The IPM formula
Feed rate is simply how much material each tooth takes, multiplied by how many teeth pass through the cut every minute. Everything else follows by rearranging the same equation:
- Feed rate: IPM = RPM × chip load (IPT) × number of flutes
- Chip load: IPT = IPM ÷ (RPM × number of flutes)
- Spindle speed: RPM = IPM ÷ (IPT × number of flutes)
- Metric: mm/min = RPM × feed per tooth (mm) × number of flutes
- Per revolution: IPR = chip load × number of flutes, so IPM = IPR × RPM
Worked example: 3000 RPM, a 0.002 in/tooth chip load and a 2-flute end mill give 3000 × 0.002 × 2 = 12 IPM. Swap to a 4-flute cutter at the same speed and chip load and the feed doubles to 24 IPM — the flute count scales the feed rate exactly.
Getting from SFM to IPM
Surface speed and feed rate are two different things, and you cannot convert one into the other without the tool diameter. The route is always two steps:
- Step 1 — speed: RPM = (12 × SFM) / (π × D) ≈ 3.82 × SFM / D (D in inches)
- Step 2 — feed: IPM = RPM × chip load × flutes
Example: 300 SFM on a 1/4″ (0.25 in) end mill gives RPM = 12 × 300 / (π × 0.25) ≈ 4584. With a 0.001 in/tooth chip load and 4 flutes that is 4584 × 0.001 × 4 ≈ 18.3 IPM. The panel above does both steps for you.
IPM vs IPR — which one does your machine want?
IPM (inches per minute) is a time-based feed: change the RPM and the tool travels at a different speed. IPR (inches per revolution) is tied to the spindle instead — one revolution, one fixed distance, whatever the speed. Milling is normally programmed in IPM (G94), while turning and drilling are normally programmed in IPR (G95). They convert with IPM = IPR × RPM.
Picking a starting chip load
Chip load depends on tool material, diameter, and how deep you are cutting. Small tools need small chip loads because they cannot survive the deflection; large tools want more feed or they rub. Start conservative, listen to the cut, and always check your tool manufacturer's data — the numbers below are starting points, not specifications.
| Material | 1/8″ tool | 1/4″ tool | 1/2″ tool |
|---|---|---|---|
| Aluminum (6061 / 7075) | 0.001 | 0.002 | 0.004 |
| Steel (carbon & low alloy) | 0.0005 | 0.0015 | 0.003 |
| Stainless (303 / 304 / 316) | 0.0001 | 0.0005 | 0.0015 |
| Plastics | 0.001 | 0.003 | 0.006 |
Values in inch/tooth for solid carbide end mills, compiled from Harvey Tool and Kennametal published data. The aluminium row is confirmed identically by both; where the two disagreed, the lower (safer) figure is shown. Dedicated plastic O-flute cutters run considerably heavier than the plastics row above — check your cutter's own data sheet.
- Rule of thumb: heavier chip load in aluminium and plastics, lighter in stainless and titanium
- Small tools: deflection, not the edge, is the limit — stay at the low end under 1/8″
- Rubbing is worse than cutting: too light a feed work-hardens stainless and burns edges
Material-by-material cutting speeds with cited sources → SFM chart
Frequently asked questions
What is the IPM formula in machining?
IPM = RPM × chip load per tooth × number of flutes. In metric the identical formula returns mm/min using feed per tooth in millimetres.
How do I convert SFM to IPM?
Two steps: convert SFM and tool diameter to RPM with RPM = (12 × SFM) / (π × D), then multiply that RPM by chip load and flute count. Open the "Don't know your RPM?" panel above to do both at once.
What is the difference between IPM and IPR?
IPM is distance per minute and depends on spindle speed; IPR is distance per revolution and does not. IPM = IPR × RPM, and IPR = chip load × flutes. Mills usually run IPM, lathes and drills usually run IPR.
What happens if my feed rate is too high or too low?
Too high overloads the edge — chipping, breakage, deflection, poor finish. Too low is not "safe": the tool rubs instead of cutting, which work-hardens the material and burns the edge. Dust instead of chips means the feed is too light.
Does this feed rate calculator work for drilling and turning?
Yes. For drilling, treat the flute count as the number of cutting lips (usually 2) — many machinists program drills in IPR instead, which is chip load × flutes. For turning, a single-point tool has one "flute", so IPM = RPM × feed per revolution.