Speeds and feeds: spindle speed, feed rate and power

It turns the cutting speed (sfm) and feed recommended for the material into machine numbers: spindle rpm, table feed, metal removal rate, power, torque and time per pass. It covers OD turning, milling and drilling with high-speed steel or carbide. Use it when programming a new part, switching materials or checking whether the machine has the horsepower for a roughing cut.

The best source is the tool maker’s catalog, which lists speed and feed by insert grade and ISO 513 material group (P, M, K, N, H). Changing material, tool or operation loads a typical starting value taken from tool makers’ guides and Machinery’s Handbook. Then tune it by wear: edges that wear fast call for a lower speed.

In the example, a 2 in medium-carbon steel bar turned at 720 sfm with carbide needs 1,375 rpm. At 0.010 in/rev and 0.08 in depth, the table moves 13.8 in/min, removes 6.9 in³ of chips per minute and the cut takes 6.06 hp at the tool, or 7.58 hp at the motor (76% of a 10 hp motor). Each 4 in pass takes 17.5 s.

kc1.1 and mc are the two numbers of the Kienzle equation, which says how much force it takes to cut the material: kc1.1 is the specific force for a chip 1 mm thick (1,700 N/mm² for medium-carbon steel) and mc shows how it rises as the chip gets thinner. US handbooks express the same idea as unit power, in hp per in³/min. In the example the page shows 0.88 hp per in³/min, the same order as handbook unit-power tables for medium-carbon steel.

Compare motor power with the spindle nameplate rating: below 85% the motor runs comfortably. The second chart shows how far you can go: in the example the 10 hp motor can take up to about 0.106 in depth at the same feed. Many spindles deliver less power at low rpm; check the power curve in the machine manual.

Using the wrong diameter (the workpiece in turning, the tool in milling and drilling), forgetting that maximum spindle speed caps the surface speed on small diameters, and using feed per revolution where the catalog gives chip load per tooth. The calculator does not account for workholding rigidity, chatter, tool stick-out or required finish, which often limit before power does.

With a carbide drill in medium-carbon steel, a typical speed is around 260 sfm, which gives about 2,650 rpm; with an HSS drill, around 60 sfm, or about 610 rpm. Typical feed runs about 0.004 to 0.007 in/rev depending on the drill. Pick Drilling as the operation to also see power, torque and time, and use the tap drill button if the hole will be threaded.