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

Re: [taigtools] repeatibility and spindle mods

Expand Messages
  • Tony Jeffree
    Joe - Fitting a high speed spindle would be no problem although the stock spindle is already good for 15K. The stock spindle is identical to the lathe
    Message 1 of 13 , May 12, 2013
    • 0 Attachment
      Joe -

      Fitting a high speed spindle would be no problem although the stock spindle
      is already good for 15K. The stock spindle is identical to the lathe
      headstock & clamps onto a short section of aluminium dovetail attached to
      the Z ways. It is easy enough to machine up a motor mount that will hold a
      high speed spindle, either clamping it to the dovetail plate in the same
      way, or bolted ditectly to the Z axis in place of that plate.

      Holding half a thou (or better) is possible, but will depend on a number of
      things. The stock Taig mill has plain V thread leadscresw; the feed nuts
      are backlash adjustable though, so you can adjust out backlash due to that
      part of the system. It isn't very practical to replace the screws with
      ballscrews because of the limited space under the table.

      The standard motor couplers can be problematic - I replaced mine with
      Oldham couplings which dramatically improved the performance of my machine
      to the point where I could no longer measure any backlash in the X and Y
      axes. See http://www.jeffree.co.uk/pages/taigcncpt1.htm

      Regards,
      Tony


      On 12 May 2013 19:03, nickelcarver <gtsport@...> wrote:

      > Hi all,
      >
      > I am searching for a CNC machine that will do what I want and I am curious
      > about the Taig and what it is capable of. My goal is to cut dies for coin
      > striking. At present, I use a hand cut plastic pattern and a Gorton
      > pantograph to cut the text into my dies and I hand engrave any sculptural
      > portion of the design. What I wiuld like to do is design the coin in a CAM
      > program and export it to a CNC machine to cut the design. What I need to
      > know is what tolerances are users of the Taig CNC mill able to hold and are
      > there any fast spindles available to replace the stock one. Usually, die
      > cutting CNC machines need to hold their tolerances to no more than .0005
      > inch in each axis and spindle speeds need to be at least 15k, 30k or more
      > being better. The cutting bits I use are 1/8 inch carbide that I cut on an
      > Alexander cutter/grinder with a tip diameter of around .2-.3mm and each
      > cutting pass on the pantograph is usually no more than .003 inch in depth.
      > Any help would be greatly appreciated.
      >
      > Thanks,
      >
      > Joe
      >
      >
      >
      > ------------------------------------
      >
      > To Post a message, send it to:
      > taigtools@yahoogroups.com
      >
      > To Unsubscribe, send a blank message to:
      > taigtools-unsubscribe@yahoogroups.com
      >
      > Let the chips fly!
      > Yahoo! Groups Links
      >
      >
      >
      >


      [Non-text portions of this message have been removed]
    • Jeffrey Birt
      When you are first getting started with CNC it is quite common to have elevated expectations with regards to accuracy and repeatability. There are several
      Message 2 of 13 , May 13, 2013
      • 0 Attachment
        When you are first getting started with CNC it is quite common to have
        elevated expectations with regards to accuracy and repeatability. There are
        several things that can influence how accurate a part you make will be,
        these include:



        1) Tool wear (how accurate is the tool diameter and how well does it
        cut)

        2) Tool deflection (how much tool bends/flexes while cutting)

        3) Backlash (amount of 'play' between driven components)

        4) Lead screw pitch error (how accurately lead screw is made)

        5) Quality of GCode (how you try to cut the part will greatly influence
        the outcome)

        6) Temperature changes in material and/or machine



        Let's take these items one at a time.



        #1 - The accuracy of your tool (and spindle) is big, big factor. You simply
        cannot grind a tool by hand and get the level of accuracy you are after.
        Even with a 5 axis CNC grinder the way they go about doing the grinding
        process can greatly influence the accuracy of the bit/part produced. Unless
        you can very accurately measure each bit you won't know what the true size
        of run out of the bit is. As the tool wears the size of your cut will vary.
        You will need to keep this in mind and try to employ the tool table feature
        of Mach3 to account for the wear.



