Feeds and Speeds Calculator

What this calculator does — and its lane

This is the surface-speed and feed-rate tool for chip-making operations: it converts a cutting speed into spindle RPM, and RPM into a feed rate, for milling, drilling, turning, tapping and CNC routing. It is built around the universal machinist relations — the same arithmetic every shop uses — not a database of tools or materials. The two numbers that actually depend on your tool and stock, the surface speed and the chip load, are yours to type in and tune; the calculator turns them into RPM, inches per minute and a removal rate. It is a place to start, then you dial it in by sound, chip colour and finish. It does not replace your cutting-tool maker’s recommended data, and it knows nothing about your specific tool — that is the honest friction here, and it is also why the answer is trustworthy: every figure comes from your inputs, not from a copied chart that may not match your tool at all.

Surface speed to RPM (SFM ↔ RPM)

Surface speed — SFM (surface feet per minute, also written SFPM), or in metric Vc in metres per minute — is how fast the cutting edge travels through the material. It is set by the material and tool, and stays roughly constant whatever the diameter, which is why a small cutter has to spin fast and a big one slowly to reach the same surface speed. Converting between surface speed and spindle RPM is the heart of every feeds-and-speeds calculation:

RPM = (SFM × 12) ÷ (π × D in) = 3.8197 × SFM ÷ D in
SFM = (RPM × π × D in) ÷ 12 = RPM × D in ÷ 3.8197
Metric: RPM = (Vc × 1000) ÷ (π × D mm) = 318.31 × Vc ÷ D mm

For example, 300 SFM with a half-inch tool is 3.8197 × 300 ÷ 0.5 ≈ 2,292 RPM; run it back the other way and 2,292 RPM on the same tool gives 300 SFM. The SFM ↔ RPM mode does exactly this and the same engine feeds every other operation. To go between systems, 1 SFM ≈ 0.3048 m/min and 1 inch = 25.4 mm.

Milling feeds and speeds

For an end mill, face mill, slitting saw or thread mill, first get the RPM from the surface speed and cutter diameter, then build the feed from how much each tooth bites:

IPM = RPM × z × fz
where z = number of flutes (teeth), fz = feed per tooth (chip load)
solve chip load: fz = IPM ÷ (RPM × z)

So 2,292 RPM on a 3-flute cutter at a 0.004 inch chip load is 2,292 × 3 × 0.004 ≈ 27.5 IPM. Enter a feed rate instead and the milling mode runs the formula backwards to tell you the chip load you are actually at — useful for checking a program against a sensible range. The metric form is the same shape: Vf (mm/min) = RPM × z × fz mm.

How to calculate feed per tooth (chip load)

Feed per tooth, feed per tooth (fz), chip load and IPT all name the same thing: the thickness of material each cutting edge should peel off per revolution. It is the single most important — and most misunderstood — number in milling. Rearranging the feed formula, chip load = IPM ÷ (RPM × flutes). Leave the feed-rate box filled and the chip-load box empty (or vice versa) and the tool solves whichever you left blank. Chip load lives in a narrow band, typically somewhere around 0.001 to 0.010 inch depending on tool size and material — you enter your own. Too small is not “gentle”: below a certain thickness the edge stops cutting and starts rubbing.

Drilling speed and feed

A drill feeds per revolution rather than per tooth, so its feed math is simpler:

RPM = 3.8197 × SFM ÷ D in
IPM = IPR × RPM  (IPR = feed per revolution)

A reamer uses the same formula but is run differently: a noticeably lower surface speed with a higher feed per revolution than a drill of the same diameter, because it is sizing and finishing an existing hole, not creating one. The drilling mode covers both — just enter the lower SFM and larger IPR for reaming.

Lathe / turning speed and feed

Turning uses the same surface-speed-to-RPM step, with one twist: the diameter is the workpiece, and it changes as you cut. The feed is again per revolution:

RPM = 3.8197 × SFM ÷ D workpiece in
IPM = IPR × RPM

Because the diameter falls as material comes off, the RPM needed to hold a constant surface speed rises — which is why most lathes offer constant-surface-speed (CSS) mode and you program the surface speed directly. This calculator gives the RPM for the diameter you enter; in CSS you would simply set the surface speed and let the machine track it.

Tapping speed and feed

Tapping is the one operation where the feed is not yours to choose: a tap advances exactly one thread pitch per revolution, so the feed is locked to the thread.

