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

drilling issues

Expand Messages
  • Chris Ghent
    I have a Taig CNC mill with the 240v Dayton motor and I am wondering if my problem with a particular job might be that the spindle motor is not strong enough.
    Message 1 of 25 , Jan 7, 2011
    • 0 Attachment
      I have a Taig CNC mill with the 240v Dayton motor and I am wondering if
      my problem with a particular job might be that the spindle motor is not
      strong enough.

      The job entails putting two conical holes in a piece of titanium rod 5mm
      in diameter. The conical holes come in from 180° apart so they meet,
      leaving a single hole through the rod which is conical on both sides.

      I have been using a centre drill to do this job. For no real reason I
      have increased the clearance behind the cutting edge hoping to cut down
      on heat build up.

      What I find is that I am forced to run the spindle very fast, about
      6000rpm, and the speed of cut at .5" pm to have any chance of getting
      through the rod without a spindle stall. This seems much faster (and the
      speed of cut much slower) than I would like to run it, which would be
      more like 1.5" speed of cut and 1500 rpm. There is a lot of heat
      generated and the tool gets damaged quickly. But I can't slow the motor
      without guaranteeing a stall. I used to run a Sherline DC motor and the
      situation was still marginal but I could get away with it. Unfortunately
      as regular readers of this space might the Sherline started putting out
      noise which got into the motor circuits.

      I am wondering if someone might be able to suggest a cutter that might
      do a better job or suggest any ideas that might help..?

      Best Wishes

      Chris
    • Tony Jeffree
      Sounds to me as if you may be going in the wrong direction by increasing the spindle speed - see: http://www.titek.co.uk/cutting.asp Also, if your cutting
      Message 2 of 25 , Jan 7, 2011
      • 0 Attachment
        Sounds to me as if you may be going in the wrong direction by increasing the
        spindle speed - see:

        http://www.titek.co.uk/cutting.asp

        Also, if your cutting tools aren't absolutely sharp, they will tend to
        work-harden the material rather than cut it.

        Regards,
        Tony


        On 7 January 2011 13:49, Chris Ghent <cghent@...> wrote:

        > I have a Taig CNC mill with the 240v Dayton motor and I am wondering if
        > my problem with a particular job might be that the spindle motor is not
        > strong enough.
        >
        > The job entails putting two conical holes in a piece of titanium rod 5mm
        > in diameter. The conical holes come in from 180° apart so they meet,
        > leaving a single hole through the rod which is conical on both sides.
        >
        > I have been using a centre drill to do this job. For no real reason I
        > have increased the clearance behind the cutting edge hoping to cut down
        > on heat build up.
        >
        > What I find is that I am forced to run the spindle very fast, about
        > 6000rpm, and the speed of cut at .5" pm to have any chance of getting
        > through the rod without a spindle stall. This seems much faster (and the
        > speed of cut much slower) than I would like to run it, which would be
        > more like 1.5" speed of cut and 1500 rpm. There is a lot of heat
        > generated and the tool gets damaged quickly. But I can't slow the motor
        > without guaranteeing a stall. I used to run a Sherline DC motor and the
        > situation was still marginal but I could get away with it. Unfortunately
        > as regular readers of this space might the Sherline started putting out
        > noise which got into the motor circuits.
        >
        > I am wondering if someone might be able to suggest a cutter that might
        > do a better job or suggest any ideas that might help..?
        >
        > Best Wishes
        >
        > Chris
        >
        >
        >
        >
        > ------------------------------------
        >
        > 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]
      • chuck
        Chris, I am not familiar with machining titanium but one thing that was not mentioned if your using the Taig step pulley system for speed change the faster you
        Message 3 of 25 , Jan 7, 2011
        • 0 Attachment
          Chris,
          I am not familiar with machining titanium but one thing that was not mentioned if your using the Taig step pulley system for speed change the faster you run the spindle the lower the torque available to the tool.
          using a lower setting will increase the torque and not try to stall the motor as easily as well as generating less heat at the cut.

          Chuck

          ----- Original Message -----
          From: Chris Ghent
          To: taigtools@yahoogroups.com
          Sent: Friday, January 07, 2011 8:49 AM
          Subject: [taigtools] drilling issues



          I have a Taig CNC mill with the 240v Dayton motor and I am wondering if
          my problem with a particular job might be that the spindle motor is not
          strong enough.

          The job entails putting two conical holes in a piece of titanium rod 5mm
          in diameter. The conical holes come in from 180° apart so they meet,
          leaving a single hole through the rod which is conical on both sides.

          I have been using a centre drill to do this job. For no real reason I
          have increased the clearance behind the cutting edge hoping to cut down
          on heat build up.

          What I find is that I am forced to run the spindle very fast, about
          6000rpm, and the speed of cut at .5" pm to have any chance of getting
          through the rod without a spindle stall. This seems much faster (and the
          speed of cut much slower) than I would like to run it, which would be
          more like 1.5" speed of cut and 1500 rpm. There is a lot of heat
          generated and the tool gets damaged quickly. But I can't slow the motor
          without guaranteeing a stall. I used to run a Sherline DC motor and the
          situation was still marginal but I could get away with it. Unfortunately
          as regular readers of this space might the Sherline started putting out
          noise which got into the motor circuits.

          I am wondering if someone might be able to suggest a cutter that might
          do a better job or suggest any ideas that might help..?

          Best Wishes

          Chris





          [Non-text portions of this message have been removed]
        • Ken Cline
          I agree with Tony about the feeds and speeds. This source [http://www.timet.com/fab-p18.htm] suggests speeds in the 10-40ft/min range for drilling Ti with HSS
          Message 4 of 25 , Jan 7, 2011
          • 0 Attachment
            I agree with Tony about the feeds and speeds. This source [http://www.timet.com/fab-p18.htm%5d suggests speeds in the 10-40ft/min range for drilling Ti with HSS drills, which works out to 250-1000rpm for your task. Slowing the feed below the suggested .002-.005in/rev range may be asking for trouble since it places the cutting edge closer to work hardened surface that was just cut. You can find faster speeds and wider feed ranges at other sources which might contradict my advice, so take it as a suggestion rather than a hard and fast rule.

            Assuming you are cutting properly (feed & speed, sharp bit, ample coolant, pecking cycle to clear chips, etc.), the power required to cut titanium is a little less that for steel. I ran the numbers for your drilling operation and got an estimate of 0.1 HP required at the bottom of the cut, where the diameter being drilled is widest. It seems reasonable to expect that kind of power from your spindle, but I don't know anything about the motor on your mill other than brand name. You might want to check whether you can drill mild steel with the same parameters (I would run at my lowest speed, 1000 RPM, and 0.002in/rev = 2in/min feed). If the steel cuts without stalling, something is going wrong when you drill titanium.

