Milling Feed Rate Calculator (Chip Load)
Work out milling feed rate from chip load, flutes and spindle speed, with the radial chip thinning correction that light stepovers make essential.
How to use this calculator
- 1Set the cutter diameter and flute count first - both scale the feed rate directly.
- 2Enter the stepover as an actual distance rather than a percentage; the page reports the percentage back to you.
- 3Leave the chip thinning correction on. Turn it off only to see what an uncorrected calculator would have told you.
- 4Use the tool maker's chip load when you have one; the material defaults are generic starting figures for a half inch cutter.
- 5Treat the result as a first setting. Watch the chips - they should come off as chips, not dust and not blue.
How the calculation works
Feed rate = RPM x feed per tooth x flutes
Engagement angle: cos(phi) = 1 - 2 x ae / D
Chip thinning factor = 1 / sin(phi) [when ae < D/2]
Programmed feed per tooth = target chip x thinning factor- fz
- Feed per tooth - what you programme. Not the same as the chip thickness unless the stepover is half the diameter or more
- ae
- Radial depth of cut, the sideways bite. Equal to the diameter in a full slot
- ap
- Axial depth of cut. It sets the removal rate and the load, but has no effect on radial chip thinning
- phi
- The arc of the cut the tooth is engaged over. 180 degrees in a slot, 90 at half diameter, and small at light stepovers
At half diameter of engagement and above the factor is exactly 1 and nothing needs correcting - the tooth reaches perpendicular somewhere in the cut and takes a full chip.
Below that the maximum chip thickness is fz x sin(phi), and the correction just divides it back out.
Axial depth does not enter the radial thinning calculation. A ball nose cutter has its own separate axial thinning effect, which is not modelled here.
Worked example
Half inch four flute in mild steel, half diameter stepover
- 1.Coated carbide in 1018 runs 375-625 sfm; the middle, 500 sfm on 0.5 in, is 3820 rpm.
- 2.The starting chip load for low carbon steel at half inch diameter is 0.003 in per tooth.
- 3.At 0.25 in stepover the engagement is exactly 90 degrees, so sin(phi) = 1 and the thinning factor is 1.00 - nothing to correct.
- 4.Feed = 3820 x 0.003 x 4 = 45.8 in/min, removing 0.25 x 0.25 x 45.8 = 2.86 cubic inches a minute.
Result: 45.8 in/min - no thinning correction at half diameter
The same cutter at a 10% stepover
- 1.At 0.05 in of a 0.5 in cutter, cos(phi) = 1 - 2(0.1) = 0.8, so phi = 36.9 degrees and sin(phi) = 0.6.
- 2.The book 0.003 in per tooth would give a chip of only 0.0018 in - 40% thinner than intended.
- 3.Correcting: 0.003 / 0.6 = 0.005 in per tooth programmed, which restores the 0.003 in chip.
- 4.Feed goes from 45.8 to 76.4 in/min. With the axial depth opened to 0.75 in, removal is 0.05 x 0.75 x 76.4 = 2.86 in³/min - the same as the heavy cut, on a much happier tool.
Result: 76.4 in/min - the feed rises 67% to keep the chip the same
What the uncorrected arithmetic would say
- 1.The same light stepover, with the correction switched off.
- 2.Feed = 3820 x 0.003 x 4 = 45.8 in/min, and the chip comes out at 0.0018 in.
- 3.That is the number a plain feeds-and-speeds calculator gives, and the tool spends the cut rubbing rather than shearing.
- 4.In stainless the same mistake also work hardens the surface, so the next pass has to cut through a harder skin than the one before it.
Result: 45.8 in/min and a 0.0018 in chip - 40% too thin
A three flute in aluminium, full slot
- 1.A full slot means the cutter is engaged the whole 180 degrees, so there is no thinning to correct - the factor is 1.
- 2.Feed = 8000 x 0.004 x 3 = 96 in/min.
- 3.Removal is 0.375 x 0.1875 x 96 = 6.75 cubic inches a minute, which is a lot for a 3/8 in cutter and is the aluminium doing the work rather than the tool.
- 4.Three flutes rather than four leaves flute space for the chips, which in a slot have nowhere to go except back through the cut.
Result: 96 in/min in a full slot - no correction, and chip clearance is the limit
Feed per tooth is not chip thickness
The two are the same only in a full slot, and the difference between them is where most of the tool life on a modern toolpath is won or lost.
Picture one tooth entering the cut. It follows a circular arc, and the material in front of it is a crescent that starts at zero thickness, thickens as the tooth swings in, and thins back to nothing as it leaves. If the cutter is buried half its diameter or more, somewhere in that sweep the tooth is moving straight into the work and the chip reaches its full programmed thickness. If the cutter is only touching the edge of the material, the tooth never gets to perpendicular, and the thickest chip it manages is a fraction of the feed per tooth.
That fraction is the sine of the engagement angle, and the geometry gives it exactly: cos(phi) = 1 - 2ae/D. At 50% stepover phi is 90 degrees and the sine is 1. At 10% it is 36.9 degrees and the sine is 0.6. At 5% it is 25.8 degrees and the sine is 0.436 - the chip is well under half what you asked for.
