SizingKitFree chip load calculator
Feed per tooth, and the thinner chip a light pass really takes
Chip load is the distance a milling cutter advances while one tooth passes through the cut, and it is feed rate divided by spindle speed and flute count. This works that relation in all three directions and then does the part most calculators leave out: below half the cutter diameter the chip the edge actually takes is thinner than the feed you programmed, so the feed has to go up rather than down. Free, no signup, and the starting table and the correction are both printed rather than hidden.
- 100% free
- No signup
- 42-cell table
- Chip thinning applied
- in and mm per tooth
Sets both the tabulated chip load and the engagement ratio below.
Tabulated 0.0020–0.0040 in per tooth at this diameter.
Divides the feed rate. It does not change what one tooth is allowed to take.
Stepover, not depth. Equal to the diameter in a slot; the correction switches off at half of it.
FEED PER TOOTH, AS PROGRAMMED
0.0025 in
0.064 mm per tooth, as programmed
- Radial engagement
- 20.0% of diameter
- Thinning factor
- ×1.250
- Programmed per tooth
- 0.0025 in / 0.064 mm
- Thickest chip the edge takes
- 0.0020 in / 0.051 mm
- Feed rate
- 30.00 in/min / 762 mm/min
- Advance per revolution
- 0.0100 in
Chip thinning is what set this feed. At 20.0% of the diameter the tooth is in the cut for too small an arc to reach its own center line, so the thickest chip it takes is 0.800 of the programmed feed per tooth. Multiplying the feed by 1.250 puts the chip back where it was. Program the table figure instead and the edge is cutting 80% of the intended thickness, which is not a gentle cut — it is the one that rubs, work-hardens the surface ahead of the tooth and glazes the edge.
The chip thinning correction, by stepover
Radial engagement as a fraction of cutter diameter against the factor the programmed feed per tooth has to be multiplied by. The last column applies it to 0.003 in per tooth, a mid-band figure for a 1/2 in cutter in mild steel.
| Stepover, ae/D | Factor | Chip at the edge, per 0.0010 in programmed | 0.003 in becomes |
|---|---|---|---|
| 5% | ×2.294 | 0.0004 in | 0.0069 in |
| 10% | ×1.667 | 0.0006 in | 0.0050 in |
| 15% | ×1.400 | 0.0007 in | 0.0042 in |
| 20% | ×1.250 | 0.0008 in | 0.0038 in |
| 25% | ×1.155 | 0.0009 in | 0.0035 in |
| 30% | ×1.091 | 0.0009 in | 0.0033 in |
| 40% | ×1.021 | 0.0010 in | 0.0031 in |
| 50% | ×1.000 | 0.0010 in | 0.0030 in |
Generated from h = fz √(1 − (1 − 2ae/D)²) rather than transcribed. At 20% the geometry is a 3-4-5 triangle and the factor is exactly 1.25; at 50% and above there is no correction.
Starting feed per tooth, by cutter diameter and material
Inches per tooth for a solid end mill at moderate engagement. The panel above interpolates between these rows on diameter; the table itself is what it interpolates.
| Cutter | Mild / low-carbon steel | Alloy steel, annealed | Stainless steel, austenitic | Gray cast iron | Aluminum | Brass, free-machining | Titanium alloy |
|---|---|---|---|---|---|---|---|
| 1/8 in | 0.0005–0.0010 | 0.0005–0.0010 | 0.0004–0.0008 | 0.0006–0.0012 | 0.0010–0.0020 | 0.0010–0.0020 | 0.0003–0.0007 |
| 1/4 in | 0.0010–0.0020 | 0.0010–0.0018 | 0.0008–0.0015 | 0.0012–0.0025 | 0.0020–0.0040 | 0.0020–0.0040 | 0.0007–0.0012 |
| 3/8 in | 0.0015–0.0030 | 0.0015–0.0025 | 0.0012–0.0022 | 0.0020–0.0035 | 0.0030–0.0050 | 0.0030–0.0050 | 0.0010–0.0018 |
| 1/2 in | 0.0020–0.0040 | 0.0020–0.0035 | 0.0015–0.0030 | 0.0025–0.0045 | 0.0040–0.0070 | 0.0040–0.0070 | 0.0012–0.0022 |
| 3/4 in | 0.0030–0.0055 | 0.0030–0.0050 | 0.0022–0.0040 | 0.0035–0.0060 | 0.0050–0.0090 | 0.0050–0.0090 | 0.0018–0.0030 |
| 1 in | 0.0040–0.0070 | 0.0035–0.0060 | 0.0028–0.0050 | 0.0045–0.0075 | 0.0060–0.0110 | 0.0060–0.0110 | 0.0022–0.0038 |
Conventional starting feed-per-tooth ranges for solid end mills, of the kind published in tooling manufacturers' technical sections and in the milling feed tables of Machinery's Handbook, tabulated by cutter diameter and workpiece material.