        The Taig spindle is a well-built unit. Some of the things folks try to use
        for a high speed spindle are not well made. You can count out things like a
        Dremel tool or similar hand help tools. PreciseBits does make some very
        precise collets for the Dewalt 611 which is a small laminate trimming
        router. This might be a route worth exploring.



        #2 - As you are machining the tool will be deflected by some amount. Carbide
        will deflect less than tool steel but it will deflect none the less. Your
        machining strategy (#5) will have a big influence on this.



        #3 - Backlash, every machine has it. The Taig mills lead nuts are
        adjustable so you can dial it down to less than 0.001" backlash without much
        trouble. Mach 3 also has open loop backlash compensation which might or
        might not help. Many times the cutting forces will tend to push the mill
        table around so it is impossible for the control program to compensate for
        it. With the light cuts you mention it might be of some help, but then it
        might not be.



        #4 - Every type of lead screw (be it a V profile, Acme or ball screw) will
        have some amount of pitch error. If you look up the specs on a high quality
        screw you will see the pitch error listed as something like 0.002" per foot.
        This means that along any 1 foot section of the screw you should be within
        0.002" of the correct position. The thing is though that you don't know
        'where' the error is. A high quality screw might come with a 'screw map'
        which will tell you the error amounts along the length of the screw. You can
        input this into Mach3 and it will try to compensate for the pitch error. For
        a tiny part the pitch error may not be important, but for a larger part it
        can be.



        #5 - How your GCode tells the machine to cut something has a big impact on
        its precision and finish. For different materials and type of cutting there
        are different machining strategies that can help. I built part of a laser
        micrometer system that PreciseBits uses to measure the run out of their
        collets and bits. They found that they could see the influence of different
        machining strategies on the run out of their precision collets, this let
        them fine tune the GCode to produce collets with extremely low run out.
        Unless you have very accurate measurement equipment, like a CMM in a
        temperature controlled environment, it might be hard to know if a change in
        machining strategy is making any difference. A good rule of thumb is that
        you need to be able to accurately measure at ten times the resolution of
        what you are worried about. For example if you are worried about a
        resolution of 0.0005" then you will need to be able to measure at 0.00005"
        accuracy. This level of measurement accuracy is not possible for most folks.



        #6 - Temperature can make a difference when you are worried about being very
        accurate. I was running some test samples for a customer a few weeks ago on
        some small brass stock that was formed from a flat sheet. He was thinking he
        needed 0.001" accuracy over the length of the mill bed. After we
        investigated the accuracy of how the pieces were formed, the thermal
        expansion of the brass, etc we came to the conclusion that the Taig mill
        could cut the ends of the brass more accurately than the piece could be
        formed. The limitation was not in the mill so there was no need to be
        worried about achieving a very high level of accuracy, a 'good' level of
        accuracy was all that was really required.





        I hope this all is of some help. When I'm talking to a 'newbie' about CNC
        machining I like to find out what they want to machine and what results they
        expect to receive. Many folks get obsessed with achieving accuracy levels
        that are very difficult to get and in the end are not really required.
        Mostly I want folks to get started with a reasonable expectation about what
        the results are they can achieve from a small CNC machine so they are not
        disappointed or spend a whole lot of time chasing pie-in-the-sky numbers.



        If I can be of any further help you can find my contact information on my
        website (below.)



