Designing for CNC Milling

Principles

A part that is easy to machine is cheap, accurate and fast to make. Design for machining means making choices that fit what a rotating round tool can do. Three ideas explain nearly every rule: tools are round and finite (so inside corners have a radius, and deep features need long tools); tools can reach only from outside (so features must be visible from a few directions); and every set-up, tool change and tight tolerance costs time.

• Design for the process you will use. A part designed for a 3D printer, with sharp inside corners and hidden cavities, needs redesign for milling.
• Fewer set-ups: put as many features as possible on as few faces as possible, and orient them so that each can be reached from the top.
• Use the standard: standard hole sizes, standard threads, the same radius throughout, and standard stock sizes.
• Specify only what matters. Tolerance only the functional features; accept a general tolerance on the rest.

Inside corners and corner radii

• Inside vertical corners always have a radius, at least that of the smallest tool that can reach: the tool’s diameter is at most twice the corner radius. A sharp corner needs a second process (EDM or broaching), which is expensive.
• Make the radius at least one-third of the pocket depth (R ≥ depth ÷ 3). A deeper pocket needs a longer tool, a longer tool must be thicker to stay stiff, and a thicker tool needs a bigger radius.
• Better: radius slightly bigger than the tool, about 1.2 × the tool radius, so that the tool cuts a smooth path. If the radius equals the tool radius, the tool is fully engaged in the corner and loads suddenly.
• The same radius in every corner means one tool and no tool changes.
• Where a mating part must fit into a square corner, add a relief (a dog-bone or T-bone) in the corner so that the mating part’s sharp corner fits. The relief makes the tool path simple and keeps the radius.
• Floor corners. The corner between the floor and a wall can be sharp (flat end mill) or have a radius (bull-nose or ball). A radius equal to the tool’s corner radius is cheapest. A large floor fillet needs a ball or bull-nose tool.

Pockets, walls and floors

Feature	Good	Possible with care	Why
Pocket depth	Up to 4 × tool diameter	6 × with a long reach tool; beyond 10 × is very difficult	Long tools deflect and chatter; chips are hard to clear
Wall thickness (metal)	1.5 mm or more	0.8 mm	Thin walls vibrate and bend away from the tool
Wall thickness (plastic)	2 mm or more	1.5 mm	Plastic is soft and flexible, and warms
Wall height-to-thickness	Up to 8 ÷ 1	10 ÷ 1 or more with a support	A tall thin wall acts like a cantilever
Floor thickness	1.5 mm or more	0.8 mm	Prevents the floor flexing and breaking through
Slot width	Standard tool size (3, 4, 6, 8, 10 mm)	Any, with a smaller tool	Matches the tool diameter and avoids repeated passes
Floor radius	None (flat) or equal to the tool corner radius	Larger with a ball nose	A ball finish takes much longer
Boss and rib height	Up to 4 × the width	10 × with care	Tall thin features chatter

Holes and threads

• Use standard drill sizes. A hole at a standard size is drilled; any other size is bored or milled with a plain tool, which costs time. Metric: 3, 4, 5, 6, 8, 10 mm and so on; inch: fractions, number and letter drills.
• Depth. Up to 4 × the diameter is standard (24 mm for a 6 mm hole); beyond about 10 × needs pecking and care; a deep, small hole needs a gun drill. The bottom of a drilled blind hole is conical (118° or 135° point), so allow for the point in the depth.
• Through holes are cheaper than blind holes (no depth control, easier chips). If a hole is blind, make it only as deep as the thread or fit needs.
• Threads. Engage about 1.5 × the diameter in steel and 2 × in aluminum; more adds no strength. Drill the tap hole a little deeper than the thread (about 1.25 × the thread depth, plus the drill point), so that the tap does not hit the bottom. For the tap drill see the Tap Drill Size & Thread Pitch Lookup.
• Smallest thread: M3 or #4-40 is the practical minimum for hand or machine tapping in metal, and larger is better; very small threads break taps. Use a thread mill for small fine threads in hard metal.
• Thread class. Do not specify a tight class (such as 4H/6g or 3B) unless needed; see Fits in Practice.
• Hole position. Holes close to an edge (less than 1 × the diameter) are weak; keep at least 1.5 × the diameter from edges and from each other.
• Counterbores and countersinks. Standard sizes for screw heads (ISO 4762, ISO 10642) use standard cutters.
• Reamed holes (H7) cost more than drilled; specify only where a pin or bearing fits.

