Chinas Machine Tool Segment: How PCB Drilling Gets to 0.10 mm
This page is for process engineers and sourcing engineers who buy or specify drilled parts. It explains how chinas machine tool segment moved into micro-hole drilling, which machine parameters decide hole quality, and when a job belongs on a high-speed drilling center instead of a general CNC mill.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
Key takeaways
How chinas machine tool segment moved into micro-hole drilling
The move into small-hole drilling did not come from one invention. It came from machine builders, drill makers, and board shops improving the same loop at the same time. Spindle speed climbed, runout dropped, and the tool geometry was redesigned to cut fiberglass and copper without tearing the resin. That combination is what people mean when they talk about chinas machine tool segment today.
A high-speed drilling center for boards looks different from a general machining center. The spindle turns far faster, the table moves in short fast strokes, and the tool changer handles shanks under 3 mm. The control is tuned for hit rate, which means how many holes land in position per minute, not for heavy material removal.
That difference matters when you quote a job. A part with 0.20 mm holes in a 0.8 mm thick laminate does not belong on a 40-taper mill. The spindle cannot reach the surface speed, and the tool will deflect before the edge cuts. Move that job to a drilling center and the same hole holds position and wall finish.
The same logic works in reverse. A 12 mm hole in a 20 mm aluminum plate is a job for a machining center, not a drilling center. The drilling center has the speed but not the rigidity for deep, large-diameter cuts. Match the machine to the hole, not the other way around.
Spindle, tool holder, and runout: the checks that decide everything
Runout is the amount the tool tip moves off center as the spindle turns. For a 0.10 mm drill, a runout of 10 μm already uses a fifth of the drill diameter. The edge on one side cuts deeper and the other side rubs. The drill walks, the hole goes oval, and the bit snaps on the next panel.
Measure runout at the tool holder, not at the spindle nose. A clean taper and a worn collet can hide behind a good spindle reading. Use a dial indicator with 1 μm resolution and turn the spindle by hand through one full turn. If the reading moves more than 5 μm, stop and fix the holder before running the job.
Heat matters too. A spindle that has been idle for an hour runs cooler than one that has drilled for 30 minutes. Run a warm-up cycle, then re-check runout. The change is usually small, but on a 0.10 mm drill a 2 μm shift is enough to change the breakage rate.
Keep the tool holder and collet clean. Dust from laminated board is abrasive and packs into the taper. Wipe the taper with a lint-free cloth and check the collet for scoring under light. A scored collet holds the shank off center, and no parameter change will fix that.
- 1Target runoutUnder 5 μm at the holder for drills below 0.30 mm.
- 2Warm-up firstSpindle temperature shifts runout by 1–3 μm after 30 minutes.
- 3Collet conditionAny visible scoring means replace the collet, not the drill.
Micro-drill geometry and what it does to hole quality
A micro-drill is not a scaled-down twist drill. The web is thicker relative to diameter, the flute is shorter, and the point angle is often 130° to 150° for board work. The shank is usually 3.175 mm so it fits a standard collet, with the cutting section ground down to the final diameter.
The flute length controls chip removal. A drill with a flute shorter than the stack height will pack chips in the flutes and break. For a stack of three panels at 0.8 mm each, use a drill with at least 3.0 mm of flute, and peck in steps no deeper than one panel thickness.
Point angle changes the entry. A 130° point starts cutting sooner and reduces the bell-mouth effect at the top of the hole. A 150° point is stiffer but pushes more material sideways, which raises the risk of pad lift on thin copper. Pick the angle to match the copper weight, not the drill catalog default.
Coating is optional for board work. Diamond coating extends life in abrasive laminate, but it also changes the effective diameter by 1–2 μm. If the hole tolerance is tight, measure the coated drill and adjust the recipe, or the first holes will come out undersized.
Reading hit rate, taper, and burr to find the real problem
Hit rate tells you if the machine is keeping up with the program. A drop in hit rate usually means the control is slowing to avoid a fault, which points to runout, chip load, or a worn drill. Check runout first, then chip load, then the drill wear land.
Wall taper shows up as a hole wider at the top than the bottom. That is a sign of drill walk or low surface speed. Raise spindle speed in 10 percent steps and re-measure. If taper does not change, the runout is the cause, and no speed change will help.
