Okay, still interested? Let's dive in, then. The first "proper" section of this guide deals with shopping for a mill and understanding its operating characteristics; picking the appropriate cutting tools; and monitoring the performance of your setup to achieve perfect results every time.
Again, if you're using another manufacturing process and are interested strictly in the CAD tutorial or the resin casting bits, feel free to skip ahead.
General purpose, benchtop-sized CNC mills start at around $600 and go up to $20,000 or so. Somewhat surprisingly, quite a few of the sub-$2,000 devices are already perfectly sufficient for most jobs, and certainly for the workflows discussed in this guide. In fact, even the most picky shoppers can get all the useful features under $5,000; past that point, you are paying for functionality of relatively little significance to light-duty hobby work.
There are numerous manufacturers of benchtop CNC mills around the world; some of the best-known brands include Roland DG, Sherline, Taig, and Syil. But be sure to search around; there are quite a few other companies that cater to local markets - say, Probotix, Deepgroove1, LittleMachineShop, Romaxx, Microkinetics, MAXNC, Microproto, Light Machines, Minitech, Flashcut, Tormach, Smithy, ShopBot, Torchmate, CNC Masters, ACT, Charlyrobot, EasyCut, or Laguna Tools. Some people had luck with ultra-low cost mills made in China, too.
Of course, it is also possible to build your own machine from scratch. Doing so is not necessarily economically sound, because there is a significant price tag attached to high-precision linear motion systems, machine spindles, and powerful servos or stepper motors; on top of that, you will probably have to iterate through several designs, and the project will consume several months of your time. Still, if you are so inclined, there are low-cost plans and kits available on the Internet.
When shopping for a pre-made system, there are several key characteristics to pay attention to; let's have a look at them, and use them as an excuse to discuss some of the inner workings of CNC milling jobs.
This is perhaps the most fundamental quality of any CNC mill. In the most basic design, the cutting head can move in three directions - X, Y, and Z - and the tool itself always points down, aligned with the Z axis. In this setup, the machine can only machine shapes that can be represented using a two-dimensional "depth map" projected onto the workpiece: the cutter may descend lower for some X-Y coordinates, and move up for others, but it will not enter the workpiece from any other side. This video is a pretty good illustration of the process:
In this machining mode, the machinable geometries are outlined here:
Note: CAM applications are designed to fail safely; that is, if any of the features of the model cannot be reached without plowing through another essential section of the geometry, the problematic region simply won't be machined at all. The gray regions in the two workpieces on the right correspond to the material that will be left in place.
The limitations of three-axis machining may seem severe, but seldom truly are. Every section of an industrial injection mold or a metal forming die typically needs to be a depth projection anyway, so that the processed material could be pulled out of it easily. Even in direct machining, it is common to simply flip the workpiece with the aid of registration pins. This video illustrates the manual rotation process fairly well.
That said, there are some shapes that truly benefit from automated, multi-directional machining; this includes exotic types of gears (helical, herringbone, and worm geometries) and certain categories of jewelry (say, rings). For these uses, some CNC mills come with additional rotary "axes": the so-called A axis corresponds to rotating the workpiece around the X axis (see video); B axis stands for rotation around Y; and C axis is the rotation around Z. The four-axis AXYZ setup is the most common one.
The premium for fourth axis starts at around $100 for manual indexers (a precision rotary chuck that holds the workpiece, but where the angle needs to be dialed in manually); and from $500-$1,000 for computer controlled units.
What to buy: 99% of your moldmaking work will not appreciably benefit from a fourth axis, so three axes are perfectly fine. You may want to get a mill where fourth axis is an option, though, especially if you are also planning to do artistic work.
Greater X-Y-Z tool movement ranges translate to the ability to make larger parts in a single pass. It's important to pick a mill that won't get in the way of your imagination - but to make this call, you need to calibrate your expectations sensibly.
As an extreme example, let's consider building a man-sized biped robot. You don't need a man-sized mill for that job - for at least three reasons:
Although the entire project would be obviously pretty big, virtually all the individual parts should be much smaller. In fact, most of the components will likely fall into the range of 1 to 30 cm.
Any oversized part can be broken into sequentially machined segments. If you are using the resin casting process, this scales up almost arbitrarily; in other types of work, you will see some (usually modest) constraints.
Many large and simple elements do not have to be machined at all; for example, it would be sensible to make the frame out of pipes or metal rods sawed to the desired length, and then simply machine custom connectors and joints that hold the frame together.
What to buy: do your own math. In my experience, about 15 x 10 cm in the X-Y plane is a good starting point, and about 30 x 20 cm will accommodate almost any medium-size robotic job. In the Z axis, you will probably not need more than 4 cm or so; and going over 8 cm is usually pointless. Whatever you do, do not confuse movement ranges with table dimensions, though.
Spindle - the part that connects the motor and the rotating tool - has a profound impact on the accuracy of any CNC mill. Its role is to ensure that the rotation of the tool is highly concentric and vibration-free, and that it stays this way under load. If the whole rig is not perfectly centered, you may end up with a situation such as this:
The total amount of back-and-forth wobble - in other words, the difference between the intended and effective diameter of the tool - is known as total indicated runout, or TIR. High TIR will not only affect the dimensional accuracy of machined parts, but will also ruin surface finish, and prematurely wear the tool. In fact, the effect is pretty dramatic: in some materials, eccentricity of 0.01 mm can reduce tool life by 50%.
Proper CNC spindles are usually long, round or rectangular blocks of metal with precision ball bearings mounted on both ends (and often pre-tensioned with a spring). Inside, there is a heavy-duty rotating shaft that couples the motor belt drive system to the tool holder. With quality spindles, TIR usually can be kept below 2 µm.
