CNC machining design guidelines

Radius internal corners to at least 1/3 of the cavity depth and never below 0.030 in (0.8 mm). Keep pockets no deeper than 4× their width, walls at least 0.030 in (0.8 mm) in metal and 0.060 in (1.5 mm) in plastic, drilled holes near 4× diameter, and tapped threads near 1.5× diameter. Default to ±0.005 in (±0.13 mm) or ISO 2768-m.

Try the interactive lab Check a part in the builder

Inside corner radius: ≥ 1/3 depth, 0.030 in min
Pocket depth: ≤ 4× pocket width
Tapped thread depth: 1.5× diameter
Standard tolerance: ±0.005 in (±0.13 mm)

SSG MFG · design guideDG-10 · 13 rules

What are the cnc machining design rules?

13 rules, in the order you meet them on a model. Every value is typical; the principal quoting your part confirms its own limits.

Design rules and typical values
#	Rule	Typical value
01	Design to stock sizesLeave 0.030–0.060 in (0.8–1.5 mm) under standard bar or plate size per side	Leave 0.030–0.060 in (0.8–1.5 mm) under standard bar or plate size per side
02	Radius internal cornersAt least 1/3 of cavity depth; 0.030 in (0.8 mm) minimum; about 0.005 in larger than the cutter radius	At least 1/3 of cavity depth; 0.030 in (0.8 mm) minimum; about 0.005 in larger than the cutter radius
03	Limit pocket depthDepth no more than about 4× pocket width; cutter reach ideally under 3× its diameter	Depth no more than about 4× pocket width; cutter reach ideally under 3× its diameter
04	Keep walls thick enough to cut0.030 in (0.8 mm) in metal, 0.060 in (1.5 mm) in plastic; height under about 10× thickness	0.030 in (0.8 mm) in metal, 0.060 in (1.5 mm) in plastic; height under about 10× thickness
05	Size undercuts to standard cuttersMatch standard keyseat, T-slot and 45° or 60° dovetail cutters; keep about 4× the undercut depth clear to any opposing wall	Match standard keyseat, T-slot and 45° or 60° dovetail cutters; keep about 4× the undercut depth clear to any opposing wall
06	Use standard hole sizesStandard fractional, letter, number or metric drills; reamed holes at standard reamer sizes	Standard fractional, letter, number or metric drills; reamed holes at standard reamer sizes
07	Limit drilled hole depthAbout 4× diameter standard; up to 10× with peck drilling; beyond that, gun drilling	About 4× diameter standard; up to 10× with peck drilling; beyond that, gun drilling
08	Allow a drill point on blind holes118° or 135° cone at the bottom; dimension depth to the full diameter	118° or 135° cone at the bottom; dimension depth to the full diameter
09	Limit tapped thread depthAbout 1.5× diameter in steel; up to 2× in aluminum and plastic	About 1.5× diameter in steel; up to 2× in aluminum and plastic
10	Drill past the last full threadAt least 3 pitches, or about 0.5× diameter, of extra drilled depth in blind tapped holes	At least 3 pitches, or about 0.5× diameter, of extra drilled depth in blind tapped holes
11	Chamfer or break edges0.010–0.020 in (0.25–0.5 mm) × 45°; call out "break sharp edges" for the rest	0.010–0.020 in (0.25–0.5 mm) × 45°; call out "break sharp edges" for the rest
12	Put features on as few faces as possibleOne or two setups on 3-axis; five-sided parts on 5-axis	One or two setups on 3-axis; five-sided parts on 5-axis
13	Tolerance only what mattersDefault to ±0.005 in (±0.13 mm) or ISO 2768-m; tighten only fits and datums	Default to ±0.005 in (±0.13 mm) or ISO 2768-m; tighten only fits and datums

These build on the short list on the cnc machining process page, with the failure each rule prevents and a drawing for each.

How deep can a pocket be for a given corner radius?

