End Mill Speeds and Feeds Calculator
Spindle speed is 3.82 times the surface speed divided by the cutter's diameter, and the feed is that speed times the chip load times the flutes. A 1/2 in, 3-flute carbide end mill in 6061 aluminum at 1,150 SFM runs at 8,785 rpm and 105 in/min. Pick your material and cutter below for the numbers from Harvey Tool's chart.
Work out the speed and feed
Pick the material, the cutter's diameter and its flutes. The spindle speed and the feed come from Harvey Tool's published chart for solid carbide end mills, with the working shown.
100% is a full slot. Below 50% the chips get thinner than the feed per tooth, so the feed is raised to keep the chip the chart's size. The axial depth only sets the removal rate.
- Surface speed
- Chip load from the chart
- Chip load after thinning
- Feed per revolution
- Metal removed
A starting point from the chart, not a guarantee: rigidity, stickout, coolant and the tool's own maker's figures come first.
This material across the chart's sizes
How the speed and feed are worked
Harvey Tool's General Machining Guidelines give two numbers for each material when cutting with a solid carbide end mill: a surface speed range in surface feet per minute (SFM), and a chip load in inches per tooth (IPT) for each cutter size from 1/8 in to 1 in. The page gives the formulas that turn them into machine settings:
- RPM = 3.82 × SFM ÷ D, with D the cutter's diameter in inches. The 3.82 is 12 ÷ π rounded, the inches in a foot over the circumference; the calculator uses 12 ÷ π itself.
- IPM = RPM × IPT × T, the feed in inches per minute, with T the number of flutes (teeth).
In metric the same speed is meters per minute: 1 SFM is 0.3048 m/min, so Harvey's 800 to 1,500 SFM for wrought aluminum is 244 to 457 m/min, and a feed in inches per minute times 25.4 is millimeters per minute. Switch the calculator to millimeters and it takes the diameter in millimeters and gives the feed in mm/min, worked from the same chart.
The chart gives a range of speeds, not one figure. The calculator opens in the middle of the range and the slider moves it from the bottom to the top. That starting point is our choice; Harvey does not say where in the range to start. Where your cutter falls between two of the chart's sizes, say 5/16 in or 10 mm, the calculator takes the chip load on a straight line between the sizes either side, which is also our choice. Outside 1/8 in to 1 in it gives no answer, because the chart does not go there.
The chart for common shop materials
A few rows from Harvey's chart, with what a 1/2 in cutter runs at in the middle of each range, in a full-width slot. The calculator has all 33 of the chart's rows that we kept.
| Material (Harvey's grades) | SFM | IPT at 1/4 in / 1/2 in | 1/2 in cutter, mid-range |
|---|---|---|---|
| Wrought aluminum (2024, 6061, 7075) | 800 to 1,500 | 0.002 / 0.004 | 8,785 rpm, 105 in/min with 3 flutes |
| Carbon steel (10XX, 11XX, 13XX) | 100 to 300 | 0.0015 / 0.003 | 1,528 rpm, 18.3 in/min with 4 flutes |
| Austenitic stainless (304, 316) | 100 to 250 | 0.0005 / 0.0015 | 1,337 rpm, 8.0 in/min with 4 flutes |
| Gray cast iron | 100 to 400 | 0.002 / 0.004 | 1,910 rpm, 30.6 in/min with 4 flutes |
| Titanium (CP, 6Al-4V) | 50 to 250 | 0.0005 / 0.001 | 1,146 rpm, 4.6 in/min with 4 flutes |
| Nickel superalloys (Inconel 718) | 40 to 60 | 0.001 / 0.002 | 382 rpm, 3.1 in/min with 4 flutes |
| Acrylic, phenolic | 200 to 600 | 0.003 / 0.006 | 3,056 rpm, 36.7 in/min with 2 flutes |
Harvey's figures are general ones for any maker's carbide end mill. Where the maker of your tool publishes its own speeds and feeds for that exact tool, use those: Harvey itself points its own customers to tool-specific figures rather than this chart. A tool's coating, helix and flute count change what it can take, and the chart cannot know them. For choosing the tool in the first place, see the carbide end mill selection guide.
Light stepovers and chip thinning
The chart's chip load assumes the cutter is at least half buried in the cut. When the stepover (the radial depth of cut) is under half the diameter, each tooth meets the metal at a shallow angle and the chip it cuts is thinner than the feed per tooth. Harvey Performance explains that this "can lead to poor part finish, inefficient cycle times, and premature tool wear," and gives the feed that brings the chip back to the chart's thickness:
IPT = CT × D ÷ (2 × √(D × RDOC − RDOC²)), with CT the chip thickness you want (the chart's chip load), D the diameter and RDOC the stepover.
| Stepover | Feed per tooth, times the chart's | 1/2 in, 4 flutes, carbon steel at 200 SFM |
|---|---|---|
| 50% or more | 1.00 | 18.3 in/min |
| 25% | 1.15 | 21.2 in/min |
| 10% | 1.67 | 30.6 in/min |
| 5% | 2.29 | 42.1 in/min |
That is why the light, fast cuts of high-efficiency milling run at feeds that look far too fast against the chart: the chip is the same thickness. Adaptive and trochoidal toolpaths, which hold a light stepover all the way round, are covered in CNC machining techniques explained, and the CAM packages that write them in the best CAM software for small shops.
When the spindle cannot reach the speed
Small carbide cutters in aluminum want more revolutions than many machines have. A 1/4 in cutter at 1,150 SFM needs 17,571 rpm, and even at the bottom of Harvey's range, 800 SFM, it needs 12,223. Type your spindle's top speed and the calculator holds the speed there and works the feed from it at the same chip load: a 4,000 rpm knee mill turns that 1/4 in cutter at only 262 SFM and 24 in/min with 3 flutes. The calculator says when the capped speed falls below the bottom of the chart's range. The guide to choosing carbide end mills has what machinists report about carbide on speed-limited knee mills.
How many flutes
Harvey Performance's guide to selecting an end mill gives 2 or 3 flutes for non-ferrous materials, where the chips need room, and for ferrous work 4 for slotting, 3 to 5 for roughing, 5 to 7 for high-efficiency milling and 5 to 14 for finishing. The calculator fills in 3 flutes for metals like aluminum and brass, 2 for plastics and 4 for steels and the rest when you change material; type your own. More flutes at the same chip load means a faster feed, which is the point of them, but only if the chips have somewhere to go.
What the chart leaves out
The calculator carries 33 of Harvey's rows for carbide end mills. It leaves out three: Harvey's row for malleable and chilled iron gives a range of 90 to 2,500 SFM, which looks like a slip on the page, and its two "medium alloy" rows (grades listed as 200, 250, 301 and as 200, 250, 300) are too alike to tell a reader which is which. Harvey's separate table for diamond-coated end mills is not in the calculator either, and nor are high-speed steel cutters, which run slower than carbide: use the tool maker's figures for those. Holding the part is half of getting the numbers to work, so see dovetail workholding and four other techniques and 5-axis machining shortcuts.
Sources, read on 19 October 2026: Harvey Tool, General Machining Guidelines (surface speeds, chip loads by diameter and the milling formulas for solid carbide end mills); Harvey Performance, How to Combat Chip Thinning (the chip thinning formula); Harvey Performance, selecting an end mill (flute counts); NIST Handbook 44, Appendix C (1 in is exactly 25.4 mm; 1 ft is 0.3048 m). A starting point from published charts, not a guarantee: the machine, the setup and the tool maker's own figures come first.