Some of the low-end manufacturers don't bother with a proper spindle, however; the most common example of this are CNC mills that use repurposed manual rotary tools. These cases are a bit of a gamble: some of them may have still somewhat bearable TIR in the vicinity of 0.01 mm - but some will be as bad as 0.10 mm, which makes them completely useless for precision work. Runout aside, you also can't be sure if the tool is perfectly aligned with the Z axis or not; if it isn't, that opens a yet another can of worms.
Note: to put all these numbers in perspective, 0.10 mm is roughly the diameter of a human hair; level differences of this magnitude can be easily felt when sliding your finger across a hard surface. Notches down to about 0.05 mm can be easily seen on smooth but matte finishes - and on glossy surfaces, the threshold may be closer to 0.01 mm or so.
What to buy: try to avoid CNC mills without real spindles; if you need to get one, ask the manufacturer about TIR. If they are not sure, it's an obvious red flag: the parameter can be trivially measured with a $50 tool, and is one of the most rudimentary things to examine when designing a mill. Note that there are aftermarket spindles that can be fitted into certain mills, though!
There are many factors that contribute to the real-world precision of a CNC mill, but one of the most important aspects is repeat accuracy: the ability to return to the same position over and over again. Along with spindle characteristics, this quality has a tremendous impact on surface finish, and on the dimensional accuracy of small parts.
Repeat accuracy is affected chiefly by two things:
Backlash: many types of transmissions will have some amount of play, which often leads to imperfections in positioning. This play tends to be greater in CNC mills that use stepper motors or acme screw drives; and lower with servo motors and ball screws.
Mill rigidity: machines that use low-cost materials (HDPE, plywood, sheet metal) to hold everything together, rely on rudimentary slides to support the moving parts, or use timing belts as a motion system, will deflect more significantly under load, or in response to own acceleration and deceleration. This problem is much less pronounced in mills with heavy-duty cast frames and ball-bearing linear ways.
Unfortunately, there is no widely accepted standard for testing repeat accuracy; many manufacturers don't bother to advertise it, and others test it with varying levels of honesty. In fact, the good guys will give you a figure that represents the worst-case, momentary deviation following a rapid long-distance movement - but that's not really representative of most types of fine work with sub-millimeter tools.
Now, don't despair: the good news is that most of the commercially available mills are actually pretty good in this department, especially when moving slower and doing precision cuts in easily machinable stock. You can expect many entry-level mills to conduct themselves within 0.02 mm or better during normal work; more expensive units with ball screws and servo motors will probably stay around 2-5 µm.
Accuracy aside, mechanical resolution is the other important piece of the puzzle. Stepper or servo motors in a CNC mill can assume only a certain number of positions per turn, and that translates to a specific minimum distance by which the table or the cutting head can be moved around. Insufficient mechanical resolution means that the mill will have difficulty smoothly approximating certain curves, and may end up producing unattractive finish.
What to buy: The basic rule is that you should not expect a plywood-based contraption with acme screws to reach 1 µm repeat accuracy. If the manufacturer advertises an improbable value, ask them to explain. If they advertise a suspiciously high figure (over 0.1 mm or so), be wary, too. As for the mechanical resolution: look for 5 µm or better.
Time is money. When it comes to CNC machining, the time needed to complete a job is to a surprising extent dependent on your skill and the capabilities of your software - but with a skilled operator and good toolpath decisions, the final part of the equation is always the performance of the mill itself.
To understand how the mill's performance is tied to the numbers you see in the datasheet, it is helpful to look at the geometry of a typical end mill. Upon closer inspection, the tool closely resembles a drill: it consists of a round shaft with several blades (flutes) wrapped around it in a spiral fashion. As opposed to a drill, however, these flutes have a sharp, exposed edge running along their entire length; this is because the bulk of their work is meant to be done by moving sideways. This is how it looks from the top:
Even in the most easily machinable material imaginable, the cutter is able to scoop away only a certain amount of swarf per turn - just enough to fit under the flute. If you exceed that capacity, you will end up dragging a clogged, non-cutting tool across the workpiece - which ends with one or the other eventually giving up.
For every material and cutter geometry, there is an optimal ratio of linear speed and cutter RPM that leads to efficient, high-quality machining. This is often expressed as feed per tooth. In plastics, the ideal values are:
Up to 0.1-0.2 mm for larger tools used to do the bulk of material removal in every cutting job. These tools frequently have four flutes, so this translates to 0.4-0.8 mm per turn.
Down to 0.01 mm or less for sub-miniature, 2-flute cutters used to reproduce minutiae detail (0.02 mm per turn).
In practical terms, it's healthy to aim for mills where the ratio between maximum movement speed (mm/min) and maximum RPM hovers around 0.4 to 0.8 for optimum performance during rough cutting. At the same time, there is also some value in shopping for the highest maximum RPM you can get - as it lets you move faster during the precision finishing steps.
Of course, there are some gotchas:
Very high spindle speeds tend to be problematic; going over 25,000 RPM or so may cause problems with heat dissipation, tool oscillation, and so on.
High traverse speed can help even without high RPM. This is because certain types of cutting jobs involve a fair amount of rapid, non-cutting movements between various locations to be machined. Good CAM applications should know to avoid excess travel, but not all CAM applications are very good.
Acceleration matters. Fast-moving mills need to be good at accelerating and braking to fully utilize their capabilities during series of short, stop-and-go movements that are often involved in CNC work. Rates of at least 0.1 G (~1 m/s²) are desirable in any mill capable of four-digit speeds.