        Jeff Birt

        Soigeneris.com





        From: taigtools@yahoogroups.com [mailto:taigtools@yahoogroups.com] On Behalf
        Of nickelcarver
        Sent: Sunday, May 12, 2013 1:04 PM
        To: taigtools@yahoogroups.com
        Subject: [taigtools] repeatibility and spindle mods





        Hi all,

        I am searching for a CNC machine that will do what I want and I am curious
        about the Taig and what it is capable of. My goal is to cut dies for coin
        striking. At present, I use a hand cut plastic pattern and a Gorton
        pantograph to cut the text into my dies and I hand engrave any sculptural
        portion of the design. What I wiuld like to do is design the coin in a CAM
        program and export it to a CNC machine to cut the design. What I need to
        know is what tolerances are users of the Taig CNC mill able to hold and are
        there any fast spindles available to replace the stock one. Usually, die
        cutting CNC machines need to hold their tolerances to no more than .0005
        inch in each axis and spindle speeds need to be at least 15k, 30k or more
        being better. The cutting bits I use are 1/8 inch carbide that I cut on an
        Alexander cutter/grinder with a tip diameter of around .2-.3mm and each
        cutting pass on the pantograph is usually no more than .003 inch in depth.
        Any help would be greatly appreciated.

        Thanks,

        Joe





        [Non-text portions of this message have been removed]
      • nickelcarver
        Thanks for the quick responses guys. You ve given me a lot of info to digest and several things to look up on line. I do like the idea of using the mill to
        Message 3 of 13 , May 13, 2013
        • 0 Attachment
          Thanks for the quick responses guys. You've given me a lot of info to digest and several things to look up on line. I do like the idea of using the mill to drive the arm of the pantograph at 10:1 which should mean as long as the arms are tight, a .001 on the mill will give me .0001 plus whatever runout is on my cutter. At least I think that is what it means. Have any of you done anything similar to this, using small cutters to anything like a coining die? Also, Will, what is a hydraulic Z-axis? Also, last year I just happened into a $300 Hansvedt EDM machine that only needed a new oil level switch to get running, but I only have charts for settings using an electrode no larger than .75 sq in. Do you know where I can find charts for bigger work? I'm going to do a little more googleresearch and will be back with more questions.

          Thanks!

          Joe
        • Will Schmit
          Hydraulic tool positioning is an art that is shrouded in mystery.  One of the reasons is that when you start getting too accurate, you wander into places that
          Message 4 of 13 , May 13, 2013
          • 0 Attachment
            Hydraulic tool positioning is an art that is shrouded in mystery.  One of the reasons is that when you start getting too accurate, you wander into places that trillion dollar defense corporations would prefer you not even know about.  I am sure you know, coin making hits a technological brick wall at some point.  The guys that know how to do it, protect the craft from counterfeiters.  After the obvious, when the techniques get too accurate, the descriptions get murky, or become totally bullshit. 

            The way it was described to me is relatively simple (in theory).  Imagine buying two avionics grade hydraulic cylinders.  For the sake of argument lets say a 1" cylinder with 10" travel, and a 10" cylinder with 1" travel.  If you put a big spring on each (to get them to return, and maintain pressure in the system).  Put a ballscrew on the 1" cylinder, and a spindle on the 10" cylinder (directly coupled - no linkages).  Basically, you end up with a 10:1 hydraulic pantograph, with zero backlash.  The accuracy is up to you -- you can make it 88:1 if that suits you.  Daedal makes optical slides that are as perfect as your budget will allow.  You can build an X/Y table with 2" of travel, and fit them with hydraulic cylinders.  Set your design software to make facets of .001mm, and make your 1" coin design 10" in diameter.  When your CAM software outputs line segments of .0001 intol, and outol (which are terms used in CAD/CAM to cheat the path of a
            tool around a curve -- even the most perfectly plotted curve is output as a series of line segments --- well, at least in the "real world of hobby CNC) it will be sent to your ballscrew and the resolution will be magnified to .00001mm (but the rounded parts will always be faceted).  If you always design and output beyond the ability of the next tool to reproduce it, you are as accurate as you can be (within your world).

