Micro CNC milling explains how tiny features get cut
This page is for engineers who need slots, pockets and holes smaller than a grain of rice. We cover how micro CNC milling removes material, which dimensions a 0.2 mm cutter can really hold, and when the process stops being the right answer.
What actually happens at the cutting edge
Micro CNC milling is not a small version of a normal milling job. It is a different balance of forces. A 0.5 mm end mill spins at 30,000 to 60,000 rpm and takes chips only a few microns thick. At that scale the edge radius of the tool is a large share of the chip thickness, so the tool cannot simply slice the material. It has to press until the material shears.
That pressing action creates the main problem. Below a certain feed per tooth, the tool rubs instead of cutting. Heat builds in a very small volume, the edge dulls, and the surface turns rough. The practical fix is to keep the feed per tooth high enough that each edge bites. Many shops run micro tools at 0.5 to 2 percent of the tool diameter per tooth. For a 0.5 mm cutter that is roughly 2.5 to 10 μm per tooth.
Tool runout matters more than spindle speed on these jobs. A 5 μm runout on a 0.5 mm tool means one flute does most of the work. That flute wears twice as fast, and the slot comes out wider than the cutter. We check runout on every micro setup with a dial indicator before the first cut. If it reads above 5 μm, the holder gets changed.
Chip evacuation sets the floor on how small a pocket can go. A 0.3 mm wide slot has almost no room for chips to leave. Compressed air at 0.4 to 0.6 MPa and a shallow depth of cut of 0.02 to 0.05 mm per pass keep the flutes clear. Without that, the tool recuts its own chips and snaps within a few seconds.
What micro CNC milling can and cannot hold
A common claim is that micro milling holds ±0.005 mm on everything. That figure is real at GreatLight, but it describes the best case on a stable setup, not a default on every feature. The tolerance a micro feature can hold depends on the feature itself. A 0.5 mm wide slot in aluminium 6061 will hold ±0.01 mm more reliably than a 0.2 mm wide slot in 316 stainless. The narrower and deeper the cut, the more the tool deflects and the wider the tolerance band becomes.
Aspect ratio is the practical limit engineers run into first. Tool deflection grows with the cube of the length-to-diameter ratio. A 0.5 mm cutter at 3× diameter depth is comfortable. At 8× it starts to wander and needs a stepped approach with light finish passes. Past 10×, the cutter will chatter or break no matter how slow you run it.
Surface finish follows the same logic. We hold Ra 0.2–0.8 μm on micro features when the tool is fresh and the stepover is small. On a deep slot in hardened steel, Ra 1.6–3.2 μm is the honest number without a separate finishing pass. Promising a mirror finish inside a 0.3 mm slot is not realistic.
Wall thickness has its own floor. A 0.1 mm wall in aluminium can be milled, but it will move when the clamps come off. We usually design micro walls at 0.2 mm minimum, or leave them thick and take the last 0.05 mm off after stress relief.
How a micro job is planned before the spindle turns
Planning a micro CNC milling job starts with the drawing. We look for the smallest internal radius, the deepest pocket, and the tightest tolerance callout. Those three numbers decide the tool list. If the smallest radius is 0.15 mm, the largest cutter that can reach it is 0.3 mm. That one tool then sets the stepover, the pass count, and the cycle time.
We run a DFM review on every file and return it within 12 hours. Most micro parts come back with two or three changes: open a corner radius from 0.1 mm to 0.2 mm, reduce a pocket depth from 5 mm to 3 mm, or add a small chamfer so the tool does not have to plunge into a square corner. These changes cut cycle time without touching function.
Fixturing is where micro jobs fail. A vise jaw with 0.05 mm of flex will let the part move during a 0.03 mm finishing pass. We use custom soft jaws machined in place, or vacuum chucks for thin plates. The part is measured on the machine after roughing and again after finishing, so any shift shows up before the part comes off.
Workholding and tool setting together decide whether the first part is good. A 0.3 mm cutter that touches off 0.02 mm too deep will scrap the feature. We set tools with a laser presetter and confirm the first article with a video measuring system before running the rest of the batch.
Which materials behave well at the micro scale
Aluminium is the easiest place to start. Grades 6061, 7075 and 2024 cut cleanly with a 0.3 mm tool at 40,000 rpm and leave a good finish. Brass C36000 and copper C110 also machine well, though copper tends to stick to the cutting edge and needs a sharper tool and more coolant.