What to buy: at least 6,000 RPM is nice; and if the aforementioned speed ratio is favorable, there are no real downsides to going up to 20,000 RPM. Maximum movement speed, in mm/min, should be ideally at least 6-10 times the movement range, so that it doesn't take more than several seconds to traverse the table.
Spare for some pathological situations, the mill is intrinsically aware of the position of its spindle at any given time; but the actual cutting action takes place beneath the spindle - at a distance dictated by how far the tool sticks out from its holder.
And here lies the problem: most toolholding systems do not allow you to precisely preset tool extension length, or to maintain it when you replace the cutter. If you switch the tool in the middle of a machining process, and don't compensate for the difference, the results will be off; in fact, the tool may unexpectedly hit an uncut area and break.
There are several manual tricks that can be used to work around this issue. One of them is to place a thin strip of paper or foil in a fixed reference location, and then slowly lower the tool until the strip gets caught between the cutter and whatever happens to be underneath. By comparing the Z position of the spindle at that point with the reading obtained for the previous tool, the appropriate offset can be calculated and communicated to the machine. But of course, this technique is somewhat inconvenient, and accurate only to perhaps 0.05 mm.
A better approach is to incorporate a tool height sensor into the mill. The sensor is typically just a flat block of precisely machined soft metal; the mill automatically lowers the tool onto the sensor until contact is made - which, in the simplest design, is detected by noticing the flow of current between the probe and spindle body. The accuracy of this approach is often better than 0.01 mm.
What to buy: try to find a mill that has a built-in sensor, or can be equipped with one. Failing this, you can always rig a manual tester that uses the same operating principle, and simply illuminates a LED.
The spindle must be terminated with some sort of a tool holding device. There are several common systems that you will bump into when shopping around:
Jaw chuck: this is the design familiar from drills and other hand tools. These devices tend to offer poor concentricity (TIR can be as high as 0.1 mm) and should be avoided if possible.
Fixed diameter chuck: essentially a metal sleeve with its inner diameter matching the size of the tool. It is operated with a set screw or with heat (shrink-fit). It's pretty accurate, but can make tool changes costly or cumbersome. For example, in Roland MDX-15, you have to replace the entire spindle assembly to switch between two different diameters of the shank.
R8 collets: these are popular in the States, cheap, easy to use - but because of the way they grip the tool, they usually have relatively poor TIR (0.01 to 0.02 mm). That's a bit high for comfort.
Morse taper (MT3) collets: a superior alternative to R8, typically with TIR below 5 µm.
ER collets: probably the best option for small CNC mills. These collets can accommodate a wider range of tool shanks, and the "ultra-precision" variety from reputable manufacturers tend to have TIR under 2 µm.
What to buy: If you can get ER16 or MT3, go for it. Otherwise, just make sure that the toolholding system is versatile enough to accommodate common shank sizes (3, 4, and 6 mm for metric cutters; 1/8" and 1/4" for imperial system tools), and will be sufficiently precise for your needs.
Manually programming your CNC machine is about as much fun as building a steamboat out of toothpicks.
For a higher-level approach, you need to turn to
it automatically analyzes the provided geometry (created with any 3D modelling application) and converts
it to a set of paths that need to be retraced by the tool to approximate the desired shape. Once these
toolpaths are ready, the software then breaks them down into a sequence of painfully basic instructions
that actually make sense to the controller embedded in the mill; say,
"set speed to 12,000 RPM" or
"move cutter to X = 10.245, Y = 5.000, Z = -2.000".
The toolpath generation stage is largely hardware-agnostic; but the program generation one isn't. It's good to shop for a machine that speaks a common and well-documented language - or, lacking this, is popular enough to be supported by some of the best-known CAM apps. Keep in mind that even if the manufacturer bundles the mill with some starter software, you don't want to be left out in the cold if the application one day refuses to work with your new PC - or if it simply turns out to be of poor quality.
The most common quasi-standard language used by almost all CNC mills is called G-code (aka "NC"). Calling it a real standard may be a stretch: there are very significant variations in how the syntax is implemented by the manufacturers. Still, having support for G-code spells rudimentary compatibility, or at least easy integration, with almost any CAM application on the market. For other languages, this is not always given.
What to buy: check if the mill is supported by common third-party packages (Deskproto, VisualMILL, madCAM, MeshCAM, Mayka, etc); if it's not, and if it speaks something else than a clearly documented variant of G-code, be wary.
We're almost done: the last thing to do is a quick reality check. Benchtop mills span from units no larger than an inkjet printer, to ones weighing in excess of 200 kg and taking up almost 1 x 1 m of desk space. When shopping for the larger models, be sure to account for their physical characteristics, and make sure you have a way to get them in your workshop to begin with (some doors are barely 70 cm wide).
For heavier mills, it is also important to have a piece of sturdy furniture; it's not just the static load that you have to worry about, as the machine may also produce horizontal shear forces due to acceleration and deceleration of the cutting head. Not every wobbly desk from Ikea can handle that - but any proper workbench should.
Benchtop mills usually run on standard, single-phase 110 / 230 VAC power supply, but of course, make sure to double-check. They may require several amps in peak, so you don't want them to share a single circuit with a vacuum cleaner, an electric kettle, or a space heater - especially in an older home.
Okay - that sums up the list of parameters that are worth looking at. There are also some characteristics that sound important, but usually aren't - so to help you decide, here's a quick list to consult when in doubt:
Positioning accuracy: this value tells you how true the machine's idea of a millimeter is to a calibrated reference. The difference is usually negligible, and even if it wasn't, you can compensate in software without any special effort.
