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

Re: CNC tapping

Expand Messages
  • neilalbert2001
    Marcus, Thanks. I intend to tap a lot of holes, so anything to speed it up would be helpful. also I am tapping platic, so I don t expect many broken taps.
    Message 1 of 25 , Oct 12, 2004
    View Source
    • 0 Attachment
      Marcus,


      Thanks. I intend to tap a lot of holes, so anything to speed it up
      would be helpful. also I am tapping platic, so I don't expect many
      broken taps. However, I think your pointing out that CNC'g to each
      hole position helps, and the mill keeps the tap vertical. I indeed
      appreciate you sharing your extensive experience in approaching this
      particular problem. Your approach using the drill chuck in an end mill
      seems like a notch or two better than what I did the last time, which
      was mount a 4-jaw chuck on the spindle, and use it to guide a tap
      handle as I turned the handle and tap manually.


      Neil
      --- In SherlineCNC@yahoogroups.com, "Marcus and Eva" <implmex@a...> wrote:
      > Hi Tony and others:
      > I've got a CNC that has the whole nine yards on it (rigid
      tapping, which
      > means the spindle can be timed to rotate at the correct speed while
      the Z
      > axis drives down at the right rate) and you know how I end up doing
      most of
      > my tapping???
      > I stick a drill chuck on a stubby arbor into an end mill holder.
      > I position the drill chuck with tap in it over the hole.
      > I drop the spindle down till the tap is within 1/4" of the top of
      the hole.
      > I release the setscrew that holds the stub arbor in the endmill
      holder so
      > the tap and drill chuck can drop down.
      > I spin the chuck by hand to get the tap started.
      > I back it out by hand and move to the next hole.
      > I finish the holes with a tap wrench by hand.
      >
      > Why do I do this, you ask, when I've got the full meal deal on the super
      > dooper CNC???
      > Because it's faster for small numbers of holes, and because it's a
      lot less
      > risky.
      > Setting up for production tapping can be a royal pain in the rear.
      > It just ain't worth it for only a few holes, especially if you bust
      a tap!!!
      >
      > It's awfully tempting to think you'll reap tremendous benefits by
      harnessing
      > all this cool technology...I did it too when I first got the machine.
      > Interestingly, I find myself moving away from CNC for many
      operations as I
      > get better at identifying which ones will be time wasters.
      > I'd find myself piddling away hours of time to do a 5 minute job, and
      > holemaking has been one of the worst offenders for my kind of work
      > (moldmaking).
      > I had to EDM out a lot more broken taps too, ususally from slamming
      the tap
      > into a chip at the bottom of the hole.
      >
      > I'd recommend staying away from tapping heads and fancy CNC rigs for the
      > homebrew setup unless you've got hundreds or thousands of holes to
      tap on a
      > typical job.
      > Anything less than 30 holes or so, and I don't bother with the tapping
      > setup...even when I've co-ordinate drilled the holes in the CNC.
      > Of course, I still position the tap over all the locations with the CNC.
      >
      > Cheers
      >
      > Marcus
    • john_haddy
      You might like to try thread milling. Provided that your controller will handle helical toolpaths, there s no need to have your spindle sync d to the motion.
      Message 2 of 25 , Oct 13, 2004
      View Source
      • 0 Attachment
        You might like to try thread milling. Provided that your
        controller will handle helical toolpaths, there's no need
        to have your spindle sync'd to the motion. There's also
        lower cutting forces required, since you're effectively
        milling just a small part of the thread at a time.

        Check out

        http://www.sct-usa.com/millhelp.asp
        http://www.toolfab.com/schmarje/threadmills.html
        http://www.micro100.com/Inch/m100page2.html
        http://www.micro100.com/Downloads/ThreadMillAssist.htm

        Although many of the professional threadmills are multi-thread,
        there's no particular reason why you couldn't grind a single
        point tool (like an internal threading boring bar for a lathe)
        if you weren't in a tremendous hurry.

        John Haddy
        Sydney, Australia


        --- In SherlineCNC@yahoogroups.com, "neilalbert2001"
        <neilalbert@c...> wrote:
        >
        > Marcus,
        >
        >
        > Thanks. I intend to tap a lot of holes, so anything to speed it up
        > would be helpful. also I am tapping platic, so I don't expect many
        > broken taps. However, I think your pointing out that CNC'g to each
        > hole position helps, and the mill keeps the tap vertical. I indeed
        > appreciate you sharing your extensive experience in approaching this
        > particular problem. Your approach using the drill chuck in an end
        mill
        > seems like a notch or two better than what I did the last time,
        which
        > was mount a 4-jaw chuck on the spindle, and use it to guide a tap
        > handle as I turned the handle and tap manually.
        >
        >
        > Neil
        > --- In SherlineCNC@yahoogroups.com, "Marcus and Eva" <implmex@a...>
        wrote:
        > > Hi Tony and others:
        > > I've got a CNC that has the whole nine yards on it (rigid
        > tapping, which
        > > means the spindle can be timed to rotate at the correct speed
        while
        > the Z
        > > axis drives down at the right rate) and you know how I end up
        doing
        > most of
        > > my tapping???
        > > I stick a drill chuck on a stubby arbor into an end mill holder.
        > > I position the drill chuck with tap in it over the hole.
        > > I drop the spindle down till the tap is within 1/4" of the top of
        > the hole.
        > > I release the setscrew that holds the stub arbor in the endmill
        > holder so
        > > the tap and drill chuck can drop down.
        > > I spin the chuck by hand to get the tap started.
        > > I back it out by hand and move to the next hole.
        > > I finish the holes with a tap wrench by hand.
        > >
        > > Why do I do this, you ask, when I've got the full meal deal on
        the super
        > > dooper CNC???
        > > Because it's faster for small numbers of holes, and because it's a
        > lot less
        > > risky.
        > > Setting up for production tapping can be a royal pain in the rear.
        > > It just ain't worth it for only a few holes, especially if you
        bust
        > a tap!!!
        > >
        > > It's awfully tempting to think you'll reap tremendous benefits by
        > harnessing
        > > all this cool technology...I did it too when I first got the
        machine.
        > > Interestingly, I find myself moving away from CNC for many
        > operations as I
        > > get better at identifying which ones will be time wasters.
        > > I'd find myself piddling away hours of time to do a 5 minute job,
        and
        > > holemaking has been one of the worst offenders for my kind of work
        > > (moldmaking).
        > > I had to EDM out a lot more broken taps too, ususally from
        slamming
        > the tap
        > > into a chip at the bottom of the hole.
        > >
        > > I'd recommend staying away from tapping heads and fancy CNC rigs
        for the
        > > homebrew setup unless you've got hundreds or thousands of holes to
        > tap on a
        > > typical job.
        > > Anything less than 30 holes or so, and I don't bother with the
        tapping
        > > setup...even when I've co-ordinate drilled the holes in the CNC.
        > > Of course, I still position the tap over all the locations with
        the CNC.
        > >
        > > Cheers
        > >
        > > Marcus
      • Fred Smith
        ... axis? The Sherline lathe threading attachment will synchronize the spindle rotation to the Z axis. As far as I know that is the only device that you can
        Message 3 of 25 , Oct 13, 2004
        View Source
        • 0 Attachment
          --- In SherlineCNC@yahoogroups.com, "neilalbert2001"
          <neilalbert@c...> wrote:
          >
          > Is there a way I could use my 2000 mill to turn a 1/4-20 tap into
          > fairly soft plastic to make 4 threaded holes at the corners of a
          > rectangle measuring 9" x 3-5/8", possibly with the use of a rotary
          > table? Is there a way to mount a Sherline rotary table onto the Z
          axis?

