Cutting speed is not a property of the drill. It is a property of the pair: this tool material in this work material. Diameter turns it into revolutions per minute.
Getting that order right avoids most parameter errors.
The only formula you need
n = 1000 x vc / (pi x D)
n is spindle speed in rpm, vc is cutting speed in m/min, D is diameter in mm.
At 1.0 mm and 100 m/min this gives 31,800 rpm. At 0.5 mm it gives 63,700 rpm. At 3.0 mm it gives 10,600 rpm.
The same cutting speed therefore demands very different spindle speeds across the catalogue, and small diameters run into the spindle limit rather than the tool limit.
Starting values by material
| Work material | vc (m/min) | rpm at 1.0 mm | rpm at 0.5 mm |
|---|---|---|---|
| Aluminium alloys | 150-250 | 48,000-80,000 | 95,000-159,000 |
| Carbon steel | 100-180 | 32,000-57,000 | 64,000-115,000 |
| Alloy steel | 70-130 | 22,000-41,000 | 45,000-83,000 |
| Austenitic stainless | 60-120 | 19,000-38,000 | 38,000-76,000 |
Two observations follow.
First, most micro spindles top out at 20,000-25,000 rpm. At that ceiling a 0.5 mm drill in aluminium runs at an effective 39 m/min, far below what the material allows. That is not a mistake; it is what the machine can do.
Second, the table is a starting point, not a target. Tool life, surface finish and hole position decide where you end up.
From speed to feed
Feed per revolution for micro drills runs 0.5-2% of diameter:
- 0.1 mm: 0.0005-0.002 mm/rev
- 0.5 mm: 0.0025-0.010 mm/rev
- 1.0 mm: 0.005-0.020 mm/rev
- 3.0 mm: 0.015-0.060 mm/rev
Feed rate in mm/min is feed per revolution times spindle speed. At 1.0 mm, 10,000 rpm and 0.01 mm/rev, that is 100 mm/min.
Under-feeding is the more common error. A drill that rubs work-hardens the material and destroys itself, while a drill that cuts a proper chip stays cool.
Adjusting from the starting point
Change one variable at a time and record what happened.
Short life with flank wear: reduce vc by 20%. Cutting speed has the strongest effect on wear rate.
Short life with built-up edge: increase vc or change coating. Built-up edge is a friction problem, but the two interact.
Poor surface finish: increase feed per revolution slightly, or check runout. Finish follows edge condition more than speed.
Chatter or a squealing hole: reduce speed until it stops, then reduce overhang. Do not chase it with feed.
Oversized holes: check runout and built-up edge before blaming parameters.
Worked example
Take a 1.0 mm drill in 304 stainless, target vc = 50 m/min, feed per revolution 0.008 mm.
- n = 1000 x 50 / (3.1416 x 1.0) = 15,900 rpm.
- vf = 0.008 x 15,900 = 127 mm/min.
- A 6 mm deep hole is 6 x D, so peck at 1 x D: six passes of 1 mm, retract at rapid.
- Time in cut is 6 mm at 127 mm/min plus retracts. Budget about 90 seconds per hole, including the pecks.
The same arithmetic at 3.0 mm gives 5,300 rpm and 42 mm/min. Feed rate in mm/min falls with diameter even though feed per revolution rises: smaller tools spin faster but cut a much thinner chip.
Reading the machine instead of the table
The table cannot know your spindle, holder or coolant. Three signals tell you whether the starting point is right.
- Chip colour. Straw-coloured steel chips mean a healthy temperature. Blue chips mean the edge is too hot.
- Sound. A steady cut sounds even. A rising pitch means the edge is loading up.
- Spindle load. On a small machine, load should sit at 30-60% of rated power. Below 20% you are rubbing; at 90% there is no margin.
If all three look right and the tool still fails, the problem is usually runout rather than parameters. See why a micro drill breaks.
Peck by depth
| Depth | Peck | Note |
|---|---|---|
| Up to 2 x D | None | Single pass |
| 2-5 x D | 2 x D | Standard |
| 5-10 x D | 1 x D | Through-coolant recommended |
| Above 10 x D | 0.5-1 x D | Extended-length series, coolant-through |
FAQ
My spindle only reaches 12,000 rpm. Is that a problem?
Above 2 mm, no. At 0.3 mm in aluminium, yes: you run at a fraction of the recommended speed, so compensate with slightly higher feed per revolution and a shorter peck.
Should I reduce speed with an extended-length drill?
Yes. An extended-length tool is less stiff. Reduce vc by 20-30% and peck more often.
Does coating change the starting speed?
It changes the ceiling, not the starting point. Start from the material table and let tool life tell you whether the coating allows more.
What about feed at breakthrough?
Reduce to 30-50% of the cutting feed for the last 0.2 mm. Breakthrough is where the drill loses support and where most micro drills are lost.