Origin reproducibility: this indicates how good the machine is about resuming the same starting location after being power cycled. Not particularly important in normal work, unless your power goes out in the middle of a cutting job.
Software resolution: unlikely to be lower than mechanical resolution, and fairly meaningless if it's higher.
Motor power: spindle motors delivering as little as 75-100 W should be perfectly sufficient for the processes advocated in this guide. More powerful mills are beneficial chiefly in heavy-duty metal work.
Table size: easy to confuse with the actual machinable area, but nowhere near as important. The difference between a 2 cm margin and a 10 cm one usually doesn't matter at all.
List of millable materials: every mill should be able to cope with a wide variety of materials; don't read too much into the list provided by the manufacturer. The only real difference is that some units are not rigid or powerful enough to handle steel. (Some people insist that smaller and less rigid machines that can't machine steel should be called "CNC routers" and not "CNC mills", but this is not a particularly well-established practice, and other definitions exist.)
Tool changer (ATC): it's a convenient device for unattended factory jobs, but an expensive and unnecessary gimmick in hobby work.
Contact scanner accessory: contact scanning heads are a gadget available for some CNC mills, but chances are, you will use them to scan a couple of coins or pendants, and then lose all interest. For reverse engineering of mecanical designs, just using a caliper works a lot better, and takes less time.
Noise ratings: probably not what you think. These parameters describe the noise produced by the mill when in standby mode (spindle off); or when operating, but not making contact with a workpiece. Benchtop mills are fairly quiet in no-load conditions; and even the most compact and underpowered devices can be pretty loud when actually machining something.
The actual noise level will range from barely perceptible when working in waxes or using sub-mm cutters, to pretty unpleasant when rapidly plowing through metal with a large-diameter tool. In fact, just imagine the noise made by a saw or a drill.
Well, that's probably it. If you spot any other puzzling parameters, please let me know.
That really depends on your budget and the scale of the projects you want to be working on. Here is a list of some of the fairly popular, inexpensive mills, along with their catalog prices. Many of them sell for around 15% less if you talk to the right distributor:
Chinese "3020" mill - around $500.
Roland iModela - $900 (no longer available in the US?).
Probotix FireBall V90 + several options - $1,300.
MAXNC-10 - $1,600.
Deepgroove1 CNC mill - $1,700.
Sherline 5400 + CNC package - $1,800.
Taig 2026ER - $2,300.
Nomad 883 - $2,500 (preorder, looks very promising).
MicroMill DSLS 3000 - $3,000.
Flashcut 2000 - $3,000.
Roland MDX-15 - $3,400 (discontinued, replaced by SRM-20).
LittleMachineShop 3501 - $4,900.
Roland SRM-20 - $4,900.
Syil X4 - $5,800.
A good place to search for user opinions is CNCzone.com. Good luck!
Ordering a CNC machine? Well, the next stop is getting some cutters. The selection available on the market is quite overwhelming, so to save you time and money, let's talk about some of the properties that set these tools apart. Oh, before we dive in... here's a drawing of a typical end mill, and all the lingo you will have to memorize soon:
All right - so here are the differences you will see:
Material: end mills are made either out of cobalt steel alloys (known as high speed steel, or HSS), or from tungsten carbide in a cobalt lattice (colloquially shortened to "carbide"). The latter option is considerably harder, more rigid, and more wear-resistant - and for the tool sizes we are interested in, carries a relatively small premium (30% or so).
What to buy: Stick to carbide.
Coatings: carbide cutters may be further coated with ceramics such as titanium aluminum nitride (TiAlN, aka AlTiN), titanium nitride (TiN), titanium carbon nitride (TiCN), or with amorphous or crystalline diamond. The coatings tend to improve hardness or reduce friction; the bluish-gray TiAlN coating is probably the most common one. In non-abrasive plastics, this particular coating doesn't have a very pronounced effect, but it extends tool life by some 20% or so - and the cost is only 10% extra, so it's not a bad deal.
Of course, in some situations, tool wear is a more pronounced concern; for example, glass or carbon fiber composites can leave a mark on carbide tools in a matter of hours. In the same vein, in ultra-precise micromachining, you may have to worry even about early-stage wear, because it can subtly affect the dimensions of the tool. In such cases, amorphous "diamond" coatings offer more definite benefits compared to TiAlN, often extending tool life by a factor of 2-3x. Alas, the coating at a 30%-40% premium and is available only for some tools. (True, crystalline diamond works, too, but costs a lot more and is reserved for more demanding jobs.)
What to buy: If you're on a tight budget, skip any coatings and pocket the change. Otherwise, TiAlN or amorphous diamond is probably not a complete waste of money, although you can still skip it on your first set of "training wheel" tools. Stay clear of more pricey coatings: crystalline diamond will probably never pay for itself in our work.
Tip geometry: precision machining operations in plastics will almost always rely on "vanilla", single-end finishing tools with no chip-breaking ridges, no taper, no coolant outlets, and so forth. The tips of these standard tools come in three basic flavors:
Flat tip cutters are the primary tool in all sorts of mechanical work. Ball nose cutters come handy when you need to reproduce gentle slopes and other organic designs. And lastly, corner radius cutters offer a compromise design that combines 90° arcs in the corners, and a flat mid-section - but you can safely ignore them until you have a specific itch to scratch. About the only other type of a cutter worth mentioning here are conical engraving cutters, which look like this; these are useful for making very fine but shallow cuts, for example when machining traces on a PCB.
What to buy: build a competent collection of flat tip cutters first. If you want to experiment, grab one or two ball nose cutters, but you probably won't be using them that much in non-artistic work.