          The Sherline lathe threading attachment will synchronize the spindle
          rotation to the Z axis. As far as I know that is the only device
          that you can use without replacing the spindle controller with a
          servo motor and encoder. There might be a way to rig this up for
          tapping.

          If you replaced the spindle motor with a servo motor and encoder, you
          can use the sherline CNC mill as a tapping machine. Just treat it as
          a rotary axis in your controller software. A little bit of spring
          tension on the tap holder will allow you to disregard any backlash or
          slop in the setup.

          Fred Smith - IMService
        • Marcus and Eva
          Hi Neil: If you re contemplating a production setup or there is a low risk of smashing taps (through holes are very nice!!), then all of what I said no longer
          Message 4 of 25 , Oct 13, 2004
          View Source
          • 0 Attachment
            Hi Neil:
            If you're contemplating a production setup or there is a low risk of
            smashing taps (through holes are very nice!!), then all of what I said no
            longer applies.
            The key is to assess the risk and cost of unattended tapping with which you
            cannot intervene, vs the economies you can achieve.
            Add into that, whether you can do other productive work while the tapping is
            in progress, and your decision may well be to automate for this particular
            job.
            What I wished to point out primarily, is that setting up and automating
            carries a cost too, and that fact sems to be often forgotten in the
            enthusiasm for driving the cool new toy.
            The hybrid hand method I described is pretty quick, and needs no expensive
            gadgets.
            It can be done just as well on a Sherline as on my Haas.
            Best of all, you can stop before the big crack (snapping sound of the tap
            hitting the chip at the bottom of the hole and breaking in half).
            So, if you're going to do this on a Sherline, get yourself a 3/8" endmill
            holder, and a spare #1 MT drill chuck arbor.
            Turn the arbor down to 3/8" diameter (I think you'll have enough meat on the
            arbor to get 3/8" diameter but better check before you buy!!)
            Make it a nice easy sliding fit in the endmill holder and you're all set.
            If you want, you can make a big knurled collar for the drill chuck
            too...that way you can spin it quickly...very nice to back the tap out fast.
            Cheers

            Marcus
          • Marcus and Eva
            Hi John: You are correct; this is an excellent method for achieving threaded holes. A couple of limiting factors all should be aware of: 1) Aspect ratio (hole
            Message 5 of 25 , Oct 13, 2004
            View Source
            • 0 Attachment
              Hi John:
              You are correct; this is an excellent method for achieving threaded
              holes.
              A couple of limiting factors all should be aware of:
              1) Aspect ratio (hole depth vs hole diameter) is important in thread
              milling...far more so than in tapping, so deep narrow holes are poor choices
              for this technique.
              2) There is a practical lower limit to the diameter you can threadmill...I
              haven't found it yet, but the smallest I've gone is #10:40 about 3/8" deep.
              3) The biggest challenge is getting the cutting tool... I can cheat here
              because I'm very well set up for cutter grinding, but for most, this is the
              big obstacle if they can't readily get a commercial tool.
              Sometimes a broken tap can be pressed into service by grinding off every
              point save one.
              Pick the finest pitch, biggest diameter one you can...the lead of a coarse
              pitch tap will make it rub on the trailing flank if it's used as a
              threadmill.
              4) High lead helices don't threadmill well..the helix angle creates
              interference with the trailing aspect of the cutter (it's really a single
              tooth saw) so the threadform becomes badly distorted: coarse pitch and small
              diameter threads are no good for this technique.
              5) The mechanical condition of the machine is highly important...it's
              essential to have no backlash in X and Y to avoid major distortion of the
              threadform...so you really need a ballscrew or recently mogliced machine to
              do this acceptably well.
              Cheers

              Marcus
            • Neil Albert
              I m sure you re right, Alan. The small holes, although they make coming up with a cutter a little tricky, would not impart much X-Y motion on what is already a
              Message 6 of 25 , Oct 13, 2004
              View Source
              • 0 Attachment
                I'm sure you're right, Alan. The small holes, although they make coming up
                with a cutter a little tricky, would not impart much X-Y motion on what is
                already a big part for a Sherline.

                Should I expect any any reduction in speed from the controller due to the
                small radius, or will the fact that it is a fixed radius run by a single
                G02/G03 command allow it to feed as fast as asked for?

                Neil
                -----Original Message-----
                From:
                sentto-10186656-4724-1097688324-neilalbert=compuserve.com@...
                oo.com
                [mailto:sentto-10186656-4724-1097688324-neilalbert=compuserve.com@...
                oups.yahoo.com]On Behalf Of Alan Marconett
                Sent: Wednesday, October 13, 2004 2:26 PM
                To: SherlineCNC@yahoogroups.com
                Subject: Re: [SherlineCNC] CNC tapping


                Hi Neil,

                You could probably use helical arcs, these would move down in Z while
                moving a single point cutter around an arc. 1/4-20 is a little small,
                but with the right cutter...

                Alan KM6VV

                neilalbert2001 wrote:

                >
                > Is there a way I could use my 2000 mill to turn a 1/4-20 tap into
                > fairly soft plastic to make 4 threaded holes at the corners of a
                > rectangle measuring 9" x 3-5/8", possibly with the use of a rotary
                > table? Is there a way to mount a Sherline rotary table onto the Z axis?
                >
                > Neil
                >



                Yahoo! Groups Sponsor
                ADVERTISEMENT





                ----------------------------------------------------------------------------
                --
                Yahoo! Groups Links

                a.. To visit your group on the web, go to:
                http://groups.yahoo.com/group/SherlineCNC/

                b.. To unsubscribe from this group, send an email to:
                SherlineCNC-unsubscribe@yahoogroups.com

                c.. Your use of Yahoo! Groups is subject to the Yahoo! Terms of Service.