Why a thin chip is worse than a thick one
Intuition says a lighter chip is gentler. It is not, and the reason is that a cutting edge is not infinitely sharp. It has a radius - a few microns on a fresh carbide edge, more once it has worn a little - and a chip has to be several times that radius before the edge can shear it cleanly.
Below that, the edge ploughs. The material is pushed down and around the edge rather than lifted off as a chip, which generates heat with no metal removed to carry it away, deforms the surface layer, and wears the edge in a way that makes the problem worse on the next pass. In austenitic stainless and nickel alloys, the deformed layer work hardens, so a rubbing pass leaves a harder skin for the following one to cut through - the classic downward spiral where the operator responds to a struggling tool by taking a lighter cut.
Specific cutting energy tells the same story from the power side: the force per unit of metal removed climbs steeply as the chip thins. A very light chip is expensive per cubic inch and hard on the edge at the same time.
The correction is what makes high speed machining work
Once chip thinning is understood, adaptive and trochoidal toolpaths stop looking like a trick. Their whole basis is to trade radial engagement for feed rate: take 5% to 15% of the diameter sideways, apply the thinning correction so the chip is still the right thickness, and cut deep axially instead.
Three things follow. The tooth is in the cut for a short arc and out of it for a long one, so it has time to shed heat. The engagement is spread up the length of the flute rather than concentrated near the tip, so the wear is distributed and a longer stretch of the cutting edge does the work. And the radial force is low, so a light machine or a long tool can sustain it without chatter.
The removal rate can end up higher than a conventional heavy slot despite the light stepover, because the feed rate is several times greater. The one non-negotiable part is the correction. Programme a light stepover at the book chip load and you get every disadvantage - the slow removal, the long cycle - with none of the benefit, and a cutter that rubs itself out at a fraction of its rated life.
What the number does not include
This page corrects for radial chip thinning only. A ball nose cutter has a second, separate thinning effect: at a shallow axial depth the effective cutting diameter is smaller than the tool diameter, which changes both the surface speed and the chip geometry. Cutting a shallow contour with a ball nose at its nominal diameter runs it far slower in surface terms than intended.
Nor does it account for lead angle. A face mill with a 45 degree lead spreads the same feed over a longer edge, thinning the chip by sin(45) = 0.707 in exactly the same way, which is why 45 degree face mills take a higher feed per tooth than 90 degree ones for the same chip.
And none of it substitutes for rigidity. Deflection goes as the cube of overhang, so the same correct chip load applied through a tool held a quarter inch further out is a different cut entirely. Every number here assumes the setup can take it.
What this assumes, and where it stops
Assumptions
- Feed per tooth defaults are generic starting values for a half inch cutter, scaled by the square root of diameter for other sizes.
- The cutter is running true and all flutes are cutting. A cutter with runout has one tooth taking a heavier chip than the rest and the others taking less.
- Radial chip thinning only. Ball nose axial thinning and face mill lead angle effects are not applied.
- The machine can hold the calculated feed rate. Small machines and long programmes are often limited by acceleration between moves rather than by the feed itself.
Limitations
- It does not check whether the tool or the machine can take the resulting force - see the machining power page for the spindle load that goes with the removal rate.
- It does not model deflection, which is usually the real limit on small or long tools.
- Chip evacuation is not modelled at all, and in deep slots and pockets it is often what actually governs.
- Runout is ignored. On a small tool a few tenths of runout can double the chip on one flute.
- Ball nose and lead angle geometries need their own corrections that this page does not apply.
Common questions
What is chip thinning in milling?
When the cutter is engaged less than half its diameter sideways, each tooth sweeps a shallow arc and never cuts perpendicular to the surface. The thickest chip it takes is the feed per tooth times the sine of the engagement angle, so at a 10% stepover the chip is only 60% of the programmed feed per tooth. The fix is to raise the programmed feed by dividing by that sine.
At what stepover does chip thinning start to matter?
Below 50% of the cutter diameter. At exactly 50% the engagement angle is 90 degrees, sin is 1, and no correction is needed. From there it grows slowly at first - about 3% at 40% stepover - and then sharply: 1.67x at 10% stepover and 2.29x at 5%.
What is the feed rate formula for milling?
Feed rate in inches per minute = spindle RPM x feed per tooth x number of flutes. The subtlety is that the feed per tooth you programme should be the chip thickness you want divided by the thinning factor, not the chip thickness itself.
Why does a light cut wear my tool out faster?
Almost always because the chip is too thin to be cut. A cutting edge has a real radius, and a chip thinner than a few times that radius gets ploughed and pushed rather than sheared, which puts heat into the edge without removing metal. In stainless it also work hardens the surface for the next pass. Either raise the feed to restore the chip, or take a heavier bite.
How many flutes should I use?
Enough teeth to get the feed rate you want, and enough flute space to clear the chips. Aluminium makes bulky chips and wants two or three; steel chips are more compact and four or more is normal. In a slot, where chips can only come back out through the cut, err towards fewer flutes whatever the material.
Sources
- Machining Doctor - chip thinning and effective feed — Machining Doctor
Formula and content last reviewed on .
Results are estimates for information only, not professional advice.
Related calculators
Tools people commonly use alongside the milling feed rate calculator (chip load).