Cutting diameter: end mills come in cutting diameters from 0.01 mm (a lot thinner than human hair) to 50 mm and more. For most intents and purposes, cutters below 0.25 mm or so are just not very useful, unless you are doing some truly hardcore micromachining; and over 8 mm or so, they get too big to mount and meaningfully use on benchtop mills.
Your cutters need to strike a sensible balance: large tools can't machine tiny features, but small tools remove very little material in every pass, making them useful mostly for selective refinishing work. In fact, a two-fold reduction in tool cutting diameter often translates to a 10-fold reduction in effective material removal speed!
What to buy: try to get a 3 mm (or 1/8") cutter to handle most of the machining work; for large projects, 6 mm (or 1/4") may come handy, too. On top of that, keep 0.4 mm and 1 mm cutters for touching up fine details.
Cutting diameter tolerance (tricky!): "1 mm" cutters don't always have a diameter of 1 mm. In a nod to the legacy of drilling and tapping applications, many manufacturers make their tools to non-symmetric tolerances, as denoted either with a pair of explicit values (say, +0.00 / -0.04 mm), or with an ISO tolerance code such as "e8".
Of course, modern tool grinding machines are often a lot more precise than that; micron accuracy is not unheard of. The machine is therefore preset to simply crank out tools at the mid-point of the specified range. Using the example of a 1 mm tool specified as +0.00 / -0.04 mm, the actual diameter will end up being 0.98 mm or so. In most uses, you won't even notice - but then, every now and then, such a subtle difference can bite back.
Okay, so the case of explicit tolerances is pretty clear; as for the "e8" case: for cutters with diameters below or equal to 3 mm, the offset is -0.021 mm. For cutters over 3 mm and up to 6 mm, the difference is -0.029 mm.
What to buy: whatever you want, just make sure to double-check the tolerance, and write down the actual diameter of the tool. Also, if the vendor declares a suspiciously sloppy tolerance, approach such tools with caution, and perhaps ask the company if they mean it.
Shank diameter: this is the diameter of the top portion of the end mill - the one that goes into the holder. It has no significant effect on the cutting process, so you simply need to make sure that you have a matching collet for all the tools you intend to buy.
Cutting length: the cutter will have flutes extending only through some of its length. The height of the cutting region sets the upper limit of how deep the tool can be driven into the workpiece in a single pass.
What to buy: for the processes outlined here, you typically only need the flutes to extend to a distance equal to about 50% of tool diameter. Because the flute-bearing section somewhat more vulnerable than the rest of the end mill, and may also be subject to uneven wear, it's actually beneficial to opt for stub-flute tools when you have a choice.
Reach length: many end mills have a neck - a section between the flutes and the shank, across which the diameter of the tool does not exceed that of the cutting tip (and in most cases, is about 10% percent smaller). The distance from the tip of the tool to the end of this section puts an absolute limit on the depth of machining near any vertical walls:
As you can see in the rightmost drawing, the problem can be avoided by introducing a non-zero draft angle: a subtle slant on any tall, vertical walls. Draft angles also help with removing cured parts from rigid molds - but are not always desirable or practical. That's why having a tool with a decent reach length is still a good plan.
On the flip side, more is not always better: with miniature long-reach tools, as the neck gets longer, the cutter becomes more prone to deflection and easier to break. A 1 mm tool with a 3 mm reach can be operated with few worries; at 10 mm, you need to be a bit more careful; and at 30 mm, it starts to require ninja skills.
Oh, of course, some tools don't have a neck to speak of; in these cases, there is a taper that immediately follows the flutes, and reach length is identical to cutting length. That may be good or bad, depending on whether flute length is sufficient for your needs.
Note: there is an interesting special case - some 3 mm or 6 mm tools have shank diameter identical to their nominal cutting diameter; the same goes for their imperial 1/8" and 1/4" counterparts. You can think of them as having reach length equal to total tool length, minus about 20 mm needed for the collet.
There are some drawbacks of driving these tools deeper than their cutting length, though: their pretend "neck" doesn't have a reduced diameter, so when dealing with zero draft angles, it may end up rubbing against the workpiece. This usually has no effect in prototyping plastics, but quickly becomes a problem in metals and other tough stuff.
The situation gets slightly worse if the actual cutting diameter is smaller than the nominal one, due to non-symmetric tolerances. In these cases, driving such a tool too deep may have a minor but noticable impact on dimensional accuracy or surface finish.
What to buy: moldmaking often involves relatively deep cuts and vertical walls. Make sure that your 3 mm tools have a reach of at least 20-30 mm; for 1 mm, stick closer to 10 mm; and for 0.4 mm, 2-4 mm should do the trick.
Overall length (OAL): self-explanatory. Typical mold cutters have lengths of about 50 to 75 mm; some lower cost or subminiature tools may be available as 38 mm, too. Longer end mills - up to 150 mm or so - are also available, but seldom worth the price.
The main significance of this parameter is that the tool will stick out of the spindle by no more than OAL, less something around 15 mm for the part that needs to be gripped by the collet. Life gets more complicated when the collet nut and the rest of the spindle gets in the vicinity of the workpiece, so it's preferable to have tools long enough to deal with the typical depth of the molds you are planning to work on.
What to buy: if your projects will be anything like mine, your molds will probably range from about 6 to 22 mm in depth, with infrequent excursions down to 40 mm or so. If so, OAL of 50-75 mm is a good pick.
Number of flutes: higher flute count translates to faster material removal rates and superior finish, because there are more cutting passes per every turn of the spindle. Unfortunately, there are modest limits to how many sufficiently robust flutes you can cram onto a small cutter, and still have enough room for swarf; 4 flutes are the common limit, although 6 are not unheard of.