                [Non-text portions of this message have been removed]
              • Alan Marconett
                Hi Neil, You could probably use helical arcs, these would move down in Z while moving a single point cutter around an arc. 1/4-20 is a little small, but with
                Message 7 of 25 , Oct 13, 2004
                View Source
                • 0 Attachment
                  Hi Neil,

                  You could probably use helical arcs, these would move down in Z while
                  moving a single point cutter around an arc. 1/4-20 is a little small,
                  but with the right cutter...

                  Alan KM6VV

                  neilalbert2001 wrote:

                  >
                  > Is there a way I could use my 2000 mill to turn a 1/4-20 tap into
                  > fairly soft plastic to make 4 threaded holes at the corners of a
                  > rectangle measuring 9" x 3-5/8", possibly with the use of a rotary
                  > table? Is there a way to mount a Sherline rotary table onto the Z axis?
                  >
                  > Neil
                  >
                • Neil Albert
                  Alan, I just tried a helical arc of 8mm diameter and even at 500mm/min, it s slow, because of the repeated acceleration and deceleration of each axis. Neil ...
                  Message 8 of 25 , Oct 13, 2004
                  View Source
                  • 0 Attachment
                    Alan,

                    I just tried a helical arc of 8mm diameter and even at 500mm/min, it's slow,
                    because of the repeated acceleration and deceleration
                    of each axis.

                    Neil
                    -----Original Message-----
                    From:
                    sentto-10186656-4724-1097688324-neilalbert=compuserve.com@...
                    oo.com
                    [mailto:sentto-10186656-4724-1097688324-neilalbert=compuserve.com@...
                    oups.yahoo.com]On Behalf Of Alan Marconett
                    Sent: Wednesday, October 13, 2004 2:26 PM
                    To: SherlineCNC@yahoogroups.com
                    Subject: Re: [SherlineCNC] CNC tapping


                    Hi Neil,

                    You could probably use helical arcs, these would move down in Z while
                    moving a single point cutter around an arc. 1/4-20 is a little small,
                    but with the right cutter...

                    Alan KM6VV

                    neilalbert2001 wrote:

                    >
                    > Is there a way I could use my 2000 mill to turn a 1/4-20 tap into
                    > fairly soft plastic to make 4 threaded holes at the corners of a
                    > rectangle measuring 9" x 3-5/8", possibly with the use of a rotary
                    > table? Is there a way to mount a Sherline rotary table onto the Z axis?
                    >
                    > Neil
                    >



                    Yahoo! Groups Sponsor
                    ADVERTISEMENT





                    ----------------------------------------------------------------------------
                    --
                    Yahoo! Groups Links

                    a.. To visit your group on the web, go to:
                    http://groups.yahoo.com/group/SherlineCNC/

                    b.. To unsubscribe from this group, send an email to:
                    SherlineCNC-unsubscribe@yahoogroups.com

                    c.. Your use of Yahoo! Groups is subject to the Yahoo! Terms of Service.



                    [Non-text portions of this message have been removed]
                  • Alan Marconett
                    HI Marcus, Very good points! Well stated. I agree, although I don t have a full boat shop. I don t have a stubby arbor, I just remove the drawbar holding
                    Message 9 of 25 , Oct 13, 2004
                    View Source
                    • 0 Attachment
                      HI Marcus,

                      Very good points! Well stated. I agree, although I don't have a "full
                      boat" shop. I don't have a stubby arbor, I just remove the drawbar
                      holding the drill chuck, and do about the same thing with the taper
                      loosened in the spindle. It draws out as the hole is tapped. But I
                      like the stubby arbor idea. What if the arbor was long, went all the
                      way up through the spindle, and had some sort of quick disconnect device
                      above the pulleys? Something similar to the sensitive drill attachment.
                      I too like using CNC to position to holes to tap after I've already
                      CNC drilled them.

                      A tommy bar in the holes of the chuck give me a little leverage to turn
                      the chuck and the tap. Although I like to finish the thread while I'm
                      at it.

                      Alan KM6VV


                      Marcus and Eva wrote:

                      > Hi Tony and others:
                      > I've got a CNC that has the whole nine yards on it (rigid tapping, which
                      > means the spindle can be timed to rotate at the correct speed while the Z
                      > axis drives down at the right rate) and you know how I end up doing most of
                      > my tapping???
                      > I stick a drill chuck on a stubby arbor into an end mill holder.
                      > I position the drill chuck with tap in it over the hole.
                      > I drop the spindle down till the tap is within 1/4" of the top of the hole.
                      > I release the setscrew that holds the stub arbor in the endmill holder so
                      > the tap and drill chuck can drop down.
                      > I spin the chuck by hand to get the tap started.
                      > I back it out by hand and move to the next hole.
                      > I finish the holes with a tap wrench by hand.
                      >
                      > Why do I do this, you ask, when I've got the full meal deal on the super
                      > dooper CNC???
                      > Because it's faster for small numbers of holes, and because it's a lot less
                      > risky.
                      > Setting up for production tapping can be a royal pain in the rear.
                      > It just ain't worth it for only a few holes, especially if you bust a tap!!!
                      >
                      > It's awfully tempting to think you'll reap tremendous benefits by harnessing
                      > all this cool technology...I did it too when I first got the machine.
                      > Interestingly, I find myself moving away from CNC for many operations as I
                      > get better at identifying which ones will be time wasters.
                      > I'd find myself piddling away hours of time to do a 5 minute job, and
                      > holemaking has been one of the worst offenders for my kind of work
                      > (moldmaking).
                      > I had to EDM out a lot more broken taps too, ususally from slamming the tap
                      > into a chip at the bottom of the hole.
                      >
                      > I'd recommend staying away from tapping heads and fancy CNC rigs for the
                      > homebrew setup unless you've got hundreds or thousands of holes to tap on a
                      > typical job.
                      > Anything less than 30 holes or so, and I don't bother with the tapping
                      > setup...even when I've co-ordinate drilled the holes in the CNC.
                      > Of course, I still position the tap over all the locations with the CNC.
                      >
                      > Cheers
                      >
                      > Marcus
                    • Alan Marconett
                      Hi Neil, The downward motion is but a small fraction of the XY motion, so it shouldn t matter. That said, I don t know how well TurboCNC does helical arcs,
                      Message 10 of 25 , Oct 13, 2004
                      View Source
                      • 0 Attachment
                        Hi Neil,

                        The downward motion is but a small fraction of the XY motion, so it
                        shouldn't matter. That said, I don't know how well TurboCNC does
                        helical arcs, there have been speed problems on arcs before.

