How do I calculate RPM from surface speed?

In inch units, RPM = SFM x 12 / (pi x D), which shops shorten to SFM x 3.82 / D with D in inches. A 1/2" end mill at 600 SFM runs 4,584 RPM. In metric, RPM = Vc x 1000 / (pi x D) with Vc in m/min and D in mm, so a 10 mm tool at 200 m/min runs 6,366 RPM.

How do I calculate the milling feed rate?

Feed rate = RPM x number of flutes x chip load per tooth. Four flutes at 0.002 in/tooth and 4,584 RPM is 36.7 in/min. For turning and drilling the feed is RPM x feed per revolution.

What is radial chip thinning?

When the radial width of cut (ae) is less than half the tool diameter, each tooth enters the cut at a shallow angle and the chip it makes is thinner than the programmed chip load. A chip that is too thin rubs, heats the edge and shortens tool life. Multiply the target chip load by 1 / sqrt(1 - (1 - 2 ae / D)^2) to get the chip load to program. At 10% radial engagement the factor is about 1.67.

Why is my RPM limited by the machine?

Small tools often ask for more RPM than the spindle has. When the calculator clamps to your machine maximum it recalculates the surface speed you actually get and the feed rate at that RPM, so the chip load stays where you set it. On a lathe running constant surface speed, set a maximum spindle speed so the part does not overspeed as the diameter gets small.

Are the starting values safe to run?

They are deliberately conservative starting points for general-purpose tooling, not maximums. Your tooling vendor publishes speeds and feeds for each tool, coating and material, and those numbers should win. Adjust from there by chip color and shape, sound, finish and tool wear.

Free tool

Speeds and Feeds Calculator

Spindle RPM and feed rate for milling, turning and drilling from surface speed, diameter and chip load, in inch or metric. Pick a work material and tool material for a conservative starting point, add the radial width of cut to correct for chip thinning, and clamp to your machine's maximum RPM.

Speeds & feeds

Work material

Rigid machines with uncoated or ZrN-coated 2 and 3 flute tools often run several times faster. Clear chips so they are not recut.

Tool diameter (in)

Surface speed (SFM)

Starting value: 800 SFM. Leave blank to use it.

Chip load (in/tooth)

Enter the tool diameter for a starting value.

Flutes

Radial width of cut, ae (in), optional

Machine max RPM, optional

Enter a diameter and the flute count. Pick a work material for starting values, or choose Other and enter your own surface speed and chip load.

Starting values are conservative. Adjust them with your tooling vendor's data for the exact tool, then by how the cut sounds and looks.

Find CNC machine shops

Rather have a shop cut it? Send the drawing and , or browse CNC machining shops.

The formulas

RPM, inch: RPM = SFM x 12 / (π x D), or SFM x 3.82 / D with D in inches
RPM, metric: RPM = Vc x 1000 / (π x D), with Vc in m/min and D in mm
Milling feed: F = RPM x flutes x chip load per tooth
Turning and drilling feed: F = RPM x feed per revolution
Radial chip thinning factor: RCTF = 1 / √(1 - (1 - 2 ae / D)²) for ae < D / 2; program chip load x RCTF
Surface speed at a clamped RPM: SFM = RPM x π x D / 12 (m/min = RPM x π x D / 1000)

Worked example: a 1/2" four-flute end mill at 600 SFM turns 600 x 3.82 / 0.5 = 4,584 RPM. At 0.002 in/tooth it feeds 4,584 x 4 x 0.002 = 36.7 in/min. Take a 0.050" radial step (10% of the diameter) and the chip thinning factor is 1 / √(1 - 0.8²) = 1.67, so program 0.0033 in/tooth, about 61 in/min, to keep the same 0.002" chip.

Starting surface speeds by material

Conservative starting points for general-purpose coated carbide and HSS or cobalt tools, shown as SFM / m/min. They sit at or below the low end of what tooling vendors publish. Adjust them with the vendor's data for the exact tool, then by what the cut tells you.

