Charts

Drill Speed Chart: RPM by Drill Size and Material

Recommended spindle RPM for metric and imperial drills in six common metals, with cutting-speed conversions and practical adjustment guidance.

This drill speed chart gives practical starting spindle speeds for common workshop metals. Values are deliberately conservative: the HSS columns use ordinary jobber-drill recommendations, while the carbide columns assume a rigid machine, low runout and a drill intended for the material. Treat every number as a starting point rather than a guarantee. Alloy condition, hardness, depth, coolant delivery, drill geometry and machine stiffness can move the correct setting substantially.

Metric drill speed chart: 1–25 mm

Each pair of columns shows RPM for HSS and solid carbide. Cobalt HSS normally sits between them: start around 1.3 to 1.5 times the HSS figure if the drill maker permits it. Large tables are horizontally scrollable on a phone.

Imperial drill speed chart: 1/16–1 inch

Imperial speeds use the exact decimal diameter behind each common fractional size. The result is rounded to the nearest ten RPM, which is more precision than most stepped-pulley drills can reproduce. Select the closest lower available speed when in doubt.

Recommended cutting speeds

Surface speed describes how quickly the cutting lip moves around the hole circumference. It is independent of diameter, so it is the useful starting input from a tooling catalogue. SFM means surface feet per minute; one metre per minute equals approximately 3.281 SFM.

The drill RPM formula

For example, a 10 mm HSS drill in mild steel at 25 m/min gives 25 × 1,000 ÷ (3.1416 × 10), or about 796 RPM. A machine setting of 750 RPM is sensible. Halving diameter doubles RPM because the smaller circumference must rotate twice as often to cover the same distance at the cutting edge. The formula calculates rotational speed only; feed per revolution remains a separate choice.

How to use the chart

Identify the work material as closely as practical, choose the column for the actual drill substrate, and find the diameter row. Set the nearest available spindle speed without exceeding the value. Establish a firm feed so both lips cut rather than rub. Make a short trial hole, then examine sound, chip shape, spindle load, hole size and cutting-edge colour. Stable cutting produces repeatable chips and a steady sound. Squealing, blue chips from a material that should cut cool, a polished margin or rapidly rising thrust all call for investigation.

HSS figures suit sharp, conventional twist drills. Cobalt is still high-speed steel, but its hot hardness often permits moderately more speed in stainless and tougher alloys. Solid carbide tolerates much higher edge temperature and surface speed, yet it dislikes vibration, interrupted contact and hand-fed wobble. Do not simply use a carbide number for a carbide-tipped masonry bit: its geometry and brazed construction are not designed for accurate metal drilling.

When to reduce drill speed

Reduce the tabulated speed by 10–20% for uncertain material identity, slightly worn tools, marginal workholding or a drill press with noticeable spindle play. Reduce by 20–30% for holes deeper than roughly three diameters, cross holes, scale, flame-cut surfaces or interrupted entry. Long-series drills and extended holders have less bending stiffness, so slower speed and lighter, controlled feed protect them from chatter. A hand drill usually needs an even more cautious setting because alignment and feed are inconsistent.

Heat is another clear reason to slow down, but speed alone is not always the cause. A drill that rubs because feed is too light can overheat even at low RPM. First confirm that the lips are sharp, equal in length, centred and receiving enough feed to form chips. For stainless and titanium, never dwell at the bottom of a peck: dwelling work-hardens the surface directly in front of the edge. Retract positively, clear chips and return under control.

Coolant, depth and chip evacuation

Flood coolant supports the higher end of a recommendation by lubricating the margins, cooling the edge and carrying chips away. A brush-applied cutting oil helps HSS in steel or stainless, though it cannot remove heat as efficiently as flood delivery. Aluminium benefits from an aluminium-safe soluble coolant or light lubricant that prevents built-up edge. Brass and grey cast iron are commonly drilled dry; compressed-air extraction or a vacuum keeps abrasive cast-iron dust away from slideways. Avoid blowing hazardous dust toward the operator.

Deep holes change the thermal and mechanical conditions because coolant struggles to reach the point and chips travel farther through the flutes. Peck before the flutes pack, with shorter increments in gummy aluminium and work-hardening stainless. Through-tool coolant and purpose-made parabolic-flute drills can preserve a higher speed at depth. On a basic machine, the safer response is a lower speed, positive feed and complete chip-clearing retracts.

Feed must match speed

RPM without feed is only half a cutting condition. Small drills need a light feed per revolution because their web and lips are fragile; large drills require a thicker chip to prevent rubbing. As broad workshop starts, use about 0.03–0.06 mm/rev at 3 mm diameter, 0.08–0.12 at 6 mm, 0.15–0.20 at 10 mm and 0.22–0.32 at 16–25 mm. Reduce for a weak setup, but do not starve the cut. Multiply feed per revolution by RPM to obtain linear feed in millimetres per minute.

Reading the evidence at the machine

Two similar, regularly curled chips suggest both cutting lips share the load. One heavy chip and one fine chip often reveal an uneven grind or runout. Long stringers require guarding and controlled chip breaking; never pull them by hand. A bell-mouthed hole points toward poor alignment or excessive runout. Chatter marks call for better support, less overhang, corrected speed or a more rigid tool. Record successful values by material batch, drill and machine so this general chart becomes a reliable shop-specific reference.

Manufacturer data takes priority whenever it is available because modern coated carbide drills can have application ranges far beyond these conservative values. Check whether published speeds assume internal coolant, a minimum pressure, a particular engagement or CNC rigidity. For one-off repair work, begin low and increase only while chips, sound and edge condition remain healthy. For production, use controlled trials and tool-life records rather than choosing the fastest setting that survives one hole.

Frequently asked questions