Exit burr is a separate problem. It forms when the drill pushes the last layer of copper instead of cutting it. Reduce feed in the final 0.3 mm of travel by 40 to 60 percent, and check the exit side under magnification. A clean exit edge is the sign that the step drill is set right.
If the hole looks good on the entry side but the wall is rough, the flute is packing chips. Shorten the peck depth or switch to a drill with a longer flute. Do not raise spindle speed to clear chips. That pushes the drill harder and usually breaks it.
Step by step: setting up a micro-hole drilling job
- 1Check the tool holder and measure runoutWipe the taper and collet. Mount the drill and read total indicated runout at the holder with a 1 μm indicator. Target under 5 μm. Replace the collet if the reading moves more than 2 μm between two mounting attempts.
- 2Warm up the spindle and re-checkRun the warm-up cycle for 20 to 30 minutes. Re-measure runout. If it moved more than 3 μm from the cold reading, hold the job until the spindle stabilizes.
- 3Set entry feed and spindle speedFor 0.10 to 0.20 mm drills in FR-4, start at 80,000 to 120,000 rpm and an entry feed of 0.8 to 1.2 m/min. Watch the first ten holes for bell-mouth before running the full stack.
- 4Set peck depth to one panel thicknessPeck no deeper than the thickness of a single panel, typically 0.5 to 1.0 mm. Deeper pecks pack the flutes and raise breakage on the second or third panel.
- 5Reduce feed for the last 0.3 mmDrop the feed by 40 to 60 percent through the exit layer. This keeps the copper edge clean and holds exit burr under 25 μm.
- 6Inspect position, taper, and burrMeasure hole position with a vision system and wall taper with a plug gauge. Check exit burr under 30× magnification. If position is out by more than 0.05 mm, re-fixture the stack and re-run the first panel as a check.
When to use a drilling center, a mill, or a re-fixture
Match the job to the machine and the setup.
| Job condition | Best machine | Why |
|---|---|---|
| Holes below 0.30 mm in laminate | High-speed drilling center | Surface speed and runout control |
| Holes above 6 mm in metal | Machining center | Rigidity for deep, large-diameter cuts |
| Hole position drifting over the stack | Re-fixture and re-measure | Clamping shift, not tool wear |
| Wall taper with good runout | Drilling center, raise speed | Low surface speed, not deflection |
| Exit burr over 25 μm | Same machine, step feed | Feed reduction at the exit layer |
| Drill breaking on panel two | Same machine, shorter peck | Chip packing in the flute |
Match the machine to the hole, then set the recipe
A 0.10 mm hole in laminate belongs on a high-speed drilling center with runout under 5 μm. A 12 mm hole in aluminum belongs on a machining center. Get that match right first, then tune feed and peck depth from there.
Questions engineers ask before running the job
What runout should I hold for a 0.10 mm drill?
Keep total indicated runout under 5 μm at the tool holder. At 0.10 mm diameter, 5 μm is five percent of the drill size. Above that, the cutting edge loads unevenly and the drill walks.
Measure at the holder, not the spindle nose, and re-check after the warm-up cycle.
How deep can I peck in a three-panel stack?
Peck no deeper than one panel thickness, usually 0.5 to 1.0 mm. The flute must clear chips between pecks. If the flute is shorter than the stack, use a drill with a longer flute or split the stack.
If the drill breaks on the second panel, the peck is too deep or the flute is packing.
Why does the top of the hole bell out?
Bell-mouth at entry comes from drill walk or too high an entry feed. Lower the entry feed to 0.8 m/min and check runout before changing spindle speed.
A 130° point angle also reduces the bell-mouth effect compared with a 150° point.
Can I run the same recipe on a general CNC mill?
Only for holes above roughly 1 mm in metal. Below that, the mill cannot reach the surface speed and the runout is usually higher than a drilling center. The drill will deflect and the hole will come out tapered.
For laminate work below 0.30 mm, use a high-speed drilling center.
When do I re-fixture instead of changing the drill?
Re-fixture when hole position drifts across the stack while runout, taper, and burr stay within limits. That pattern points to clamping shift, not tool wear.
Measure position on the first and last panel. If both moved in the same direction, check the clamps and the stack alignment.
Send us the drawing and hole schedule
We review the hole sizes, stack height, and tolerance, then quote with a DFM note on runout and peck depth.
12-hour quote100% inspection
More process notes
We publish setup notes, tooling trials and inspection data from the factory floor.
