Feed Per Tooth Calculator

What feed per tooth measures

Every milling job has three settings that matter more than the rest: how fast the spindle turns, how many teeth are in the cut, and how fast the table moves. Feed per tooth ties them together. It is the distance the cutter advances while one tooth passes through the material, so it describes the load on a single cutting edge rather than the load on the whole cutter.

Shops call it several things. Feed per tooth, chip load, fz, ipt and millimeters per tooth all mean the same measurement. The formula is one division: table feed divided by spindle speed times the flute count. A 0.500 inch three-flute end mill running at 3,000 RPM with a 27 inch per minute table feed works out to 27 ÷ (3,000 × 3) = 0.003 inch per tooth.

That 0.003 is the whole point of the page. Push it too low and the edge rubs instead of cutting: the material work hardens, the finish turns shiny and smeared, and the tool wears on its flank. Push it too high and the edge cannot carry the load, so the tool deflects and a small cutter snaps. The window between those two failures is wide in aluminum and narrow in stainless steel.

The numbers in the formula, and the units each one uses

Six measurements sit behind the calculation, and most of them have two homes: inches on an older American control, millimeters on a machine set to metric. Mixing the two is the most common way to get a feed rate that looks reasonable and cuts wrong.

Spindle speed is in revolutions per minute on both systems, so it never needs converting. Flute count is a whole number. Everything else does. A feed of 27 inches per minute is 685.8 millimeters per minute, and a chip load of 0.003 inch per tooth is 0.0762 millimeter per tooth, both from multiplying by 25.4. The NIST metric conversion tables give the exact factor, and NIST Special Publication 811 covers how far to round the result.

Keep the diameter in the same units as the feed. The diameter sets both the surface speed at the edge and how much the chip thins on a shallow cut, so a diameter typed in millimeters against a feed in inches throws the answer off by a factor of 25.4.

Worked example: 3 flutes, 3,000 RPM, 27 ipm

Take a 0.500 inch carbide end mill with three flutes, cutting a 0.250 inch radial depth in 6061 aluminum on a machine set to inches. The operator has dialed 3,000 RPM and 27 inches per minute. Here is the check, step by step.

First, teeth per minute. Each revolution brings three teeth past the cut, so 3,000 × 3 = 9,000 teeth per minute. Second, feed per tooth: 27 ÷ 9,000 = 0.003 inch per tooth. Third, feed per revolution, which is the same number times the flute count: 0.003 × 3 = 0.009 inch per revolution, and 27 ÷ 3,000 = 0.009 confirms it.

Fourth, the metric side. 0.003 × 25.4 = 0.0762 millimeter per tooth, and 27 × 25.4 = 685.8 millimeters per minute. Fifth, surface speed: 0.262 × 0.5 × 3,000 = 393 surface feet per minute, which is 119.7 meters per minute.

Is 0.003 inch per tooth sensible for 6061? Yes, and slightly conservative. A 0.500 inch carbide cutter in aluminum usually takes 0.004 to 0.008 inch per tooth, so this cut leaves room for a finish pass or for a machine with modest spindle power. The same chip load in 304 stainless would be aggressive, because stainless work hardens the moment the edge starts to rub.

Running the formula backward: chip load to table feed

Most of the time you start with a chip load from a tooling catalog and need the feed rate to type into the control. The same three numbers work in reverse: feed per tooth times spindle speed times flute count equals table feed.

At 3,000 RPM and 0.003 inch per tooth, a three-flute cutter runs at 0.003 × 3,000 × 3 = 27 inches per minute. Swap in a four-flute cutter at the same speed and chip load and the feed climbs to 0.003 × 3,000 × 4 = 36 inches per minute, because more teeth pass the cut. That is why a four-flute tool removes more material at the same chip load, and why it also needs more spindle power.

The same calculation in metric: 0.0762 millimeter per tooth at 3,000 RPM with three flutes gives 685.8 millimeters per minute. A router at 10,000 RPM with a 0.010 millimeter chip load and four flutes runs 400 millimeters per minute.

Read that table as a starting point, not a rule. Rigidity, overhang and coolant all move the safe chip load, and a long, thin cutter needs a lighter load than a stubby one of the same diameter.