Every cell here is a starting point rather than a fixed value, and is meant to be overwritten. Four things move it out of range. Radial engagement: below half the cutter diameter the chip thins and the feed per tooth must be raised to compensate — see radialChipThinningFactor. Axial depth: a full-depth slot at these feeds will break a small cutter; slotting is roughly half these values. Flute count: a 5-flute finisher in steel and a 2-flute in aluminum are not comparable at the same chip load. Tool overhang: the figures assume a cutter held short. A long-reach tool is deflection-limited and nothing in this table applies.
How to set a chip load for a light radial pass
Two of the three numbers, the stepover, and the pair of chip figures that come back.
Say which of the three numbers you are missing
Feed per tooth, feed rate and spindle speed sit in one relation and any two produce the third. Reading a chip load out of a program that is already running is the diagnostic direction; producing a feed rate from a table figure is the setup direction; producing a spindle speed is the direction you end up in when the feed rate is capped by the machine and the chip is the thing that has to be protected.
Enter the cutter, the material and — this is the one people skip — the radial width
Diameter and material read the starting band out of the table, interpolated to the exact diameter rather than snapped to the nearest row. Radial width is the stepover, not the depth of cut, and it is what decides whether the correction applies at all: anything from half the cutter diameter up to a full slot needs no correction, and everything below half needs one that grows quickly.
Read the two chip figures as a pair, never one alone
The panel reports what the control is being told and what the edge is actually taking, and the ratio between them. Those two are equal only at 50% radial engagement or more. At 10% stepover the programmed figure has to be 1.67 times the chip you want, and typing the table value straight into the control means the edge takes 60% of it — thin enough to rub instead of cut.
Technical specifications
| Starting table | 42 cells — six cutter diameters from 1/8 to 1 in against seven materials, spanning 0.0003 in per tooth (titanium, 1/8 in) to 0.0110 in (aluminum, 1 in) |
|---|---|
| Diameter handling | Linear interpolation between the tabulated rows, clamped at both ends, so a 0.30 in cutter is not fed like a 1/4 in one |
| Thinning relation | h = fz √(1 − (1 − 2ae/D)²), generated rather than transcribed. At 20% radial engagement the geometry is a 3-4-5 triangle and the factor is exactly 1.25 |
| Correction at light stepovers | ×1.400 at 15%, ×1.667 at 10%, ×2.294 at 5% — and ×1.000 at 50% and above, where a tooth reaches the center line while still cutting |
| Solved three ways | Feed per tooth, feed rate or spindle speed, whichever of the three you are short of; the other two plus the geometry produce it |
| Slotting | Not corrected and not tabulated: at full width the factor is 1.000 and the honest figure is about half the table, which the source table states rather than this page inventing |
| Units | Inches and millimeters per tooth on both chip figures, feed rate in in/min and mm/min; diameters accept 1/2, 0.5 or 12.7 mm |
| No network | The 42-cell table and the correction are both compiled into the page, so the numbers you type stay in the tab and the chart prints without a connection |
Frequently asked questions
Is chip load the same thing as feed per tooth?
In ordinary shop use, yes — chip load, feed per tooth and fz all name the same quantity, the distance the cutter advances while one tooth passes through the cut. The pedantic distinction is worth knowing anyway, because this page depends on it: feed per tooth is a programmed distance and chip thickness is a measured geometry, and the two are only equal when the cutter is engaged to at least half its diameter. Every catalog table is written as feed per tooth. Every failure of the cut is caused by chip thickness.
Why does a lighter radial cut need more feed per tooth rather than less?
Because a tooth cutting a narrow arc never reaches the cutter's own center line, which is where its bite would be at its thickest. The chip starts at nothing where the tooth enters, thickens as it swings round, and gets cut off early when the tooth exits the shallow engagement — so the thickest chip it ever produces is thinner than the advance per tooth. The relation is h = fz √(1 − (1 − 2ae/D)²), and at 20% stepover it works out to exactly 0.8, so the feed has to go up by 1.25 to get the intended chip back. Instinct says a light cut should be fed gently and instinct is wrong here, which is why high-efficiency toolpaths at 8 to 12% stepover run at feed rates that look like a typing error.
What do I change when the cut is a full-width slot?
Drop the feed per tooth to roughly half the tabulated figure and take far less axial depth. The table assumes moderate engagement, and a slot is the opposite of that in three ways at once: the tool is cutting on both sides so there is no free side for the chip to leave by, the radial force no longer pushes the cutter against one side of its own runout, and the chips are recut in the bottom of the groove. The thinning correction is switched off in a slot — engagement is 100% of the diameter — so nothing on this page will warn you. Slotting is the one case where a lower number than the table is the right answer.
