Guerrilla guide to CNC machining, mold making, and resin casting
Copyright (C) 2013, 2014, 2015, 2016 by Michal Zalewski (
Follow the author on Twitter: @lcamtuf
You are viewing chapter 2 of 8. Click this box for table of contents.

2. Setting up a CNC mill

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.

2.1. Picking the right machine

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.

2.1.1. Number of axes

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.

2.1.2. Mechanical movement ranges

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:

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.

2.1.3. Use of a specialized spindle

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!

2.1.4. Movement precision

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:

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.

2.1.5. Machining speeds

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:

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:

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.

2.1.6. Tool sensor support

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.

2.1.7. Tool mounting method

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:

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.

2.1.8. Availability of CAM software

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 CAM software: 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.

2.1.9. Size, weight, power needs

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.

2.1.10. And now, all the things you don't have to worry about

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:

Well, that's probably it. If you spot any other puzzling parameters, please let me know.

2.1.11. So, which one should I buy?!

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:

A good place to search for user opinions is Good luck!

2.2. Stocking up on end mills

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:

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:

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.

2.3. Periodic testing and troubleshooting

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).

2.3.1. Spindle TIR

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:

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.

2.3.2. Axial alignment of the tool

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.

2.3.3. Spindle vibration

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:

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.

2.3.4. Repeat accuracy

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:

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.

2.3.5. Deflection under load

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.

2.4. Ongoing maintenance

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:

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.

2.5. Cutter management

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...