                        Marcus reminded me how easy it is to just use a tap in a slip-mount.
                        It's the way I always do it, and I'd have to recommend it over helical
                        cuts, which are really more appropriate for larger diameters (remember
                        your backlash and the tooling required).

                        OF COURSE, if you had a tapmatic ($200+) to use in a drill press...
                        But plastic is to easy to tap anyway.

                        Alan KM6VV


                        Neil Albert wrote:

                        > I'm sure you're right, Alan. The small holes, although they make coming up
                        > with a cutter a little tricky, would not impart much X-Y motion on what is
                        > already a big part for a Sherline.
                        >
                        > Should I expect any any reduction in speed from the controller due to the
                        > small radius, or will the fact that it is a fixed radius run by a single
                        > G02/G03 command allow it to feed as fast as asked for?
                        >
                        > Neil
                        > -----Original Message-----
                        > From:
                        > sentto-10186656-4724-1097688324-neilalbert=compuserve.com@...
                        > oo.com
                        > [mailto:sentto-10186656-4724-1097688324-neilalbert=compuserve.com@...
                        > oups.yahoo.com]On Behalf Of Alan Marconett
                        > Sent: Wednesday, October 13, 2004 2:26 PM
                        > To: SherlineCNC@yahoogroups.com
                        > Subject: Re: [SherlineCNC] CNC tapping
                        >
                        >
                        > Hi Neil,
                        >
                        > You could probably use helical arcs, these would move down in Z while
                        > moving a single point cutter around an arc. 1/4-20 is a little small,
                        > but with the right cutter...
                        >
                        > Alan KM6VV
                        >
                        > neilalbert2001 wrote:
                        >
                        > >
                        > > Is there a way I could use my 2000 mill to turn a 1/4-20 tap into
                        > > fairly soft plastic to make 4 threaded holes at the corners of a
                        > > rectangle measuring 9" x 3-5/8", possibly with the use of a rotary
                        > > table? Is there a way to mount a Sherline rotary table onto the Z axis?
                        > >
                        > > Neil
                        > >
                        >
                      • Alan Marconett
                        HI Neil, Maybe you can up your acceleration a little? I don t have mine optimized all the way out . A higher starting speed might also help. I believe Tony
                        Message 11 of 25 , Oct 13, 2004
                        View Source
                        • 0 Attachment
                          HI Neil,

                          Maybe you can up your acceleration a little? I don't have mine
                          optimized "all the way out". A higher starting speed might also help.

                          I believe Tony posted some steps for optimizing last week or so on the
                          TurboCNC list.

                          Alan KM6VV

                          Neil Albert wrote:

                          > Alan,
                          >
                          > I just tried a helical arc of 8mm diameter and even at 500mm/min, it's slow,
                          > because of the repeated acceleration and deceleration
                          > of each axis.
                          >
                          > Neil
                          >
                          > Subject: Re: [SherlineCNC] CNC tapping
                          >
                          >
                          > Hi Neil,
                          >
                          > You could probably use helical arcs, these would move down in Z while
                          > moving a single point cutter around an arc. 1/4-20 is a little small,
                          > but with the right cutter...
                          >
                          > Alan KM6VV
                          >
                          > neilalbert2001 wrote:
                          >
                          > >
                          > > Is there a way I could use my 2000 mill to turn a 1/4-20 tap into
                          > > fairly soft plastic to make 4 threaded holes at the corners of a
                          > > rectangle measuring 9" x 3-5/8", possibly with the use of a rotary
                          > > table? Is there a way to mount a Sherline rotary table onto the Z axis?
                          > >
                          > > Neil
                        • Tom Hubin
                          ... ********************* Hello Neil, I use single thread mills that I get from MSC. Thread mills can cut inside or outside, right or left handed, and a range
                          Message 12 of 25 , Oct 13, 2004
                          View Source
                          • 0 Attachment
                            neilalbert2001 wrote:
                            >
                            > Is there a way I could use my 2000 mill to turn a 1/4-20 tap into
                            > fairly soft plastic to make 4 threaded holes at the corners of a
                            > rectangle measuring 9" x 3-5/8", possibly with the use of a rotary
                            > table? Is there a way to mount a Sherline rotary table onto the Z axis?
                            >
                            > Neil

                            *********************

                            Hello Neil,

                            I use single thread mills that I get from MSC. Thread mills can cut
                            inside or outside, right or left handed, and a range of diameters and
                            threads for each bit. At $40 to $55 they seem pricey until you get used
                            to using one.

                            I routinely cut 4-40 threads in 0.275 inch deep blind holes. I also do
                            1.008 inch diameter 40 tpi threads that mate with lens tubes from
                            Thorlabs.

                            You should be able to do 1/4-20 with the tool below. MSC has several
                            models depending on the range of threads and diameters needed.

                            http://www1.mscdirect.com/CGI/NNSRIT?PARTPG=NNLMK32&PMPXNO=4412210

                            Many Gcode interpreters, like TurboCnc and EMC, can generate a helical
                            path. No synchronization with spindle rotation needed. Some interpreters
                            use G72 and G73 for helix and some use G02 and G03 circles with Z
                            parameter added to specify a helix rather than a simple circle.

                            Manufacturers seem to recommend that the cutting start at the bottom of
                            the hole and climb mill out of the hole. I find that works well. Very
                            little debris but it is below the tool. Also, spindle is being lifted
                            against gravity so no sudden lurches downward as backlash slips.

                            Execute slowly the first couple of runs while watching closely. If you
                            mess up royally you will break an expensive bit. When I am sure of the
                            path I plunge into the open hole at 5 inches per minute and mill the
                            helix at 15 inches per minute. My max speed is for rapids 20 inches per
                            minute. I seldom program faster than 15 ipm when cutting aluminum 6061.

                            BTW, if you do break the bit, it won't be stuck in your workpiece. No
                            EDM needed. Just mourn the loss of the bit and get another. If no thread
                            mill available then tap by hand the old fashioned way.

                            Tom Hubin
                            thubin@...
                          • Neil Albert
                            Thanks, Tom. Sorry that I didn t get to read your post until now. I am guessing that the thread mill will allow a greater depth of thread to be cut with fewer
                            Message 13 of 25 , Oct 18, 2004
                            View Source
                            • 0 Attachment
                              Thanks, Tom.