Does a cutter with twice the flutes take twice the feed rate?
Yes for the feed rate and no for anything else, and the difference matters. Feed rate is spindle speed times flute count times chip load, so a 4-flute at the same speed and chip load feeds twice as fast as a 2-flute. What does not change is what one tooth is allowed to take, or the space available to carry the chip away. In aluminum a 4-flute at full depth packs the flutes solid and welds material to the edge, which is why 2 and 3-flute cutters exist for it at all. In steel the extra flutes are free performance up to the point where the machine cannot deliver the feed rate or the power.
Why is the chip load table organized by cutter diameter instead of just by material?
Because on a small cutter the limit is the shank, not the edge. A 1/8 in end mill in mild steel is tabulated at 0.0005 to 0.0010 in per tooth and a 1 in one at 0.0040 to 0.0070 — an eight-fold spread in the same material — and the reason is bending stiffness, which falls with the fourth power of diameter. The edge on the small cutter could take a bigger chip quite happily; the tool would snap before it got the chance. That is also why the small end of the table is where a rigid setup and a short stick-out buy the most.
What actually goes wrong when the chip is too thin?
The edge stops cutting and starts ploughing, and the heat that should have left in the chip goes into the tool and the workpiece instead. Every cutting edge has a small radius on it, and below a chip thickness of roughly that radius the material is pushed under the edge and smeared rather than sheared. In austenitic stainless this is catastrophic rather than merely inefficient: the smeared layer work-hardens ahead of the next tooth, so each pass is cutting harder material than the last and the tool is dead within minutes. It is the reason a heavy chip in 304 is safer than a light one, and the reason a dwell at the bottom of a hole ruins the next cut.
Does chip thinning happen in the axial direction as well?
It does, on any cutter whose edge is not parallel to the axis — a ball nose, a toroidal or button cutter, a face mill with a lead angle. The mechanism is the same one, applied to depth instead of width: the effective cutting geometry is inclined, so the chip presented to the edge is thinner than the axial advance and the feed has to be raised again. This page corrects the radial case only, because that is the one that applies to a square end mill doing ordinary work. The related correction on a ball nose is the surface speed one, which is a different quantity and is handled on the surface footage page.
About feed per tooth, and the correction that reverses the obvious answer
A milling cutter does not remove metal continuously. Each tooth swings in, peels a crescent-shaped chip and swings out, and the size of that crescent is what the tool life, the surface, the cutting force and the heat all depend on. Feed per tooth is the number that sets it: the table or the carriage advances a certain distance while one tooth is in the cut, and that distance is the chip. Everything else in a milling setup is downstream of it — the feed rate is only feed per tooth multiplied out by spindle speed and flute count, which is why changing the speed on a machine without changing the feed silently changes the chip and is such a reliable way to lose a cutter. Where the tabulated figures come from is a diameter and a material, and the diameter matters as much as the material does, because a small cutter fails by bending long before its edge is overloaded.
The correction this page is built around inverts what instinct says. Take a 1/2 in cutter stepping over 0.050 in — a tenth of its diameter — and the tooth is only in the cut for a short arc near the outside of the circle. It never gets round to the cutter's own center line, where its bite would have been thickest, so the thickest chip it produces is 0.6 of the programmed feed per tooth. Feed it at the table figure and it is taking a chip forty percent thinner than the table intended, which on a cutting edge with a real radius on it means burnishing rather than shearing: heat into the tool instead of into the chip, and in stainless a work-hardened layer waiting for the next tooth. The fix is to multiply the feed by 1.67 and put the chip back. This is the entire reason high-efficiency toolpaths work — they take a deep, narrow, fast cut whose chip is the same size as a shallow wide slow one, and spread the wear over the full flute length instead of the bottom quarter inch of it.
Two things this page deliberately does not do. It does not correct axially, because a square end mill has nothing to correct there and the cutters that do — ball noses, toroidal cutters, lead-angle face mills — need the surface speed handled first, which is what the surface footage page does. And it says nothing about whether the machine can deliver the feed it just recommended, which is a question about power and rigidity rather than geometry and belongs on the milling feed rate page, where the removal rate is turned into spindle horsepower. Drilling has no feed per tooth at all — a drill is fed per revolution and the drilling page explains why treating it as a two-flute end mill doubles the feed you meant to use. If the finish rather than the tool is what is driving the feed, the roughness a process can realistically hold is set out on the surface finish chart.
What happens to the cut you described
Every number on this page is worked out by JavaScript running in the tab you are reading it in. Nothing you type — loads, lengths, nameplate ratings, the rates your utility charges you — is uploaded, logged or kept, which is also why the calculators carry on working in a mechanical room with no signal.
The cutter, the stepover and the program values you were checking are read by JavaScript in this tab and never sent anywhere, so pasting a feed rate off a running program here tells nobody what you are making.