Tool access and set-ups

• All features should be reachable by a straight tool from one of a few directions. On a 3-axis mill, a feature must be visible from above in its set-up. Features on several sides need a new set-up for each.
• Undercuts and internal cavities cannot be cut with a normal tool; they need special T-slot or lollipop cutters, EDM, casting, or a split design.
• Minimize set-ups. Each flip or re-clamp costs 15–60 minutes of labor and adds position error. A part with features on two sides can often be split into two simple parts that are screwed together.
• Datum features first. Machine the face and holes you will use for locating in the first set-up, so that the second set-up can locate on them. Dimension from those datums on the drawing. See Datums and Datum Reference Frames.
• Leave a way to hold the part. A flat of at least 5–10 mm around the edge, or an extra tab removed at the end, lets the vise grip it; see Workholding and Fixturing.
• Avoid features that need a very long tool deep in a part, such as a small pocket at the bottom of a big one.
• Allow for the tool holder. The holder is wider than the cutter; a deep pocket next to a tall wall may be unreachable.

Tolerances and surface finish

• Standard tolerance for machined parts is often around ±0.1 mm (ISO 2768-m: ±0.2 mm for sizes 6–30 mm, ±0.3 mm for 30–120 mm). Tighter than ±0.05 mm raises the cost, and ±0.01 mm or tighter needs special measurement and often grinding. See General Tolerances and Drawing Notes.
• Tolerance only what matters: holes for bearings and pins, mating faces, locating features. Let everything else take the general tolerance.
• Surface finish. A normal milled surface is Ra 3.2 µm. Ra 1.6 µm needs a finishing pass; Ra 0.8 µm needs a fine pass and often a polished tool; below that, grinding or polishing. Do not specify a finish on a surface that does not need one.
• Geometric tolerances (flatness, position) cost money in measurement and set-ups. See GD&T.
• Thin or large parts move after machining as stress is released, so that a flatness of 0.02 mm may not be possible without a stress-relieving step.
• Tolerance is a conversation with the shop. Ask what they hold routinely and design to it.

Edges, chamfers and fillets

• Break all sharp edges. A sharp machined edge is a burr risk and cuts hands. Specify “break edges 0.2–0.5 mm” or a chamfer of 0.5 × 45°.
• Chamfers are cheaper than fillets on outside edges, because a chamfer tool does the job in one pass.
• Outside fillets on a profile (a rounded outside corner) are free with a profiling tool. Specify the same radius around the part.
• Chamfer the tops of holes, to start a screw or a pin and to remove the burr.
• Avoid a tangent fillet to a wall that stops short, which leaves a small step; run the fillet to the edge.
• Text and logos. Engrave with a stroke at least 0.5 mm wide and 0.3–0.5 mm deep; small, fine text and a deep engraving cost more.

Material and stock

• Pick a material that machines well if it meets the need: 6061 aluminum, free-machining brass and 1018 or 12L14 steel machine easily; stainless and titanium cost several times more in cutting time. See Machining Metals and Machining Plastics, Wood and Composites.
• Use standard stock sizes (plate thickness and bar widths), so that the blank needs little facing: 3, 6, 10, 12, 20, 25 mm plate; 1/4, 1/2, 3/4, 1 in.
• Plate against bar against casting. A pocketed part from solid turns a large share of the block into chips (a 60 × 40 × 15 pocket in a 70 × 50 × 20 blank removes 51 % of its volume). For big runs, a casting or extrusion near the final shape is cheaper.
• Stress and flatness. Cold-rolled plate bends when one side is removed; use cast or stress-relieved plate for flat parts.
• Finishes after machining (anodizing, plating, painting) change dimensions and affect fits; see Temperature, Coatings and Fit Problems.