Surface speed sets the RPM, not the feed

Feed per tooth and surface speed are two separate decisions that people often collapse into one. Surface speed is how fast the cutting edge travels through the material, measured in surface feet per minute or meters per minute. It depends on the material and the coating on the tool, and it decides the spindle speed.

Two forms of the same formula cover both directions: surface speed equals 0.262 times diameter times RPM, and RPM equals 3.82 times surface speed divided by diameter. Both constants assume the diameter is in inches. The Sandvik Coromant formula reference lists the same relationships in metric form, which is where 318.3 comes from. For a 0.500 inch cutter at 600 surface feet per minute, 600 × 3.82 ÷ 0.5 = 4,584 RPM. In mild steel at 90 surface feet per minute, 90 × 3.82 ÷ 0.5 = 687.6 RPM.

Now put a feed rate on each of those. Aluminum, three flutes, 0.004 inch per tooth at 4,584 RPM: 0.004 × 4,584 × 3 = 55 inches per minute, or 1,397 millimeters per minute. Mild steel, four flutes, 0.002 inch per tooth at 687.6 RPM: 0.002 × 687.6 × 4 = 5.5 inches per minute. The steel cut looks slow because both the surface speed and the chip load came down.

Small cutters need high spindle speeds to reach a sane surface speed, which is why a 1/8 inch end mill in aluminum wants 9,000 RPM or more.

Chip thinning on light radial cuts

Every number above assumes the cutter is engaged at least half its diameter. When the radial depth drops below half the diameter, the chip comes out thinner than the feed per tooth, because the tooth enters and leaves the material on a shallow arc. The programmed feed per tooth stays the same; the chip it cuts does not.

The correction is a factor built from the radial depth and the diameter. Double the radial depth, divide by the diameter, subtract that from 1, square the result, subtract it from 1 again, then take the square root. With a 0.125 inch radial depth on a 0.500 inch cutter, 2 × 0.125 ÷ 0.5 = 0.5, so 1 - 0.25 = 0.75 and the square root of 0.75 is 0.866. The chip is 86.6 percent of the programmed feed per tooth: 0.003 × 0.866 = 0.0026 inch.

To hold a real 0.003 inch chip on that light cut, divide instead of multiply: 0.003 ÷ 0.866 = 0.0035 inch per tooth. High feed mills are built around this effect, which is why their inserts run at chip loads that look far too heavy for the depth of cut they take.

The effect disappears at half immersion, where the factor is 1.000, and grows below 25 percent of the diameter, where it drops under 0.8.

Checking the number against the machine and the part

The arithmetic gives a feed the cutter can survive, not a feed the machine can execute. Three limits sit downstream of the formula.

Machine limits come first. Every control has a maximum feed rate, often 200 to 500 inches per minute on a small vertical mill, and a maximum acceleration. A feed that is fine in a straight line can outrun the control in a pocket full of short moves, where the machine never reaches the programmed rate and the chip load collapses.

Power and rigidity come second. Material removal rate is radial depth times axial depth times feed rate, and spindle power has to cover it. A 5 horsepower spindle will not pull a 0.500 inch cutter at full width and full depth in steel, whatever the chip load table says. Keep tool overhang below four times the diameter where the setup allows it.

Finish and workholding come third. A heavy feed leaves a visible scallop, and a part held in a vise by 0.100 inch of material will move before the cutter does.

Unit mistakes that change the answer

Three conversions cause most of the bad numbers on shop floors.

Inches per tooth against millimeters per tooth. A metric catalog might list 0.08 millimeter per tooth, which is 0.0031 inch, close to the 0.003 used above. Type 0.08 into a control that expects inches and the tool breaks on the first pass.

Inches per minute against millimeters per minute. The same 27 inch per minute feed is 685.8 millimeters per minute. A control set to metric reads 27 as 27 millimeters per minute, about one twenty-fifth of the intended feed, and the cutter rubs instead of cutting.

Diameter units inside the surface speed formula. The constants 0.262 and 3.82 assume inches. For a diameter in millimeters, use RPM equals 318.3 times surface speed in meters per minute divided by diameter in millimeters: 318.3 × 120 ÷ 12.7 = 3,008 RPM for a 12.7 millimeter cutter at 120 meters per minute.

One check costs nothing and catches all three. Multiply the chip load by the flute count and compare it with the feed per revolution on the control. If the two do not match, an input is in the wrong unit.