Set a pocket depth and corner radius and see which cutter fits, what its length-to-diameter ratio becomes, and where chatter, deflection and cycle time start to climb.

CORNER R 0.250 IN · DEPTH 1.00 IN · 3/8 IN END MILL

Start from

Inside corner radius

Pocket depth

Largest end mill that fits: 3/8 in(9.5 mm)
Depth to diameter: 2.7 : 1usual ≤ 4
Tool reach needed: 1.05 in

Works: standard cutter, full feed

A 3/8 in end mill fits the 0.250 in corner and reaches 1.000 in at 2.7× its diameter, inside the usual 4×.

Typical shop practice: corner radius about 10% over the tool radius, and pockets up to about 4× the cutter diameter at normal feeds.

Why does each rule matter?

Each rule with its typical value, the reason behind it and what happens on the floor when it's ignored. Switch any drawing between Do and Avoid; point at a callout to pick it out.

Rule 01

Design to stock sizes

Leave 0.030–0.060 in (0.8–1.5 mm) under standard bar or plate size per side

Why: Stock is sold in fixed diameters and thicknesses. A part that fits just inside a standard size is squared up in one pass instead of cut from the next size up.
If you ignore it: The shop buys the next size up and pays for extra material and a roughing pass on every part.

Fig. 1Design to bar stock

Do. Set the largest diameter at a standard bar size, such as 0.500 or 0.750 in, and the bar's own surface becomes the part's OD.

Avoid. A largest diameter just over a stock size forces the next bar up; every part turns that difference into chips and cycle time.

Rule 02

Radius internal corners

At least 1/3 of cavity depth; 0.030 in (0.8 mm) minimum; about 0.005 in larger than the cutter radius

Why: End mills are round, so every inside vertical corner carries at least the cutter radius. A corner slightly larger than the tool lets it arc through instead of stopping and wrapping, and a large radius allows a short, stiff cutter.
If you ignore it: A small cutter runs long and slow, chatters in the corner, and the cycle can run 3× longer.

Fig. 2Internal corner radius

Do. Corner radius a little larger than the cutter radius lets the end mill arc through the corner at full feed.

Avoid. A sharp inside corner can't be milled: a rotating tool always leaves its radius, so a square corner means EDM or a broach, at several times the cost.

Rule 03

Limit pocket depth

Depth no more than about 4× pocket width; cutter reach ideally under 3× its diameter

Why: Standard end mills cut cleanly to about 3× diameter. Past 4–5× the tool deflects, so feeds drop and long-reach tooling is needed.
If you ignore it: The cutter deflects and chatters, walls come out tapered and rough, and feeds drop by half or more.

Fig. 3Pocket depth and tool reach

Do. Pockets no deeper than about 4× the cutter diameter cut with a standard-length tool at normal feeds.

Avoid. Past about 4×, the tool sticks out far enough to deflect: chatter marks on the walls, tapered walls, slow feeds and broken cutters.

Rule 04

Keep walls thick enough to cut

0.030 in (0.8 mm) in metal, 0.060 in (1.5 mm) in plastic; height under about 10× thickness

Why: Thin walls vibrate and spring away from the tool, and plastic walls also warp from heat and clamping.
If you ignore it: Walls chatter, bow and miss tolerance, and the shop adds light finishing passes that double the time on that feature.

Fig. 4Minimum machined wall

Do. Walls at least 0.030 in (0.8 mm) in metal and 0.060 in (1.5 mm) in plastic, kept short relative to their thickness, stay flat and hold size.

Avoid. A tall, thin wall rings under the cutter, springs away from it and comes out wavy, thin at the top or cracked.

Rule 05

Size undercuts to standard cutters

Match standard keyseat, T-slot and 45° or 60° dovetail cutters; keep about 4× the undercut depth clear to any opposing wall

Why: Undercuts need a cutter with a head wider than its neck, and the neck needs room to enter.
If you ignore it: The shop grinds a special cutter or adds EDM, and the undercut becomes the most expensive feature on the part.

