Minimum Feature Sizes, Tools and Tolerances in Micro Milling and Turning

By the Micropartz editorial team · Published October 26, 2026

Designing a micro part means working with limits that do not exist at normal scale. A 0.2 mm end mill bends, a 5 μm spindle runout is significant and a burr can be as big as the feature. This guide gives typical minimum feature sizes, tool sizes and tolerances for micro milling and micro turning, and the design rules that keep a part machinable. If you are new to the field, the micro machining buyer’s guide is the better starting point.

Why the rules change below 1 mm

Three physical effects set the limits in micro machining.

Tool stiffness. The stiffness of an end mill falls roughly with the fourth power of its diameter. Halve the diameter and the tool is about 16 times less stiff. A 0.2 mm tool deflects under forces that a 2 mm tool would not notice, which shows up as tapered walls and undersized features.

Minimum chip thickness. Every cutting edge has a small radius. When the chip load per tooth becomes comparable to that edge radius, typically a few microns, the tool stops cutting cleanly and starts to plough and rub. That limits how fine a finishing pass can be and causes burrs.

Runout and thermal growth. Runout of 5 μm on a 6 mm tool is minor. On a 0.2 mm tool it means one flute does most of the cutting and wears or breaks early. Spindles also grow a few microns as they warm up. Micro machining shops use precision shrink-fit or collet holders, check runout per tool and run warm-up cycles before critical work.

Typical minimum feature sizes

The table below gives typical production limits in micro machining shops. Specialists go further, usually at higher cost.

Feature	Typical production minimum	Specialist limit	Main constraint
Milled slot width	0.3 mm	about 0.05 mm	Tool diameter and depth
Inside corner radius	0.1 to 0.15 mm	about 0.025 mm	Tool radius
Drilled hole	⌀0.2 mm	about ⌀0.05 mm	Drill strength, chip removal
Wall thickness, metal	0.15 mm	about 0.05 mm	Deflection, vibration
Wall thickness, plastic	0.3 mm	about 0.15 mm	Heat and clamping
Turned diameter	⌀0.3 mm	about ⌀0.1 mm on short length	Deflection, bar support
Thread	M0.8 / 0-80 UNF	M0.3	Tool form, gauge availability
Overall part envelope	1 mm	below 1 mm	Handling and workholding

Values are typical for metals unless noted, not a guarantee. The smallest feature of 0.3 mm, holes from ⌀0.2 mm and walls from 0.15 mm are the practical planning numbers for most RFQs.

Micro tools, depth and aspect ratio

Diameter is not the only question. Depth decides whether a feature is realistic.

Tool diameter	Typical max depth with standard tool	Typical spindle speed
1.0 mm	3 mm	20,000 to 40,000 rpm
0.5 mm	1.5 mm	30,000 to 50,000 rpm
0.3 mm	0.6 to 0.9 mm	40,000 to 60,000 rpm
0.2 mm	0.3 to 0.6 mm	40,000 to 80,000 rpm
0.1 mm	0.15 to 0.3 mm	60,000 rpm and above

Typical values for metals. Long-neck tools and special strategies extend depth at lower feed rates.

For drilling, the equivalent rule is depth to diameter. Up to about 5 times diameter is routine, 10 times is achievable with peck drilling, and beyond that shops use special drills, gun drilling methods or EDM. A ⌀0.2 mm hole 2 mm deep is at the edge of normal production. The same hole 5 mm deep is a specialist job.

Tolerances in micro milling and turning

Tolerances in micro machining are best read as three tiers.

Tier	Linear tolerance	Where it applies	Effect on cost
General	±0.02 to ±0.05 mm	Non-functional features	Baseline
Production precision	±0.01 mm	Most dimensioned features	Moderate
Selected features	±0.005 mm	Fits, datums, optical and fluidic features	Extra passes and full measurement
Specialist	±0.002 mm and below	Bores, ferrules, gauge parts	Grinding, lapping or climate-controlled work

Typical values, not a guarantee.

Turning holds diameters tighter than milling holds positions, because a turned diameter is generated by the spindle rotation. On Swiss-type work, diameters of ±0.005 mm and shaft fits of h5 are routine, as described in the guide on Swiss-type turning. In milling, position tolerances depend on machine accuracy, temperature and setup, so ±0.005 mm on hole position is a selected-feature tolerance.

Surface finish follows the same logic. Ra 1.6 μm is typical for micro milled faces, Ra 0.8 μm is achievable with finishing passes, and below that shops usually add polishing, lapping or electropolishing.