            If all else fails, it may be possible to reduce power requirements by first drilling a pilot hole (use a spotting drill to locate the hole), then widening it with a larger drill or countersink.

            Carbide is often recommended for cutting Ti, but I would start with good cobalt (hss) tools. Steel tools are sharper, though they won't last as long. Also if my calculations are correct, Taig mills lack the power to make effective use of carbide's higher speeds - at 6000 rpm my motor would be maxed out, with no margin for error. I have also heard advice from a local titanium fabricator (bicycle frames) who told me he prefers HSS tooling over carbide for the kind of work he does (typically drilling, "mitering" tubing with a hole saw, reaming, and tapping).

            Good luck!
          • Robert Robert
            Hi Chris: I have a Taig mill also (base motor) not the upgrade motor. I noticed the first time I tried to drill a 5/16 hole on med speed in mild steel 3/8
            Message 5 of 25 , Jan 7, 2011
            • 0 Attachment
              Hi Chris:

              I have a Taig mill also (base motor) not the upgrade motor. I noticed the first time I tried to drill a 5/16" hole on med speed in mild steel 3/8" thick and it was a no go. It was nice to use the Taig and a center drill to get a nice precise location but that's it, then I took it to my table top drill press with a AC motor twice the size, has a belt drive also and the belt is like 20x the diameter as the Taig, and the drill press went right through with no issues. In the future I plan on upgrading this to a larger motor and a wider belt.

              Rob




              --- In taigtools@yahoogroups.com, Chris Ghent <cghent@...> wrote:
              >
              > I have a Taig CNC mill with the 240v Dayton motor and I am wondering if
              > my problem with a particular job might be that the spindle motor is not
              > strong enough.
              >
              > The job entails putting two conical holes in a piece of titanium rod 5mm
              > in diameter. The conical holes come in from 180� apart so they meet,
              > leaving a single hole through the rod which is conical on both sides.
              >
              > I have been using a centre drill to do this job. For no real reason I
              > have increased the clearance behind the cutting edge hoping to cut down
              > on heat build up.
              >
              > What I find is that I am forced to run the spindle very fast, about
              > 6000rpm, and the speed of cut at .5" pm to have any chance of getting
              > through the rod without a spindle stall. This seems much faster (and the
              > speed of cut much slower) than I would like to run it, which would be
              > more like 1.5" speed of cut and 1500 rpm. There is a lot of heat
              > generated and the tool gets damaged quickly. But I can't slow the motor
              > without guaranteeing a stall. I used to run a Sherline DC motor and the
              > situation was still marginal but I could get away with it. Unfortunately
              > as regular readers of this space might the Sherline started putting out
              > noise which got into the motor circuits.
              >
              > I am wondering if someone might be able to suggest a cutter that might
              > do a better job or suggest any ideas that might help..?
              >
              > Best Wishes
              >
              > Chris
              >
            • Ron Thompson
              ... I d think twice about the wider belt. Especially if you want to turn 10K RPM. These belts are pretty tough. -- Ron Thompson On the Beautiful Florida Space
              Message 6 of 25 , Jan 7, 2011
              • 0 Attachment
                On 1/7/2011 4:02 PM, Robert Robert wrote:
                >
                > Hi Chris:
                >
                > I have a Taig mill also (base motor) not the upgrade motor. I noticed
                > the first time I tried to drill a 5/16" hole on med speed in mild
                > steel 3/8" thick and it was a no go. It was nice to use the Taig and a
                > center drill to get a nice precise location but that's it, then I took
                > it to my table top drill press with a AC motor twice the size, has a
                > belt drive also and the belt is like 20x the diameter as the Taig, and
                > the drill press went right through with no issues. In the future I
                > plan on upgrading this to a larger motor and a wider belt.
                >
                > Rob
                >
                I'd think twice about the wider belt. Especially if you want to turn 10K
                RPM. These belts are pretty tough.

                --


                Ron Thompson
                On the Beautiful Florida Space Coast, right beside the Kennedy Space Center, USA

                There are two kinds of posts on newsgroups.
                1. This is what I have done...
                2. This is what I think...
                Be aware of the difference!

                http://www.ourcadguy.com/

                http://www.plansandprojects.com My hobby pages are here:
                http://www.plansandprojects.com/My%20Machines/

                Visit the castinghobby FAQ:
                http://castinghobbyfaq.bareboogerhost.com/








                [Non-text portions of this message have been removed]
              • Clint
                Interesting situation with the drilling - but I am only drilling steel and brass. I have similar problem on my Taig lathe, when trying to drill a piece in
                Message 7 of 25 , Jan 7, 2011
                • 0 Attachment
                  Interesting situation with the drilling - but I am only drilling steel and brass. I have similar problem on my Taig lathe, when trying to drill a piece in the cross-slide vise, with the drill bit located in the head-stock collet. It usually takes lots of pressure on the cross-slide carriage wheel to drill through the metal. I can take the same drill bit and put it in my drill press and it drills through like butter. In drilling a piece of round stock, with the bit in the tail-stock chuck, it drills through very easily.

                  Regards,
                  Clint


                  From: Ron Thompson
                  Sent: Friday, January 07, 2011 2:28 PM
                  To: taigtools@yahoogroups.com
                  Subject: Re: [taigtools] Re: drilling issues



                  On 1/7/2011 4:02 PM, Robert Robert wrote:
                  >
                  > Hi Chris:
                  >
                  > I have a Taig mill also (base motor) not the upgrade motor. I noticed
                  > the first time I tried to drill a 5/16" hole on med speed in mild
                  > steel 3/8" thick and it was a no go. It was nice to use the Taig and a
                  > center drill to get a nice precise location but that's it, then I took
                  > it to my table top drill press with a AC motor twice the size, has a
                  > belt drive also and the belt is like 20x the diameter as the Taig, and
                  > the drill press went right through with no issues. In the future I
                  > plan on upgrading this to a larger motor and a wider belt.
                  >
                  > Rob
                  >
                  I'd think twice about the wider belt. Especially if you want to turn 10K
                  RPM. These belts are pretty tough.