Rule 06

Use standard hole sizes

Standard fractional, letter, number or metric drills; reamed holes at standard reamer sizes

Why: A standard drill or reamer makes a hole in one plunge. Odd sizes are interpolated with an end mill.
If you ignore it: Each odd hole is circle-milled, adding cycle time and a size that depends on tool wear.

Rule 07

Limit drilled hole depth

About 4× diameter standard; up to 10× with peck drilling; beyond that, gun drilling

Why: Chips must evacuate up the flutes. Past about 4× diameter the drill has to retract to clear them, and past about 10× it needs coolant-through or gun drilling.
If you ignore it: Chips pack in the flutes and the drill wanders or breaks in the hole, scrapping the part.

Fig. 5Drilled hole depth

Do. A blind hole about 4× its diameter deep drills in one pass; call the full-diameter depth and let the 118° point sit below it.

Avoid. Deep holes pack chips and let the drill wander off the axis; past about 6× you're into peck cycles, and past about 10× gun drilling.

Rule 08

Allow a drill point on blind holes

118° or 135° cone at the bottom; dimension depth to the full diameter

Why: Twist drills leave a cone. A flat bottom needs a second tool such as a flat-bottom drill or end mill.
If you ignore it: A flat-bottom callout adds a tool change and a second plunge to every blind hole.

Rule 09

Limit tapped thread depth

About 1.5× diameter in steel; up to 2× in aluminum and plastic

Why: Most of the load is carried by the first few engaged threads. Longer engagement adds little strength and raises tap torque.
If you ignore it: Deep tapping raises torque and the tap breaks in the hole, which usually scraps the part.

Standard: ASME B1.1 (unified), ISO 965 (metric)

Fig. 6Tapped hole depth

Do. About 1.5× D of full thread carries the bolt to failure in steel; the tap drill runs a few pitches deeper so a plug tap never bottoms out.

Avoid. Thread past 1.5–2× D adds almost no strength, and a tap that bottoms in a blind hole packed with chips breaks off in the part.

Rule 10

Drill past the last full thread

At least 3 pitches, or about 0.5× diameter, of extra drilled depth in blind tapped holes

Why: Taps have a tapered lead of 3–5 threads that cannot cut full form, and chips need somewhere to collect.
If you ignore it: The tap bottoms out on packed chips, and the last threads come out short or the tap snaps.

Fig. 7Thread runout and relief

Do. A relief groove at least two pitches wide, cut to the minor diameter, gives the threading tool room to exit and the nut a full thread to seat against.

Avoid. Without relief the last threads are incomplete: the nut stops short of the shoulder and the tool can crash into it.

Rule 11

Chamfer or break edges

0.010–0.020 in (0.25–0.5 mm) × 45°; call out "break sharp edges" for the rest

Why: A chamfer is cut in the same pass and removes the burr. External fillets need a corner-rounding tool and a separate pass.
If you ignore it: Parts leave the machine with sharp burrs that are removed by hand, and hand deburring varies part to part.

Fig. 8Edge break

Do. A small 45° chamfer on every outside edge removes the burr, guides assembly and costs almost nothing when it's in the program.

Avoid. A sharp edge keeps its burr: it cuts hands and seals, and stops mating parts from starting straight.

Rule 12

Put features on as few faces as possible

One or two setups on 3-axis; five-sided parts on 5-axis

Why: Every flip adds a fixture, an indicate-in and a new datum transfer.
If you ignore it: Each added setup adds labor and stacks about 0.001–0.002 in (0.025–0.05 mm) of location error between faces.

Fig. 9Setups

Do. Features grouped on one or two faces machine in one or two setups, with every feature referenced to the same datum.

Avoid. Each extra face is another fixture, another setup charge and another chance for position error between features.