                              Sorry that I didn't get to read your post until now.

                              I am guessing that the thread mill will allow a greater depth of thread to
                              be cut with fewer rotations than using a single point cutter.

                              This sounds very interesting. I had contemplated using thread mills for
                              another task in the past, but ended up doing it
                              using a single point cutter, because I new that I might have to use a non
                              standard thread pitch, and the cost was too high for experimentation.


                              Neil
                              -----Original Message-----
                              From:
                              sentto-10186656-4730-1097696796-neilalbert=compuserve.com@...
                              oo.com
                              [mailto:sentto-10186656-4730-1097696796-neilalbert=compuserve.com@...
                              oups.yahoo.com]On Behalf Of Tom Hubin
                              Sent: Wednesday, October 13, 2004 4:48 PM
                              To: SherlineCNC@yahoogroups.com
                              Subject: Re: [SherlineCNC] CNC tapping


                              neilalbert2001 wrote:
                              >
                              > Is there a way I could use my 2000 mill to turn a 1/4-20 tap into
                              > fairly soft plastic to make 4 threaded holes at the corners of a
                              > rectangle measuring 9" x 3-5/8", possibly with the use of a rotary
                              > table? Is there a way to mount a Sherline rotary table onto the Z axis?
                              >
                              > Neil

                              *********************

                              Hello Neil,

                              I use single thread mills that I get from MSC. Thread mills can cut
                              inside or outside, right or left handed, and a range of diameters and
                              threads for each bit. At $40 to $55 they seem pricey until you get used
                              to using one.

                              I routinely cut 4-40 threads in 0.275 inch deep blind holes. I also do
                              1.008 inch diameter 40 tpi threads that mate with lens tubes from
                              Thorlabs.

                              You should be able to do 1/4-20 with the tool below. MSC has several
                              models depending on the range of threads and diameters needed.

                              http://www1.mscdirect.com/CGI/NNSRIT?PARTPG=NNLMK32&PMPXNO=4412210

                              Many Gcode interpreters, like TurboCnc and EMC, can generate a helical
                              path. No synchronization with spindle rotation needed. Some interpreters
                              use G72 and G73 for helix and some use G02 and G03 circles with Z
                              parameter added to specify a helix rather than a simple circle.

                              Manufacturers seem to recommend that the cutting start at the bottom of
                              the hole and climb mill out of the hole. I find that works well. Very
                              little debris but it is below the tool. Also, spindle is being lifted
                              against gravity so no sudden lurches downward as backlash slips.

                              Execute slowly the first couple of runs while watching closely. If you
                              mess up royally you will break an expensive bit. When I am sure of the
                              path I plunge into the open hole at 5 inches per minute and mill the
                              helix at 15 inches per minute. My max speed is for rapids 20 inches per
                              minute. I seldom program faster than 15 ipm when cutting aluminum 6061.

                              BTW, if you do break the bit, it won't be stuck in your workpiece. No
                              EDM needed. Just mourn the loss of the bit and get another. If no thread
                              mill available then tap by hand the old fashioned way.

                              Tom Hubin
                              thubin@...


                              Yahoo! Groups Sponsor
                              ADVERTISEMENT





                              ----------------------------------------------------------------------------
                              --
                              Yahoo! Groups Links

                              a.. To visit your group on the web, go to:
                              http://groups.yahoo.com/group/SherlineCNC/

                              b.. To unsubscribe from this group, send an email to:
                              SherlineCNC-unsubscribe@yahoogroups.com

                              c.. Your use of Yahoo! Groups is subject to the Yahoo! Terms of Service.



                              [Non-text portions of this message have been removed]
                            • Neil Albert
                              Tom, I m confused by the specs on this 1/4 thread mill sold by MSC http://www1.mscdirect.com/CGI/NNSRIT?PARTPG=NNLMK32&PMPXNO=4412210 I just looked st the
                              Message 14 of 25 , Oct 18, 2004
                              View Source
                              • 0 Attachment
                                Tom,


                                I'm confused by the specs on this 1/4" thread mill sold by MSC
                                http://www1.mscdirect.com/CGI/NNSRIT?PARTPG=NNLMK32&PMPXNO=4412210

                                I just looked st the specs with its photo, and see what is I guess is called
                                a "Single Profile" type thread mill,
                                since it has no Z height like some others I've seen. However, the length of
                                cut is listed as 0.4".

                                Does this make sense to you? That doesn't seem to correlate to the
                                circumference, either, if that's how LOC is specified in thread mills

                                However, it seems like a nice generic tool in that it is single profile, and
                                would tend not to get clogged at all, which I had envisioned happening with
                                the mutiple profile thread mill in plastic, which is what I would be using
                                it for.

                                Neil


                                -----Original Message-----
                                From:
                                sentto-10186656-4730-1097696796-neilalbert=compuserve.com@...
                                oo.com
                                [mailto:sentto-10186656-4730-1097696796-neilalbert=compuserve.com@...
                                oups.yahoo.com]On Behalf Of Tom Hubin
                                Sent: Wednesday, October 13, 2004 4:48 PM
                                To: SherlineCNC@yahoogroups.com
                                Subject: Re: [SherlineCNC] CNC tapping


                                neilalbert2001 wrote:
                                >
                                > Is there a way I could use my 2000 mill to turn a 1/4-20 tap into
                                > fairly soft plastic to make 4 threaded holes at the corners of a
                                > rectangle measuring 9" x 3-5/8", possibly with the use of a rotary
                                > table? Is there a way to mount a Sherline rotary table onto the Z axis?
                                >
                                > Neil

                                *********************

                                Hello Neil,

                                I use single thread mills that I get from MSC. Thread mills can cut
                                inside or outside, right or left handed, and a range of diameters and
                                threads for each bit. At $40 to $55 they seem pricey until you get used
                                to using one.

                                I routinely cut 4-40 threads in 0.275 inch deep blind holes. I also do
                                1.008 inch diameter 40 tpi threads that mate with lens tubes from
                                Thorlabs.

                                You should be able to do 1/4-20 with the tool below. MSC has several
                                models depending on the range of threads and diameters needed.

                                http://www1.mscdirect.com/CGI/NNSRIT?PARTPG=NNLMK32&PMPXNO=4412210

                                Many Gcode interpreters, like TurboCnc and EMC, can generate a helical
                                path. No synchronization with spindle rotation needed. Some interpreters
                                use G72 and G73 for helix and some use G02 and G03 circles with Z
                                parameter added to specify a helix rather than a simple circle.