                  --

                  Ron Thompson
                  On the Beautiful Florida Space Coast, right beside the Kennedy Space Center, USA

                  There are two kinds of posts on newsgroups.
                  1. This is what I have done...
                  2. This is what I think...
                  Be aware of the difference!

                  http://www.ourcadguy.com/

                  http://www.plansandprojects.com My hobby pages are here:
                  http://www.plansandprojects.com/My%20Machines/

                  Visit the castinghobby FAQ:
                  http://castinghobbyfaq.bareboogerhost.com/

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





                  [Non-text portions of this message have been removed]
                • Des
                  chris, can t help on the drilling so much, but I can say my work with titanium shows it sticks to cutting tools, then galls badly and heats up until it
                  Message 8 of 25 , Jan 7, 2011
                  • 0 Attachment
                    chris,

                    can't help on the drilling so much, but I can say my work with titanium shows it sticks to cutting tools, then galls badly and heats up until it ignites, taking the tool edge with it.
                    In lathe work with titanium, I make 1 or 2 passes with the HSS tool, then swipe the edge clear with a small slip stone, and repeat until the job is done. - makes it labour intensive, but saves anymore surprises. (lucky my stack of swarf didn't go up the first time)

                    The first few times I'd see a small puff of white smoke, and my surface quality would immediately suffer - took me a little while to figure out that the smoke was the galled titanium igniting, and the edge would melt away in the heat (seen under magnifying glass) and that would destroy my surface if I kept cutting.

                    Maybe a peck drilling method, with tool cleaning at each step will achieve what you desire?

                    After all, the edges of the countersink would be similar to a form cutter....

                    Des

                    --- In taigtools@yahoogroups.com, Chris Ghent <cghent@...> wrote:
                    >
                    > I have a Taig CNC mill with the 240v Dayton motor and I am wondering if
                    > my problem with a particular job might be that the spindle motor is not
                    > strong enough.
                    >
                    > The job entails putting two conical holes in a piece of titanium rod 5mm
                    > in diameter. The conical holes come in from 180° apart so they meet,
                    > leaving a single hole through the rod which is conical on both sides.
                    >
                    > I have been using a centre drill to do this job. For no real reason I
                    > have increased the clearance behind the cutting edge hoping to cut down
                    > on heat build up.
                    >
                    > What I find is that I am forced to run the spindle very fast, about
                    > 6000rpm, and the speed of cut at .5" pm to have any chance of getting
                    > through the rod without a spindle stall. This seems much faster (and the
                    > speed of cut much slower) than I would like to run it, which would be
                    > more like 1.5" speed of cut and 1500 rpm. There is a lot of heat
                    > generated and the tool gets damaged quickly. But I can't slow the motor
                    > without guaranteeing a stall. I used to run a Sherline DC motor and the
                    > situation was still marginal but I could get away with it. Unfortunately
                    > as regular readers of this space might the Sherline started putting out
                    > noise which got into the motor circuits.
                    >
                    > I am wondering if someone might be able to suggest a cutter that might
                    > do a better job or suggest any ideas that might help..?
                    >
                    > Best Wishes
                    >
                    > Chris
                    >
                  • Ken Cline
                    ... Interesting. I had a lot of trouble one time when I tried to drill a hole radially through a piece of stainless steel rod. Your story makes me wonder if
                    Message 9 of 25 , Jan 7, 2011
                    • 0 Attachment
                      On 7 Jan 2011, at 3:04 PM, Clint wrote:

                      > Interesting situation with the drilling - but I am only drilling steel and brass. I have similar problem on my Taig lathe, when trying to drill a piece in the cross-slide vise, with the drill bit located in the head-stock collet. It usually takes lots of pressure on the cross-slide carriage wheel to drill through the metal. I can take the same drill bit and put it in my drill press and it drills through like butter. In drilling a piece of round stock, with the bit in the tail-stock chuck, it drills through very easily.


                      Interesting. I had a lot of trouble one time when I tried to drill a hole radially through a piece of stainless steel rod. Your story makes me wonder if I would have had better luck clamping the rod in, e.g., on top of a grooved piece of aluminum which would have solidly resisted downward forces, compared to letting it hang off the end of my vise.

                      Of course, titanium is twice as prone to flexing as steel (its Young's modulus is half that of steel), and will work harden in the blink of an eye.



                      [Non-text portions of this message have been removed]
                    • Ron Thompson
                      ... As someone already pointed out, you can t pussy foot around with material that work hardens. If you cut too shallow or rub it by cutting too fast, your
                      Message 10 of 25 , Jan 7, 2011
                      • 0 Attachment
                        On 1/7/2011 8:11 PM, Ken Cline wrote:
                        >
                        > On 7 Jan 2011, at 3:04 PM, Clint wrote:
                        >
                        > > Interesting situation with the drilling - but I am only drilling
                        > steel and brass. I have similar problem on my Taig lathe, when trying
                        > to drill a piece in the cross-slide vise, with the drill bit located
                        > in the head-stock collet. It usually takes lots of pressure on the
                        > cross-slide carriage wheel to drill through the metal. I can take the
                        > same drill bit and put it in my drill press and it drills through like
                        > butter. In drilling a piece of round stock, with the bit in the
                        > tail-stock chuck, it drills through very easily.
                        >
                        > Interesting. I had a lot of trouble one time when I tried to drill a
                        > hole radially through a piece of stainless steel rod. Your story makes
                        > me wonder if I would have had better luck clamping the rod in, e.g.,
                        > on top of a grooved piece of aluminum which would have solidly
                        > resisted downward forces, compared to letting it hang off the end of
                        > my vise.
                        >
                        > Of course, titanium is twice as prone to flexing as steel (its Young's
                        > modulus is half that of steel), and will work harden in the blink of
                        > an eye.
                        >
                        > [Non-text portions of this message have been removed]
                        >
                        As someone already pointed out, you can't pussy foot around with
                        material that work hardens. If you cut too shallow or rub it by cutting
                        too fast, your done.
                        Step into it and take a good bite. If you are having sticking issues,
                        you are most likely running too fast.

                        --


                        Ron Thompson
                        On the Beautiful Florida Space Coast, right beside the Kennedy Space Center, USA

                        There are two kinds of posts on newsgroups.
                        1. This is what I have done...
                        2. This is what I think...
                        Be aware of the difference!