            Use a spindle with very accurate bearings, use high precision collets, buy the best bits you can afford (I use "bits and bits" carbide tools).  Bring your shop to 72 degrees.  Run your spindle for 5 minutes before starting the run.  Make a test patch outside the "live area" of your tooling, so you can see that the second or third tool is set at a proper depth.  I would run a tool at .01 mm high, replace the tool, then run it again.

            I would machine my masters in high quality graphite, then send them out to an EDM shop to have hardened steel dies made.  For coins, I would make a 3 piece die (top/bottom/edges).  Don't even try to make the middle die -- just give the EDM shop the parameters, and they will wire-EDM the die.

            Your Hansvedt EDM should be able to handle it.  Screw the charts -- just keep experimenting until you get it right.  You should be able to predict the curve from the charts and be in the ballpark on the first try.  You may also want to experiment with progressive EDM electrodes.

            Jeffrey Birt's advice is darned good, I always consult him when I am wandering into the murky water, and am trying to do something just because someone said I couldn't.

            FWIW, my machinery is all home-made with re-purposed, re-engineered, and re-modeled "off the shelf" materials (much of it from Ebay).  My 4th axis is a Taig lathe.  I make jewelry, and sewing thimbles (with 3d relief on 4th-axis milling or lathe processes).  I typically use 3 steps: 1/8" ball nose, 1/32" ball nose, and .005" ball nosed tool with 15 degree taper.
            If I use a sharper taper, the reliefs don't release from the rubber molds very easily.

            Hope this helps...


            ________________________________
            From: nickelcarver <gtsport@...>
            To: taigtools@yahoogroups.com
            Sent: Monday, May 13, 2013 4:15 PM
            Subject: [taigtools] Re: repeatibility and spindle mods



             

            Thanks for the quick responses guys. You've given me a lot of info to digest and several things to look up on line. I do like the idea of using the mill to drive the arm of the pantograph at 10:1 which should mean as long as the arms are tight, a .001 on the mill will give me .0001 plus whatever runout is on my cutter. At least I think that is what it means. Have any of you done anything similar to this, using small cutters to anything like a coining die? Also, Will, what is a hydraulic Z-axis? Also, last year I just happened into a $300 Hansvedt EDM machine that only needed a new oil level switch to get running, but I only have charts for settings using an electrode no larger than .75 sq in. Do you know where I can find charts for bigger work? I'm going to do a little more googleresearch and will be back with more questions.

            Thanks!

            Joe




            [Non-text portions of this message have been removed]
          • Boman33
            I am working with a customer that manufactures custom medallions. The dies are directly CNCed in a super-accurate small CNC milling machine. Afterwards they
            Message 5 of 13 , May 14, 2013
            • 0 Attachment
              I am working with a customer that manufactures custom medallions. The dies are directly CNCed in a super-accurate small CNC milling machine. Afterwards they are hardened and used in a minting press.

              Bertho



              [Non-text portions of this message have been removed]
            • nickelcarver
              Ah, I see what you are saying. This is the same as the hydraulic parison unit on the blow molding machines I work with. To be honest, that level of precision
              Message 6 of 13 , May 14, 2013
              • 0 Attachment
                Ah, I see what you are saying. This is the same as the hydraulic parison unit on the blow molding machines I work with. To be honest, that level of precision is beyond the market that I deal with. I rarely charge more than $200 a piece for my dies which makes me a profit and keeps them coming back. I am looking for decent quality, not a homebrew $300K Impala. The Daedal cross slide does sound interesting, has anyone out there used these to make an XY table? Can they be held to below .001 inch tolerance? This is starting to get interesting.