                                Manufacturers seem to recommend that the cutting start at the bottom of
                                the hole and climb mill out of the hole. I find that works well. Very
                                little debris but it is below the tool. Also, spindle is being lifted
                                against gravity so no sudden lurches downward as backlash slips.

                                Execute slowly the first couple of runs while watching closely. If you
                                mess up royally you will break an expensive bit. When I am sure of the
                                path I plunge into the open hole at 5 inches per minute and mill the
                                helix at 15 inches per minute. My max speed is for rapids 20 inches per
                                minute. I seldom program faster than 15 ipm when cutting aluminum 6061.

                                BTW, if you do break the bit, it won't be stuck in your workpiece. No
                                EDM needed. Just mourn the loss of the bit and get another. If no thread
                                mill available then tap by hand the old fashioned way.

                                Tom Hubin
                                thubin@...


                                Yahoo! Groups Sponsor
                                ADVERTISEMENT





                                ----------------------------------------------------------------------------
                                --
                                Yahoo! Groups Links

                                a.. To visit your group on the web, go to:
                                http://groups.yahoo.com/group/SherlineCNC/

                                b.. To unsubscribe from this group, send an email to:
                                SherlineCNC-unsubscribe@yahoogroups.com

                                c.. Your use of Yahoo! Groups is subject to the Yahoo! Terms of Service.



                                [Non-text portions of this message have been removed]
                              • Tom Hubin
                                Hello Neil, The 0.4 inch length of cut is the max depth in which you can insert the tool. That means that only 0.4 inches of the shank, just above the teeth,
                                Message 15 of 25 , Oct 18, 2004
                                View Source
                                • 0 Attachment
                                  Hello Neil,

                                  The 0.4 inch length of cut is the max depth in which you can insert the
                                  tool. That means that only 0.4 inches of the shank, just above the
                                  teeth, is narrower than the teeth. The rest of the shank is wider than
                                  the teeth so cannot go into the hole.

                                  MSC has a variety of "length of cut" for several of their thread mills.
                                  Shorter is more rigid and better choice if you don't need lots of depth.
                                  Longer is available if you really need it or just want to be able to use
                                  it for a greater variety of hole depths.

                                  I often thread mill a little too tight for screws. I use a standard
                                  bottom tap afterward to true up the threads. I do this mostly cuz I
                                  sometimes cannot hit the perfect diameter for small threads like 4-40.
                                  Cleaning up thread milled threads with a hand tap is a lot easier than
                                  hand tapping a blank hole from scratch.

                                  Also, many manufacturers suggest threadmilling from the bottom up rather
                                  than from the top down like you must do with a hand tap. They don't say
                                  why this is better but I can think of two reasons. Chips fall to the
                                  bottom but the cutter is exiting the hole so no matter. Z axis is rising
                                  and pulling against weight of spindle so no backlash problems like
                                  sudden shift.

                                  Tom Hubin
                                  thubin@...

                                  *********************************

                                  Neil Albert wrote:
                                  >
                                  > Tom,
                                  >
                                  > I'm confused by the specs on this 1/4" thread mill sold by MSC
                                  > http://www1.mscdirect.com/CGI/NNSRIT?PARTPG=NNLMK32&PMPXNO=4412210
                                  >
                                  > I just looked st the specs with its photo, and see what is I guess is called
                                  > a "Single Profile" type thread mill,
                                  > since it has no Z height like some others I've seen. However, the length of
                                  > cut is listed as 0.4".
                                  >
                                  > Does this make sense to you? That doesn't seem to correlate to the
                                  > circumference, either, if that's how LOC is specified in thread mills
                                  >
                                  > However, it seems like a nice generic tool in that it is single profile, and
                                  > would tend not to get clogged at all, which I had envisioned happening with
                                  > the mutiple profile thread mill in plastic, which is what I would be using
                                  > it for.
                                  >
                                  > Neil
                                • Marcus and Eva
                                  Hi Tom: Milling from the bottom up with a threadmill will allow you to climb cut the thread if it is a RH thread. Much nicer finish and better size control
                                  Message 16 of 25 , Oct 18, 2004
                                  View Source
                                  • 0 Attachment
                                    Hi Tom:
                                    Milling from the bottom up with a threadmill will allow you to climb
                                    cut the thread if it is a RH thread.
                                    Much nicer finish and better size control too.

                                    Cheers

                                    Marcus
                                    ----- Original Message -----
                                    From: "Tom Hubin" <thubin@...>
                                    To: <SherlineCNC@yahoogroups.com>
                                    Sent: Monday, October 18, 2004 11:24 AM
                                    Subject: Re: [SherlineCNC] CNC tapping


                                    >
                                    > Hello Neil,
                                    >
                                    > The 0.4 inch length of cut is the max depth in which you can insert the
                                    > tool. That means that only 0.4 inches of the shank, just above the
                                    > teeth, is narrower than the teeth. The rest of the shank is wider than
                                    > the teeth so cannot go into the hole.
                                    >
                                    > MSC has a variety of "length of cut" for several of their thread mills.
                                    > Shorter is more rigid and better choice if you don't need lots of depth.
                                    > Longer is available if you really need it or just want to be able to use
                                    > it for a greater variety of hole depths.
                                    >
                                    > I often thread mill a little too tight for screws. I use a standard
                                    > bottom tap afterward to true up the threads. I do this mostly cuz I
                                    > sometimes cannot hit the perfect diameter for small threads like 4-40.
                                    > Cleaning up thread milled threads with a hand tap is a lot easier than
                                    > hand tapping a blank hole from scratch.
                                    >
                                    > Also, many manufacturers suggest threadmilling from the bottom up rather
                                    > than from the top down like you must do with a hand tap. They don't say
                                    > why this is better but I can think of two reasons. Chips fall to the
                                    > bottom but the cutter is exiting the hole so no matter. Z axis is rising
                                    > and pulling against weight of spindle so no backlash problems like
                                    > sudden shift.
                                    >
                                    > Tom Hubin
                                    > thubin@...
                                    >
                                    > *********************************
                                    >
                                    > Neil Albert wrote:
                                    > >
                                    > > Tom,
                                    > >
                                    > > I'm confused by the specs on this 1/4" thread mill sold by MSC
                                    > > http://www1.mscdirect.com/CGI/NNSRIT?PARTPG=NNLMK32&PMPXNO=4412210
                                    > >
                                    > > I just looked st the specs with its photo, and see what is I guess is
                                    called
                                    > > a "Single Profile" type thread mill,
                                    > > since it has no Z height like some others I've seen. However, the length
                                    of
                                    > > cut is listed as 0.4".
                                    > >
                                    > > Does this make sense to you? That doesn't seem to correlate to the
                                    > > circumference, either, if that's how LOC is specified in thread mills
                                    > >
                                    > > However, it seems like a nice generic tool in that it is single profile,
                                    and
                                    > > would tend not to get clogged at all, which I had envisioned happening
                                    with
                                    > > the mutiple profile thread mill in plastic, which is what I would be
                                    using
                                    > > it for.
                                    > >
                                    > > Neil
                                    >
                                    >
                                    >
                                    >
                                    >
                                    > Yahoo! Groups Links
                                    >
                                    >
                                    >
                                    >
                                    >
                                    >
                                    >
                                    >
                                  • Neil Albert
                                    Tom, Thanks. Your explanation makes the LOC very clear. I ordered one, and received it today. The 0.4 LOC may be slightly on the short side. for what I need.
                                    Message 17 of 25 , Oct 19, 2004
                                    View Source
                                    • 0 Attachment
                                      Tom,

