Feed Rate Calculator

Feed Rate in Plain Terms

Feed rate is how fast the cutting tool travels through the workpiece, and on a mill it is set at the table: inches per minute of axis motion. Every revolution of the spindle, each flute slices a chip out of the material, and the thickness of that slice is the chip load, measured in inches per tooth (MIT Machine Shop Glossary). The table has to move fast enough that every tooth takes its bite, and the arithmetic that ties the three together is short enough to do in your head once you have done it twice.

The three inputs are spindle speed, chip load and flute count. Spindle speed sets how often each tooth hits the material. Chip load sets how much material each hit removes. Flute count sets how many teeth hit per revolution, so a 4 flute cutter at the same speed and chip load feeds twice as fast as a 2 flute cutter, because four teeth take a bite per revolution instead of two. Cutting too slow is as damaging as cutting too fast: a tooth that rubs instead of cutting work hardens the surface and dulls the edge, which is why the formula, not a feel for it, should set the dial.

The Two Formulas Every Mill Job Uses

The feed formula multiplies three numbers.

Feed (IPM) = RPM x chip load x flutes. A 4 flute end mill at 2,000 RPM with a 0.004 inch chip load gives 2,000 x 0.004 x 4 = 32 IPM.

To report feed in metric, multiply by 25.4, because one inch is exactly 25.4 millimeters: 32 IPM x 25.4 = 812.8 mm/min.

The reverse formula starts from surface speed instead. Tool makers publish a cutting speed for the material and tool combination, in surface feet per minute (SFM), which is the speed of the tool edge around its own circle. Convert it to spindle speed with RPM = SFM x 3.82 / cutter diameter in inches. The constant 3.82 is 12 inches per foot divided by pi, and it comes straight from the circumference of the cutter: SFM = pi x D x RPM / 12, rearranged. Using the exact value 12 / pi = 3.8197 instead of 3.82 moves the answer by well under half a percent, so 3.82 is the working constant.

The two formulas chain together in practice: surface speed picks the RPM, chip load and flute count turn that RPM into a table feed. The widget above runs both panels, so a job that starts from a catalog SFM number ends at a dial setting.

Three Worked Examples

Example 1 is the everyday case: a 0.5 inch, 4 flute carbide end mill in aluminum, spindle at 2,000 RPM, chip load 0.004 inch per tooth. Feed: 2,000 x 0.004 x 4 = 32 IPM, which is 32 x 25.4 = 812.8 mm/min.

Example 2 starts from surface speed. A first year manufacturing course at MIT works a 0.25 inch, 4 flute cutter in aluminum at 150 SFM with a 0.002 inch chip load. The spindle speed is 150 x 3.82 / 0.25 = 2,292 RPM, and the feed is 2,292 x 0.002 x 4 = 18.34 IPM. The MIT solution sheet, keeping more digits of pi, reports 2,291.8 RPM and 18.33 IPM, so the rounding difference is one hundredth of an inch per minute (MIT 2.008, Practice Quiz 1 solutions, 2025 course).

Example 3 is a lighter cut on a smaller machine: 3 flutes, 1,500 RPM, chip load 0.003 inch. Feed: 1,500 x 0.003 x 3 = 13.5 IPM, or 13.5 x 25.4 = 342.9 mm/min.

Type each set of inputs into the widget and the outputs match the table. Example 2 is worth doing twice, once through the RPM panel and once through the feed panel, because the chain from SFM to dial setting is the whole point of the tool.

Choosing a Chip Load

Chip load is the one input the formulas cannot give you, because it depends on the material, the cutter material, the rigidity of the setup and the depth of cut. The honest sources are tool maker catalogs and machining textbooks, which publish starting values per material family.

For a feel of the magnitudes, MIT's 2.008 course assigns free machining aluminum with uncoated or coated tools a feed per tooth of 0.08 to 0.46 mm per tooth and a surface speed of 300 to 3,000 m/min, citing the General Recommendations for Milling Operations table in Kalpakjian and Schmid's Manufacturing Engineering and Technology (Table 24.2) (MIT 2.008 Homework 2, 2025). In inch units that chip load range is 0.08 / 25.4 = 0.003 up to 0.46 / 25.4 = 0.018 inch per tooth, and the surface speed range is 300 / 0.3048 = 985 to 3,000 / 0.3048 = 9,843 SFM. These are coursework and textbook ranges for a specific material family, not official standards; for steel, stainless or titanium, use the range printed for your cutter by its maker.

Start low in the range on a light or chattering machine and move up until chips stay formed and the spindle load settles. The range matters more than the midpoint, because rigidity differs more between two hobby shops than between two textbooks.

From Surface Speed to RPM

The reverse panel answers the question catalogs pose: a data sheet says 150 SFM for this material and cutter, so what number goes on the spindle dial? Divide SFM x 3.82 by the cutter diameter in inches. Small cutters spin fast and large ones spin slow at the same surface speed, because a big cutter sweeps more circumference per turn.

At a fixed 150 SFM the same formula gives every diameter its own speed:

Halving the diameter doubles the RPM, which the table shows plainly: 2,292 at a quarter inch becomes 4,584 at an eighth. Two cautions belong next to this table. Spindle speed limits are real, so an unusually small cutter at high SFM can demand more RPM than the machine has, and the answer then is a lower SFM rating or a bigger cutter. And the diameter that matters is the effective cutting diameter: for a ball nose, the effective diameter shrinks with depth of cut, so the catalog RPM for the full diameter over speeds the edge at the bottom of the ball.

Units and Conversions

The formulas work in any consistent units, but machine dials and data sheets mix systems, so four conversions cover almost every job:

The 3.82 constant is itself a unit conversion in disguise: it converts a surface speed in feet per minute into a spindle speed for a diameter in inches, because 12 inches of circumference per foot divided by pi flattens the circle into a line. If you work in metric throughout, the equivalent form is RPM = 1000 x V (m/min) / (pi x D in mm), and it lands on the same spindle speed: for the 0.25 inch cutter, 45.72 m/min over a 6.35 mm diameter gives 1000 x 45.72 / (pi x 6.35) = 2,292 RPM, matching the inch calculation exactly.

Mistakes That Ruin Cutters

Feeding too slow is the quiet killer. A flute that takes no real bite rubs the surface instead of cutting it, generating heat that work hardens aluminum and stainless and rounds over the cutting edge in minutes. If chips come off as dust or fine powder instead of curls, the feed is too low for the RPM, and the fix is more feed or less speed, not less of both.

Feeding too fast breaks flutes, usually on the first pass into a corner where engagement spikes. The formula gives the table feed for steady cutting; corners, slots and full width cuts load every flute at once, so ease into them or reduce the feed. Ignoring flute count is the third classic: swapping a 2 flute bit for a 4 flute bit at the same dial setting doubles the effective chip load, which is the same as doubling the feed.

Two smaller traps finish the list. Confusing feed per revolution with feed per tooth leads to feeds that are a flute count off; feed per revolution is chip load x flutes, and the table feed is feed per revolution x RPM. And mixing diameter units, feeding an inch value into the metric form of the RPM formula or the reverse, misses by a factor of 25.4, which is the difference between a working cut and a snapped cutter.