Cutting Tool Engineering
July 2014 / Volume 66 / Issue 7

Understanding cutting equations

By Christopher Tate

Surface feet per minute, chip load, unde-formed chip thickness and chip thinning are familiar shop terms. Over the last few weeks, however, several occurrences in our shop have made me realize there are a lot of metalworking professionals who don’t understand these terms and the calculations that go along with them. Whether you work at a small job shop or a large contract manufacturer, it is important to under-stand cutting tool calculations and how to use them to help drive significant efficiency gains.

Cutting speed calculations might well be the most important ones. They are easy to use and, with a little explanation, easy to understand. The cutting speed of a tool is expressed in surface feet per minute (sfm) or surface meters per minute (m/min.). Similar to mph for a car, sfm is the linear distance a cutting tool travels per minute. To get a bet-ter sense of scale, 300 sfm, for example, converts to 3.4 mph.

Toolmakers recommend cutting speeds for different types of workpiece materials. When a toolmaker suggests 100 sfm, it is indicating the outside surface of the rotating tool should travel at a rate of speed equal to 100 linear feet per minute. If the tool has a circumference (diameter × π) of 12", it would need to rotate at 100 rpm to achieve 100 sfm.

All images courtesy C. Tate

Imagine the cutting tool as a rolling ring or cylinder. The distance traveled in one revolution times rpm is its surface speed. If the circle above had a diameter of 3.82", the circumference would be 12". As a result, every revolution would produce a linear distance of 1', and a spindle speed of 100 rpm would be a cutting speed of 100 sfm.

The following equation is used to cal-culate spindle speed: rpm = sfm ÷ diame-ter × 3.82, where diameter is the cutting tool diameter or the part diameter on a lathe in inches, and 3.82 is a constant that comes from an algebraic simplifica-tion of the more complex formula: rpm = (sfm × 12) ÷ (diameter × π).

Because the tool diameter is measured in inches, the “feet” in sfm must be con-verted 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 diame-ter by π, or 3.14 to simplify. The result is: rpm = (sfm × 12) ÷ (diameter × π) = (sfm ÷ diameter) × (12 ÷ π) = (sfm ÷ di-ameter) × 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 par-ticular 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 revo-lutions across the shop floor. In that sce-nario, it would travel 100'; do it in 60 seconds and it would be traveling 100 sfm.

Lathes are different, of course, be-cause the workpiece rotates instead of the cutter. Because the formula for cut-ting speed is dependent on diameter, as the diameter of the workpiece decreases, rpm must increase to maintain a con-stant surface speed. After each circular cut on the lathe, the workpiece OD de-creases or the ID increases, and it is nec-essary 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 chang-ing diameter.

While the tool or part is spinning, the machine must know how fast to travel while the cutter is engaged in the work-piece. 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.

What is chip load? When milling, it is the amount of material that the cut-ting edge removes each time it rotates. When turning, it is the distance the part moves in one revolution while engaged with the tool. It is sometimes referred to as chip thickness, which is sort of true. Chip thickness can change when other parameters like radial DOC or the tool’s lead angle change.

Toolmakers publish chip load recom-mendations along with cutting speed recommendations and express them in thousandths of an inch (millimeter for metric units). For milling and drilling operations, chip load is expressed in thousandths of an inch per flute. Flutes, teeth and cutting edges all describe the same thing and there must be at least one, but, in theory, there is no limit to the number a tool can have.

Chip load recommendations for turn-ing operations are most often given in thousandths of an inch per revolution, or feed per rev. This is the distance the tool advances each time the part com-pletes one rotation.

What rpm and feed rate should be programmed for a 4-flute, 1" endmill, running at a recommended cutting speed of 350 sfm and a recommended chip load of 0.005 inch per tooth (ipt)? Using the equation, rpm = sfm ÷ diameter × 3.82 = 350 ÷ 1.0 × 3.82 = 1,337, the feed rate = rpm × no. of flutes × chip load = 1,337 × 4 × 0.005 = 26.74 ipm.

Here is where things get interesting, because by changing the values in the formula, the relationships of the differ-ent variables become evident. Try applying a 2" tool instead of the 1" tool. What happens? The rpm and feed rate decrease by half.

Understanding these relationships and applying some creative thought can pro-vide significant gains in efficiency. I will discuss how to take advantage of these relationships in my next column. CTE

About the Author: Christopher Tate is senior advanced manufacturing engineering for Milwaukee Electric Tool Corp., Brookfield, Wis. He is based at the company’s manufacturing plant in Jackson, Miss. He has 19 years of experience in the metalworking industry and holds a Master of Science and Bachelor of Science from Mississippi State University. E-mail:

CUTTING TOOL ENGINEERING Magazine is protected under U.S. and international copyright laws. Before reproducing anything from this Web site, call the Copyright Clearance Center Inc. at (978) 750-8400.