Stainless 303 and 316L are workable but slower. The material work hardens right at the cutting edge, so any rubbing pass makes the next pass harder. We take a minimum feed per tooth of about 1 percent of the tool diameter in stainless and never let the cutter dwell. 17-4PH in the H900 condition is harder still and is usually finished with a fresh tool.
Titanium TC4 (Ti-6Al-4V) and Inconel are the difficult end. Both hold heat at the edge, and a 0.4 mm cutter in titanium will not survive a deep pass. We keep depth of cut under 0.03 mm, run high pressure coolant, and accept cycle times three to four times longer than the same feature in aluminium.
Micro milling versus other routes for small features
Use this table to pick a process before you send a drawing.
| Route | Best feature size | Typical tolerance | When it wins |
|---|---|---|---|
| Micro CNC milling | 0.2–2 mm slots and holes | ±0.005 to ±0.02 mm | Metal parts, tight tolerance, low to mid volume |
| Conventional CNC milling | Above 2 mm features | ±0.01 to ±0.05 mm | Larger parts, faster cycle, lower tool cost |
| Wire EDM | Through slots from 0.1 mm | ±0.003 mm | Hardened steel, straight through cuts |
| Micro die casting | Above 1 mm walls | ±0.05 mm | High volume, one alloy, less precision |
| 3D printing | From 0.1 mm layers | ±0.1 mm | Plastic prototypes, no load bearing |
When micro CNC milling is the right call
If your smallest feature is 0.2 mm or larger, the part is metal, and you need ±0.005 to ±0.02 mm, micro CNC milling is the right route from one prototype to 10,000+ parts. If the feature is a straight through slot in hardened steel, wire EDM holds tighter and costs less. If the wall is thinner than 0.2 mm or the part is plastic, look at 3D printing instead.
Questions engineers ask before sending a micro part
What is the smallest tool you run?
We run end mills down to 0.2 mm diameter in aluminium and brass, and 0.3 mm in stainless and titanium. Below that, tool breakage drives the cost up faster than the precision improves, so we usually suggest a different route for features under 0.15 mm.
The smallest practical feature is a 0.2 mm wide slot, and only when the depth stays under 1 mm. Deeper than that, the aspect ratio pushes the tool past its limit.
Does micro CNC milling work for hard materials?
Yes, with limits. Hardened tool steel and 17-4PH machine well at micro scale if the depth of cut stays under 0.03 mm and the tool is fresh. Inconel and titanium are possible but slow, and we quote them with a longer cycle.
If the part is already heat treated above 45 HRC and the feature is a through slot, wire EDM is usually cheaper and more accurate.
How do you measure micro features?
We use a video measuring system for features under 0.5 mm and a CMM with a 0.5 mm stylus for larger ones. Both run against the drawing before the batch ships. Every part gets a final inspection, and reports are available on request.
For a 0.2 mm slot, the measuring uncertainty is a real share of the tolerance. We tell you the measurement method up front so the numbers on the report match what your incoming inspection will see.
Can you hold ±0.005 mm on a 0.2 mm slot?
No. ±0.005 mm is realistic on features around 1 mm and larger with a stable setup. On a 0.2 mm slot, the honest band is ±0.01 to ±0.02 mm, because tool deflection and runout take up most of the budget.
We would rather quote the real number than win the job on a tolerance we cannot repeat across a batch.
What file format and information do you need for a quote?
Send a STEP or IGES file plus a 2D drawing with the critical dimensions marked. Tell us the material, the quantity, and which tolerances actually matter to function.
We return a quotation and a free DFM analysis within 12 hours. Production can start within 24 hours of approval, and parts ship in 3–5 days. No minimum order quantity, from one prototype to 10,000+ part runs. Uploads are secure and confidential, and an NDA is available on request.
When should I not use micro CNC milling?
Skip it when the smallest feature is above 2 mm and the tolerance is loose. Conventional milling is faster and cheaper. Skip it for straight through slots in hardened steel, where wire EDM wins. Skip it for plastic parts with thin walls, where 3D printing or vacuum casting gives a better result.
If your part is a 0.1 mm wall in any metal, the wall will move after machining. Redesign it thicker or pick another process.
Send a micro part and get a real tolerance back
Upload your STEP file and drawing. We return a quotation and a free DFM analysis within 12 hours, with the tolerance we can actually hold on each micro feature.
12-hour quote±0.005 mm on stable features100% inspectionNo minimum order quantity
More from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
