Micro-Hole Drilling: Holding 0.5 mm Holes On Centre
By CHX Metal Engineering Team · Published 2026-11-18
Below about 1 mm, a hole is decided by tool runout rather than by the machine. Runout past roughly 10 µm loads one flute and the hole walks; past L/D 5 the flutes cannot clear chips without pecking. Our 70 Tsugami Swiss-type units drill from 0.3 mm, and fit holes hold ±0.005 mm.
The hole decides the batch, not the outside diameter
Outside diameters are forgiving: measure one with a micrometer, watch it drift over a run, adjust the offset and keep cutting. A hole under a millimetre gives you none of that. It is finished in a single pass, you cannot see inside it, and by the time a pin gauge says it is off centre the parts are already at the deburring bench. We have scrapped a run of brass nozzles where every external dimension sat inside its band and the 0.6 mm through-hole was a few hundredths of a millimetre off centre - enough to fail a position callout, not enough to see.
Almost all of that was settled before the drill touched metal: how the tool was held, what the surface underneath it looked like, and whether the chip had anywhere to go.
Why 0.5 mm does not behave like 5 mm
A 5 mm drill is stiff enough to correct its own entry: the point finds the spot, the web pushes the tool straight. A 0.5 mm carbide drill is a sliver with almost no bending stiffness. Runout past about 10 µm at the shank loads one flute and unloads the other, and a tool cutting on one edge drills a hole that walks in the direction of that load.
Parameters move with it: surface speed stays up at the edge, and feed per revolution falls to a few microns - thinner than the edge radius unless the tool is sharp and the flutes are polished. A drill that rubs instead of cutting work-hardens the wall and then breaks. A lathe that turns a 20 mm shaft to ±0.005 mm will still snap 0.4 mm drills if the collet has a burr.
Entry, chips, and where a micro drill actually breaks
A micro drill does not correct a bad start. On a flat face, spot with a 90 or 120 degree included angle, shallow enough to leave a cone rather than a crater, then feed without dwelling at the surface. On a curved, angled or cast face the spot has to be deep enough to present a full circle to the point, or the first contact is on one lip and the hole begins offset. Cross holes are worse: the drill meets an interrupted cut twice per revolution, and no feed control fixes a tool pushed sideways - drill the cross hole before the bore is finished, or guide the tool in a fixture.
At L/D 3 a small drill clears its own chips. Past L/D 5 the flutes carry more than they can lift, and past L/D 8 the chip is recut - which is where heat and breakage start, usually two or three holes after the first sign of trouble. Peck with full retracts and enough coolant pressure to flush rather than dribble. Material still decides the cycle: brass breaks chips and tolerates aggression, 316L work-hardens the moment the edge rubs, aluminium builds up on the edge until the hole tightens, and PEEK pushes a stringy chip that wraps the tool. Beyond about L/D 10 the route changes, and we say that at RFQ instead of quoting a cycle we cannot hold.
The exit side: burr, and the hole that has to fit
A drilled hole leaves a burr at the entry and a crown at the exit, and on a 0.5 mm hole that crown can be a fifth of the diameter. On a part that seals, or slides inside another, the burr is the defect - not the diameter. Abrasive flow or electrochemical deburring reaches where a hand tool cannot; thermal methods clean the whole part but change surface condition; a back-chamfer needs an accessible exit. Which one is planned belongs in the quote, because the cost does.
Inside the hole the logic is the same: drilling leaves a wall that is rough and slightly tapered, so where the drawing calls a fit the route is drill and ream - the drill makes the hole, the reamer makes the size. We hold ±0.005 mm on holes that carry a fit, with unmarked dimensions to ISO 2768-m. Surface expectations inside a small hole are covered in the surface finish guide, and the wider tolerance picture in CNC machining tolerances.
Measuring a hole you cannot see
A pin gauge gives the smallest diameter that will enter, and on a tapered or bowed hole that number flatters you. Go/no-go pins are a production check on a straight hole; they say nothing about position or straightness. Position reads better optically, looking down the axis. A CMM can touch down to roughly 0.3 mm with a small ruby stylus, below which the stylus is the limit rather than the machine. Where the inside geometry matters, a sectioned sample is still the most honest measurement - and it is destructive, so it belongs in first-article.
