Speeds and Feeds Calculator

Calculate milling and drilling RPM and feed from diameter, material, and chip load. Turning uses the same page.

Calculator

Operation

Units

Workpiece material

Tool material

Tool diameter Example: 0.5 in end mill or drill.

Flutes Used for milling only. Example: 4-flute end mill.

Cutting speed (SFM) Starting value for the material. You can type a toolmaker SFM.

Chip load (in/tooth) Milling: chip load per tooth. Drilling and turning: feed per revolution.

About this calculator

One speeds and feeds calculator for milling, drilling, and turning RPM. Starting surface speeds are shop starting points, not a guaranteed cut. Browse the machining calculator hub.

Calculation Results

6112 RPM

Feed 97.8 IPM · 800 SFM · Milling

Formula: RPM = SFM × 12 / (π × D); Feed = RPM × chip load × flutes

How to use this result

Set the spindle to the RPM and the table or axis to the feed. The number is a starting estimate from the surface speed you entered. It is not a toolmaker limit, and it ignores stickout, slotting, coolant, and machine rigidity. If the cut chatters, lower speed or chip load before you change diameter.

Continue Your Calculation

After the cutting RPM, check whether the spindle motor can deliver torque at that speed.

Check motor torque →

Starting surface speed (SFM)

Workshop starting points for milling. Drilling on this page uses about 70% of the milling speed (60% for 304). Confirm with the toolmaker.

Material	HSS SFM	Carbide SFM	Mill chip load (0.5 in class)
Aluminum 6061	300	800	0.004 in/tooth
Mild steel 1018	90	350	0.003 in/tooth
Stainless 304	50	180	0.002 in/tooth
Cast iron	70	250	0.003 in/tooth
Brass	200	500	0.004 in/tooth
Acrylic	300	600	0.005 in/tooth

Speeds and feeds formula

Inch RPM: RPM = SFM × 12 / (π × D) ≈ SFM × 3.82 / D, with D in inches.

Metric RPM: RPM = Vc × 1000 / (π × D), with Vc in m/min and D in mm.

Milling feed: IPM = RPM × chip load × flutes.

Drilling or turning feed: IPM = RPM × feed per revolution.

Example: 0.5 in, 4-flute carbide end mill, aluminum, 800 SFM, 0.004 in/tooth. RPM = 800 × 3.82 / 0.5 = 6112 RPM. Feed = 6112 × 0.004 × 4 = 97.8 IPM.

Reverse direction (surface speed from RPM): SFM = π × D × RPM / 12. A 0.5 in cutter spinning 2,292 rpm runs at π × 0.5 × 2292 / 12 = 300 SFM. If you know your machine's top spindle speed and the cutter you own, this tells you the surface speed you can actually reach — useful when a tooling catalog asks for SFM but your spindle caps out first.

The spindle speed this calculator returns is the RPM in the formula above — "spindle speed calculator" and "RPM calculator" queries land on the same number. Likewise surface speed (sometimes written Vc or cutting speed) is the SFM input: one word family, two directions, one machine reality. Enter SFM from the tooling catalog, get spindle RPM; or enter the RPM your spindle can hold, get the surface speed you are really running.

Next, check shaft torque at that RPM with the motor torque calculator. Hub: machining calculator.

Surface speed from spindle RPM (lookup)

The reverse direction in one table: what surface speed (SFM) a cutter diameter actually sees at a given spindle speed. Read it two ways — check that your spindle's top RPM can reach the catalog SFM for the tool you own, or sanity-check the RPM you are about to program against the material's SFM band.

Surface speed in SFM = π × D × RPM / 12
Cutter Ø	1,000 rpm	2,000 rpm	3,000 rpm	6,000 rpm	10,000 rpm
1/8 in	33	65	98	196	327
1/4 in	65	131	196	393	654
1/2 in	131	262	393	785	1,309
3/4 in	196	393	589	1,178	1,963
1 in	262	524	785	1,571	2,618

The table explains the small-tool speed trap: a 1/8 in cutter at a modest 3,000 rpm only cuts at 98 SFM — far below most catalog minimums — which is why tiny tools want high-RPM spindles, while a 1 in cutter at the same 3,000 rpm is already at 785 SFM, past most steel values and into carbide-only territory.

Which mode to use

Job	Mode on this page	Feed input
End mill, face mill	Milling	in/tooth × flutes
Twist drill	Drilling	in/rev
Lathe OD or facing	Turning	in/rev
Spindle motor at the calculated RPM	Motor torque calculator	Not a cutting feed

Frequently Asked Questions

How do I calculate milling RPM from SFM?

Use RPM = SFM × 12 / (π × D), often written SFM × 3.82 / D with D in inches. A 0.5 in carbide end mill in aluminum at 800 SFM is 6112 RPM.

What is the difference between milling feed and drilling feed?

Milling feed is RPM × chip load × flutes. Drilling and turning use RPM × feed per revolution. Do not multiply a drill by flute count.

What SFM should I start with for aluminum and mild steel?

On this page, aluminum 6061 starts near 300 SFM HSS or 800 SFM carbide. Mild steel 1018 starts near 90 SFM HSS or 350 SFM carbide. Lower the speed for slotting, long stickout, or no coolant, then confirm with the toolmaker.

Does this replace a drill and tap chart?

No. This calculator returns spindle RPM and feed. It does not list tap drill diameters for thread sizes.

How do I use the RPM result with a spindle motor?

Open the motor torque calculator and enter that RPM with the motor power. Cutting speed is not the motor nameplate rating.

Is a spindle speed calculator different from this?

No — spindle speed is the RPM this page outputs. Spindle speed means how fast the tool rotates, in RPM. Enter the surface speed from your tooling catalog and cutter diameter, and the RPM result is your spindle speed setting on the machine.

What is surface speed (SFM) and where do I find it?

Surface speed is how fast the cutting edge travels through the material, measured in surface feet per minute (SFM) — metric catalogs call it Vc in m/min. Tooling catalogs list it per material and coating. It is the input here; the calculator converts it to spindle RPM for your cutter diameter. Going the other way, RPM back to surface speed is SFM = π × D × RPM / 12.

Is chip load the same as feed rate?

No. Chip load is per tooth per revolution (in/tooth or mm/tooth); feed rate is table travel per minute. Feed = chip load × flutes × RPM. Two cutters at the same table feed can load teeth very differently if flute counts differ — that is why the calculator asks for chip load, not IPM.

How do I avoid breaking small end mills?

Small diameters snap from runout and chip packing, not from raw speed. Derate chip load 30–50% for tools under 1/8 in, check the shank is clean in the collet, and clear chips with air or flood — recutting chips doubles the load. If it squeals, back off feed before you back off RPM: rubbing at low feed work-hardens the surface and dulls the tool faster.

Do drilling and milling use different feed math?

Yes. Mills feed per tooth: IPM = RPM × chip load × flutes. Drills and lathes feed per revolution: IPM = RPM × feed/rev. Selecting the operation in the calculator switches the formula — using the milling formula on a drill overstates feed by the flute count.

How do I convert to metric?

Switch the unit selector: Vc in m/min replaces SFM (1 SFM = 0.3048 m/min) and diameter in mm replaces inches (RPM = Vc × 1000 / (π × D_mm)). A 300 SFM aluminum cut is about 91 m/min; the RPM result for the same 0.5 in (12.7 mm) cutter matches either way.