What to buy: for the materials we will be using for moldmaking, the more flutes, the better; at least three or four are strongly desirable on 3 mm cutters, and nice to have on smaller tools. For aluminum, rubbers, and malleable plastics, one or two flutes may be a better pick.
Helix angle: zero degree flutes are perfectly straight, and run vertically along the tool. The industry standard is 30°, which offers a sensible balance between edge sharpness, vibration, and swarf removal speed. Lower angles are used to rapidly engage and remove softer materials (e.g., rubbers, thermoplastics); while higher angles improve tool life and reduce vibration in hard materials.
What to buy: there is virtually no difference between 15, 30, 45, and 60° when working with easily machinable plastics; you can safely disregard this parameter, and just focus on finding the most interesting and the most affordable tool.
Center cutting ability: almost all the cutters of interest to CNC work have a bottom flute that extends through the entire diameter of the tool - which allows it to be plunged straight down into the workpiece, and effectively act as a somewhat competent drill. But a small minority of end mills are not center-cutting, and can't be operated this way. You probably don't want that.
What to buy: avoid non-center-cutting tools.
Phew! My favorite tool manufacturer is Hanita (now a division of Kennametal, confusingly sold under the brand name of WIDIA): they have an unmatched selection of metric tools at reasonable prices, and are available all over the world. If you are in the States, Sierra Tool is a good reseller; Centerline Industrial is a bit cheaper, but for some reason, refuses to ship to residential addresses. And if you are anywhere in Europe, I can strongly recommend ordering Hanita products with ITC.
Hanita aside, Harvey Tool has a very interesting selection of imperial system miniature tools in the US - and I found K&H Sales to be a dependable distributor. Other US manufacturers include OSG Tap & Die, Monster Tool, Micro100, and Microcut, but their catalogs are not as impressive. Readers in the EU may want to check out Nachreiner.
Here are the catalogs of the three most interesting manufacturers:
Hanita: full end mill range (most are "e8").
Harvey Tool: all tools (some have non-symmetrical tolerances).
As for practical recommendations, I would suggest starting with Hanita 401403000, 402403000, or Harvey 73118-C4, as the baseline "3 mm" cutter ($15-$30); Hanita 7N2201021 or Harvey 76440-C3 for 1 mm work ($30-35); and Hanita 7N2200410 or Harvey 992515-C3 as a long-reach ~0.4 mm tool ($35). If you are not on a very tight budget, it makes sense to order two of each - it's easy to mess something up in the heat of initial experimentation.
With the tools selected, you also need to make sure you have the right set of collets. For ER16, if you are not desperate to save a few bucks, try Rego-Fix "UP" (ultra-precision) collets; they retail for about $45 a pop, and are carried by K&H; another good option are "DNA" collets from Techniks (about $30, require a custom nut). You can find lower-cost collets from many other, more obscure brands - but they are not always particularly good.
Oh, one more thing: for ER16, every collet has a specified clamping range - for example, 3.00-2.00 mm. It is always preferable to use the upper value: a 3.00-2.00 mm collet is better than a 4.00-3.00 one when holding a 3 mm tool.
Before embracing any complex or high-precision projects, it is important to understand the performance of your mill, and see if anything needs to be fixed, adjusted, or compensated for. While CNC mills don't require constant tuning, making several simple measurements after unpacking the device can save you a lot of time. If you neglect this step, you will find that troubleshooting mill accuracy issues in complex, real-world projects tends to be a daunting task, simply due to the sheer number of variables to look at.
The essential tool that you will need to perform the initial measurements is a micron-resolution dial indicator with a magnetic base. You can get a no-name unit on eBay for about $50 (link), or go with Mitutoyo or other reputable brand for about $220 (indicator, base). For lower-cost mills with a rotary tool acting as a spindle, you may be better served by a 0.01 mm indicator, though; in this case, you can get a Mitutoyo one for about $80 (link, base not included).
The first thing to check is the runout of the spindle and the tool holder. Wipe clean the internal spindle taper and the collet (use WD-40 if there is any excess grease or other accummulated dirt; a small brass brush works well for any stubborn gunk), and install a tool that extends at least about 20-30 mm from the collet. Tighten until you feel definite resistance, but don't overdo it - excess force may deform the collet, and is not essential in lightweight work.
Next, affix the dial indicator to the table or other sturdy surface, make the tip of the indicator touch the tool near the spindle, and observe the change in readings as you gently turn the spindle by hand, preferably at the top (the mill should be turned off, of course). Be very careful not to exert any unnecessary pressure on any of the parts.
Let's call the result of this measurement
Rcollet. Move the indicator about 10 mm lower (stay clear of the flutes) and
repeat the test; we'll refer to it as
Rmiddle. Finally, if possible, remove the tool and the collet,
and reposition the indicator to make contact with the internal taper of the spindle (the measuring tip now pointing up).
Repeat the procedure, and write down the result -
Rtaper. Here's how to interpret the data:
Rtaper: this measurement tells you about the concentricity of the spindle itself. If it is excessive, it may be time to service the spindle (e.g., adjust the internal tension spring; disassemble it and install a new pair of precision bearings; or, insert a shim somewhere to fine-tune the concentricity).
Rcollet: if the spindle measurement looks OK (and only then!), this value helps you estimate the
eccentricity contributed by the tool holder (on top of
Rtaper). If the value is high, examine the collet for
dirt and damage (again, WD-40 is a pretty good cleaning liquid). Small tool holder misalignment can be often "fixed" simply by
adjusting the tightening torque, or applying a gentle pressure to the appropriate side of the tool when tightening the nut.