Starting surface speeds in SFM and m/min by work material, tool material and operation
Material	Carbide mill	Carbide turn	Carbide drill	HSS mill	HSS turn	HSS drill
Aluminum 6061 / 7075T6 / T6516061 7075	800 / 244	1,000 / 305	600 / 183	300 / 91	400 / 122	250 / 76
Low-carbon steel 12L14 / 1018Hot rolled or cold drawn12L14 1018	400 / 122	500 / 152	300 / 91	90 / 27	100 / 30	80 / 24
4140 alloy steel, annealedAbout 200 HB4140	350 / 107	450 / 137	250 / 76	70 / 21	80 / 24	60 / 18
4140 alloy steel, pre-hard28 to 32 HRC4140	250 / 76	350 / 107	180 / 55	45 / 14	50 / 15	35 / 11
Stainless 304 / 316Annealed304 316	250 / 76	350 / 107	180 / 55	50 / 15	60 / 18	40 / 12
17-4 PH stainlessCondition A to H115017-4 PH	200 / 61	300 / 91	150 / 46	40 / 12	45 / 14	30 / 9
Titanium Ti-6Al-4VAnnealed, about 36 HRCTi-6Al-4V	150 / 46	180 / 55	100 / 30	30 / 9	35 / 11	25 / 8
Inconel 718Solution treated and agedInconel 718	60 / 18	100 / 30	40 / 12	12 / 4	15 / 5	10 / 3
Free-cutting brass C360Half hardC360	600 / 183	800 / 244	400 / 122	250 / 76	300 / 91	200 / 61
Delrin (acetal) / nylonUnfilledDelrin Nylon 6/6	500 / 152	600 / 183	300 / 91	300 / 91	400 / 122	200 / 61

Starting chip loads and feeds

Milling chip load and drilling feed grow with tool size, so they are given as a percent of the tool diameter: 0.5% of a 1/2" end mill is 0.0025 in/tooth, and of a 12 mm end mill 0.06 mm/tooth. Turning feed assumes a general-purpose insert with about a 1/32" (0.8 mm) nose radius. Values are carbide / HSS.

Starting milling chip load, turning feed and drilling feed by work material and tool material
Material	Milling chip load, % of D	At a 1/2" end mill, in/tooth	Turning, in/rev (mm/rev)	Drilling, % of D per rev
Aluminum 6061 / 7075T6 / T6516061 7075	0.8% / 0.6%	0.0040 / 0.0030	0.008 / 0.006 (0.20 / 0.15)	2.0% / 1.6%
Low-carbon steel 12L14 / 1018Hot rolled or cold drawn12L14 1018	0.5% / 0.4%	0.0025 / 0.0020	0.008 / 0.006 (0.20 / 0.15)	1.6% / 1.4%
4140 alloy steel, annealedAbout 200 HB4140	0.45% / 0.35%	0.0023 / 0.0017	0.008 / 0.005 (0.20 / 0.13)	1.4% / 1.2%
4140 alloy steel, pre-hard28 to 32 HRC4140	0.35% / 0.25%	0.0017 / 0.0013	0.006 / 0.004 (0.15 / 0.10)	1.2% / 1.0%
Stainless 304 / 316Annealed304 316	0.4% / 0.3%	0.0020 / 0.0015	0.006 / 0.004 (0.15 / 0.10)	1.2% / 1.0%
17-4 PH stainlessCondition A to H115017-4 PH	0.35% / 0.25%	0.0017 / 0.0013	0.006 / 0.004 (0.15 / 0.10)	1.0% / 0.8%
Titanium Ti-6Al-4VAnnealed, about 36 HRCTi-6Al-4V	0.35% / 0.25%	0.0017 / 0.0013	0.005 / 0.004 (0.13 / 0.10)	1.0% / 0.8%
Inconel 718Solution treated and agedInconel 718	0.25% / 0.2%	0.0013 / 0.0010	0.005 / 0.003 (0.13 / 0.08)	0.8% / 0.6%
Free-cutting brass C360Half hardC360	0.6% / 0.5%	0.0030 / 0.0025	0.006 / 0.005 (0.15 / 0.13)	1.8% / 1.6%
Delrin (acetal) / nylonUnfilledDelrin Nylon 6/6	0.8% / 0.6%	0.0040 / 0.0030	0.006 / 0.005 (0.15 / 0.13)	2.0% / 1.6%

