Designing Machinable Parts

October 14, 2016


I first learned machining during my time on the high school robotics team, using typical wood shop tools (band saw, drill press). In college, I had access to a more serious shop (with mills, lathes, and CNC equipment) where I started on metalwork in earnest. Something about machining captivated me, and I would spend long hours at the shop working on increasingly more complicated parts. Yet more often than not, I would feel frustrated standing in front of the mill, waiting for the part to be done, and wishing it would not have required such a long, complex operation. My fascination with machining (and also a bit of stubbornness) got me through a few years of this, but now that the initial curiosity has worn off I am starting to see machining in a more pragmatic way, with a focus on attaining desired performance at minimized cost. The purpose of this article is to provide aspiring designers and engineers with an overview of an approach to improve designs for easier machining, and offer specific examples that show how this approach might be applied.

While it is nice in theory to have parts that are easy to machine, this sometimes does not happen because of practical impacts:

What I hope to convey in this article is that an awareness of machining requirements during the design phase is extremely valuable in reducing time and cost required to complete a project. This requires not only knowledge of different machine capabilities, tooling, and already-manufactured parts (which is provided in this article to an extent) but also an effort to keep asking 'why is this part designed this way?' and 'can it be made simpler and still serve the desired purpose?'. Still probably the toughest requirement is an emotional distancing from one's own designs so if they turn out to be sub-optimal there will not be hesitation to adapt a better design.

Machine Choice for Speed and Accuracy

In my experience both as student and instructor of milling, people start their work with a constant watch for precision. This is because the mill's digital readout displays up to 4 decimal points (in inches), for instance 1 inch is 1.0000, and for many students this is their first experience of physically controlling a machine with such precision. So when a drawing gives a dimension as 1 inch, they adjust the mill to read exactly 1.0000. And why not? It doesn't take much effort and it is better than having an improperly made part. Yet the thickness of a piece of paper is around 0.0020 inches - and being off by 0.0100 inches would only be noticeable in careful examination. Even more insidiously - it is likely that whatever served as the reference for the origin (0.0000) was not measured even within 0.0010 inches, and that in the process of the operation (drilling, milling) the tool deflects from the desired 1.0000 to something like 0.9900 (for instance with a long, 'wandering' drill bit).

The unfortunate conclusion is that unless you are in a precision machine shop, or perhaps have a CMM in regular use, your parts are much less accurate than you thought. It is possible that you already have evidence of this, for instance in poor press fits or misaligned bolt holes despite great care in machining. When the designer takes the practical requirements of accurate machining into account, the result is typically an easier to machine and more accurate part (you can definitely get both at once!). But in order to do this, the designer must be aware of the different possibilities for machining a part. This section will outline different machines and tools that can be used for part production. Methods of design optimization for these machines are considered further in the article.

Inverse Relation of Speed and Accuracy

My reason for mentioning the '1.0000' story above was so the reader might question the need for such accuracy. Physically, all assembled parts must fit together, but even the best machine shops cannot make parts perfectly flat or exactly the right size (in fact words like 'exact' and 'perfect' are a great indicator that one has not thought about actual tolerances required). If no dimensions exactly match, how can complex parts be assembled at all? The resolution is in elastic deformation of parts - all materials deform to some extent when they are assembled into a structure, 'absorbing' any errors in machining. Materials like plastics and wood deform easily, metals offer more resistance, and ceramics deform minimally (instead shattering or cracking). It is no coincidence that the more deformable materials are considered easier to work with, since they take less force to machine and are more forgiving in assembly. So before even getting to the more nuanced machinability improvements below, consider whether an easier to machine material can be used for the part.

Usually the more accurate (in an absolute sense) a machining method is, the more time it will require to complete (and the more difficult it will be to carry out). This is because higher accuracy requires control over more microscopic physical features of the sample, and high speed/high force motions are difficult to control to such a level. Thus the first thing the designer should consider is how accurate the parts actually need to be. Here we will make a simple distinction - low accuracy (features that 'look close enough'), medium accuracy (parts should match each other but exact match is not critical), and high accuracy (relative or even absolute position of parts needs precise control). The machines described below will be analyzed in terms of these labels. By the end of the article I hope the reader will find that surprisingly few parts need high accuracy machining, and thus will achieve significant time savings on future projects.

