Milling Speeds and Feeds: How to Calculate and Adjust

Every milling operation is defined by a small set of numbers: cutting speed, feed per tooth, and the width and depth of cut. Catalogues give recommended values, but the machine needs spindle speed and table feed, and the catalogue values assume a short, rigid setup that the shop floor does not always have. This article gives the formulas, a table of starting values for common mold and die materials, and a guide to adjusting them when the cut does not behave.

The parameters

The four formulas

1. Spindle speed: n = (1000 × Vc) ÷ (3.14 × D)
2. Table feed: vf = n × z × fz
3. Metal removal rate: Q = (ae × ap × vf) ÷ 1000
4. Spindle power: P ≈ (ae × ap × vf × kc) ÷ (60,000,000 × 0.8) in kW

In the last formula, kc is the specific cutting force of the material in N/mm², and 0.8 is a typical machine efficiency.

Starting values

For coated solid-carbide end mills, side milling with a radial width of 30–50 % of the diameter. Feed per tooth is given for a 10 mm cutter.

Scaling feed per tooth with diameter. For steels, fz is roughly 0.5–1 % of the cutter diameter:

Always start from the tool maker's data for the specific tool when it is available. Use the tables when it is not, and begin at the lower end.

Worked example

Side milling pre-hardened mold steel (30 HRC) with a 10 mm, four-flute coated carbide end mill. Radial width 3 mm, axial depth 10 mm.

The Milling Cutting Conditions Calculator on this site runs the same calculation.

Three corrections the basic formulas miss

1. Effective diameter of ball-nose cutters. A ball-nose cutter working at a small depth cuts on a much smaller diameter than its nominal size.

• Effective diameter = 2 × √(ap × (D − ap))

A 10 mm ball at 0.3 mm depth cuts at 3.4 mm diameter. To reach 150 m/min it needs about 14,000 rev/min, not 4,775. If the spindle speed is calculated from the nominal diameter, the tool rubs at one third of the intended speed and finish and tool life suffer. Tilting the tool or the surface so the tip is not cutting also helps: the centre of a ball has zero cutting speed.

2. Chip thinning at small radial widths. When ae is below half the diameter, the actual chip is thinner than fz. At 10 % engagement, the chip is only 60 % of fz. Increase the feed per tooth to compensate, or the edge rubs instead of cutting.

3. Spindle speed limit. When the calculated speed is above what the spindle can reach, run at maximum speed and calculate the table feed from the real speed with the normal fz. Do not keep the table feed that belonged to the higher speed: that overloads each tooth.

Choosing ae and ap

Adjusting at the machine

Change one parameter at a time and note the result.

Two general rules:

• Stick-out matters more than anything else. Deflection grows with the cube of the unsupported length. A tool hanging out 5 × D deflects about eight times as much as one at 2.5 × D under the same force. For long reach, reduce ae and fz, not only speed.
• Run-out shortens tool life quickly. With 0.02 mm run-out and a feed of 0.04 mm per tooth, one tooth takes most of the load. Use good holders and check run-out on small tools.