                        http://www.ourcadguy.com/

                        http://www.plansandprojects.com My hobby pages are here:
                        http://www.plansandprojects.com/My%20Machines/

                        Visit the castinghobby FAQ:
                        http://castinghobbyfaq.bareboogerhost.com/








                        [Non-text portions of this message have been removed]
                      • Steve Blackmore
                        ... There are many different alloys of Titanium and the FPM varies quite a bit from 20FPM for some Beta alloys to 100FPM for pure Ti (110-150HB) Ball park
                        Message 11 of 25 , Jan 7, 2011
                        • 0 Attachment
                          On Fri, 7 Jan 2011 12:08:41 -0700, you wrote:

                          >I agree with Tony about the feeds and speeds. This source [http://www.timet.com/fab-p18.htm%5d suggests speeds in the 10-40ft/min range for drilling Ti with HSS drills, which works out to 250-1000rpm for your task. Slowing the feed below the suggested .002-.005in/rev range may be asking for trouble since it places the cutting edge closer to work hardened surface that was just cut. You can find faster speeds and wider feed ranges at other sources which might contradict my advice, so take it as a suggestion rather than a hard and fast rule.

                          There are many different alloys of Titanium and the FPM varies quite a
                          bit from 20FPM for some Beta alloys to 100FPM for pure Ti (110-150HB)

                          Ball park figure for a 3mm HSS drill and a mid range Ti Alloy

                          MATERIAL= Titanium 5Al-2.5Sn - Alpha/Alpha-Beta Alloy (300-350 HB)
                          SURFACE SPEED= 50 FPM
                          DRILL MATERIAL= HSS
                          DRILL DIAMETER= 0.11811 inches 3 mm
                          LOAD PER FLUTE= 0.00625 inches
                          NUMBER OF FLUTES= 2
                          SPINDLE SPEED= 1617 RPM
                          FEEDRATE= 20.2125 IPM 513.3975 mmPM
                          MATERIAL REMOVAL RATE= 0.22145 in³/min
                          MATERIAL POWER CONSTANT= 0.73
                          REQUIRED HORSEPOWER= 0.19019


                          For pure Ti that would be 3200rpm and 33ipm, Beta Alloy would be 640rpm
                          and 4IPM

                          As you can see - a huge range, so without knowing the alloy type it's
                          impossible to give accurate cutting figures.

                          Steve Blackmore
                          --
                        • Ken Cline
                          ... This seems like too much to ask of a Taig mill. My calculations (see below) indicate the power required is 0.35HP, that doesn t leave the kind of margin
                          Message 12 of 25 , Jan 8, 2011
                          • 0 Attachment
                            On 7 Jan 2011, at 11:50 PM, Steve Blackmore wrote:

                            > Ball park figure for a 3mm HSS drill and a mid range Ti Alloy
                            >
                            > MATERIAL= Titanium 5Al-2.5Sn - Alpha/Alpha-Beta Alloy (300-350 HB)
                            > DRILL DIAMETER= 0.11811 inches 3 mm
                            > LOAD PER FLUTE= 0.00625 inches
                            > SPINDLE SPEED= 1617 RPM
                            > REQUIRED HORSEPOWER= 0.19019


                            This seems like too much to ask of a Taig mill. My calculations (see below) indicate the power required is 0.35HP, that doesn't leave the kind of margin for error I would be looking for, especial for someone who has had motor stalling issues. If that's not bad enough, the required Z-axis thrust is 560 lbs, way over what I would consider attempting on with my CNC setup.

                            The power calculation relies on formulas and data from Machinery's Handbook (the section on estimating drilling power). Admittedly, I substituted 6Al4V which is a somewhat higher strength alpha-beta alloy, though with similar hardness to 5Al2.5Sn.

                            Power at the cutter P_c = K_d * F_f * F_M * A * W * N / 63025 = 0.35HP,
                            where
                            K_d = 18000 Work material factor
                            F_f = 0.030 Feed factor
                            F_M = 0.018 Torque factor for drill diameter
                            A = 1.085 Chisel edge factor for torque for a typical twist drill
                            N = 1617 Spindle speed

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

                            One other thing: I suggested drilling a pilot hole as a way to reduce the power needed on the final operation, but forgot to mention the advice to use the shortest bit possible when drilling titanium to reduce flex.

                            [Non-text portions of this message have been removed]
                          • Steve Blackmore
                            ... There seem to be some factors missing from that calculation? Removal rate? Machine tool efficiency factor, Wear Factor? Also Feed factor and Feed factor
                            Message 13 of 25 , Jan 8, 2011
                            • 0 Attachment
                              On Sat, 8 Jan 2011 01:38:59 -0700, you wrote:


                              >This seems like too much to ask of a Taig mill. My calculations (see below) indicate the power required is 0.35HP, that doesn't leave the kind of margin for error I would be looking for, especial for someone who has had motor stalling issues. If that's not bad enough, the required Z-axis thrust is 560 lbs, way over what I would consider attempting on with my CNC setup.
                              >
                              >The power calculation relies on formulas and data from Machinery's Handbook (the section on estimating drilling power). Admittedly, I substituted 6Al4V which is a somewhat higher strength alpha-beta alloy, though with similar hardness to 5Al2.5Sn.
                              >
                              >Power at the cutter P_c = K_d * F_f * F_M * A * W * N / 63025 = 0.35HP,
                              >where
                              > K_d = 18000 Work material factor
                              > F_f = 0.030 Feed factor
                              > F_M = 0.018 Torque factor for drill diameter
                              > A = 1.085 Chisel edge factor for torque for a typical twist drill
                              > N = 1617 Spindle speed

                              There seem to be some factors missing from that calculation? Removal
                              rate? Machine tool efficiency factor, Wear Factor? Also Feed factor and
                              Feed factor for power constant (not the same and both needed)?

                              Where do you get the thrust figure from? As an example work out the
                              thrust, using the same source, on something you know you can drill with
                              a Taig and see what that is. I've worked plenty of Ti and know you don't
                              need over 500lbs force to drill it. I'd have to dangle in mid air on the
                              drill press handle to exert that!

                              Even if it were .35HP, a 400W motor should be able to manage that
                              without stalling.

                              The stalling is likely caused by blunt drill, and not running the motor
                              at optimum power/speed.

                              Drills will only last seconds rubbing them on Ti :)

                              Steve Blackmore
                              --
                            • Rick Reyes
                              Would an endmill work better? ________________________________ From: Ken Cline To: taigtools@yahoogroups.com Sent: Sat, January 8, 2011
                              Message 14 of 25 , Jan 8, 2011
                              • 0 Attachment
                                Would an endmill work better?



