and the tool position if I need to rerun the program?

          Thanks

          Scott Meyer
          http://www.penpride.com
          http://www.onlyonecreations.com
          Creating artistic handcrafted pens of all types for special gifts,
          collectors, and corporations.


          -----Original Message-----
          From: SherlineCNC@yahoogroups.com [mailto:SherlineCNC@yahoogroups.com] On
          Behalf Of Fred Smith
          Sent: Wednesday, March 01, 2006 12:01 PM
          To: SherlineCNC@yahoogroups.com
          Subject: [SherlineCNC] Re: threading

          --- In SherlineCNC@yahoogroups.com, "Fred Smith" <imserv@...> wrote:
          > Make a plug gage by using a pitch gage to assure that the "nut" you
          > are making will fit other screws.

          By pitch gage I meant, by measuring with thread wires, or a pitch mic.

          >Cut the ID thread
          > slightly undersize, then make additional cuts, just slightly
          adjusting
          > the tool position, similar to the method used for OD thread diameter
          > adjustment.

          Here I meant to say, until the plug gage can be screwed into the id of the
          "nut".

          Fred Smith - IMService







          Yahoo! Groups Links
        • Fred Smith
          ... the same ... If you cut a thread on a CNC lathe, using IMService s servos, encoder, and ... adjust if ... between the ... Yes, of course, if you adjust
          Message 4 of 5 , Mar 2, 2006
          • 0 Attachment
            --- In SherlineCNC@yahoogroups.com, "baldysm" <baldysm@...> wrote:

            > Can I test the thread, change my X0 as necessary, and then rerun
            the same
            > program recutting the same thread?
            >

            If you cut a thread on a CNC lathe, using IMService's servos,
            encoder, and
            > DeskCNC, can you "make another pass"? Will DeskCNC remember (and
            adjust if
            > the spindle moved while testing the thread) the relationship
            between the
            > spindle and the tool position if I need to rerun the program?

            Yes, of course, if you adjust only the X coordinate position. The
            encoder tracks spindle index and 2000 incremental positions per
            revolution.

            You can also chuck up a threaded part and pick up the thread by
            using the servo reset button (cutting out the servo power) and
            turning the X and Z handles so the tool lines up with the part to be
            repaired. Just turn off the spindle in the middle of a programmed
            cut ( not the first pass) and the tool will stop moving, use the
            hand wheels to move in close and make sure the tool tip is right up
            against the trailing flank of the thread. Release the servo reset
            button and resume the threading cycle.

            Fred Smith - IMService
            http://www.cadcamcadcam.com/hobby
          Your message has been successfully submitted and would be delivered to recipients shortly.