Speeds and feeds

Speed is surface speed, not RPM

Cutting speed is how fast the cutting edge moves past the material: surface feet per minute (SFM) in inch shops, meters per minute (m/min) in metric ones. Tooling makers give it per material and per tool material, because it is what sets the heat at the edge.

RPM is just how you get that speed. The same SFM needs fewer RPM on a bigger diameter, because each turn covers more distance. RPM = SFM × 12 ÷ (π × diameter in inches), or about 3.82 × SFM ÷ diameter. In metric, RPM = 1000 × m/min ÷ (π × diameter in mm).

On a lathe the diameter is the part’s; on a mill or drill it is the tool’s. Facing toward center, the diameter shrinks, so constant surface speed (G96) raises the RPM as it goes, up to the limit you set with G50.

Feed is how big a bite each edge takes

On a lathe, feed is per revolution: inches per rev (IPR) or mm/rev. On a mill, it is per tooth: the chip load. The machine needs a feed rate, so you multiply: IPM = RPM × number of teeth × chip load.

Feed sets the chip’s thickness, the cutting force and the finish. Too light and the edge rubs instead of cutting, which wears it and can harden the surface. Too heavy and the edge chips or the part chatters.

Which knob does what

Speed has the biggest effect on tool life: run too fast and the edge wears out from heat. Feed has the biggest effect on finish and on how much metal you remove for the same tool life. When a cut needs to be more productive, the usual order is: deeper cut first, then more feed, then more speed.

Light radial cuts in milling thin the chip, so the chip load has to go up to keep a real chip. The milling calculator does that for you.