                                ________________________________
                                From: Ken Cline <cline@...>
                                To: taigtools@yahoogroups.com
                                Sent: Sat, January 8, 2011 1:38:59 AM
                                Subject: Re: [taigtools] drilling issues



                                On 7 Jan 2011, at 11:50 PM, Steve Blackmore wrote:

                                > Ball park figure for a 3mm HSS drill and a mid range Ti Alloy
                                >
                                > MATERIAL= Titanium 5Al-2.5Sn - Alpha/Alpha-Beta Alloy (300-350 HB)
                                > DRILL DIAMETER= 0.11811 inches 3 mm
                                > LOAD PER FLUTE= 0.00625 inches
                                > SPINDLE SPEED= 1617 RPM
                                > REQUIRED HORSEPOWER= 0.19019

                                This seems like too much to ask of a Taig mill. My calculations (see below)
                                indicate the power required is 0.35HP, that doesn't leave the kind of margin for
                                error I would be looking for, especial for someone who has had motor stalling
                                issues. If that's not bad enough, the required Z-axis thrust is 560 lbs, way
                                over what I would consider attempting on with my CNC setup.

                                The power calculation relies on formulas and data from Machinery's Handbook (the
                                section on estimating drilling power). Admittedly, I substituted 6Al4V which is
                                a somewhat higher strength alpha-beta alloy, though with similar hardness to
                                5Al2.5Sn.

                                Power at the cutter P_c = K_d * F_f * F_M * A * W * N / 63025 = 0.35HP,
                                where
                                K_d = 18000 Work material factor
                                F_f = 0.030 Feed factor
                                F_M = 0.018 Torque factor for drill diameter
                                A = 1.085 Chisel edge factor for torque for a typical twist drill
                                N = 1617 Spindle speed

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

                                One other thing: I suggested drilling a pilot hole as a way to reduce the power
                                needed on the final operation, but forgot to mention the advice to use the
                                shortest bit possible when drilling titanium to reduce flex.

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







                                [Non-text portions of this message have been removed]
                              • Ken Cline
                                ... The usual formula for estimating power is not very accurate for drilling operations. Machinery s Handbook puts it this way: Although the lips of a drill
                                Message 15 of 25 , Jan 8, 2011
                                • 0 Attachment
                                  On 8 Jan 2011, at 8:47 AM, Steve Blackmore wrote:

                                  > Power at the cutter P_c = K_d * F_f * F_M * A * W * N / 63025 = 0.35HP,
                                  > >where
                                  > > K_d = 18000 Work material factor
                                  > > F_f = 0.030 Feed factor
                                  > > F_M = 0.018 Torque factor for drill diameter
                                  > > A = 1.085 Chisel edge factor for torque for a typical twist drill
                                  > > N = 1617 Spindle speed
                                  >
                                  > There seem to be some factors missing from that calculation? Removal
                                  > rate? Machine tool efficiency factor, Wear Factor? Also Feed factor and
                                  > Feed factor for power constant (not the same and both needed)?

                                  The usual formula for estimating power is not very accurate for drilling operations. Machinery's Handbook puts it this way: "Although the lips of a drill cut metal and produce a chip in the same manner as the cutting edges of other metal cutting tools, the chisel edge removes the metal by means of a very complex combination of extrusion and cutting. For this reason a separate method must be used to estimate the power required for drilling."

                                  The recommended method uses separate terms that depend on drill diameter, feed per revolution, and rpm. The parameters you mentioned do not apply. Except the tool wear factor, which I accidentally omitted. I used W=1.3, though 1.5 is specified for hard-to-work materials and would increase required power to 0.40HP at the cutter.

                                  > Where do you get the thrust figure from? As an example work out the
                                  > thrust, using the same source, on something you know you can drill with
                                  > a Taig and see what that is. I've worked plenty of Ti and know you don't
                                  > need over 500lbs force to drill it. I'd have to dangle in mid air on the
                                  > drill press handle to exert that!

                                  Thrust is given by the formula T = (2 * K_d * F_f * F_T * B * W) + (K_d * D^2 * J * W), where
                                  K_d = 29000 Work material for 6Al4V (note: different K_d for thrust and torque calculations for Ti)
                                  F_f = 0.030 Feed factor
                                  F_T = 0.178 Thrust factor for drill diameter
                                  B = 1.355 Chisel edge factor for thrust (B)
                                  W = 1.3 Tool wear factor
                                  D = 0.11811 Drill diameter
                                  J = 0.030 Chisel edge factor for thrust (J)

                                  Just to be clear, you are exaggerating (presumably for effect?) when you talk about dangling in mid air. My drill press like object has 6:1 mechanical advantage, and I could provide the 90 pounds of force necessary. But I doubt I would cut as aggressively as .012"/rev on a manual drill press.

                                  > Even if it were .35HP, a 400W motor should be able to manage that
                                  > without stalling.

                                  OK... But Taig mills are supplied with either 1/5HP or 1/4HP motors. Attempting an operation that requires 1/3HP is asking for trouble.

                                  > Drills will only last seconds rubbing them on Ti :)

                                  Indeed: Thou salt not dwell!
                                • Ken Cline
                                  ... Better stick with drill bits, which are optimized for drilling. [Non-text portions of this message have been removed]
                                  Message 16 of 25 , Jan 8, 2011
                                  • 0 Attachment
                                    On 8 Jan 2011, at 2:06 PM, Rick Reyes wrote:

                                    > Would an endmill work better?


                                    Better stick with drill bits, which are optimized for drilling.

                                    [Non-text portions of this message have been removed]
                                  • Chris Ghent
                                    Thank you to everyone who contributed in answer to my slightly anguished question. I especially appreciate Tony, Ken and Steve, who have advised me on many
                                    Message 17 of 25 , Jan 8, 2011
                                    • 0 Attachment
                                      Thank you to everyone who contributed in answer to my slightly anguished
                                      question. I especially appreciate Tony, Ken and Steve, who have advised
                                      me on many occasions over the last 5 years or so and whose advice is
                                      always steady. This is not to denigrate the contribution of others.

                                      I am still caught in a few different ways. One is in myself, sometimes I
                                      just want to get on with things; this impatience is my biggest issue
                                      with my work and I fight it where I recognise it. In this case it had me
                                      looking for a quick solution, hoping for a single fact I had not
                                      appreciated and could easily adapt to. My feeling was I need more low
                                      speed power and the replies have confirmed that. Ken's estimate of the
                                      power needed is about 1/10th horsepower and some specification lists put
                                      the power of the Dayton motor at that exact number.n Throw in a not
                                      quite ideal tool and insufficient coolant and it does not look unusual I
                                      am having trouble.