Under ISO 286, the standard tolerance for sizes over 3 up to 6 mm is 5 μm at IT5, 8 μm at IT6 and 12 μm at IT7. That is a useful sanity check: if you are asking for IT5 on a milled feature, you are asking for specialist work.

Design rules that keep micro parts machinable

Most cost in micro parts is decided on the drawing. These rules come up again and again in DFM feedback.

• Give inside corners a radius. Use at least the radius of the tool that can reach the pocket depth, and add a margin. Sharp inside corners need EDM.
• Keep pocket depth to about 3 times the smallest tool diameter. Deeper pockets need long-neck tools, slow feeds and more scrap risk.
• Support thin walls. A 0.15 mm wall should be short or backed by material during machining. Tall thin walls chatter.
• Put tight tolerances only where the function needs them. Use ISO 2768 or a general tolerance block for the rest.
• Define the edge condition. State whether edges must be burr-free, broken to a given size or left sharp, and how that is inspected.
• Choose datums you can measure. A micro part often cannot be probed where a normal part would be. Datums on turned diameters or faces that a CMM or vision system can reach save arguments later.
• Tolerance holes by function. A clearance hole does not need the same tolerance as a dowel fit.

Hypothetical example: an optical mount of 8 x 8 x 6 mm in 6061 has four ⌀0.4 mm holes at ±0.005 mm position, a 0.2 mm wide slot 1 mm deep and sharp inside corners. DFM feedback would typically suggest opening the slot to 0.3 mm or reducing its depth, adding a 0.1 mm corner radius and relaxing two of the four hole positions to ±0.01 mm. Each change cuts cycle time and inspection with no loss of function.

For drawing changes that cut cost, see design for micro machining.

See also: the micro milling reference page for tool diameter, depth, runout and spindle speed tables.

Workholding and handling at micro scale

A feature is only as accurate as the way the part is held while it is cut. At micro scale, clamping becomes a design constraint.

• Clamping distortion. A thin-walled 5 mm housing clamped in a vise can deform by more than its tolerance, then spring back when released. Shops use soft jaws, custom fixtures, vacuum or low-melt adhesives to hold parts gently.
• Machining from a larger blank. Many micro milled parts are machined while still attached to a bigger piece of stock, then separated in a final operation. That keeps the part rigid, but the separation point leaves a witness mark. Tell the shop where a witness mark is acceptable.
• Tabs and frames. Several small parts can be milled from one plate and held by small tabs, like a sprue on a model kit. Tabs must be removed and the spots finished, which adds handling.
• Part collection. On Swiss-type lathes, finished parts drop into a catcher. Without one, tiny parts get lost in the chip conveyor or damaged by falling.

Holding method	Suits	Watch out for
Precision collet	Turned and round parts	Marks on the clamped diameter
Custom soft jaws	Small prismatic parts	Setup cost, distortion if overtightened
Vacuum fixture	Thin flat parts	Limited holding force, small tools only
Part held in parent stock	Complex 5-axis micro parts	Witness mark at the separation point
Tabs in a plate	Many identical flat parts	Tab removal and finishing

Typical practice for orientation.

For the buyer, this means two things. Mark the surfaces where clamp marks, witness marks or tab remnants are not allowed. And accept that a shop may ask to add a small feature, such as a flat or a boss, to hold the part. It often makes the rest of the tolerances easier to meet.

Measuring what you specify

A feature you cannot measure cannot be accepted. For features below about 0.5 mm, standard CMM styli may not fit, and contact force can deflect thin walls. Vision systems, measuring microscopes and pin gauges take over. The guide on how micro parts are measured goes into detail. For now, the rule is simple: agree the measurement method for every critical feature before production.

Next step

Use the tolerance and materials reference to check your drawing against typical values. When you are ready, send an RFQ with your smallest feature and tightest tolerance stated. Micropartz matches it with up to 3 micro machining shops that fit and replies within 24 business hours.

Frequently asked questions

Reviewed against

• ISO 286-1:2010, ISO code system for tolerances on linear sizes
• ASME Y14.5-2018, Dimensioning and Tolerancing
• Wikipedia: Engineering tolerance

Numbers in this guide are typical values for orientation. The drawing, the material certificate and the matched shop set the real ones.

Keep reading

• Micro Machining: A Buyer's Guide to Very Small Precision Parts
• Swiss-Type Turning for Micro Parts: When a Sliding-Head Lathe Is the Right Call
• How Micro Parts Are Measured: CMM, Optical and Vision Inspection