What drives the cost

Driver	Effect	How to reduce it
Set-up time	Fixed per job; large for single parts	Fewer set-ups and tool changes; standard vise work
Machining time	Proportional to material removed and the care needed	Larger corner radii, shallower features, less material to remove
Tolerances	Extra passes, inspection and scrap	Specify only where the function needs them
Material	Cost per kg and machinability	Standard, easy-to-machine stock
Number of operations	Each extra process adds handling	Combine features; avoid EDM or grinding unless needed
Finishing	Anodizing, plating, polishing	Skip decorative finishes on non-visible surfaces
Quantity	Set-up cost spread over the lot	Order in batches; design families of parts together

Router and sheet parts

• Kerf and fits. The cutter is round, so slots and tabs need a compensated width. A tight finger joint needs a test cut; make a fit coupon first.
• Inside corners on a joint: add a dog-bone relief where a square corner must fit, or round the mating corner to the tool radius.
• Grain and tear-out. Cut with the grain where you can; tear-out is worst across it. Use a downcut or compression bit for clean faces; see Machining Plastics, Wood and Composites.
• Tabs hold parts in the sheet; allow for removing them.
• Minimum feature size. The smallest slot is the tool diameter (3 mm on a hobby router); the smallest hole you can cut by interpolation is about 1.5 × the tool diameter.
• Part spacing. Leave at least one tool diameter between parts, and a margin from the sheet edge for clamps or screws.

Design review checklist

Question	Fix if the answer is no
Does every inside corner have a radius larger than the tool needs?	Add radii; use one size
Is every pocket no deeper than about 4 × its smallest width?	Widen it or reduce the depth
Are walls at least 1.5 mm (metal) and not very tall?	Thicken or add a rib
Are holes standard sizes and not more than 4 × D deep?	Change to a standard size or make it a through hole
Are threads no smaller than M3 and not deeper than 1.5 × D?	Increase the size or reduce the depth
Can every feature be reached from a few directions?	Split the part or reposition features
Can the part be held for every operation?	Add flats or tabs
Are tolerances tight only where the function needs them?	Loosen the rest
Are edges broken and the finish specified only where needed?	Add a general note
Can the part be made from standard stock?	Adjust the size to stock

Related

• CNC Machining: the overview of this guide.
• Designing for Turning: the same ideas for turned parts.
• Milling: Operations and Tooling: tool reach, stiffness and chip load.
• Fits & Tolerances and GD&T: specifying tolerances.
• 3D Printing: an alternative when the shape cannot be machined.

FAQ

Why can’t a mill cut a sharp inside corner?

The cutter is round, so it leaves a radius in every inside corner equal to its own radius. A sharp corner needs a different process (EDM, broaching) or a relief that lets the mating part fit.

What is the smallest wall I can machine?

About 0.8 mm in metal and 1.5 mm in plastic, but thin walls vibrate and bend away from the tool, so go thicker if you can: 1.5 mm in metal is much easier and cheaper.

Why are deep pockets expensive?

They need a long, thin tool, which deflects and chatters, so the shop takes light cuts at a slow feed, may need several tools, and risks breakage. Keep depth to 4 × the tool diameter or less.

How tight a tolerance should I specify?

As loose as the function allows. The general ±0.1 mm covers most features; reserve ±0.05 mm or tighter for fits, bearings and locating features. Each step tighter raises the cost.

Should I design a part for CNC or for 3D printing?

Choose the process first, then design for it. A part made for printing (internal channels, organic shapes, sharp internal corners) is hard to machine, and a part made for machining (tight tolerances, flat faces, threads) is usually stronger and more accurate.

References

• Oberg, E. et al., Machinery’s Handbook, 31st ed., Industrial Press: milling, drilling, tapping, tolerances and surface texture.
• ISO 2768-1, General tolerances: tolerances for linear and angular dimensions without individual tolerance indications.
• Design-for-manufacturing guides from CNC service providers (for example Protolabs, Xometry, Fictiv, Hubs): corner radii, wall thickness, hole depth and tolerances.
• Bralla, J., Design for Manufacturability Handbook, McGraw-Hill.
• ASME Y14.5-2018, Dimensioning and Tolerancing.

Last reviewed: October 2026. Cutting data are starting points: machines, tools and materials differ, so test on scrap and follow the tool maker’s data.