Aluminum 6061 / 7075: Rigid machines with uncoated or ZrN-coated 2 and 3 flute tools often run several times faster. Clear chips so they are not recut.
Low-carbon steel 12L14 / 1018: Set for 1018. Leaded 12L14 is free machining and can often run up to about twice as fast.
4140 alloy steel, pre-hard: Use cobalt HSS if HSS at all. Above about 35 HRC switch to carbide.
Stainless 304 / 316: Work hardens. Keep the tool cutting: do not dwell or rub, and do not let the chip load drop too low.
17-4 PH stainless: H900 and H1025 are harder: start lower still.
Titanium Ti-6Al-4V: Heat stays in the tool. Use flood coolant, sharp edges and light radial engagement at higher chip loads.
Inconel 718: Carbide is strongly preferred. The HSS row is for cobalt drills and taps in small quantities.
Free-cutting brass C360: Use zero or neutral rake drills and tools so they do not pull in.
Delrin (acetal) / nylon: Sharp, polished tools. Heat melts and gums the cut before it wears the tool, so keep the chip thick.

Getting from a start to a good number

Run the starting value, then raise surface speed in steps until tool life or finish tells you to stop. Raise chip load until the part, the fixture or the tool pushes back.
Long stick-out and thin walls need lower speed and feed. Short, rigid setups can run well above these numbers.
Do not starve the tool. A chip load that is too light rubs instead of cutting, which work hardens stainless and burns plastics.
At light radial engagement, raise the chip load for chip thinning; do not raise the surface speed to make up the time.

When the spindle runs out

Small end mills on a 6,000 or 8,000 RPM spindle rarely reach carbide aluminum speeds. Clamp to the machine maximum and keep the chip load; the feed drops with the RPM.
On a lathe in constant surface speed mode, set a spindle clamp (G50 on many Fanuc-style lathe controls) before facing to center.
Drilling runs slower than milling in the same material: the cut is enclosed, chips and heat leave through the flutes, and edge speed falls to zero at the chisel point.

Related processes

CNC milling CNC turning CNC machining

Related tools and charts

Machining time calculator CNC machining cost estimator Bolt circle calculator Thermal expansion calculator Tap and drill size chart Surface finish chart Manufacturing glossary

Frequently asked questions

How do I calculate RPM from surface speed?: In inch units, RPM = SFM x 12 / (pi x D), which shops shorten to SFM x 3.82 / D with D in inches. A 1/2" end mill at 600 SFM runs 4,584 RPM. In metric, RPM = Vc x 1000 / (pi x D) with Vc in m/min and D in mm, so a 10 mm tool at 200 m/min runs 6,366 RPM.
How do I calculate the milling feed rate?: Feed rate = RPM x number of flutes x chip load per tooth. Four flutes at 0.002 in/tooth and 4,584 RPM is 36.7 in/min. For turning and drilling the feed is RPM x feed per revolution.
What is radial chip thinning?: When the radial width of cut (ae) is less than half the tool diameter, each tooth enters the cut at a shallow angle and the chip it makes is thinner than the programmed chip load. A chip that is too thin rubs, heats the edge and shortens tool life. Multiply the target chip load by 1 / sqrt(1 - (1 - 2 ae / D)^2) to get the chip load to program. At 10% radial engagement the factor is about 1.67.
Why is my RPM limited by the machine?: Small tools often ask for more RPM than the spindle has. When the calculator clamps to your machine maximum it recalculates the surface speed you actually get and the feed rate at that RPM, so the chip load stays where you set it. On a lathe running constant surface speed, set a maximum spindle speed so the part does not overspeed as the diameter gets small.
Are the starting values safe to run?: They are deliberately conservative starting points for general-purpose tooling, not maximums. Your tooling vendor publishes speeds and feeds for each tool, coating and material, and those numbers should win. Adjust from there by chip color and shape, sound, finish and tool wear.