RPM = 3.8197 × SFM ÷ D in
IPM = RPM × (1 ÷ TPI)  [inch]  or  RPM × pitch mm [metric]

A 1/4–20 tap at 500 RPM feeds 500 ÷ 20 = 25 IPM — not a number you set, a number the thread dictates. Taps also run far slower in surface speed than milling or drilling. The tapping mode swaps between threads-per-inch and a millimetre pitch with the unit toggle.

CNC router feeds and speeds

A router uses the milling engine — IPM = RPM × flutes × chip load — with two differences worth respecting. First, router spindles usually run a fixed RPM (commonly 10,000–24,000), so it is often cleaner to type your actual RPM and let the feed follow. Second, the Z (plunge) move matters: many bits should not be plunged straight down at full feed. A common rule of thumb is to limit the plunge rate to roughly half the cutting feed, and to ramp or helix in rather than drilling straight down — the router mode shows that suggested plunge rate. Burning is the number-one router complaint, and it comes from feeding too slowly for the RPM, not too fast: if the wood scorches, speed the feed up or slow the spindle down.

Surface feet per minute chart (RPM by diameter)

This is pure geometry — the spindle speed that holds one chosen surface speed across a range of diameters. Set the surface speed and the table fills in. It works as a milling-cutter speed chart, a drill-speed chart or a lathe chart alike, because the conversion does not care what the tool is.

Geometry only: RPM = 3.8197 × surface speed ÷ diameter (inch), or 318.31 × Vc ÷ diameter (mm). Round to a speed your spindle actually offers.

Generic starting surface speeds by material

These are broad, generic starting points only — editable, and always defer to your cutting-tool manufacturer’s recommended data for your exact tool and material. They are deliberately wide because the right number depends on the tool material, coating, coolant and rigidity, which this table cannot know. As a rule, HSS tools run toward the low end and carbide toward the high end; coolant and coatings let you push higher. Type a value into the calculator above and tune from there.

Chip load is similarly a starting point you enter, typically around 0.001–0.010 inch and scaling with tool size — a rough rule is a fraction of a percent of the cutter diameter, narrowed by material and flute count. Use your tool maker’s figure where you have it.

Speeds and feeds in metric

Everything works in metric with the unit toggle. Surface speed becomes Vc in metres per minute, diameters and chip load are in millimetres, and feed rate is millimetres per minute: RPM = 318.31 × Vc ÷ D mm and Vf = RPM × z × fz mm. To convert, 1 inch = 25.4 mm and surface speed in m/min = SFM × 0.3048. For instance, 100 m/min on a 10 mm cutter is 318.31 × 100 ÷ 10 ≈ 3,183 RPM. The arithmetic is identical; only the labels and constants change.

Why a light cut can burn: radial chip thinning

The most common surprise for newcomers is that a lighter cut can be harder on the tool. When the radial width of cut (stepover) drops below half the cutter diameter, the geometry of the arc means the real chip is thinner than your programmed chip load — so at a small stepover the edge can fall below the thickness where it cuts and start rubbing, generating heat, work-hardening the surface (badly in stainless) and burning wood. The fix is counter-intuitive: raise the feed to restore the chip thickness, which is exactly what adaptive and trochoidal toolpaths do. The optional adjustment in milling mode applies the standard factor:

RCTF = 1 ÷ √(1 − (1 − 2·ae÷D)²)
adjusted feed = base IPM × RCTF  (only when stepover ae < D÷2)

With a 0.1 inch stepover on a 0.5 inch cutter, RCTF = 1 ÷ √(1 − 0.6²) = 1 ÷ √0.64 = 1.25, so the feed goes up 25% to keep the same chip thickness.

A worked milling example

Cutting aluminium with a 3-flute, half-inch carbide end mill, starting at 300 SFM and a 0.004 inch chip load:

• RPM = 3.8197 × 300 ÷ 0.5 ≈ 2,292 RPM.
• Feed = 2,292 × 3 × 0.004 ≈ 27.5 IPM.
• At a 0.1 inch stepover and 0.25 inch depth, removal rate = 0.1 × 0.25 × 27.5 ≈ 0.69 in³/min.
• Because the stepover is below half the diameter, the chip-thinning factor is 1.25, so the adjusted feed is about 34.4 IPM to hold the chip at target.

Those are first numbers. Listen to the cut, look at the chips — consistent curls, straw to light blue in steel, are the goal — and adjust.

Terms, in plain English

A note on spelling and symbols for readers outside the US: “aluminium” and “aluminum” are the same metal, surface speed appears as SFM, SFPM or surface feet per minute in inch shops and as Vc or m/min in metric ones, and feed shows up as IPM, IPR, IPT or as mm/min and mm/rev. The relationships are identical; only the units differ.