                                      Drilling a pilot hole is obviously the way to go and I have resisted
                                      this because of the number of tool changes it entails, two extra per
                                      hole because it is not possible to do more than one holeset at a time.

                                      Rather than being a machinist or enthusiast for machining, (though I
                                      enjoy it) my workshop is geared towards a single but complicated product
                                      with 2000 parts. I make about 1900 of these in-house (the rest are tiny
                                      screws) and then assemble them. Anyone who wants to see what I am
                                      talking about can look at www.concertina.com.au While it is not
                                      particularly lucrative, the waiting list for the product has ballooned
                                      out to 4 years and I feel that pressure. I try to do things on the CNC
                                      Taig in such a way as I can be doing something else at the same time.
                                      In the past while drilling this hole using the Sherline motor I have
                                      been working on the lathe doing the next step on the drilled rod and
                                      trying to keep up with the drilling process. So I put a piece of stock
                                      in the 4th axis on the Taig, gave it a squirt of lubricant and set it in
                                      motion drilling the two holes 180° apart and take the last piece it
                                      drilled to the lathe and turn it. It used to be I could have a button
                                      turned and get back to the CNC and it would have been waiting about 1
                                      minute with the next piece. I was always aware the drilling operation
                                      was a marginal enterprise from the noise and heat, but a two step
                                      process will double the length of time it takes to do the job and if I
                                      do it by the book I will need to be there for all of that time applying
                                      lubricant/coolant.

                                      It could be done with a single cutter if the straight part of the cutter
                                      was long enough to get right through the rod before the tapered part
                                      came into play. My grinding skills are not up to making this and I have
                                      looked online without finding a countersink with a pilot that is long
                                      enough.

                                      So yes, I would like to run slower but to do so needs a bigger motor.

                                      I understand the need for more lubrication/coolant, but cannot readily
                                      fit a flood system in the present space (very cramped).

                                      Pilot holes I can do and I think I will have to learn to smile while I
                                      do it.

                                      Best Wishes to all...

                                      Chris




                                      > 1b. Re: drilling issues
                                      > Posted by: "Ken Cline"cline@... hfxlhfxl
                                      > Date: Fri Jan 7, 2011 11:08 am ((PST))
                                      >
                                      > I agree with Tony about the feeds and speeds. This source [http://www.timet.com/fab-p18.htm%5d suggests speeds in the 10-40ft/min range for drilling Ti with HSS drills, which works out to 250-1000rpm for your task. Slowing the feed below the suggested .002-.005in/rev range may be asking for trouble since it places the cutting edge closer to work hardened surface that was just cut. You can find faster speeds and wider feed ranges at other sources which might contradict my advice, so take it as a suggestion rather than a hard and fast rule.
                                      >
                                      > Assuming you are cutting properly (feed& speed, sharp bit, ample coolant, pecking cycle to clear chips, etc.), the power required to cut titanium is a little less that for steel. I ran the numbers for your drilling operation and got an estimate of 0.1 HP required at the bottom of the cut, where the diameter being drilled is widest. It seems reasonable to expect that kind of power from your spindle, but I don't know anything about the motor on your mill other than brand name. You might want to check whether you can drill mild steel with the same parameters (I would run at my lowest speed, 1000 RPM, and 0.002in/rev = 2in/min feed). If the steel cuts without stalling, something is going wrong when you drill titanium.
                                      >
                                      > If all else fails, it may be possible to reduce power requirements by first drilling a pilot hole (use a spotting drill to locate the hole), then widening it with a larger drill or countersink.
                                      >
                                      > Carbide is often recommended for cutting Ti, but I would start with good cobalt (hss) tools. Steel tools are sharper, though they won't last as long. Also if my calculations are correct, Taig mills lack the power to make effective use of carbide's higher speeds - at 6000 rpm my motor would be maxed out, with no margin for error. I have also heard advice from a local titanium fabricator (bicycle frames) who told me he prefers HSS tooling over carbide for the kind of work he does (typically drilling, "mitering" tubing with a hole saw, reaming, and tapping).
                                      >
                                      > Good luck!
                                      >
                                      >
                                      >
                                    • Steve Blackmore
                                      ... I ve been out to the shop with a spring balance. I need to pull at 20lbs force to drill Ti. I don t know the mechanical advantage, but it s certainly not
                                      Message 18 of 25 , Jan 9, 2011
                                      • 0 Attachment
                                        On Sat, 8 Jan 2011 15:37:22 -0700, you wrote:


                                        >Just to be clear, you are exaggerating (presumably for effect?) when you talk about dangling in mid air. My drill press like object has 6:1 mechanical advantage, and I could provide the 90 pounds of force necessary. But I doubt I would cut as aggressively as .012"/rev on a manual drill press.

                                        I've been out to the shop with a spring balance. I need to pull at 20lbs
                                        force to drill Ti. I don't know the mechanical advantage, but it's
                                        certainly not 27:1. It's a rack and pinion design, I reckon 6:1 is about
                                        right.

                                        >> Even if it were .35HP, a 400W motor should be able to manage that
                                        >> without stalling.
                                        >
                                        >OK... But Taig mills are supplied with either 1/5HP or 1/4HP motors. Attempting an operation that requires 1/3HP is asking for trouble.
                                        >

                                        You may be right, I looked up 240V Dayton Motor Taig, and the 400W one
                                        is an upgrade people have done.

                                        Looks like they only supplied a paltry 3000 rpm 1/8th HP motor with the
                                        CNC 2019 and then some upgrade took that to whopping 1/4HP :(

                                        When I had my Taig, I fitted a 1/2HP DC Servo motor for the spindle. It
                                        worked well, even with the tiny drive belt. I bought a spare belt and
                                        never had to use it.

                                        Steve Blackmore
                                        --
                                      • Ken Cline
                                        ... Are you sure you are feeding at .012 /rev? When I plug 120 lbf (20lbf @ 6:1) into the thrust formula and solve for feed rate, it says you must be feeding
                                        Message 19 of 25 , Jan 9, 2011
                                        • 0 Attachment
                                          On 9 Jan 2011, at 2:14 AM, Steve Blackmore wrote:

                                          > On Sat, 8 Jan 2011 15:37:22 -0700, you wrote:
                                          >
                                          > >Just to be clear, you are exaggerating (presumably for effect?) when you talk about dangling in mid air. My drill press like object has 6:1 mechanical advantage, and I could provide the 90 pounds of force necessary. But I doubt I would cut as aggressively as .012"/rev on a manual drill press.
                                          >
                                          > I've been out to the shop with a spring balance. I need to pull at 20lbs
                                          > force to drill Ti. I don't know the mechanical advantage, but it's
                                          > certainly not 27:1. It's a rack and pinion design, I reckon 6:1 is about
                                          > right.


