How to calculate chip load (feed per tooth)

Chip load — also called feed per tooth and written fz — is how far a milling cutter advances for each cutting edge that passes through the work. It is the thickness of the chip each flute is asked to remove, measured in mm/tooth or inch/tooth. Get it right and the tool cuts cleanly, runs cool and lasts. Get it wrong in either direction and you pay for it in broken edges or burned-up tools.

The chip load formula

Chip load ties together feed rate, the number of flutes and spindle speed. The feed rate Vf (table feed, in mm/min or inch/min) is:

Vf = fz · Z · n

where:

• fz — the chip load (feed per tooth);
• Z — the number of flutes (teeth);
• n — the spindle speed in RPM.

Rearranged, the chip load you are actually running is simply the feed rate divided by the flutes and the RPM:

fz = Vf / (Z · n)

A closely related figure is the feed per revolution — the advance for one full turn of the cutter, regardless of speed — which is just chip load times the flute count:

feed per rev = fz · Z

Sensible starting chip loads

Chip load is not a single fixed number; it depends on the material, the tool substrate and geometry, and how rigid your setup is. The figures below are starting points for solid-carbide end mills — tune them from there based on the chips, the sound of the cut and the finish.

End mill diameter	Typical starting fz
Small (≤ 6 mm)	≈ 0.01–0.05 mm/tooth
Larger (10–20 mm)	≈ 0.05–0.20 mm/tooth

Smaller tools take a lighter chip because the flute is weaker and deflects more; bigger, stiffer cutters can take a heavier bite. Always cross-check against the tool maker's published data for your specific material and coating.

Why too low is as bad as too high

There is a temptation to dial the feed down to be "safe." It backfires. When fz is too low, the edge stops slicing and starts rubbing against the surface. Rubbing makes friction heat instead of cutting heat, and that heat goes into the tool and the part rather than leaving in the chip. In work-hardening alloys — stainless steels, nickel alloys, titanium — a too-light cut work-hardens the surface ahead of the edge, so the next pass is cutting harder material. The result is premature flank wear and a tool that dies early.

When fz is too high, the chip is thicker than the edge can handle. You overload the flute, chip or break the cutting edge, and leave a poor, torn finish. The right chip load sits in the band where the edge is genuinely cutting but not overloaded — which is exactly what the starting ranges above target.

Radial chip thinning

Here is the part most people miss. The formulas above assume the cutter is engaged at least to its radius. When your radial depth of cut (stepover, ae) is less than half the tool diameter — that is, ae < D/2, common in trochoidal milling and finishing passes — each flute only sweeps a shallow arc through the material. The actual chip it removes is thinner than the programmed fz.

That thin chip drags you straight back into the rubbing problem above, even though the numbers on paper look fine. The fix is radial chip thinning compensation: as the engagement drops, you increase the programmed fz so that the real chip thickness stays back up in the healthy range. The lighter the stepover, the larger the chip-thinning factor and the more you push the programmed feed per tooth. The exact multiplier depends on the engagement geometry, so treat it conceptually — lean on your tool maker's chip-thinning chart or a feeds-and-speeds tool rather than a single memorized formula. The practical takeaway: light stepovers let you run faster feeds than the base formula suggests.

Worked example

Take a D = 10 mm, 2-flute solid-carbide end mill running at n = 8000 rpm, with a target chip load of fz = 0.05 mm/tooth. The feed rate is:

Vf = fz · Z · n = 0.05 · 2 · 8000 = 800 mm/min

So you program 800 mm/min. The feed per revolution is 0.05 · 2 = 0.1 mm/rev. If you later run that cutter at a light stepover — say ae = 1 mm on the 10 mm tool — chip thinning means the real chip is much thinner than 0.05 mm, and you'd raise the programmed fz (and therefore the feed) to bring the true chip thickness back up.

To go the other way and solve for the chip load you're already running, drop your feed, flutes and RPM into the chip load calculator. To set the spindle speed in the first place — converting a material's cutting speed and the tool diameter into RPM — start with the SFM calculator, then bring the RPM back here to pick your feed. Once the feed is realistic, use the machining time calculator to turn toolpath length and passes into cycle time, then use the machining cost calculator to estimate per-part cost.

Frequently asked questions

What is chip load in milling?

Chip load is the feed per tooth (fz) — how far the cutter advances for each cutting edge, in mm/tooth or inch/tooth. It sets the thickness of the chip each flute removes and is the core variable behind the feed rate.

How do I calculate feed rate from chip load?

Multiply chip load by the number of flutes and the RPM: Vf = fz · Z · n. For example, fz = 0.05 mm, Z = 2 flutes and n = 8000 rpm give Vf = 0.05 · 2 · 8000 = 800 mm/min.

What happens if chip load is too low?

Too low a chip load makes the edge rub instead of cut. That generates heat, work-hardens the surface (especially in stainless and titanium) and wears the tool prematurely. Too high a chip load breaks edges and leaves a poor finish.

Last reviewed: 2026-05-29.