                Joe

                --- In taigtools@yahoogroups.com, Will Schmit <anchornm@...> wrote:
                >
                > Hydraulic tool positioning is an art that is shrouded in mystery.  One of the reasons is that when you start getting too accurate, you wander into places that trillion dollar defense corporations would prefer you not even know about.  I am sure you know, coin making hits a technological brick wall at some point.  The guys that know how to do it, protect the craft from counterfeiters.  After the obvious, when the techniques get too accurate, the descriptions get murky, or become totally bullshit. 
                >
                > The way it was described to me is relatively simple (in theory).  Imagine buying two avionics grade hydraulic cylinders.  For the sake of argument lets say a 1" cylinder with 10" travel, and a 10" cylinder with 1" travel.  If you put a big spring on each (to get them to return, and maintain pressure in the system).  Put a ballscrew on the 1" cylinder, and a spindle on the 10" cylinder (directly coupled - no linkages).  Basically, you end up with a 10:1 hydraulic pantograph, with zero backlash.  The accuracy is up to you -- you can make it 88:1 if that suits you.  Daedal makes optical slides that are as perfect as your budget will allow.  You can build an X/Y table with 2" of travel, and fit them with hydraulic cylinders.  Set your design software to make facets of .001mm, and make your 1" coin design 10" in diameter.  When your CAM software outputs line segments of .0001 intol, and outol (which are terms used in CAD/CAM to cheat the path of a
                > tool around a curve -- even the most perfectly plotted curve is output as a series of line segments --- well, at least in the "real world of hobby CNC) it will be sent to your ballscrew and the resolution will be magnified to .00001mm (but the rounded parts will always be faceted).  If you always design and output beyond the ability of the next tool to reproduce it, you are as accurate as you can be (within your world).
                >
                > Use a spindle with very accurate bearings, use high precision collets, buy the best bits you can afford (I use "bits and bits" carbide tools).  Bring your shop to 72 degrees.  Run your spindle for 5 minutes before starting the run.  Make a test patch outside the "live area" of your tooling, so you can see that the second or third tool is set at a proper depth.  I would run a tool at .01 mm high, replace the tool, then run it again.
                >
                > I would machine my masters in high quality graphite, then send them out to an EDM shop to have hardened steel dies made.  For coins, I would make a 3 piece die (top/bottom/edges).  Don't even try to make the middle die -- just give the EDM shop the parameters, and they will wire-EDM the die.
                >
                > Your Hansvedt EDM should be able to handle it.  Screw the charts -- just keep experimenting until you get it right.  You should be able to predict the curve from the charts and be in the ballpark on the first try.  You may also want to experiment with progressive EDM electrodes.
                >
                > Jeffrey Birt's advice is darned good, I always consult him when I am wandering into the murky water, and am trying to do something just because someone said I couldn't.
                >
                > FWIW, my machinery is all home-made with re-purposed, re-engineered, and re-modeled "off the shelf" materials (much of it from Ebay).  My 4th axis is a Taig lathe.  I make jewelry, and sewing thimbles (with 3d relief on 4th-axis milling or lathe processes).  I typically use 3 steps: 1/8" ball nose, 1/32" ball nose, and .005" ball nosed tool with 15 degree taper.
                > If I use a sharper taper, the reliefs don't release from the rubber molds very easily.
                >
                > Hope this helps...
                >
                >
                > ________________________________
                > From: nickelcarver <gtsport@...>
                > To: taigtools@yahoogroups.com
                > Sent: Monday, May 13, 2013 4:15 PM
                > Subject: [taigtools] Re: repeatibility and spindle mods
                >
                >
                >
                >  
                >
                > Thanks for the quick responses guys. You've given me a lot of info to digest and several things to look up on line. I do like the idea of using the mill to drive the arm of the pantograph at 10:1 which should mean as long as the arms are tight, a .001 on the mill will give me .0001 plus whatever runout is on my cutter. At least I think that is what it means. Have any of you done anything similar to this, using small cutters to anything like a coining die? Also, Will, what is a hydraulic Z-axis? Also, last year I just happened into a $300 Hansvedt EDM machine that only needed a new oil level switch to get running, but I only have charts for settings using an electrode no larger than .75 sq in. Do you know where I can find charts for bigger work? I'm going to do a little more googleresearch and will be back with more questions.
                >
                > Thanks!
                >
                > Joe
                >
                >
                >
                >
                > [Non-text portions of this message have been removed]
                >
              • nickelcarver
                Hi Bertho, That is what I am looking to do. I already cut dies by hand, harden them, and strike the coins on an antique fly press. I am looking to upgrade
                Message 7 of 13 , May 14, 2013
                • 0 Attachment
                  Hi Bertho,

