Announcement

Collapse
No announcement yet.

Lathe turning speed various material

Collapse
X
 
  • Filter
  • Time
  • Show
Clear All
new posts

  • Lathe turning speed various material

    Big time novice here: I know there are specific speeds to turn or mill various materials. I usually turn and mill aluminum and steel. I have no speed read out so I guess based on finish and chip condition. I was thinking about getting a hand held tach to read RPM, but not sure how to convert to FPM which seems to be the standard for feed rates? Any advice on this? Thanks in advance

  • #2
    One could write a book on the subject... And in fact, people have! This is one of those broad questions that is almost too broad to cover in a forum. I'll start by suggesting that you find a copy of "Machinery's Handbook". This will be an invaluable resource, especially if you don't have internet in your shop. It has speed and feed tables for many different materials (my 1945 copy includes speed/feed tables for granite and frozen rubber, among more common stuff). It also has information on many other fields like fasteners, lubrication, bearings, strength of materials, how to calculate various things like FPM from RPM, etc.

    As for that last bit, it's not too hard. Let's take a piece of steel rod in a lathe as an example. You know the RPM of the lathe. Now imagine a string wrapped around the circumference of the circle. If it doesn't overlap at all, how long would that string be if I laid it out flat? It would be the diameter of the rod times pi. During one revolution, that piece of string has come completely off the rod. So now you know that for every 1 revolution, the surface travels a distance of the diameter times pi. To get FPM, then, you just multiply RPM times the circumference:

    FPM = RPM * Diameter x 3.1415926535

    (Assuming, of course, that the length units are the same... i.e. to get feet per minute, you need the diameter measured in feet)

    Comment


    • #3
      The formula you need to know is this:

      RPM = (4 x CS) / D

      Where CS is the Cutting Speed, in Surface Feet per Minute, and D is the Diameter of your workpiece at the cutting tip (if doing lathe work), or the diameter of a milling cutter.

      For example, if I were taking a modest roughing cut in mild steel (1018 or equivalent) where my lathe tool was positioned to cut a diameter of 1.25", I would pick a surface speed of maybe 150 SFM if using a high speed steel tool. Plug those numbers into the formula, and we get RPM = (4 x 150) / 1.25 = 480 RPM. Note that the SFM values given in reference books, like Machinery's Handbook, or in tooling manufacturers' catalogs are general suggestions and will vary depending on the material, the rigidity and power of your machine or setup, and the tool geometry.

      To go the other way, from RPM to SFM, the formula becomes (RPM x D) / 4. Working from the previous example, we have a cut diameter of 1.25 and RPM of 480. (480 x 1.25) / 4 = 150 SFM.

      Hope this helps!

      Comment


      • #4
        Assuming you're using HSS - high speed steel, the kind you sharpen up yourself:

        Ally - faster than you'd think; steel - slower than you'd think;

        Small diameter - faster; large - slower;

        Steel - coloured chips mean you're a bit fast.

        With a carbide tool - three times as fast as with HSS and coloured chips are OK.
        Richard - SW London, UK, EU.

        Comment


        • #5
          Originally posted by Brian H. View Post
          The formula you need to know is this:

          RPM = (4 x CS) / D

          Where CS is the Cutting Speed, in Surface Feet per Minute, and D is the Diameter of your workpiece at the cutting tip (if doing lathe work), or the diameter of a milling cutter.
          This is an approximation that assumes the diameter is in inches, the "CS" is feet-per-minute and approximates pi as 3. In that case, my formula can be reduced:

          FPM = RPM * (Diameter inches) * (1 foot / 12 inches) * pi

          Let pi = 3 then

          FPM = RPM * (Diameter inches) * (3 foot / 12 inches) = RPM * (Diameter inches) * (1 foot / 4 inches) and if we get rid of units, replacing them with the symbols Brian H. used, this becomes:

