Machining speeds and feeds calculator
From surface speed and cutter diameter to RPM, feed and removal rate.
Starting values for solid-carbide end mills from Harvey Tool; use your tool maker’s sheet when you have one.
How do I calculate spindle RPM from surface speed?
RPM = 12 × SFM ÷ (π × D) with D, the cutter diameter, in inches and SFM in surface feet per minute. Metric: RPM = 1,000 × Vc ÷ (π × D) with Vc in meters per minute and D in millimeters. A ½-inch cutter at 800 SFM turns 6,112 RPM; a 10 mm cutter at 100 m/min turns 3,183 RPM. Harvey Tool prints the shop shorthand RPM = 3.82 × SFM ÷ D, where 3.82 is 12 ÷ π rounded.
How do I convert SFM to meters per minute?
Multiply by 0.3048, since a foot is exactly 0.3048 meters. 100 meters per minute is 328.1 SFM. A speed means the same thing in both systems: the distance a point on the cutting edge travels along the work in one minute. The same RPM comes out either way: a 0.394-inch cutter at 328.1 SFM gives 3,183 RPM, the 10 mm cutter at 100 m/min.
How do I calculate the feed rate?
Feed rate = RPM × number of flutes × chip load per tooth. With the aluminum example, 6,112 RPM × 3 flutes × 0.004 inch per tooth = 73.3 inches per minute. Chip load is the thickness of the chip each tooth cuts per revolution. Too small a chip load makes the tooth rub rather than cut, which heats the tool and hardens the work; too large a load can break the cutter.
What is the material removal rate?
For milling it is the width of cut times the depth of cut times the feed rate, in cubic inches per minute. A ¼-inch radial width and a ½-inch depth at 73.3 inches per minute remove 9.17 cubic inches per minute (150.2 cm³/min). Divide it by the spindle power you have to see whether the cut is realistic; the calculator gives the removal rate only.
Where do the SFM numbers in the table come from?
From one source, Harvey Tool's General Machining Guidelines page (https://harveytool.com/resources/general-machining-guidelines), for solid carbide end mills, read October 27, 2026. Harvey gives an SFM range and a chip load for each cutter diameter from ⅛ to 1 inch. The page carries no revision date. These are the toolmaker's starting recommendations for its own cutters, not universal constants: other makers publish other numbers for other coatings and geometries, and the range is wide because a rigid machine with coolant can run faster than a light one.
Which end of the SFM range should I use?
Start at the low end, especially on an unfamiliar machine, a long tool stickout or a hard alloy, and increase the speed while watching the chip color, noise and tool wear. The calculator lets you pick the low end, the middle or the high end of the range. Titanium and nickel alloys have narrow practical windows because they work-harden and conduct heat poorly, so overspeeding wears the tool out faster than slow feeds do.
Does this work for drills, lathes and HSS tools?
The formula for RPM works for any rotating tool or workpiece: use the diameter of the drill, or of the workpiece on a lathe. The table, though, is for solid-carbide end mills, and high-speed steel tools run at a fraction of carbide speeds, so enter your own surface speed from the tool maker's chart for those. Drilling feeds are given per revolution rather than per tooth.
The formulas, step by step
Surface speed is the speed of the cutting edge past the work, and RPM follows from the circumference: a cutter D inches across travels π × D inches per revolution, which is π × D ÷ 12 feet. Dividing the SFM by that distance gives RPM = 12 × SFM ÷ (π × D). The feed rate then comes from how many teeth cut per revolution and how thick a chip each one takes. Both are shown with their intermediate numbers in the table of the result, and the unit toggle switches inputs between inches and millimeters.
Worked example
A ½-inch, three-flute end mill cutting 6061 aluminum, starting at the low end of Harvey's 800–1500 SFM range: RPM = 12 × 800 ÷ (π × 0.5) = 6,112. The table gives 0.004 inch per tooth for a ½-inch cutter, so the feed is 6,112 × 3 × 0.004 = 73.3 inches per minute, and a ¼ by ½ inch cut removes 9.17 cubic inches per minute. The same cutter in 304 stainless at the low end of 100–250 SFM runs 764 RPM; with four flutes at 0.0015 inch per tooth the feed is only 4.6 inches per minute. The stainless chip load is under half the aluminum one and the speed about an eighth, so the material comes off many times slower.
Common mistakes
Using the nominal tool size instead of the real cutting diameter (a worn or tapered tool changes it), forgetting that the SFM from a drill chart does not apply to an end mill, and adding flutes without checking the chip load: a four-flute tool at the same feed per tooth feeds a third faster than a three-flute one, and the machine has to supply that power. Another is ignoring chip thinning: when the radial width is less than half the cutter diameter the chip is thinner than the chip load suggests, and this calculator does not correct for that. Finally, remember that spindle speed is limited by the machine: a result above the maximum RPM only tells you the machine is the limit, and the tool will run at a lower surface speed.
Limits of this method
The vendor values are starting points for one family of tools. They do not know your coating, your tool stickout, your fixturing, whether you use flood coolant or an air blast, the hardness of the particular heat of steel or whether you are roughing or finishing. Chip load in the table is for the nearest listed cutter diameter that is not larger than yours; outside ⅛ to 1 inch, treat it as a rough guide only. The page does not cover turning, drilling feeds, threading or high-speed machining strategies, which have their own parameters. Use the manufacturer's recommendation for your specific tool whenever you have one.
Starting values for carbide end mills
| Material | SFM | m/min | Chip load, 1/4 in | Chip load, 1/2 in |
|---|---|---|---|---|
| Aluminum 6061, 7075, 2024 (wrought) | 800–1500 | 244–457 | .002 | .004 |
| Aluminum, cast (356, 380) | 500–1000 | 152–305 | .002 | .004 |
| Brass, yellow, red or high-lead | 800–1500 | 244–457 | .002 | .003 |
| Acrylic and phenolic plastics | 200–600 | 61–183 | .003 | .006 |
| Gray cast iron | 100–400 | 30–122 | .002 | .004 |
| Low-alloy steel, 10XX, 11XX, 13XX (mild steel) | 100–300 | 30–91 | .0015 | .003 |
| High-strength steel, 4340, 6150, H-13 | 50–250 | 15–76 | .001 | .001 |
| Stainless steel, austenitic 304, 316, 321 | 100–250 | 30–76 | .0005 | .0015 |
| Stainless steel, precipitation-hardening 17-4 | 90–250 | 27–76 | .001 | .002 |
| Titanium, commercially pure and 6Al-4V | 50–250 | 15–76 | .0005 | .001 |
| Nickel alloys, Inconel 718, Waspaloy | 40–60 | 12–18 | .001 | .002 |
Chip loads in inches per tooth. Full tables for eight cutter sizes, from 1/8 to 1 inch (0.125 to 1 in), are used by the calculator.
Sources: Harvey Tool (Harvey Performance Company), “General Machining Guidelines,” https://harveytool.com/resources/general-machining-guidelines, tables for carbide end mills (read October 27, 2026; the page carries no revision date). The tabulated figures are the manufacturer’s suggested starting points; verify them for your tool and machine and follow safe machining practice. Related: RPM to mph calculator, torque calculator, horsepower calculator, inches to centimeters. How we check our calculators.