How Small Can a CNC Machine Cut?
Most shops stop around 0.5 mm features. A rigid 5-axis setup with the right micro tool can hold 0.05 mm slots and Ø0.1 mm holes. This guide shows the factors that set the floor for a CNC machine cut and the steps to get there.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
Key takeaways
What Sets the Minimum Size of a CNC Machine Cut
Every micro job starts with the same question: how small can a CNC machine cut before the process stops being reliable? The honest answer is a range, not a number. On a well-maintained 5-axis machining center with a rigid frame, a 0.05 mm slot or a Ø0.1 mm hole is repeatable. On a light 3-axis router with a stock collet, the practical floor is closer to 0.5 mm.
The gap comes from four things that stack on top of each other: machine rigidity, tool diameter and runout, control resolution, and the material in the vise. Change one and the floor moves. A 0.2 mm end mill in a hydraulic chuck on a granite-bed machine behaves nothing like the same cutter in a worn drill chuck on a benchtop mill.
Feature size is also not the same as tolerance. A shop can hold ±0.005 mm on a 10 mm bore and still fail on a 0.1 mm slot, because the slot depends on tool diameter, not on axis positioning. When you review a quote, ask which one the shop is quoting. It matters more than the machine list.
One more distinction: a through slot, a blind pocket, and a sharp internal corner are three different problems. A 0.1 mm cutter can mill a 0.1 mm slot. It cannot produce a true 90° internal corner at that width. The corner radius equals the tool radius unless you add EDM or a corner-relief design.
- 1Rigid frame first
- 2Runout under 0.002 mm
- 3Resolution, not just accuracy
- 4Material sets the depth
Micro Tooling: Where a Small CNC Machine Cut Breaks Down
Tool diameter is the most visible limit. Micro end mills run from Ø0.1 mm down to Ø0.01 mm, but the smaller you go, the less room there is for error. A cutter under 0.3 mm snaps from side load long before it wears out. Runout of 0.001 mm on a 0.1 mm tool means one flute does almost all the cutting, and that flute fails in minutes.
Tool holding decides whether the cutter survives. Hydraulic chucks and precision collets hold runout near 0.002 mm. Standard drill chucks sit at 0.02–0.05 mm, which is fine for a 6 mm cutter and fatal for a 0.2 mm one. If your shop cannot tell you the measured runout at the spindle, they are guessing.
Cutting parameters for micro tools are conservative on purpose. Start at 0.3–0.5 × tool diameter axial depth and 0.2–0.3 × diameter radial width. Spindle speed climbs to 20,000–60,000 rpm to keep chip load per tooth in the 0.001–0.005 mm range. Feed too slow and the tool rubs; too fast and it snaps.
Chip evacuation is the quiet killer. A 0.05 mm chip sitting in a 0.1 mm slot gets recut, welds to the edge, and tears the wall. Air blast or oil mist at 4–6 bar clears micro chips better than flood coolant, which can push them back into the cut. On deep micro pockets, peck or add a retract pass every 0.2 mm of depth.
- 1Match tool to slot
- 2Check runout at the spindle
- 3Add a retract pass
- 4Air blast over flood
Material Rules for Micro Cutting
Soft materials reach smaller features because they push back less. Aluminium 6061, 7075, POM, ABS, and PEEK take a 0.05 mm slot with a sharp two-flute cutter and light chipload. Surface finish lands around Ra 0.8–1.6 μm on aluminium and Ra 1.6–3.2 μm on PEEK without extra work.
Stainless and titanium are slower but not impossible. Ti-6Al-4V and 17-4PH reach 0.1 mm features with TiAlN or AlCrN coated micro tools, oil mist, and reduced depth of cut. The trade is time: expect three to five times the cycle of the same feature in aluminium, plus more tool changes.
Copper and brass cut cleanly at small sizes but stick to the tool edge. Beryllium copper and C110 need sharp, polished flutes and a light cutting oil. If the edge builds up, the slot width drifts, and a 0.15 mm feature can measure 0.18 mm after a few parts.
Plastics behave differently again. PMMA and PC can chip or craze at the edge if the feed is too high, while POM cuts clean but burrs if the tool is dull. When the material is unknown, run a test cut on scrap before committing a full batch. Two minutes of scrap saves a scrapped lot.
- 1Aluminium and PEEK
- 2Ti-6Al-4V and 17-4PH
- 3Copper alloys
- 4Plastics
How Small Each Machine Type Can Cut
A 3-axis mill with a rigid frame and good spindle handles 0.2–0.5 mm features on soft material. That covers most sensor housings, connector bodies, and small fixture plates. It struggles when the part needs four or five faces cut in one setup, because each refixture adds position error that eats the micro budget.
A 4-axis machine adds a rotary table, so you can cut features on four sides without losing the datum. For a small part with a Ø0.2 mm cross-hole and a slot on the same axis, that saves a setup and keeps the two features aligned. Feature floor stays around 0.1–0.3 mm depending on the material and tool access.