                  That is what I am looking to do. I already cut dies by hand, harden them, and strike the coins on an antique fly press. I am looking to upgrade the die making process to CNC. Do you have any information that might help me?

                  Thanks!

                  Joe

                  --- In taigtools@yahoogroups.com, "Boman33" <boman33@...> wrote:
                  >
                  > I am working with a customer that manufactures custom medallions. The dies are directly CNCed in a super-accurate small CNC milling machine. Afterwards they are hardened and used in a minting press.
                  >
                  > Bertho
                  >
                  >
                  >
                  > [Non-text portions of this message have been removed]
                  >
                • Will Schmit
                  Bertho, I would be interested in finding out what kind of steel he/she uses. O1 would be my first choice (just as a random guess), but I wonder about
                  Message 8 of 13 , May 14, 2013
                  • 0 Attachment
                    Bertho, I would be interested in finding out what kind of steel he/she uses.
                    O1 would be my first choice (just as a random guess), but I wonder about distortion in the furnace (and the cooling). A 1 1/2" medallion (small by most accounts) would be a huge chunk of steel to heat/cool.

                    Not only that, their bit bill must be horrendous. 
                    Once I get below 1/64" I can't plunge any more than .1mm without vaporizing bits, or (worse) getting unreasonable tool deflection (and that is in brass or bronze).  Granted, steel doesn't work harden to the degree that brass does, but it must be a slow and expensive process.


                    ________________________________
                    From: Boman33 <boman33@...>
                    To: taigtools@yahoogroups.com
                    Sent: Tuesday, May 14, 2013 6:42 AM
                    Subject: RE: [taigtools] Re: repeatibility and spindle mods



                     
                    I am working with a customer that manufactures custom medallions. The dies are directly CNCed in a super-accurate small CNC milling machine. Afterwards they are hardened and used in a minting press.

                    Bertho

                    [Non-text portions of this message have been removed]




                    [Non-text portions of this message have been removed]
                  • Boman33
                    Joe, Next time I visit my customer I will get the info. If you have not heard from me in a week or two send me an email reminding me. There is nothing magical
                    Message 9 of 13 , May 14, 2013
                    • 0 Attachment
                      Joe,

                      Next time I visit my customer I will get the info. If you have not heard
                      from me in a week or two send me an email reminding me.

                      There is nothing magical about it, just a high accuracy, high RPM small work
                      area CNC milling machine. It is definitely not low-cost... As a base is a
                      big granite surface plate.

                      Bertho



                      From: nickelcarver Sent: Tuesday, May 14, 2013 18:03



                      Hi Bertho,

                      That is what I am looking to do. I already cut dies by hand, harden them,
                      and strike the coins on an antique fly press. I am looking to upgrade the
                      die making process to CNC. Do you have any information that might help me?

                      Thanks!

                      Joe

                      --- In taigtools@yahoogroups.com <mailto:taigtools%40yahoogroups.com> ,
                      "Boman33" <boman33@...> wrote:
                      >
                      > I am working with a customer that manufactures custom medallions. The dies
                      are directly CNCed in a super-accurate small CNC milling machine. Afterwards
                      they are hardened and used in a minting press.
                      >
                      > Bertho





                      [Non-text portions of this message have been removed]
                    • Low Compression
                      ... I cannot tell you that all TAIG spindles are built the same but the one that came with my TAIG CNC mill (probably 10 years old at this point) is a 2-part
                      Message 10 of 13 , May 14, 2013
                      • 0 Attachment
                        > The Taig spindle is a well-built unit. Some of the things folks try >to use for a high speed spindle are not well made. You can count out >things like a Dremel tool or similar hand help tools. PreciseBits does >make some very precise collets for the Dewalt 611 which is a small >laminate trimming router. This might be a route worth exploring.

