Cutting Speeds and Feeds Formulas
The tool moves through the material at a specified rotational speed, defined in revolutions per minute (RPM), and feed rate, defined in inches per minute (IPM). Probably the most vexing problem for the beginning CNC machinist is selecting proper cutting speeds and feeds. This selection is actually more difficult on a CNC than a manual mill because, with a manual mill, the operator can feel the cutting pressure and alter the feed based in part on the cutting force.
CNC mills require calculating speeds and feeds in advance. These speeds and feeds can, and often are, adjusted at the machine based on chip shape and color, cutting sound, and machine horsepower meter readings.
The best source of data about cutting speeds and feeds for a specific tool, application, and material is the tool supplier. Much of this data is found on manufacturer's web sites or printed tooling catalogs. Tool sales representatives can be a valuable resource, so if you do a lot of machining, develop a good relationship with a knowledgeable representative.
Another source of speeds and feeds data is CAD/CAM software. These have become increasingly sophisticated and often provide good cutting data.
Yet even the best speed and feed data is just a starting point. Speeds and feeds require adjustment due to many factors including the maximum spindle speed or horsepower of the machine, rigidity of work holding, and the quality and condition of the machine tool itself.
The following pages provide cutting data for the most commonly machined materials and a methodology for calculating speeds and feeds. As always, use common sense. If the part is held by double sided tape, feeds based on vise work holding are probably too high. If the tool is very long and thin, speeds and feeds will likely require reduction.
Speed Formula
Milling machine cutting speeds are derived from the following formula:
 |
|
Figure 3.14: Speed Formula |
Speed is the rotational frequency of the tool (Spindle Speed) in revolutions per minute (RPM).
SFM (Surface Feet per Minute) is the speed at which the material moves past the cutting edge (outside diameter) of the tool in feet per minute. SFM values depend on the tool type, tool material, and material being machined.
Circumference is the circumference of the cutting tool in feet.
How Speed Formula is Derived
Because cutting tools are defined by their diameter in inches, this formula is rewritten and simplified as follows:
 |
 |
 |
|
Figure 3.15: Speed Formula (Simplified) |
Dia is the tool diameter in inches.
3.82 is a constant derived from 12/pi which converts the tool circumference in feet to diameter in inches.
Feed Formula
Cutting feeds are in IPM and use the following formula:
 |
|
Figure 3.16: Feed Formula |
Feed is the linear feed of the tool through the material in inches per minute.
Speed is the result of the speed formula (Figure 3.15) in revolutions per minute.
CL is the chip load, or how much material each cutting edge of the tool removes per revolution. Chip load is sometimes referred to as feed per tooth (FPT) or inches per rev (IPR).
NumFlutes is the number of cutting flutes. (For a twist drill, this value is one.)
Tap Feed Formula
For tapping operations, feed rate is based on the number of threads per inch and feed rate:
 |
|
Figure 3.17: Tap Feed Formula |
Feed is the linear feed of the tool through the material in inches per minute.
Speed is the result of the speed formula (Figure 3.15) in revolutions per minute.
TPI is the threads per inch of the tap. For example the TPI of a 1/4-20 tap is 20.