If that doesn't help, replacing the collet - perhaps with a higher-quality model - may be the way to go.
Rmiddle: this value lets you estimate the eccentricity at the tip of the tool, which ultimately, is
the most important observation to make.
You can see if the TIR is increasing, decreasing, or staying about the same in relation to
- and use that to extrapolate the apparent diameter of the tip.
For a quality machine with a dedicated spindle and ultra-precision ER16 collects, after some adjustments, TIR should preferably stay within 2 µm or so; and for any mill, it is good to have runout within 0.01 mm. If you are seeing something much worse, poke around and see if you can improve it: it's usually simpler than it may seem. For example, the factory spindle that came with my MDX-540 mill had a TIR of about 6 µm; using a hook spanner to adjust the tension of the internal spring by one tenth of a turn reduced the value to 1 µm. In more complex cases, switching around or rearranging the existing bearings inside the spindle, or replacing them with new ones, will often do the trick.
Tip: try to quickly repeat the
Rcollet measurement after
every tool change, even if you are not doing high-precision work. Trapped dirt will affect the concentricity
of the tool holder, and even a tiny difference can easily reduce tool life by 50%, and increase cutting noise
by more than that.
Spindle eccentricity aside, it is also useful to verify that the tool is truly perpendicular to the X-Y plane; if that's not the case, for example because one of the screws that attach the spindle to the rest of the mill is not tightened to the same torque, you may see somewhat perplexing dimensional errors in machined parts.
The test you should perform is exceedingly simple: you need to mount a cutter that offers at least around 2-3 cm of clearance between the collet and the flutes; programmatically lower the spindle by 2 cm or so; and set up the dial indicator as shown on the previous drawing, in section 2.3.1. When done, gently rotate the tool to find the mid-point of its TIR, and then programmatically move the spindle up by about 1 cm. The same procedure should be repeated after repositioning the dial indicator to make contact with the side of the tool (rather than the front).
If everything is fine, you should see no appreciable change in the values shown by the dial indicator; a few microns may be fine, but if the difference is getting close to 0.01 mm, you should definitely investigate. The issue is almost always trivial to fix: you may need to loosen the screws that hold the spindle in place, and perhaps insert a shim made out of aluminum foil on the offending side to straighten it out.
Caution: before operating the mill, be sure to read the safety tips provided by the manufacturer, as well as the advice included in section 7 of this guide. Small CNC machines are not particularly deadly power tools, but they are still power tools - and it's your responsibility to use them safely.
The spindle assembly is typically fairly heavy, and under normal operating conditions, will be rotating rapidly. At these speeds, any poorly balanced rotating part, any malfunctioning ball bearing, and any damaged transmission belt may easily introduce significant vibration - and that vibration will inevitably propagate to the end mill or the workpiece.
It is difficult to accurately measure high-frequency vibration without the help of specialized tools, but this shouldn't stop you from performing two rudimentary checks. Try this:
Attach your dial indicator to the table or other part of the mill frame, and let the tip touch any non-rotating part of the spindle. Run the spindle at several different speeds, and observe the reading; oscillation of the indicator hand, if any, should stay well under 1 µm.
Remove the tool, grab a long screwdriver, and carefully touch any non-rotating part of the spindle with its tip. Be vigilant, and keep your body and the screwdriver itself well clear of any moving parts. When the tool is touching the spindle, you shouldn't be able to hear any ringing noise, or sense any appreciable vibration in the palm of your hand.
If any of these tests reveals excessive vibration, the first thing to do is disenage the motor from the spindle (there's usually a belt or some sort of a clutch involved); if the problem doesn't go away, you know that the problem is with the motor itself, in which case, it may be useful to have it serviced or replaced. If the spindle is to blame, replacing the internal bearings would be the obvious next step.
Whatever the cause is, fixes shouldn't be too expensive, but pinpointing the issue may take a while.
Repeat accuracy is the single most important factor limiting the precision of the parts you can make. Even if you are not planning to machine anything particularly intricate, this parameter is still worth checking: if it's alarmingly poor, it may be indicative of a problem with the mill.
To estimate the accuracy of the machine, brace the tip of the dial indicator against the side of the spindle assembly, and then programmatically move the spindle away in the X axis, in 0.01 mm increments (or whatever the nearest multiple of your mill's mechanical resolution is supposed to be). After about 5-10 steps or so, reverse the direction, and gradually move back to the starting point. Here's what to look for:
Every step should move the needle of the dial indicator by the same amount, ideally within 1 µm, and definitely within 0.01 mm. Jerky stepping may be due the increments not being a multiple of the actual hardware resolution of the mill, or due to wiring problems in the stepper motor.
The actual travel distance, as measured by the dial indicator, should match the expected distance closely. If there's any substantial error that seem to be proportional to how far you are moving, your CNC software should let you compensate.
The locations of the steps when moving away from the dial indicator should be the same as when moving back; and the spindle should return to the same starting position at the end of the test. Any observable offset is probably due to backlash - which should be in the micron range. There may be some limited ability to compensate for this in software (for example, your CNC application may offer low-level motor calibration settings), but it's not a silver bullet.
Of course, try to repeat this procedure for all axes. If in any of them, repeat accuracy is worse than 0.01 mm, it may be good to talk to the manufacturer.
We're almost done! The last parameter of note is the loss of accuracy you can expect if the mill is braking or accelerating rapidly, or aggressively plowing through a difficult workpiece. The value depends on the rigidity of mill frame, and the type and quality of its linear motion systems. If it's poor, there is no reason to despair - but it means that you may have to slow down when doing precision work.