                        I cannot tell you that all TAIG spindles are built the same but the one that came with my TAIG CNC mill (probably 10 years old at this point) is a 2-part extrusion that I pulled off and replaced with a Sherline headstock and motor setup.

                        I loaned a friend the TAIG headstock to make a grinder and he found that the spindle is not stiff enough to prevent chatter when grinding. Not a surprising finding---the headstock is not designed for grinding---but I think that points up some potential problems when trying for the best possible finish. Granted, there are other issues with the TAIG, the big one being backlash with the factory screws and nuts that probably mask the headstock inadequacies (for super finish work). It is, however, more that satisfactory for much of the work asked of it.
                      • Jeffrey Birt
                        Ten years ago I suspect you got the older ‘lathe’ style headstock, and the older dovetail Z column. The ‘new’ headstock is a single piece extrusion
                        Message 11 of 13 , May 15, 2013
                        • 0 Attachment
                          Ten years ago I suspect you got the older ‘lathe’ style headstock, and the
                          older dovetail Z column. The ‘new’ headstock is a single piece extrusion
                          that accepts a cartridge style shaft/bearing assembly. The spindle is now
                          ER16 as opposed to the old ¾-16 like the lathe. It is very stout.



                          About 5 years ago my friend used a Taig CNC mill as part of his PhD. work.
                          He had developed a new method of predicting equipment failures (predictive
                          maintenance) and since bearing failure has been widely studied it provided a
                          way to compare his method to existing methods. We flushed the grease out of
                          the bearings and he milled aluminum plate for 12-14 hours a day with the
                          machine. The headstock was fitted with accelerometers and temperature
                          sensors (as well as the base of the machine.) With no grease the spindle
                          would run about 30 hours, noticeable vibration (from a human senses
                          perspective) was only an issue towards the end of the bearing life. Most of
                          the bearings failed very quickly and very catastrophically. We put dozens of
                          bearings in two different spindles over the course of 4 mounts (or so). When
                          the research was all done I replaced the whole cartridge in both spindles
                          and still use them, and the machine to this day.



                          Jeff Birt

                          Soigeneris.com



                          From: taigtools@yahoogroups.com [mailto:taigtools@yahoogroups.com] On Behalf
                          Of Low Compression
                          Sent: Tuesday, May 14, 2013 10:00 PM
                          To: taigtools@yahoogroups.com
                          Subject: [taigtools] Re: repeatibility and spindle mods






                          > The Taig spindle is a well-built unit. Some of the things folks try >to
                          use for a high speed spindle are not well made. You can count out >things
                          like a Dremel tool or similar hand help tools. PreciseBits does >make some
                          very precise collets for the Dewalt 611 which is a small >laminate trimming
                          router. This might be a route worth exploring.

                          I cannot tell you that all TAIG spindles are built the same but the one that
                          came with my TAIG CNC mill (probably 10 years old at this point) is a 2-part
                          extrusion that I pulled off and replaced with a Sherline headstock and motor
                          setup.

                          I loaned a friend the TAIG headstock to make a grinder and he found that the
                          spindle is not stiff enough to prevent chatter when grinding. Not a
                          surprising finding---the headstock is not designed for grinding---but I
                          think that points up some potential problems when trying for the best
                          possible finish. Granted, there are other issues with the TAIG, the big one
                          being backlash with the factory screws and nuts that probably mask the
                          headstock inadequacies (for super finish work). It is, however, more that
                          satisfactory for much of the work asked of it.





                          [Non-text portions of this message have been removed]
                        Your message has been successfully submitted and would be delivered to recipients shortly.