                                          Are you sure you are feeding at .012"/rev? When I plug 120 lbf (20lbf @ 6:1) into the thrust formula and solve for feed rate, it says you must be feeding at about 0.002"/rev. That value seems a lot more reasonable to me.

                                          [Non-text portions of this message have been removed]
                                        • Will Schmit
                                          Steve, What program do you use for your Speeds & Feeds Tables? I would love to plug a couple of materials into the wizard on VisualMill.
                                          Message 20 of 25 , Jan 9, 2011
                                          • 0 Attachment
                                            Steve,
                                            What program do you use for your Speeds & Feeds Tables?
                                            I would love to plug a couple of materials into the wizard on VisualMill.





                                            ________________________________
                                            From: Steve Blackmore <steve@...>
                                            To: taigtools@yahoogroups.com
                                            Sent: Sun, January 9, 2011 2:14:05 AM
                                            Subject: Re: [taigtools] drilling issues


                                            On Sat, 8 Jan 2011 15:37:22 -0700, you wrote:

                                            >Just to be clear, you are exaggerating (presumably for effect?) when you talk
                                            >about dangling in mid air. My drill press like object has 6:1 mechanical
                                            >advantage, and I could provide the 90 pounds of force necessary. But I doubt I
                                            >would cut as aggressively as .012"/rev on a manual drill press.

                                            I've been out to the shop with a spring balance. I need to pull at 20lbs
                                            force to drill Ti. I don't know the mechanical advantage, but it's
                                            certainly not 27:1. It's a rack and pinion design, I reckon 6:1 is about
                                            right.

                                            >> Even if it were .35HP, a 400W motor should be able to manage that
                                            >> without stalling.
                                            >
                                            >OK... But Taig mills are supplied with either 1/5HP or 1/4HP motors. Attempting
                                            >an operation that requires 1/3HP is asking for trouble.
                                            >

                                            You may be right, I looked up 240V Dayton Motor Taig, and the 400W one
                                            is an upgrade people have done.

                                            Looks like they only supplied a paltry 3000 rpm 1/8th HP motor with the
                                            CNC 2019 and then some upgrade took that to whopping 1/4HP :(

                                            When I had my Taig, I fitted a 1/2HP DC Servo motor for the spindle. It
                                            worked well, even with the tiny drive belt. I bought a spare belt and
                                            never had to use it.

                                            Steve Blackmore
                                            --



                                            [Non-text portions of this message have been removed]
                                          • Steve Blackmore
                                            ... The tabular ones are produced by Machinist Toolbox, http://www.machinist-toolbox.com/ it pretty much agrees with the suggested feeds and speeds from my CAM
                                            Message 21 of 25 , Jan 9, 2011
                                            • 0 Attachment
                                              On Sun, 9 Jan 2011 09:35:58 -0800 (PST), you wrote:


                                              >What program do you use for your Speeds & Feeds Tables?
                                              >I would love to plug a couple of materials into the wizard on VisualMill.

                                              The tabular ones are produced by Machinist Toolbox,

                                              http://www.machinist-toolbox.com/

                                              it pretty much agrees with the suggested feeds and speeds from my CAM
                                              program (FeatureCam). CAM's nice though, you can limit the HP, speed or
                                              feed or any combination on the fly and it will adjust the output to
                                              suit. You can also save all the machine and tooling parameters and be
                                              sure that the code is going to work without any tweaking.

                                              Steve Blackmore
                                              --
                                            • Lewis hein
                                              Welll.. I never needed to drill a hole in an issue before. Just how is it done? ... From: Ken Cline To: Sent:
                                              Message 22 of 25 , Jan 11, 2011
                                              • 0 Attachment
                                                Welll.. I never needed to drill a hole in an issue before. Just how is it
                                                done?
                                                ----- Original Message -----
                                                From: "Ken Cline" <cline@...>
                                                To: <taigtools@yahoogroups.com>
                                                Sent: Sunday, January 09, 2011 8:34 AM
                                                Subject: Re: [taigtools] drilling issues


                                                >
                                                > On 9 Jan 2011, at 2:14 AM, Steve Blackmore wrote:
                                                >
                                                >> On Sat, 8 Jan 2011 15:37:22 -0700, you wrote:
                                                >>
                                                >> >Just to be clear, you are exaggerating (presumably for effect?) when you
                                                >> >talk about dangling in mid air. My drill press like object has 6:1
                                                >> >mechanical advantage, and I could provide the 90 pounds of force
                                                >> >necessary. But I doubt I would cut as aggressively as .012"/rev on a
                                                >> >manual drill press.
                                                >>
                                                >> I've been out to the shop with a spring balance. I need to pull at 20lbs
                                                >> force to drill Ti. I don't know the mechanical advantage, but it's
                                                >> certainly not 27:1. It's a rack and pinion design, I reckon 6:1 is about
                                                >> right.
                                                >
                                                >
                                                > Are you sure you are feeding at .012"/rev? When I plug 120 lbf (20lbf @
                                                > 6:1) into the thrust formula and solve for feed rate, it says you must be
                                                > feeding at about 0.002"/rev. That value seems a lot more reasonable to
                                                > me.
                                                >
                                                > [Non-text portions of this message have been removed]
                                                >
                                                >
                                                >
                                                > ------------------------------------
                                                >
                                                > 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
                                                >
                                                >
                                                >
                                                >
                                              • Tony Jeffree
                                                You have to pin the issue down first...then its a snap. Regards, Tony ... [Non-text portions of this message have been removed]
                                                Message 23 of 25 , Jan 11, 2011
                                                • 0 Attachment
                                                  You have to pin the issue down first...then its a snap.