The test here is extremely simple: with the mill on but the spindle turned off, brace the dial indicator against the side of the cutting head, and then use your hand to gently press the spindle from the other side - along the tested axis. Don't overdo it: the goal is to exert may be 20-50 g of force, and not to overcome the holding torque of the motors.
In a quality mill, the momentary deflection should stay under 5 µm or so - but up to 0.02 mm is something you can live with.
Once you know that your machine is behaving correctly, there isn't that much that needs to be done on an ongoing basis: it's a pretty sturdy piece of machinery, and it's usually not subject to heavy wear. Consult the manual for manufacturer-specific advice - but in most cases, the rules are pretty simple:
Always keep the collets, cutters, and the spindle taper squeaky clean and lightly lubricated. Get rid of any thick, factory-applied grease (use WD-40 or naphtha to do that); carefully remove all cutting residues (use a small brass brush for any stubborn bits); and apply WD-40 or a similar low-viscosity oil to protect all these components against corrossion - especially after handling them with bare hands. Sweat residue can quickly lead to corrosion!
Thoroughly vacuum the mill after every job. Cuttings, if allowed to pile on, may eventually make their way into the sensitive, normally shielded parts of the drivetrain - or more prosaically, may simply obstruct the movement of the table. Do not use compressed air for cleaning, as this can push dirt deeper into the machine, or just spread it around your workshop unnecessarily.
Every few hundred hours of machining (1-2 years' worth of weekend projects), wipe old grease and dirt off of ball screws and linear guides, and apply a fresh coat. Medium-viscosity lithium grease is typically the right choice - but check the manual carefully, and whatever you do, avoid mixing lubricants of different kinds.
After several thousand hours of use (5+ years), it may be time to inspect the spindle assembly for any obvious wear, loss of concentricity, noise, vibration, or elevated operating temperature - and service it as necessary. If you do it yourself, the replacement of spindle bearings should cost between $40 and $300, depending on the design.
Some of the entry-level mills may be using low-cost brushed motors to power the spindle; such motors are a consumable, and may require a replacement after anywhere from 100 to 2,000 hours - but typically don't cost much. Higher end machines usually rely on brushless motors that should last a decade or more.
Linear drivetrain motors, bearings, and so on are typically not subject to substantial wear when doing lightweight hobbyist work; if properly maintained, they should last pretty much forever. Insufficient lubrication or contamination with abrasive materials (ferrous metals, glass, etc) are about the only things to watch out for.
If you are planning to do high-precision work, or simply wish to ensure high-quality surface finish when working with organic shapes, it's useful to measure and document the diameter of every new end mill in your collection. Although the tools are usually manufactured with micron-level accuracy, the specifications can sometimes be wrong, and on top of that, manufacturing variations may occur from batch to batch - for example, due to changes in the thickness of applied coatings or the gradual wear of the grinding tool. Case in point: some of my Harvey's 0.04 inch cutters actually measure around 1.022 mm, rather than the expected 1.016 mm. At these scales, such differences can bite.
To perform the measurements, you will need an accurate micrometer. This tool, along with quality calipers, is one of the most important investments you will make, so don't fret: $50 will get you a decent no-name brand, while $140 is enough for Mitutoyo. For two- or four-flute tools, the idea is to gently tighten the jaws of the micrometer around the flutes, while simultaneously rotating the cutter (in the direction opposite to its normal operation) to find the maximum diameter. You need to stop as soon as you feel any resistance, to avoid breaking the tool or gouging the jaws; practice on larger, sturdy end mills before moving on to sub-mm ones.
Three-flute tools are a bit harder to deal with. If the flutes are long enough, you may be able to grip the cutter so that one face of the micrometer is touching the peak points of two flutes, and the opposite face is touching the remaining one. That said, with stub-length tools, you may be essentially out of luck; doing a careful test cut and measuring the result may be the way to go (you need to account for TIR and repeat accuracy).
Beyond the initial measurements, it is also a good habit to re-check your tools after every 10 hours of cutting or so, preferably measuring the diameter near the very tip. When doing heavy cutting, you may see some reduction in tool diameter as the outer edge of the flutes gets a bit more dull; for this reason, I suggest keeping your primary roughing tool separate from the finishing ones.
Tip: even when working with plastics, applying several drops of a cutting fluid to the workpiece can improve finish and limit tool wear by keeping the tool cool and helping remove chips more efficiently - give it a try! For lightweight work, sulfur-free oils, such as Oatey 30200, work best. They are also easy to clean up with a detergent and don't interfere with resin casting work.
Cutting fluids or no fluids, it makes sense to examine your tools for damage and excess wear every now and then. You can't trust your naked eye, but a simple 7x magnifier, selling for under $50, should do the trick. If you have a microscope with magnification between 10x and 50x, that's even better. Here are the two most common cutter failure modes that aren't visible with naked eye - significant wear (left) and a chipped flute (right):
Both of these tools will still work, but the one on the left will not hold tight dimensional tolerances in particularly demanding applications; while the one on the right will produce crummy finish in machined parts and will be prone to gumming up.
Tip: good bookkeeping is incredibly important in CNC work: computer-aided design and creative chaos simply don't mix. Cultivate good habits starting with end mills: make sure that you have a spreadsheet (or even a flat text file) listing all the tools you have, outlining their geometry, and making note of the measurements you have taken.Having such a list will not only help you avoid surprises, but will also make it easier to maintain a healthy stock of tools - so that you never have to put a project on hold for two weeks after accidentally breaking your last 0.4 mm end mill.
Click to proceed to chapter 3...