Rule 13

Tolerance only what matters

Default to ±0.005 in (±0.13 mm) or ISO 2768-m; tighten only fits and datums

Why: Each tighter tolerance means slower passes, more tool changes and inspection.
If you ignore it: A blanket ±0.001 in note can double inspection time and add finishing passes to every feature.

Standard: ISO 2768-1, ASME Y14.5

What tolerances can cnc machining hold?

Typical values from production machine shops. Tight values need extra passes, reaming or grinding, temperature control, or 100% inspection.

Typical and tight tolerances with the cost of going tight
Feature	Typical	Tight	Cost of tight
Milled linear dimension	±0.005 in (±0.13 mm)	±0.001 in (±0.025 mm)	Moderate
Turned diameter	±0.002 in (±0.05 mm)	±0.0005 in (±0.013 mm)	Moderate
Bored or reamed holeReaming or boring adds a tool	+0.001/−0 in (+0.025/−0 mm)	ISO 286 H7, about +0.0007/−0 in at 0.5 in	Moderate
Hole position	Ø0.010 in (0.25 mm)	Ø0.002 in (0.05 mm)	Moderate
FlatnessTight flatness usually means grinding	0.002 in (0.05 mm) per 4 in	0.0005 in (0.013 mm)	High
Surface finish	Ra 63–125 µin (1.6–3.2 µm)	Ra 16–32 µin (0.4–0.8 µm)	Moderate
Tapped thread class	2B (UN) or 6H (metric)	3B or 4H5H	Moderate
Angles	±0.5°	±0.1°	Moderate

Basis: ISO 2768-1, ISO 286 fits, ASME Y14.5. Put a general tolerance note on the drawing and tighten only the features that need it; every tight callout is priced. See the tolerance guide.

How does the material change the rules?

The same cnc machining rules shift with the alloy or compound.

Aluminum 6061-T6
Cuts about 3–4× faster than stainless, so aggressive feeds and deep pockets are affordable. Thin walls still spring, so hold the 0.030 in (0.8 mm) minimum.
Stainless steel 304
Work hardens if the tool rubs, so light finishing passes and small tools struggle. Prefer larger corner radii and 303 where the part allows it.
Titanium Grade 5 (Ti-6Al-4V)
Low stiffness and poor heat conduction make long tools chatter. Keep cutter reach near 3× diameter and expect several times the cycle of aluminum.
Acetal (POM)
Machines cleanly but moves with heat and clamping. Use the 0.060 in (1.5 mm) plastic wall minimum and hold tolerances near ±0.005 in (±0.13 mm).
Steel 4140 (annealed)
Machining prehardened 4140 at about 28–32 HRC avoids heat-treat distortion. Fully hardened parts need grinding or hard milling on the final features.
Brass C360 (free-cutting)
Free-machining and fast to tap and drill. Deep holes and fine threads are cheaper here than in any steel.

CNC machining design questions

What is the minimum internal corner radius for CNC machining?

The practical floor is about 0.030 in (0.8 mm), cut with a 1/16 in (1.5 mm) end mill that can only reach shallow depths. A better target is at least 1/3 of the pocket depth, and about 0.005 in (0.13 mm) larger than a standard cutter radius, such as 0.130 in for a 1/4 in cutter. Larger radii allow shorter, stiffer tools and faster cycles.

How deep can a CNC pocket be?

Keep pocket depth to about 4× the pocket width, and keep the cutter's reach under about 3× its diameter where you can. A 0.5 in (12 mm) wide slot is comfortable to about 1.5–2 in (38–50 mm) deep. Deeper pockets need long-reach tools, reduced feeds and more passes, which raise cycle time and hurt wall finish.

How deep should a tapped hole be?

Specify about 1.5× the nominal diameter of full thread in steel, and up to 2× in aluminum or plastic. Then drill at least 3 thread pitches deeper so the tap's tapered lead and the chips have room. A 1/4-20 thread in steel is typically 0.375 in (9.5 mm) of full thread with a drill depth near 0.525 in (13 mm).