Error Sources

Various factors can lead to a machined part having different dimensions than intended, due to the cutting tool not reaching the desired location on the part during machining. The main errors are (in order of significance) due to alignment, rigidity, and tool/machine quality. Parallels can easily be drawn between these errors and the division into low/medium/high accuracy machining.

Low Accuracy Machining

This is typically the easiest type of machining (confirming the above inverse relation), so a lot of introductory shop classes cover these tools. Just because they are 'basic', the designer should not overlook them when considering how a part can be made.

Hand Drill
The hand drill can be used to make holes quickly (no need to set up part in mill) and at angles or locations not easily accessible with other tools. It can get tedious with tough metals like steel, but for one-off parts this may still be faster than finding a way to clamp the part and programming the mill operations. The low accuracy of the hand drill comes from both the difficulty of initially placing the drill at a specified point, and from the difficulty of holding the drill steady during the cut. Hole angles can easily deviate by a few degrees from the surface normal.
Rotary Tool
The rotary tool (dremel) can be used with an abrasive cutting blade to cut even steel and hardened steel pieces. It might be the most convenient way to cut key stock and small shafts, because of the increased flexibility compared to a bandsaw. Sandpaper and other accessories can be extremely useful for wood and plastic parts. The low accuracy of this tool is because it is handheld and has a relatively thick blade, so deviations of 0.1 inch would not be uncommon.
Saw (handheld tool or material)
The saw can be used to trim large parts to shape. Power saws can be used even with steel and thick metal stock, and are usually the best choice when removing a protruding section of the part since they only remove a thin line of material (as opposed to a whole volume removed by milling or lathing to separate two pieces) and thus can finish the operation faster. The low accuracy of this tool comes partly from positioning by hand (maintaining the blade at the right angle), and partly from the difficulty of verifying where the blade will start the cut. Longer cuts will deviate more due to Abbe error (errors in cut angle leading to increasing linear offset). Without a rigidly held part or blade the cut can shift by as much as 0.5 inch on 6 inch long parts!
Heat Tools (hot bending)
The possibility for shaping of heated stock should not be overlooked. Even metal rods under half-inch diameter can be bent with relative ease when heated with a torch. This approach has the highest promise with plastics which can be heated to an easily formable state with a heat gun. The low accuracy is from the difficulty of bending the heated material at the desired centerline and within a desired radius.

Medium Accuracy Machining

Drill Press (and clamped work)
The drill press can be used to make more accurate holes than with a hand drill, and is easier to use with tough metals and deep holes. It is also faster than setting up a part in the mill. Clamping the piece to be drilled helps maintain alignment of the drill throughout the cut, placing this machine in the medium accuracy category. With care, errors can be reduced to under 0.05 inch.
Saw (with guide)
Adding a guide to a saw, such as a straight edge on a bandsaw or a vise holder in a horizontal or cold saw, increases the cut accuracy. It also increases the cut repeatability, which can be more important than accuracy in many projects. The cold saw is becoming one of my favorite tools to cut large metal pieces to size due to its speed and rigidity. Errors of about 0.05 inch can be achieved but may require adjustment of the guides based on a first rough cut.
Mill without DRO
On the manual mill, errors can be reduced to the level of 0.005 inch. Some error is introduced from the backlash of the stage drive mechanism, and some from deflection of the cutting tool (or even of the stock itself in poorly clamped conditions - especially in case of thin materials bulging upwards or downwards). The mill is the tool of choice when multiple metal parts need to be assembled with tight tolerance, because the accuracy leads to consistent hole locations in sequentially machined parts.
Lathe without DRO
The lathe can also achieve 0.005 inch errors. Doing this normally requires machining and then measuring a surface to use as a reference point. Backlash as well as a non-centered part in chuck or off-axis (slightly tilted) part in chuck can exacerbate errors to 0.05 inch levels, so a gauge should be used to ensure concentricity. Center drilled holes will usually be off from true center or wider than expected, unless the part end concentricity is measured beforehand.
Water jet and laser cutter
Both of these tools are great for 2D cuts of sheet-like stock and are thus grouped together. The accuracy is limited by compensation for the cutter size (water jet diameter, laser beam diameter) as well as inward taper of cut edge, which may be around 0.05 inch on thick metal in the waterjet. These tools generally cannot be aligned by eye beyond 0.05 inch accuracy, but the repeatability for cuts within a single operation can be around 0.005 inch because the machine does not have to handle the cutting forces in its positioning mechanism (to achieve this, the stock needs to be kept from moving/vibrating during the cut).
3D Printer
Higher end printers can achieve 0.005 inch resolution, while typical hobby type prints done on a fast print setting might have 0.01 inch errors in surface finish. Errors due to plastic extrusion and curving/bowing of parts from thermal contraction of the layers can bring overall accuracy down to 0.05 inches. Still the versatility of the 3D printer makes it useful for complicated parts. If the use of a 3D printer is acceptable, designing a part that combines the functions of multiple independent pieces may end up being simpler to fabricate.

