Engineering explainer

Micro Experience Revolutionized CNC: What Changes Below 1 mm

The micro experience revolutionized CNC by moving the limits of what a small part can hold. It is not a smaller version of ordinary milling. Tool diameter, runout, chip evacuation and thermal drift all move the numbers that decide whether a feature holds tolerance. This page explains the mechanism for design engineers and buyers who have to judge whether a part belongs on a micro machine or on a standard 3-axis mill.

Get Instant Quote Talk to an Engineer

Ø0.1–1 mm tool range±0.005 mmRa 0.2–0.8 μm16 five-axis centers

Micro experience revolutionized CNC on a small aerospace prototype part

On this page

1
Why micro tools lose rigidity before they lose accuracy
2
Where ±0.005 mm actually holds and where it does not
3
Deep cavities, small holes and the depth-to-diameter wall
4
Which materials behave and which fight back
5
How you know the micro feature is actually right
6
Micro machining vs standard 3-axis: pick by feature, not by part size

Mechanism

Why micro tools lose rigidity before they lose accuracy

A 0.5 mm end mill does not fail because the control cannot resolve a small move. It fails because stiffness scales faster than size. Deflection under a side load rises roughly with the cube of the length-to-diameter ratio, so a tool held 10 diameters deep behaves nothing like the same tool held 3 diameters deep. On a 0.5 mm cutter, a 5 mm gauge length is already a long reach.

That number, not the machine's positioning spec, usually sets the depth of cut. Many micro features are cut with an axial depth of 0.02–0.05 mm and a radial engagement under 10 percent of the cutter diameter. The tool survives because the chip is thin, not because the machine is stiff enough to push harder.

Spindle speed matters for a different reason. A 0.5 mm two-flute cutter in aluminium wants a surface speed around 200–300 m/min, which lands near 150,000 rpm. No spindle here runs that fast. So the shop runs 20,000–40,000 rpm and accepts a lower chip load, around 0.002–0.005 mm per tooth.

The practical result: micro work is slow by design. Feed rates of 100–400 mm/min are normal, and a cavity that looks trivial on screen can take 40 minutes of cutting. If the quote seems high for a small part, this is usually why.

1
Rigidity firstCheck reach before you check tolerance.
2
Chip load sets the limit0.002–0.005 mm per tooth on small cutters.
3
Speed is a compromiseSpindles top out well below the ideal surface speed.

Tolerances

Where ±0.005 mm actually holds and where it does not

±0.005 mm is a real capability here, but it is a capability, not a default. It holds on features that are cut in one setup, on a machine with a stable thermal state, with a cutter that has been measured and entered into the offset table. It does not hold across two setups on a thin wall.

Thermal drift is the quiet one. A spindle running for three hours warms and grows. On a 20 mm part, a 5 °C swing in the shop and a warming spindle can move the tool tip by 0.003–0.008 mm between the first part and the fiftieth. That is the entire tolerance band. Shops that hold tight numbers either run a controlled temperature or re-probe the workpiece between operations.

Thin walls behave differently again. A 0.3 mm wall in aluminium will deflect away from the cutter under cutting force and spring back after. The cut looks clean and measures undersize. The fix is not more speed. It is a lighter radial engagement, a sharper tool, and sometimes a support wax or a leaving-rib strategy.

So the honest answer for a drawing callout of ±0.005 mm is a question: on which feature, in how many setups, and how thick is the material around it. Those three answers decide whether the number is routine or expensive.

1
One setupTight tolerances are cheapest when features are reachable in a single orientation.
2
Wall thicknessBelow 0.5 mm, deflection dominates the result.
3
Thermal stateLong runs drift more than short ones.

Geometry

Deep cavities, small holes and the depth-to-diameter wall

The single most useful design number in micro work is depth divided by diameter. For a drilled or milled hole under 1 mm, a ratio of 3:1 is comfortable, 5:1 is possible with peck cycles and through-spindle coolant, and beyond 8:1 the tool breakage rate climbs fast enough that the shop will usually quote a different process.

Chip evacuation is the reason, not tool strength. At 0.5 mm diameter, the flute space is tiny and a packed chip recuts, heats, and snaps the tool. High-pressure coolant or an air blast through the spindle is what keeps the ratio usable. Shops without through-spindle coolant are limited to roughly 4:1 on the same feature.

Corner radii follow a simple rule: the smallest internal radius must be at least half the cutter diameter. If a pocket corner is drawn at 0.2 mm, the shop must use a 0.4 mm or smaller tool, which then limits the depth and the achievable finish. Rounding an internal corner from 0.2 mm to 0.5 mm can cut cycle time by half.

Draft, burrs and entry points also matter. A micro slot open at both ends machines far more reliably than a blind slot of the same width, because the cutter enters from the side and the chip leaves the same way.

1
3:1 is easyUnder 1 mm diameter, 3:1 depth is routine.
2
8:1 is a riskBreakage rises sharply without high-pressure coolant.
3
Corner radius ≥ half the toolSmaller corners force smaller, weaker cutters.

Materials

Which materials behave and which fight back

Aluminium is the easy case. 6061, 7075 and 6082 all cut cleanly at small diameters, hold a good finish, and tolerate the light chip loads that micro tools need. If a design can be made in aluminium, the micro route is usually predictable.