                                                  Regards,
                                                  Tony


                                                  On 11 January 2011 16:33, Lewis hein <lhein@...> wrote:

                                                  > Welll.. I never needed to drill a hole in an issue before. Just how is it
                                                  > done?
                                                  > ----- Original Message -----
                                                  > From: "Ken Cline" <cline@...>
                                                  > To: <taigtools@yahoogroups.com>
                                                  > Sent: Sunday, January 09, 2011 8:34 AM
                                                  > Subject: Re: [taigtools] drilling issues
                                                  >
                                                  >
                                                  > >
                                                  > > On 9 Jan 2011, at 2:14 AM, Steve Blackmore wrote:
                                                  > >
                                                  > >> On Sat, 8 Jan 2011 15:37:22 -0700, you wrote:
                                                  > >>
                                                  > >> >Just to be clear, you are exaggerating (presumably for effect?) when
                                                  > you
                                                  > >> >talk about dangling in mid air. My drill press like object has 6:1
                                                  > >> >mechanical advantage, and I could provide the 90 pounds of force
                                                  > >> >necessary. But I doubt I would cut as aggressively as .012"/rev on a
                                                  > >> >manual drill press.
                                                  > >>
                                                  > >> I've been out to the shop with a spring balance. I need to pull at 20lbs
                                                  > >> force to drill Ti. I don't know the mechanical advantage, but it's
                                                  > >> certainly not 27:1. It's a rack and pinion design, I reckon 6:1 is about
                                                  > >> right.
                                                  > >
                                                  > >
                                                  > > Are you sure you are feeding at .012"/rev? When I plug 120 lbf (20lbf @
                                                  > > 6:1) into the thrust formula and solve for feed rate, it says you must be
                                                  > > feeding at about 0.002"/rev. That value seems a lot more reasonable to
                                                  > > me.
                                                  > >
                                                  > > [Non-text portions of this message have been removed]
                                                  > >
                                                  > >
                                                  > >
                                                  > > ------------------------------------
                                                  > >
                                                  > > 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
                                                  > >
                                                  > >
                                                  > >
                                                  > >
                                                  >
                                                  >
                                                  >
                                                  >
                                                  > ------------------------------------
                                                  >
                                                  > 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]
                                                • Lewis hein
                                                  I know it is. Last time I tried to drill an issue it snapped my drill right off. Here in Wyoming, oil is a big issue that people drill all the time.. maybe
                                                  Message 24 of 25 , Jan 11, 2011
                                                  • 0 Attachment
                                                    I know it is. Last time I tried to drill an issue it snapped my drill right
                                                    off. Here in Wyoming, oil is a big issue that people drill all the time..
                                                    maybe I'll have to ask the derrick crews for some hints.

                                                    Lewis Hein
                                                    ----- Original Message -----
                                                    From: "Tony Jeffree" <tony@...>
                                                    To: "taigtools" <taigtools@yahoogroups.com>
                                                    Sent: Tuesday, January 11, 2011 9:42 AM
                                                    Subject: Re: [taigtools] drilling issues


                                                    > You have to pin the issue down first...then its a snap.
                                                    >
                                                    > Regards,
                                                    > Tony
                                                    >
                                                    >
                                                    > On 11 January 2011 16:33, Lewis hein <lhein@...> wrote:
                                                    >
                                                    >> Welll.. I never needed to drill a hole in an issue before. Just how is it
                                                    >> done?
                                                    >> ----- Original Message -----
                                                    >> From: "Ken Cline" <cline@...>
                                                    >> To: <taigtools@yahoogroups.com>
                                                    >> Sent: Sunday, January 09, 2011 8:34 AM
                                                    >> Subject: Re: [taigtools] drilling issues
                                                    >>
                                                    >>
                                                    >> >
                                                    >> > On 9 Jan 2011, at 2:14 AM, Steve Blackmore wrote:
                                                    >> >
                                                    >> >> On Sat, 8 Jan 2011 15:37:22 -0700, you wrote:
                                                    >> >>
                                                    >> >> >Just to be clear, you are exaggerating (presumably for effect?) when
                                                    >> you
                                                    >> >> >talk about dangling in mid air. My drill press like object has 6:1
                                                    >> >> >mechanical advantage, and I could provide the 90 pounds of force
                                                    >> >> >necessary. But I doubt I would cut as aggressively as .012"/rev on a
                                                    >> >> >manual drill press.
                                                    >> >>
                                                    >> >> I've been out to the shop with a spring balance. I need to pull at
                                                    >> >> 20lbs
                                                    >> >> force to drill Ti. I don't know the mechanical advantage, but it's
                                                    >> >> certainly not 27:1. It's a rack and pinion design, I reckon 6:1 is
                                                    >> >> about
                                                    >> >> right.
                                                    >> >
                                                    >> >
                                                    >> > Are you sure you are feeding at .012"/rev? When I plug 120 lbf (20lbf
                                                    >> > @
                                                    >> > 6:1) into the thrust formula and solve for feed rate, it says you must
                                                    >> > be
                                                    >> > feeding at about 0.002"/rev. That value seems a lot more reasonable to
                                                    >> > me.
                                                    >> >
                                                    >> > [Non-text portions of this message have been removed]
                                                    >> >
                                                    >> >
                                                    >> >
                                                    >> > ------------------------------------
                                                    >> >
                                                    >> > 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
                                                    >> >
                                                    >> >
                                                    >> >
                                                    >> >
                                                    >>
                                                    >>
                                                    >>
                                                    >>
                                                    >> ------------------------------------
                                                    >>
                                                    >> 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]
                                                    >
                                                    >
                                                    >
                                                    > ------------------------------------
                                                    >
                                                    > 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
                                                    >
                                                    >
                                                    >
                                                    >
                                                  • Will Schmit
                                                    Thanks Steve -- I ll look for it. ________________________________ From: Steve Blackmore To: taigtools@yahoogroups.com Sent: Sun, January
                                                    Message 25 of 25 , Jan 11, 2011
                                                    • 0 Attachment
                                                      Thanks Steve -- I'll look for it.





                                                      ________________________________
                                                      From: Steve Blackmore <steve@...>
                                                      To: taigtools@yahoogroups.com
                                                      Sent: Sun, January 9, 2011 4:12:03 PM
                                                      Subject: Re: [taigtools] drilling issues


                                                      On Sun, 9 Jan 2011 09:35:58 -0800 (PST), you wrote:

                                                      >What program do you use for your Speeds & Feeds Tables?
                                                      >I would love to plug a couple of materials into the wizard on VisualMill.

                                                      The tabular ones are produced by Machinist Toolbox,

                                                      http://www.machinist-toolbox.com/

                                                      it pretty much agrees with the suggested feeds and speeds from my CAM
                                                      program (FeatureCam). CAM's nice though, you can limit the HP, speed or
                                                      feed or any combination on the fly and it will adjust the output to
                                                      suit. You can also save all the machine and tooling parameters and be
                                                      sure that the code is going to work without any tweaking.

                                                      Steve Blackmore
                                                      --



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