High Accuracy Machining

Mill with DRO
With a DRO and servo with feedback (CNC), dimensions can be measured (and perhaps machined) to 0.0005 inch. Tool and sample deflection will tend to worsen this, and the highest accuracy may even be affected by temperature expansion of the parts and wear on the tool. The performance comes at the time cost of programming the mill and aligning the parts beforehand, which is particularly cumbersome for one-off parts but worthwhile for three or more parts and for complex parts.
Lathe with DRO
Similar to the mill in achievable positioning accuracy, the lathe requires greater care in stock alignment for concentricity.
Multi-axis machines
Multi-axis machines are the most difficult to program, but this is made worthwhile when precise parts are required in a production environment. The multi-axis approach allows many sides of the stock to be machined within a single clamping setup, leading to the highest relative accuracy between the machined features.

Optimizing Design to Reduce Machining Time

The rest of the article suggests some ways parts can be modified for faster and easier machining. Often this involves reduced accuracy, and while it doesn't sound like a prompt to reduce accuracy should be in an article about machining, I have found this to be one of the major hurdles in my experience of learning machining. What I am calling for is not necessarily an actual reduction in accuracy, but a reduction in perceived accuracy, that is having a more realistic view of the necessary accuracy in a machining operation.

External Dimensions

Will it be acceptable if the external dimensions of the part vary by 0.1-0.5 inches? If not, is there a simple design change that can make it acceptable? Right away it is possible to save time if nothing beyond a basic saw cutout of the piece is needed. Even the sawing time can be eliminated if the design uses stock sizes that can be bought pre-cut such as multiples of 6 inch.

(A) initial design specifies a 5.5x5.875 inch plate. To get these specific dimensions and square corners will require lengthy set-up, alignment, and cutting of the outside edges in the mill or waterjet. (B) has looser tolerances on the outer edges, in size and straightness. The shape is now irregular but if this doesn't affect the design the piece can be machined much faster, sawing the sides 'by eye'. (C) recognizes that a 6x6 inch plate is a commonly sold shape, and with the tolerances on pre-cut stock (0.084 in) being acceptable this eliminates all outer edge cutting operations.

Bolt Holes

Can the bolt holes be widened by 0.01 inches or more? The problem of hole misalignment can be alleviated by using oversized holes on the non-threaded parts, or even better by using nuts and oversized holes on all parts (washers can enable significantly oversized holes if the loading is acceptable). Better alignment can be attained by using only a single close-fit hole, potentially with other wider or slotted holes for support. Another approach, if the exact bolt locations aren't critical, is to drill bolt holes on parts clamped in the desired configuration, ensuring near-perfect alignment of the holes in multiple parts. Special tools like combined counterbore/countersink/centering drill bits can remove extra operations and set-up time.

(A) holes are so tight that the threads of the bolt barely fit through. If there are multiple holes like this, there is a great chance some bolts will not fit. (B) holes are a looser fit (10-20% diameter increase) so assembly is easy. (C) uses nuts and threaded rod, so no lengthy tapping is necessary and all holes are easily drilled through.

(A) holes are drilled in multiple parts during separate operations, introducing a possibility of misalignment. (B) holes are drilled with parts clamped in desired orientation (or using hole-transfer punches), guaranteeing matching hole locations.


Some non-rectangular parts might be made in a simple way if some piece of a machine is rotated. For instance, changing the angle of the saw blade in a cold saw, changing the angle of a lathe tool, changing the tilt of the mill head, or using an angle block when clamping a part in the vise. Such angular adjustments are usually not very accurate since in many cases errors in adjustment lead to larger errors in the part (Abbe error). But if deviations in the vicinity of 0.01 inch are acceptable, this is worth considering. Another option to keep in mind is a manual rotary table (rotation about vertical or horizontal axis) that could be attached to the mill in place of the stationary vise.

