Understanding Cutting Equations for Feeds and Speeds

Because the tool diameter is measured in inches, the “feet” in sfm must be converted to inches, and because there are 12 inches in a foot, multiply sfm by 12. In addition, the circumference of the tool is found by multiplying the tool diameter by π, or 3.14 to simplify. The result is: rpm = (sfm × 12) ÷ (diameter × π) = (sfm ÷ diameter) × (12 ÷ π) = (sfm ÷ diameter) × 3.82.

Notice the vertical lines, called tool marks, on the outside of the part being turned. As the feed rate increases, the distance between the lines also increases. The chip thickness is roughly equal to the feed.

Cutting speeds are published in sfm because the ideal cutting speed for a particular family of tools will, in theory, be the same no matter the size of the tool. The engineer, programmer or machinist is expected to calculate the rpm needed to produce the proper cutting speed for each selected tool.

So what is this telling us? Let’s say a 1″-dia. tool must run at 100 sfm. Based on the equation, that tool must turn at 382 rpm to achieve 100 sfm: 100 ÷ 1 × 3.82 = 382.

Another way to consider this concept is to think about the distance the 1″ tool would travel were it to make 382 revolutions across the shop floor. In that scenario, it would travel 100′; do it in 60 seconds and it would be traveling 100 sfm.

Lathes are different, of course, because the workpiece rotates instead of the cutter. Because the formula for cutting speed is dependent on diameter, as the diameter of the workpiece decreases, rpm must increase to maintain a constant surface speed. After each circular cut on the lathe, the workpiece OD decreases or the ID increases, and it is necessary for the rpm of the part to increase to maintain the desired cutting speed. As a result, CNC manufacturers developed the constant surface footage feature for lathe controls. This feature allows the programmer to input the desired cutting speed in sfm or m/min. and the control calculates the proper rpm for the changing diameter.

While the tool or part is spinning, the machine must know how fast to travel while the cutter is engaged in the workpiece. Feed rate is the term that describes the traverse rate while cutting.

Feed rate for milling is usually expressed in inches per minute (ipm) and calculated using: ipm = rpm × no. of flutes × chip load.

Feed-rate planning note: Start with RPM, flute count, and chip load, then verify the result against rigidity, radial engagement, and the actual finish target. For a cleaner worksheet, pair this article with Formula Resources and the Comprehensive Threading Calculators.

Formula: Feed Rate = RPM × Number of Flutes × Chip Load.