          FPM = RPM * D / 4

          Comment


          • #6
            The formula above, RPM=(4xCS)/Dia. is the way to go. The number 4 in the formula comes from rounding off 12"/pi when we convert diameter measurement in inches to speed measured in feet per minute. As for the Cutting Speeds, a general rule of thumb is; 50fpm for the tough to cut things like hard tool steels, 75fpm for high alloy steels, 100fpm for mild steel, 150fpm for brass/bronze, and 200fpm for aluminum. This is for turning and milling operations. Cut the calculated rpm in half for drilling and one quarter for reaming. Note that these numbers are for using a HSS tool, and an approximate starting point only. You will need to adjust depending on machine and part rigidity, type of cutting fluid used, etc........ If you are using carbide then take the calculated feet per minute number and multiply by three.

            It's not unusual for older machines to be lacking in spindle speed displays so if you can get an estimate with some sort of tach that's great. If the machine has step pulley speed adjustments then measure the diameters and chart out the speeds available. No matter what you do the machine will never have the exact speed required. That, and factoring in all the other variables is why these cutting speeds are approximates to be used as a starting point. Start with the calculated number, then find something close on the machine.
            Last edited by tom_d; 04-10-2018, 11:39 PM.

            Comment


            • #7
              There are lots of charts online that will tell you what the SFM should be for specific metals. The SFM ranges are quite broad. That's a good starting point. Printed out one of the charts and stuck it to the backsplash of the lathe and another to the column of the mill.

              A handheld contact or optical tachometer is a great idea. Once you get the speed for each setting, you write them down and take the batteries out of the tach. You won't need it for a while.

              Dan
              At the end of the project, there is a profound difference between spare parts and extra parts.

              Location: SF East Bay.

              Comment


              • #8
                Originally posted by kram350 View Post
                Big time novice here: I know there are specific speeds to turn or mill various materials. I usually turn and mill aluminum and steel. I have no speed read out so I guess based on finish and chip condition. I was thinking about getting a hand held tach to read RPM, but not sure how to convert to FPM which seems to be the standard for feed rates? Any advice on this? Thanks in advance
                No need for a tach if you have speed via belt position on pulleys.

                All you need is to know the motor speed, typically 1725 rpm or 3450 rpm in the US. Now for each belt setting, turn the motor (or the spindle, which ever is easier), and count the number of motor turns per spindle turn. Then divide the motor rpm by the motor turns you found, and you have rpm, as close as you need to know it.

                If, for instance, the motor is 1725 rpm, and the number of turns was 4 1/2, the spindle speed is 1725/4.5 = 383 rpm. Call it 380, or even just 400, and you will be fine. Put those results for each setting on a chart kept by the machine, and you can choose a setting easily once you know the speed you need.

                BTW, you can use any slower speed with most cutters. The slower the surface speed, the sharper the cutter wants to be, so the finish will often not be as good with carbide cutters at slow speeds, because carbide is often not very sharp.

                If you have speed set via a knob and dial, as with many small import machines, a tach could be more useful. I think some of them go from slowest to fastest in one turn of the knob, so even labeling marks on the dial might be fairly inaccurate.
                Last edited by J Tiers; 04-10-2018, 11:45 PM.
                1601

                Keep eye on ball.
                Hashim Khan

                Comment


                • #9
                  Don't forget the published figures are for industrial machines and tooling. Depending what machine you have, the smaller, lighter home shop machines might not cope and need slowing down. I haven't bothered with published figures for many years, its what sounds right, looks right and feels right. What Rohart says in post 4 makes a lot of sense
                  'It may not always be the best policy to do what is best technically, but those responsible for policy can never form a right judgement without knowledge of what is right technically' - 'Dutch' Kindelberger

                  Comment


                  • #10
                    And all those formulae fly out the window if you don't consider chip load and/or feed rate. Even more reason to use the "post 4" formula.