(A) two corners on a rectangular block are cut using a programmed CNC mill operation. (B) the CNC programming and setup time is eliminated by rotating the vise to the required angle and milling along the x axis, flipping over the piece to achieve the same angle on both sides. (C) a cold saw at the necessary angle is used to speed up machining by reducing the amount of metal cut.

Buying Accurate Parts

For parts that need to be accurate, such as bearings, gears, shafts, buy pre-made parts that can interface with less accurate machined parts. For instance: mounted (pillow block) bearings, complete gearboxes, flexible shaft couplings and universal joints. Maybe there is even a very similar mechanism that can be purchased and repurposed to get the desired features, drastically shortening machining time. Similarly, there may be an available stock size that matches one or more of the required dimensions, with some stock suppliers offering very tight tolerances. Taking this route requires the flexibility to adjust one's design to existing non-custom parts and perhaps lose some performance; usually the payoff in terms of time and effort saved is well worth it.

(A) the hole in the plate on the left needs to be milled to a precise OD to press fit the bearing. (B) a mounted bearing can be attached to the plate with two bolts, removing the need for lengthy finishing passes and measurements. (C) finding a part with bearings already built in makes it possible to just supply an external shaft and drill one hole in the plate.

Working by Eye

Machine and align parts by eye - this gives more rapid feedback and removes the necessary time for either programming an operation or constantly checking the DRO and sketches while machining. If drilling loose-fitting holes, parts may be completed quickly by printing full-scale paper drawings, then using a punch to transfer hole locations and a drill press to drill holes at the marked points (within 0.05 inches). Use of edge finders may be eliminated without sacrificing accuracy if it is possible to make an initial cut by eye and then measure the cut location with calipers, and use that to establish a zero point reference. Using a stationary point like an edge of the mill vise or lathe chuck, at least for one of the axes (and with a vise stop, for two), makes it possible to align the machine once and reduce alignment time for sequential pieces.

(A) using an edge finder adds extra time to set up. (B) using a tight-tolerance hole with a matching rod can establish a zero point more quickly and accurately than an edge finder. (C) aligning a corner by eye to tool center is fast and can be surprisingly accurate.

A technique for accurate alignment by eye. Look at the part edge along either the x or y axis with one eye shut, and place your head such that the part edge parallel to the chosen axis appears to turn into a single point. Then move the part along the other axis such that the center of the tool is in line vertically. With well-defined tool center and part edge this method can be repeatable to within 0.002 inches (a magnifying glass makes this easier to achieve).

The Z Dimension

When practical, eliminate 3D features as they are more complicated to machine. Specific-depth (blind) holes and mill cuts incur the time to ensure the correct depth is attained (which involves measuring the Z offset of each tool), and make machining slower because metal chips cannot escape from the bottom of the cut. Face milling (thickness reduction) of sheet-like parts usually leads to subpar results because of difficulty in securing the part and subsequent part movement/bowing during machining. Tapping is easier with through-holes (doesn't require a second bottoming tap) and is much less likely to break taps. 2D profiles have the added advantage of possibly being machined in one operation on a water jet cutter.

(A) this part requires a lengthy facing operation and frustrating drilling/tapping blind holes on the side. (B) all holes can now be drilled in one orientation with no tapping, but facing is still necessary. (C) the extraneous edge is removed so no face milling is necessary, saving time and metal.

Using Fewer Tools

End mills are quite versatile, as are lathe cutters, and for small batches of parts or one-off parts the time required to switch out and align the tool (and adjust the table for the tool height) may be a large fraction of the machining time. Consider altering the design so that a single size end mill (or other tool) could be used throughout.

(A) this plate has three different hole sizes and an end mill cut of a large hole, requiring 4 tools. (B) holes have been standardized so only 1 drill bit is necessary. (C) holes are slightly widened and a smaller end mill is used, enabling the whole part to be machined with one tool.

Bending Parts

Some parts may be made much quicker by bending a metal sheet as opposed to machining a metal block. Sheet metal can be surprisingly strong so it is worth trying a quick calculation of loading (or, more easily, feel the rigidity and wall thickness of existing sheet metal structures that can be found in most appliances and office furniture). Even more possibilities are available if plastic is an option, since thick plastic (up to 3/8 inch thick sheets) can be bent using heat tools. These parts are light and easy to work with, and machining leaves minimal waste.

(A) a 3D block requires drilling and countersinking on both sides. (B) the part is simplified by using plastic which can be bent to shape. (C) using sheet metal instead of plastic allows the part to be more compact.