What is the minimum wall thickness for CNC machined parts?

About 0.030 in (0.8 mm) for metal and 0.060 in (1.5 mm) for plastic, with wall height kept under about 10× thickness. Thinner or taller walls vibrate and deflect under the cutter, so they need light passes, support material or special fixturing. Aluminum tolerates thin walls better than stainless or titanium.

What does ISO 2768-m mean on a drawing?

ISO 2768-m is the medium class of general tolerances for dimensions with no individual tolerance. For linear sizes it allows ±0.1 mm up to 6 mm, ±0.2 mm from 6 to 30 mm, ±0.3 mm from 30 to 120 mm and ±0.5 mm from 120 to 400 mm. Class f is tighter and c is looser. It suits most machined parts.

How do I get a sharp inside corner on a machined part?

A milled inside corner always carries the cutter radius. If a square part must seat in the pocket, add a dog-bone or T-bone relief that cuts past the corner, or break the edge on the mating part. A true sharp corner needs wire or sinker EDM, which adds a separate operation and often doubles the cost of that feature.

Check your part against these rules.

Drop a STEP file in the builder for an instant DFM check and a budgetary estimate, then send it to principals who run cnc machining every day.

Build a part Send a drawing

CNC machining design guidelines

Rule

Design to stock sizesLeave 0.030–0.060 in (0.8–1.5 mm) under standard bar or plate size per side

Radius internal cornersAt least 1/3 of cavity depth; 0.030 in (0.8 mm) minimum; about 0.005 in larger than the cutter radius

Limit pocket depthDepth no more than about 4× pocket width; cutter reach ideally under 3× its diameter

Keep walls thick enough to cut0.030 in (0.8 mm) in metal, 0.060 in (1.5 mm) in plastic; height under about 10× thickness

Size undercuts to standard cuttersMatch standard keyseat, T-slot and 45° or 60° dovetail cutters; keep about 4× the undercut depth clear to any opposing wall

Use standard hole sizesStandard fractional, letter, number or metric drills; reamed holes at standard reamer sizes

Limit drilled hole depthAbout 4× diameter standard; up to 10× with peck drilling; beyond that, gun drilling

Allow a drill point on blind holes118° or 135° cone at the bottom; dimension depth to the full diameter

Limit tapped thread depthAbout 1.5× diameter in steel; up to 2× in aluminum and plastic

Drill past the last full threadAt least 3 pitches, or about 0.5× diameter, of extra drilled depth in blind tapped holes

Chamfer or break edges0.010–0.020 in (0.25–0.5 mm) × 45°; call out "break sharp edges" for the rest

Put features on as few faces as possibleOne or two setups on 3-axis; five-sided parts on 5-axis

Tolerance only what mattersDefault to ±0.005 in (±0.13 mm) or ISO 2768-m; tighten only fits and datums

Feature

Typical

Tight

Cost of tight

Milled linear dimension

±0.005 in (±0.13 mm)

±0.001 in (±0.025 mm)

Moderate

Turned diameter

±0.002 in (±0.05 mm)

±0.0005 in (±0.013 mm)

Moderate

Bored or reamed holeReaming or boring adds a tool

+0.001/−0 in (+0.025/−0 mm)

ISO 286 H7, about +0.0007/−0 in at 0.5 in

Moderate

Hole position

Ø0.010 in (0.25 mm)

Ø0.002 in (0.05 mm)

Moderate

FlatnessTight flatness usually means grinding

0.002 in (0.05 mm) per 4 in

0.0005 in (0.013 mm)

High

Surface finish

Ra 63–125 µin (1.6–3.2 µm)

Ra 16–32 µin (0.4–0.8 µm)

Moderate

Tapped thread class

2B (UN) or 6H (metric)

3B or 4H5H

Moderate

Angles

±0.5°

±0.1°

Moderate

What are the cnc machining design rules?

How deep can a pocket be for a given corner radius?