Whatever the method, the instrument chain has to be an order better than the callout, and a report that names the method is worth more than one that shows only a pass. Our reporting route is described in FAI and PPAP reporting.
| Field | CHX Metal |
|---|---|
| Location | Shajing, Bao'an, Shenzhen, China - 5,000 m² plant, 100+ staff, machining since 2013 |
| Equipment | 220 machines: 70 Tsugami Swiss-type lathes for small holes in bar Ø1–20 mm, 50 CNC lathes to Ø300 mm, 100 machining centres (30 of them 3+2) |
| Tolerances | ±0.005 mm on holes carrying a fit; unmarked dimensions to ISO 2768-m; Leyden CMM and optical measurement |
| MOQ | 1 piece |
| Lead times | Prototypes 3–7 days; production 7–15 days; capacity up to 5 million pieces per month |
| Materials | 303/304/316L stainless, 12L14 and 1215 free-cutting steel, 6061/7075 aluminium, H59 brass, copper, PEEK; ISO 9001:2015 and ISO 14001:2015 certified |
| Shipping | EXW Shenzhen only - we are happy to recommend reliable freight forwarders. |
What moves the price
Depth is the first. The same diameter at L/D 3 and L/D 7 are different jobs: the second needs a peck cycle, more retracts, and a drill that is inspected rather than trusted. Position is the second, because a true-position callout on a small hole usually means a fixture or a bushing rather than a coordinate. Deburr is the third, and the one most often missing from a comparison between two suppliers - which is why the cheaper quote sometimes arrives with parts that fail a leak test. A wider list of what to settle before quoting sits in our DFM checklist for turned parts.
For the part-level side - handling, cleanliness, measurement of components in the 1–20 mm range - the micro CNC machining capability page covers the shop around the hole rather than the hole. If the drawing shows a hole under a millimetre, send the section view with it; depth and exit surface set the price, and neither is visible on a plan view.
Machining capacity behind this article
- Equipment: 220 machines — 100 machining centres (30 of them 3+2), 50 CNC lathes, 70 Tsugami Swiss-type lathes.
- Tolerance: ±0.005 mm on critical features; anything unmarked defaults to ISO 2768-m.
- Volume: up to 5 million pieces a month; prototyping 3–7 days, production 7–15 days.
- Materials: 6061/7075 aluminium, 303/304/316 stainless, H59 brass, copper, TC4 titanium, carbon steel.
- Footprint: 5,000 m² in Shajing, Bao'an, Shenzhen; 100+ staff; founded 2013.
- Terms: EXW Shenzhen only — we are happy to recommend reliable freight forwarders.
Address: Building B, 3rd Floor, Haosan Maozhoushan Industrial Zone, Buyong Community, Shajing Street, Bao'an District, Shenzhen | Tel: +86-755-27427365 | Email: mc@chxmetal.com
Frequently asked questions
What is the smallest hole you can drill?
Down to 0.3 mm in brass and aluminium, and reliably in the 0.5–1 mm band on our 70 Tsugami Swiss-type lathes, where the guide bushing supports the bar close to the cut. Below 0.3 mm the tool becomes the limiting factor rather than the machine, and we would rather quote a sample run first than promise a production figure.
How deep can a micro hole go before the drill breaks?
Around three times diameter a small drill clears its own chips. Past L/D 5 it needs a peck cycle with full retracts, and past L/D 8 the chip is being recut, which is where heat and breakage start. Beyond roughly L/D 10 the process changes to gun drilling or another hole-making route, and that is a different quote.
How do you hold position on a 0.5 mm hole?
Position comes from the entry, not from the program. A 90 or 120 degree spot leaves a cone the drill can follow, the holder is checked for runout before the run, and where the callout is tight the job gets a fixture or bushing. Runout past about 10 µm is enough to make a micro drill cut on one lip and walk off centre.
Do drilled holes meet ±0.005 mm?
A drilled hole is rough and slightly tapered, so where the drawing carries a fit the route is drill and ream, and then ±0.005 mm is a size we hold. Unmarked dimensions default to ISO 2768-m. Position, roundness and straightness are separate callouts and are quoted as their own lines when they are tight.
How is a burr removed from a hole you cannot reach?
Abrasive flow or electrochemical deburring reaches where a hand tool cannot, thermal methods clean the whole part but change surface condition, and a mechanical back-chamfer needs an accessible exit. The method is chosen per part family and priced with the part, because on a 0.5 mm hole the exit crown can be a fifth of the diameter.
Send your drawings for a DFM review and a quotation
STEP, IGES, DXF, DWG or PDF — note the material, quantity and finish. Quotes usually go back within one working day. Email mc@chxmetal.com or use the quote form.