                                      Thanks. Your explanation makes the LOC very clear. I ordered one, and
                                      received it today. The 0.4" LOC may be slightly on the short side. for what
                                      I need. Since I plan to only use this for plastic, I believe I could safely
                                      machine the shank down a bit with the green stone I purchased not to long
                                      ago (the cutter is carbide.) However, I'll wait to do this since, if I do
                                      find it useful to follow up with a tap, then maybe I could cut the
                                      additional thread length, which would probably not need to be more than
                                      .125" , with the tap, before I decide to modify the tool.

                                      Thanks again
                                      Neil
                                      -----Original Message-----
                                      From:
                                      sentto-10186656-4772-1098123807-neilalbert=compuserve.com@...
                                      oo.com
                                      [mailto:sentto-10186656-4772-1098123807-neilalbert=compuserve.com@...
                                      oups.yahoo.com]On Behalf Of Tom Hubin
                                      Sent: Monday, October 18, 2004 3:25 PM
                                      To: SherlineCNC@yahoogroups.com
                                      Subject: Re: [SherlineCNC] CNC tapping


                                      Hello Neil,

                                      The 0.4 inch length of cut is the max depth in which you can insert the
                                      tool. That means that only 0.4 inches of the shank, just above the
                                      teeth, is narrower than the teeth. The rest of the shank is wider than
                                      the teeth so cannot go into the hole.

                                      MSC has a variety of "length of cut" for several of their thread mills.
                                      Shorter is more rigid and better choice if you don't need lots of depth.
                                      Longer is available if you really need it or just want to be able to use
                                      it for a greater variety of hole depths.

                                      I often thread mill a little too tight for screws. I use a standard
                                      bottom tap afterward to true up the threads. I do this mostly cuz I
                                      sometimes cannot hit the perfect diameter for small threads like 4-40.
                                      Cleaning up thread milled threads with a hand tap is a lot easier than
                                      hand tapping a blank hole from scratch.

                                      Also, many manufacturers suggest threadmilling from the bottom up rather
                                      than from the top down like you must do with a hand tap. They don't say
                                      why this is better but I can think of two reasons. Chips fall to the
                                      bottom but the cutter is exiting the hole so no matter. Z axis is rising
                                      and pulling against weight of spindle so no backlash problems like
                                      sudden shift.

                                      Tom Hubin
                                      thubin@...

                                      *********************************

                                      Neil Albert wrote:
                                      >
                                      > Tom,
                                      >
                                      > I'm confused by the specs on this 1/4" thread mill sold by MSC
                                      > http://www1.mscdirect.com/CGI/NNSRIT?PARTPG=NNLMK32&PMPXNO=4412210
                                      >
                                      > I just looked st the specs with its photo, and see what is I guess is
                                      called
                                      > a "Single Profile" type thread mill,
                                      > since it has no Z height like some others I've seen. However, the length
                                      of
                                      > cut is listed as 0.4".
                                      >
                                      > Does this make sense to you? That doesn't seem to correlate to the
                                      > circumference, either, if that's how LOC is specified in thread mills
                                      >
                                      > However, it seems like a nice generic tool in that it is single profile,
                                      and
                                      > would tend not to get clogged at all, which I had envisioned happening
                                      with
                                      > the mutiple profile thread mill in plastic, which is what I would be
                                      using
                                      > it for.
                                      >
                                      > Neil


                                      Yahoo! Groups Sponsor
                                      ADVERTISEMENT





                                      ----------------------------------------------------------------------------
                                      --
                                      Yahoo! Groups Links

                                      a.. To visit your group on the web, go to:
                                      http://groups.yahoo.com/group/SherlineCNC/

                                      b.. To unsubscribe from this group, send an email to:
                                      SherlineCNC-unsubscribe@yahoogroups.com

                                      c.. Your use of Yahoo! Groups is subject to the Yahoo! Terms of Service.



                                      [Non-text portions of this message have been removed]
                                    • johnclif@ix.netcom.com
                                      Okay... how do you mill from the bottom up with this threadmill, since you can t put the threadmill into the hole before you start cutting. You could turn the
                                      Message 18 of 25 , Nov 19, 2004
                                      View Source
                                      • 0 Attachment
                                        Okay... how do you mill from the bottom up with this threadmill,
                                        since you can't put the threadmill into the hole before you start
                                        cutting. You could turn the piece upside down and mill from the
                                        bottom DOWN, but what does that get you on a thru-hole? If the hole
                                        is blind, I don't see how you can use this threadmill in any
                                        direction but down.

                                        I also see that it would require the Z feed speed to be very-well
                                        syncronized with RPM. In short, seems like it would work better with
                                        professional machines than with a CNC'd Sherline.

                                        - jgc
                                      • Dave Hylands
                                        Hi John, ... My understanding of thread milling is that the cutting portion of the thread mill is smaller than the hole. And you can threadmill blind holes
                                        Message 19 of 25 , Nov 19, 2004
                                        View Source
                                        • 0 Attachment
                                          Hi John,

                                          > Okay... how do you mill from the bottom up with this threadmill,
                                          > since you can't put the threadmill into the hole before you start
                                          > cutting. You could turn the piece upside down and mill from the
                                          > bottom DOWN, but what does that get you on a thru-hole? If the hole
                                          > is blind, I don't see how you can use this threadmill in any
                                          > direction but down.

                                          My understanding of thread milling is that the cutting portion of the
                                          thread mill is smaller than the hole. And you can threadmill blind holes
                                          with no troubles.

                                          > I also see that it would require the Z feed speed to be very-well
                                          > syncronized with RPM. In short, seems like it would work better with
                                          > professional machines than with a CNC'd Sherline.

