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

RE: [taigtools] repeatibility and spindle mods

Expand Messages
  • 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 1 of 13 , May 13 8:18 AM
    • 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 2 of 13 , May 13 3:15 PM
      • 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 3 of 13 , May 13 4:32 PM
        • 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 4 of 13 , May 14 5:42 AM
          • 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 5 of 13 , May 14 3:01 PM
            • 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 6 of 13 , May 14 3:03 PM
              • 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 7 of 13 , May 14 3:24 PM
                • 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 8 of 13 , May 14 3:35 PM
                  • 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 9 of 13 , May 14 8:00 PM
                    • 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 10 of 13 , May 15 7:49 AM
                      • 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.