                    Comment


                    • #11
                      Originally posted by Richard P Wilson View Post
                      Don't forget the published figures are for industrial machines and tooling. Depending what machine you have, the smaller, lighter home shop machines might not cope and need slowing down. I haven't bothered with published figures for many years, its what sounds right, looks right and feels right. What Rohart says in post 4 makes a lot of sense
                      This is exceptionally wise advice. It really depends on the equipment. Monarch 10EE? I'd start with the posted industrial figures. Chinese or Southbend bench lathe? Much much slower.

                      I work on both ends of the spectrum - program and setup highly rigid CNC turning centres and also run small bench lathes.

                      If you have small hobby type equipment you should find yourself running on the slower end of your lathe for most things. If you have a backgear you'll be surprised by how often you will use it.

                      The good news is most cutting tools, including most of the fine grain carbide (which is pretty much all carbide these days) doesn't mind running slow, provided you have adequate feed (chip load). In manual machining feed is where the art and experience comes into the equation - you need to look at the chips and feel the forces in the machine to determine how things are progressing.
                      www.thecogwheel.net

                      Comment


                      • #12
                        Originally posted by enginuity View Post
                        This is exceptionally wise advice. It really depends on the equipment. Monarch 10EE? I'd start with the posted industrial figures. Chinese or Southbend bench lathe? Much much slower.

                        I work on both ends of the spectrum - program and setup highly rigid CNC turning centres and also run small bench lathes.

                        If you have small hobby type equipment you should find yourself running on the slower end of your lathe for most things.
                        Sort-of.

                        You can run as fast as the machine will allow. No reason to slow down just on the basis of the machine name, or place of origin.

                        Slow down because you get chatter, or the power of the motor will not allow a decent cut, etc etc. I run slower because the belt on the Logan slips if I run fast and take a big cut.

                        But I run as fast as the machine allows mechanically, in cases where that is called for by the material of the work and cutter.
                        1601

                        Keep eye on ball.
                        Hashim Khan

                        Comment


                        • #13
                          Originally posted by J Tiers View Post
                          Sort-of.

                          You can run as fast as the machine will allow. No reason to slow down just on the basis of the machine name, or place of origin.

                          Slow down because you get chatter, or the power of the motor will not allow a decent cut, etc etc. I run slower because the belt on the Logan slips if I run fast and take a big cut.

                          But I run as fast as the machine allows mechanically, in cases where that is called for by the material of the work and cutter.

                          You are right - you need the right speed and feed for your machine. It may not be the slowest setting.

                          But I've found with most people starting out on their bench lathe they run way too fast. Maybe it is because they are thinking about working with wood. Or maybe there is another reason.

                          The industrial suggested speeds will generally be way to fast for bench equipment (except for perhaps very small work), not because the machine is not capable of the speed, but as you say due to chatter.

                          I tell people start off slow and work your way up. Generally there is less chance of ruining your tool, and is also a safe practice from a work holding standpoint. When in doubt, reduce the speed.
                          www.thecogwheel.net

                          Comment


                          • #14
                            For HSS, you want shiny chips. For carbide you want colored chips. No math required. If your doing Cast Iron with HSS, and the tip instantly wears away, going too fast.

                            Comment


                            • #15
                              Originally posted by enginuity View Post
                              You are right - you need the right speed and feed for your machine. It may not be the slowest setting.

                              But I've found with most people starting out on their bench lathe they run way too fast. Maybe it is because they are thinking about working with wood. Or maybe there is another reason.
                              I believe they are suckered in by the term "high speed steel". I had to convince a newbie that 400 rpm was too fast for a HSS tool in a 3 in. diameter fly cutter in steel. Once he slowed down to about 100, the whole thing worked much better. CSx4/dia. is a very easy formula to remember and will get you close enough to start making chips (instead of resharpening your tool).
                              It's all mind over matter.
                              If you don't mind, it don't matter.

                              Comment

                              Working...
                              X