Cutting Speed and Spindle Speed

This equation is nothing but the circumference of a circle multiplied by how many times it goes round per minute, and it is still the most misapplied relation in the trade. Cutting speed $V$ is how fast the workpiece surface passes the cutting edge. Spindle speed $N$ is how fast the machine turns. They are different quantities in different units, and the only thing joining them is $V = \pi D N$.

The classic mistake is reading a catalogue's cutting speed as an rpm. A carbide grade rated at 250 m/min set to 250 rpm on a 50 mm bar is cutting at 39 m/min — about a sixth of what the grade was made for. The symptoms are quiet: a poor finish, a slightly odd chip, and a tool life so long that nobody suspects anything is wrong. The same error on a 500 mm flywheel runs the tool at 393 m/min and destroys it in seconds, which at least announces itself.

Which diameter goes into the equation depends on what is turning. On a lathe it is the diameter of the workpiece at the surface being cut, and that shrinks with every roughing pass, so a constant rpm means a steadily falling cutting speed. This is exactly what a CNC lathe's constant-surface-speed mode exists to correct, and why that mode needs an rpm ceiling: as the tool approaches the centre of a face the equation demands infinite rpm, and the chuck has other ideas. Facing is the honest edge case — the cutting speed genuinely does fall to zero at the centre, which is why the tool rubs rather than cuts as it arrives, and why a facing cut leaves a little pip if the tool is not on centre height.

Milling and drilling invert the roles: the cutter is what turns, so $D$ is the cutter diameter and stays fixed for the whole job. A drill has the same problem as a facing cut in miniature — the cutting speed at the outside corner is the full $\pi D N$ and at the chisel edge it is zero, which is why the centre of a drill extrudes metal rather than cutting it and why large holes get a pilot.

Notice what the equation does not contain: nothing about the material, the tool, the feed or the coolant. It is pure kinematics, and it tells you nothing whatever about whether the speed you picked is a good one. Everything about that lives in Taylor's equation and in the data your tooling supplier publishes for the material you are actually cutting. On a manual machine the answer then has to be rounded to a gear the headstock actually offers, and the rule is to round down: a little under costs a little productivity, a little over costs tool life at the rate Taylor's exponent dictates.