Skip to content
Independent manufacturing reference Formula-first · assumptions shown · production checks required
MfgWorkbenchManufacturing Reference

Machining & CNC technical guide

Drilling Speeds and Feeds: RPM, IPR & IPM Explained

Turn cutting speed and drill diameter into spindle RPM, then convert feed per revolution into penetration feed without mixing metric and inch units.

Published September 4, 2026Reviewed September 4, 2026Editorial method

A drilling speeds-and-feeds calculation has two stages. First convert cutting speed and drill diameter into spindle RPM. Then multiply RPM by feed per revolution to obtain penetration feed.

Quick answer

Metric RPM: RPM = (m/min × 1,000) ÷ (π × drill diameter in mm)

Imperial RPM: RPM ≈ (SFM × 3.82) ÷ drill diameter in inches

Penetration feed: mm/min = mm/rev × RPM or IPM = IPR × RPM.

In this guideSpindle speedFeed rateWorked exampleSelecting inputsCommon problems

Calculate drilling spindle speed

Metric drilling RPMn = (vc × 1,000) / (π × Dc)vc = m/min · Dc = drill diameter in mm
Imperial drilling RPMn ≈ (SFM × 3.82) / DSFM = surface feet per minute · D = drill diameter in inches

A larger drill requires fewer revolutions to maintain the same cutting speed. If diameter doubles, RPM halves.

Convert feed per revolution into feed per minute

Penetration feedvf = fn × nvf = mm/min or IPM · fn = mm/rev or IPR · n = RPM

Unlike a milling feed-per-tooth calculation, drill manufacturers commonly publish drilling advance as feed per revolution. Do not multiply the published feed per revolution by the number of drill lips unless the manufacturer explicitly defines the value per cutting edge.

Metric worked example

For a 10 mm drill at 30 m/min with a feed of 0.15 mm/rev:

  1. RPM = (30 × 1,000) ÷ (π × 10) = 954.9 RPM.
  2. Feed = 0.15 × 954.9 = 143.2 mm/min.
Input or result Value
Drill diameter 10 mm
Cutting speed 30 m/min
Spindle speed 954.9 RPM
Feed per revolution 0.15 mm/rev
Penetration feed 143.2 mm/min

How to select the starting inputs

Use manufacturer data for the exact drill family, substrate, coating, diameter, work material, and hole-depth range. Solid-carbide, indexable, replaceable-tip, HSS, cobalt, gun drills, and flat-bottom drills do not share one universal range.

Hole depth, through-coolant capability, coolant pressure, entry and exit conditions, interrupted surfaces, pilot holes, runout, and machine rigidity can change the usable feed and speed. Deep holes usually require a defined chip-control and coolant strategy rather than an arbitrary peck cycle.

Common drilling calculation problems

  • Mixing IPR and IPM: IPR is advance per revolution; IPM is advance per minute.
  • Multiplying feed per revolution by flute count: normally incorrect for published drilling feed data.
  • Ignoring the spindle cap: if RPM is limited, recalculate the achieved surface speed and feed rate.
  • Using one cutting speed for every drill type: cutting material, geometry, coating, and coolant delivery matter.
  • Using calculated feed as guaranteed feed: short moves and canned cycles can be acceleration- or control-limited.

Inch-to-metric conversions

  • m/min = SFM ÷ 3.28084
  • mm/min = IPM × 25.4
  • mm/rev = IPR × 25.4

When possible, keep the complete calculation in one unit system to avoid rounding the feed per revolution too early.

Technical references

Published and formula-checked by MfgWorkbench. Last reviewed September 4, 2026. See our editorial method.