                                          For thread milling, the Z axis does NOT have to be synchronized with the
                                          RPM. The edge of the tool moves in a helical path, and you can vary the
                                          RPM of the spindle with no effect (well at least no effect on the path
                                          of the tool).

                                          For single point threading (like what you would do on a CNC lathe) the
                                          RPM and the Z axis need to be very carefully synchronized.

                                          If you're doing "live threading" where you stick a tap in the spindle,
                                          then the Z motion and spindle RPM need to be carefully synchronized.

                                          --
                                          Dave Hylands
                                          Vancouver, BC, Canada
                                          http://www.DaveHylands.com/
                                        • Tom Hubin
                                          ... *********************** Hello John, A typical threadmill has 2 or 4 cutting points sticking out sideways beyond the shank. The diameter between points is
                                          Message 20 of 25 , Nov 19, 2004
                                          View Source
                                          • 0 Attachment
                                            johnclif@... wrote:
                                            >
                                            > Okay... how do you mill from the bottom up with this threadmill,
                                            > since you can't put the threadmill into the hole before you start
                                            > cutting. You could turn the piece upside down and mill from the
                                            > bottom DOWN, but what does that get you on a thru-hole? If the hole
                                            > is blind, I don't see how you can use this threadmill in any
                                            > direction but down.
                                            >
                                            > I also see that it would require the Z feed speed to be very-well
                                            > syncronized with RPM. In short, seems like it would work better with
                                            > professional machines than with a CNC'd Sherline.
                                            >
                                            > - jgc

                                            ***********************

                                            Hello John,

                                            A typical threadmill has 2 or 4 cutting points sticking out sideways
                                            beyond the shank. The diameter between points is smaller than the
                                            predrilled hole to be tapped. The #4 threadmill that I use measures
                                            about 0.080 inches from point to point.

                                            For a 4-40 thread, I drill a 0.089 inch diameter hole, just as I would
                                            for common tapping. Then I look up the outside diameter of a 4-40 thread
                                            (something like 0.112 inch). I lower the threadmill, centered on the
                                            hole, to just above the bottom. Then move it to the left 0.016 inches so
                                            the teeth are cutting into the wall. Then do the counter clockwise helix
                                            while ascending out of the hole.

                                            Below is a section of Gcode, written for TurboCnc 3.1a, that thread
                                            mills four 4-40 holes. This is done with a subroutine using relative
                                            motion.

                                            EMC does not do subroutines so you would have to embed the helix routine
                                            in four places rather than call it as a subroutine.

                                            Tom Hubin
                                            thubin@...

                                            **************************************

                                            M00 ; File: Cube05D\Cage\Drill.cnc 5 October 2004

                                            G90 ; absolute
                                            G70 ; inches

                                            M00 ; use 1.9370" x 1.9370" x 1.7323" cage
                                            M00 ; ref corner is (right, back, bottom) = (+0.9685, +0.0, -1.7323)
                                            M00 ; (0,0,0) is (center, rear, top)

                                            M00 ; Load small center drill and touch surface
                                            G92 Z 0.0 ; define surface as z=0
                                            G00 Z 0.040 ; raise the bit
                                            M00 ; Tighten bit and start spindle 2800 RPM

                                            ; four tap 4-40 holes

                                            G00 X -0.6500 Y -0.1185
                                            G82 X -0.7500 Y -0.2185 Z -0.030 R 0.040 F 1.0 #250

                                            G00 X +0.8500 Y -0.1185
                                            G82 X +0.7500 Y -0.2185 Z -0.030 R 0.040 F 1.0 #250

                                            G00 X -0.6500 Y -1.6185
                                            G82 X -0.7500 Y -1.7185 Z -0.030 R 0.040 F 1.0 #250

                                            G00 X +0.8500 Y -1.6185
                                            G82 X +0.7500 Y -1.7185 Z -0.030 R 0.040 F 1.0 #250

                                            M00 ; Load #43 (0.089 inch) drill and touch surface
                                            G92 Z 0.0 ; define surface as z=0
                                            G00 Z 0.040 ; raise the bit
                                            M00 ; Tighten bit and start spindle 2800 RPM

                                            ; four tap 4-40 holes

                                            G00 X -0.6500 Y -0.1185
                                            G83 X -0.7500 Y -0.2185 Z -0.300 I -0.09375 R 0.040 F 8.473 #250

                                            G00 X +0.8500 Y -0.1185
                                            G83 X +0.7500 Y -0.2185 Z -0.300 I -0.09375 R 0.040 F 8.473 #250

                                            G00 X -0.6500 Y -1.6185
                                            G83 X -0.7500 Y -1.7185 Z -0.300 I -0.09375 R 0.040 F 8.473 #250

                                            G00 X +0.8500 Y -1.6185
                                            G83 X +0.7500 Y -1.7185 Z -0.300 I -0.09375 R 0.040 F 8.473 #250

                                            M00 ; Load #4 threadmill and touch surface
                                            G92 Z 0.0 ; define surface as z=0
                                            G00 Z 0.040 ; raise the bit
                                            M00 ; Tighten bit and start spindle 2800 RPM

                                            ; four tap 4-40 holes

                                            G00 X -0.650 Y -0.1185
                                            G00 X -0.750 Y -0.2185
                                            N210 M60 #2000 ; threadmill helix

                                            G00 X +0.850 Y -0.1185
                                            G00 X +0.750 Y -0.2185
                                            N220 M60 #2000 ; threadmill helix

                                            G00 X -0.650 Y -1.6185
                                            G00 X -0.750 Y -1.7185
                                            N230 M60 #2000 ; threadmill helix

                                            G00 X +0.850 Y -1.6185
                                            G00 X +0.750 Y -1.7185
                                            N240 M60 #2000 ; threadmill helix

                                            M02 ; finished

                                            ;**************************************************

                                            N2000 ; 0.080 inch threadmill helix for 4-40 holes
                                            G01 Z -0.275 F 1.0 ; start just above bottom of hole

                                            G91 ; start incremental mode

                                            G01 X -0.0160 F 1.0 ; move to left side of hole
                                            G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.250
                                            G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.225
                                            G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.200
                                            G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.175
                                            G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.150
                                            G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.125
                                            G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.100
                                            G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.075
                                            G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.050
                                            G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.025
                                            G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.000
                                            G01 X +0.0160 ; move to center of hole

                                            G90 ; restore absolute mode

                                            G00 Z +0.200 ; exit the hole
                                            M62 ; end of threadmill helix subroutine
                                          Your message has been successfully submitted and would be delivered to recipients shortly.