Milling Speed and Feed: Metric Definitions and Formulas

Milling speed and feed formulas relate cutting speed, spindle speed, feed per tooth and table feed. This metric reference converts those quantities; it does not recommend cutting settings for a particular material or setup.

Cutting speed, spindle speed and feed are different

Cutting speed describes how fast the cutting edge travels around the effective cutting diameter. Spindle speed counts revolutions per minute. Table feed describes the relative advance of the tool and workpiece per minute. A spindle-speed value therefore cannot be used directly as a cutting-speed or feed value. Metric quantities and units

For a fixed cutting speed, changing the effective cutting diameter changes the required spindle speed. For a fixed feed per tooth, table feed also depends on spindle speed and effective tooth count. These relationships connect to the cutting motion explained in milling and turning.

Milling parameters and units

Use the cutting diameter and effective tooth count for the tool and operation, as defined in Sandvik Coromant’s metric reference.

Cutting speed and spindle speed formulas

• v_c = π × D_cap × n / 1000
• n = 1000 × v_c / (π × D_cap)

Keep D_cap in millimetres and v_c in metres per minute. Formula source

Table feed and feed per tooth formulas

• v_f = f_z × n × z_c
• f_z = v_f / (n × z_c)

Table feed is a distance per minute; feed per tooth is a distance assigned to each effective tooth. Do not substitute one number directly for the other. Formula source

For comparison, feed per revolution f_n = v_f / n, in mm/rev. Consequently, f_n = f_z × z_c under the same effective-tooth convention. Haas lists the per-revolution and per-tooth relationships separately. Haas metric formula sheet, PDF page 3

This page uses f_n for feed per revolution and f_z for feed per tooth. Keep that distinction when transferring values between tool documents that use different notation.

Calculate table feed: arithmetic example

Assume n = 3000 revolutions/min, f_z = 0.04 mm/tooth and z_c = 4:

v_f = 0.04 × 3000 × 4 = 480 mm/min.

Checking in reverse, 480 / (3000 × 4) = 0.04 mm/tooth. The inputs are invented for arithmetic illustration, not recommended machining values.

The same example gives f_n = 480 / 3000 = 0.16 mm/rev, which is four times the per-tooth value. This makes the difference between the two quantities explicit.

Why diameter and tooth count need checking

Haas uses D_tool and Z on its formula sheet; Sandvik uses D_cap at the cutting depth and z_c for effective teeth. The algebra agrees when the inputs describe the same operation. The symbols do not justify replacing an effective cutting diameter with an arbitrary catalogue diameter. Sandvik definitions, Haas definitions

An effective tooth count can also differ from the number of installed inserts. One Hoffmann chamfer-cutter data sheet lists three effective cutting edges and nine inserts. This is a tool-specific example, not a rule that every insert cutter needs its insert count divided by three. German tool data sheet, PDF page 2

Conditions and limitations

These relationships do not choose appropriate values or account for every tooling and setup constraint. Confirm effective geometry, cutting data and machine limits with the tool documentation and qualified personnel.

Finished-part acceptance requirements belong in the CNC quotation package; calculated cutting quantities do not prove part accuracy.