Copper and brass are nearly as friendly, and they hold sharper edges. C36000 brass is common for small fluidic and connector parts. Pure copper C110 galls a little more and needs a sharper tool and a slightly richer lubricant, but it is still a routine material at this scale.

Stainless is where the cost moves. 316L work-hardens, so a micro cutter that rubs instead of cutting will harden the surface and then break. Cutting parameters shift to a slightly heavier chip load than feels comfortable, with no dwell. 17-4PH in the H900 condition is harder again and usually needs carbide with a coating and a shorter reach.

Titanium TC4 (Ti-6Al-4V) and Inconel are the hard end. Heat stays at the cutting edge because the chip carries little of it away, so tool life drops to minutes rather than hours on the smallest cutters. These parts are machinable, but the drawing should give the shop every allowance it can: fewer tight radii, fewer deep features, and a finish callout that reflects the function.

1
Aluminium and brassPredictable at 0.3 mm and below.
2
316LMust cut, never rub, or the surface work-hardens.
3
Ti and InconelTool life is measured in minutes on the smallest cutters.

Inspection

How you know the micro feature is actually right

A 0.5 mm slot cannot be checked with calipers. It is checked with an optical comparator, a vision system, or a toolmaker's microscope at 20× to 50× magnification. That changes the inspection plan, and it changes what a first article report looks like.

The practical consequence is that inspection is a larger share of the cost than on a normal part. A part with six micro features may spend more time under the microscope than on the machine. Shops that quote micro work without a metrology line in the quote are usually planning to sample, not to verify.

Process control matters as much as final inspection. In-process probing between operations catches drift before the run is finished. On a 200-piece run of a 0.8 mm feature, an operator who measures every twentieth part will catch a thermal trend; one who measures at the end will not.

For anything regulated, the paper trail is part of the deliverable. Material certificates, inspection reports and a dimensional layout on request are normal. We hold ISO 9001:2015, IATF 16949:2016, ISO 13485:2016 and ISO 27001:2022, and uploads are treated as confidential with an NDA available on request.

1
Optical, not tactileVision or microscope at 20×–50× for sub-millimetre features.
2
Inspection is a cost lineExpect it to be a visible share of the quote.
3
Reports on requestMaterial certs and dimensional layouts.

Selection

Micro machining vs standard 3-axis: pick by feature, not by part size

Judged on the smallest feature in the drawing, not the overall envelope.

Drawing condition	Micro machine	Standard 3-axis
Smallest internal radius under 0.3 mm	Required	Not reachable
Feature size 0.1–1 mm	Cut in one setup	Often impossible
Hole depth-to-diameter above 5:1 under 1 mm	Possible with high-pressure coolant	Risky
Overall size up to 4,000 mm	Not suitable	Standard route
Wall thickness above 2 mm	Overkill	Cheaper and faster
Tolerance ±0.01 mm or looser	No advantage	Better value
Quantity 10,000+ of a small part	Slow per part	Compare with die casting

When the micro route is the right call and when it is not

If the smallest feature is under 1 mm or the tightest radius is under 0.3 mm, the micro route is the only one that works and the price reflects it. If the smallest feature is above 2 mm and the tolerance is ±0.01 mm or looser, a standard 3-axis machine will be faster and cheaper, and the micro experience buys you nothing.

Get Instant Quote Talk to an Engineer

FAQs

Questions engineers ask before sending a micro part

What is the smallest feature you can cut?

It depends on material and depth more than on the machine. In aluminium, features around 0.1–0.2 mm wide are cut routinely with cutters down to 0.1 mm. In stainless and titanium, the practical floor is closer to 0.3 mm because tool life and cutting force both get worse.

Depth matters as much as width. A 0.2 mm slot 0.4 mm deep is a different job from the same slot 3 mm deep.

Why is a tiny part sometimes more expensive than a large one?

Because the cost driver is the smallest feature, not the envelope. A 10 mm part with a 0.2 mm internal radius may need a 0.3 mm cutter, light passes and optical inspection. A 300 mm bracket with generous radii runs on a 3-axis machine in a fraction of the time.

Setup, tool changes and metrology are fixed costs that do not shrink with part size.

Can you hold ±0.005 mm on every dimension?

No, and any shop that says yes on a whole drawing is worth a second look. ±0.005 mm is achievable on features cut in one setup with a stable thermal state and a measured tool. Across multiple setups, or on thin walls, the realistic band widens.

Send the drawing and we will mark which dimensions can hold tight and which should be opened up.

Does micro machining work for prototypes and small runs?

Yes. There is no minimum order quantity here, from a single prototype to 10,000+ part runs. For a first article, the value is in proving the geometry before committing to a longer process.

A quotation and free DFM analysis come back within 12 hours, so a design iteration is usually a same-week loop.

What file format and detail should I send?

STEP or IGES for the solid, plus a PDF drawing that marks which dimensions are functional and which are reference. GD&T callouts help, especially datum choices, because they tell us what the part actually has to do.

If a feature is cosmetic rather than functional, say so. It often changes the tool and the pass strategy.

What surface finish is realistic on a micro feature?

Ra 0.8–1.6 μm is the normal machined range, and Ra 0.2–0.8 μm is achievable with finer passes and a sharp tool. On very small features the finish is limited by the cutter radius and by how much the wall deflects.

If a micro feature needs a mirror finish, bead blasting, polishing or electroless nickel are usually applied after machining rather than chased on the machine.