A simultaneous 5-axis center is where 0.05 mm slots become routine. The tool can stay normal to a curved surface, which keeps chip load even and reduces deflection on thin walls. It also reaches undercuts and angled faces in one setup. For micro fluidic channels, medical needles, and optical mounts, this is the setup that holds the print.
Machine class is not the only variable. A 5-axis center with a tired spindle bearing cuts worse than a fresh 3-axis mill. Ask about spindle runout, thermal compensation, and how often the machine is recalibrated. Those answers predict the real floor better than the spec sheet.
- 13-axis
- 24-axis
- 35-axis
- 4Condition matters
Five Steps to Plan a Micro CNC Machine Cut
- 11. Define the smallest feature and its toleranceWrite down the slot width, hole diameter, and corner radius on the drawing. Separate the features that must be 0.05 mm from the ones that can be 0.2 mm. Mark which tolerances are functional and which are cosmetic.
- 22. Pick the tool before the machineChoose a cutter at or just under the slot width. For a 0.1 mm slot, use a Ø0.1 mm two-flute end mill. Confirm runout under 0.002 mm in the holder. If no cutter fits the feature, redesign the feature or plan for EDM.
- 33. Set conservative cutting parametersStart at 0.3–0.5 × diameter axial depth, 0.2–0.3 × diameter radial width, and 0.001–0.005 mm feed per tooth. Raise spindle speed to 20,000–60,000 rpm for tools under 0.5 mm. Run a test cut on scrap and measure before the first part.
- 44. Control chips and heatUse air blast or oil mist at 4–6 bar, not flood coolant. Add a retract pass every 0.2 mm of depth on blind pockets. Check the slot floor with a loupe after the first part to catch recut chips early.
- 55. Inspect the micro feature, then releaseMeasure with an optical comparator or vision system, not calipers. Calipers squeeze a 0.1 mm slot and read wrong. Check the first part, the middle part, and the last part of the run for tool wear drift.
Feature Size vs Tool, Machine, and Material
Use this to sanity-check a design before you send it out for quote.
| Target feature | Tool diameter | Machine | Typical material |
|---|---|---|---|
| 0.5 mm slot | Ø0.4–0.5 mm | 3-axis, rigid | Aluminium, ABS, POM |
| 0.2 mm slot | Ø0.2 mm | 4-axis or 5-axis | Aluminium, brass, PEEK |
| 0.1 mm slot | Ø0.1 mm | 5-axis, granite bed | Aluminium, 17-4PH, Ti-6Al-4V |
| 0.05 mm slot | Ø0.05 mm | 5-axis, hydraulic chuck | Aluminium, PEEK only |
| Ø0.1 mm hole | Ø0.1 mm drill | 5-axis with high-speed spindle | Aluminium, brass, plastics |
| 0.05 mm wall | Ø0.1–0.2 mm | 5-axis, light radial pass | Aluminium, PEEK, PMMA |
The design decides more than the machine
A 0.05 mm feature is possible when the tool, holder, machine, and material all support it. Redesign one feature and you can often cut the cost in half without losing function.
Frequently Asked Questions
What is the smallest feature a CNC machine can cut in production?
In repeatable production, 0.05 mm slots and Ø0.1 mm holes are realistic on a rigid 5-axis center with micro tooling. Below that, the process becomes a lab exercise rather than a production route.
The limit depends more on tool diameter and runout than on the machine's stated accuracy. If the smallest cutter you can hold true is 0.2 mm, that is your real floor.
Can micro cutting handle titanium and mold steel?
Yes, with coated micro end mills in TiAlN or AlCrN, oil mist cooling, and reduced depth of cut. Expect 0.1 mm features rather than 0.05 mm in these materials.
Cycle time runs three to five times longer than the same feature in aluminium, and tool changes are more frequent. Budget for both.
Why does my 0.1 mm slot come out wider than drawn?
The usual causes are tool runout above 0.002 mm, edge buildup on the cutter, or a worn tool. Runout makes one flute cut deeper and pushes the wall outward.
Check runout at the spindle, switch to a polished flute for copper alloys, and replace the cutter before the edge rounds over.
Do I need a 5-axis machine for small features?
No. A rigid 3-axis mill holds 0.2–0.5 mm features well. The 5-axis advantage appears when features sit on curved or angled surfaces and must be cut in one setup.
If the part is flat and the features are simple, a 3-axis machine with good tooling is the cheaper and faster route.
How do you inspect a 0.05 mm feature?
Optical comparators, vision systems, and toolmaker microscopes are the standard tools. Calipers and micrometers squeeze the feature and give misleading readings at that scale.
For critical micro features, we check the first, middle, and last parts of a run to catch tool wear drift before the lot is complete.
Send us the micro feature and we will tell you if it cuts
Upload the drawing and we will review tool access, feature size, and material against our 5-axis capability. Quotation and free DFM analysis within 12 hours.
12-hour quote±0.005 mm toleranceNo minimum order quantity
More micro machining notes
We publish setup notes, tooling trials and inspection data from the factory floor.
