🛠️ CNC Speeds and Feeds

Written and maintained by the PhDino author · Last reviewed 21 September 2026 · Checked against 2 independent reference calculations · how PhDino checks its numbers

Converting a material's recommended cutting speed into the spindle RPM and feed rate a CNC machine actually runs at.

Cutting speed (surface feet per minute, SFM) describes how fast the cutting edge of a tool should move through the material being cut — a property of the material and tool combination, not of any particular machine. A tougher, harder material generally wants a lower SFM; a softer, more machinable one tolerates a higher SFM without excessive tool wear or heat.

A CNC machine doesn't take SFM directly, though — it needs spindle speed in RPM, which depends on both the target SFM and the specific tool's diameter, since a larger-diameter tool covers more surface distance per revolution than a smaller one at the same RPM.

Feed rate — how fast the tool advances through the material — is a separate setting from spindle speed, built from chip load: how thick a chip each cutting edge (flute) should take per revolution. Multiply that by the number of flutes and the RPM, and the result is the linear feed rate the machine actually moves at.

Key formula

RPM = (SFM × 12) ÷ (π × tool diameter)
Feed rate (IPM) = RPM × number of flutes × chip load per tooth

How to use the CNC Speeds & Feeds calculator

Use this to turn the numbers a tool manufacturer publishes, a cutting speed in surface feet per minute and a chip load per tooth, into the two settings you actually enter on a machine: the spindle speed in RPM and the feed rate in inches per minute.

Take the SFM and chip load from the tool maker's chart for your tool and your material, then enter your tool's diameter and flute count. The calculator only converts; it does not know whether your machine, holder or workpiece can handle the result.

Cutting Speed (SFM) (SFM)

Surface speed of the cutting edge in surface feet per minute, from the tool maker's data for the material and coating. Aluminum with carbide tooling runs several times faster than steel, and stainless and titanium slower still.

Tool Diameter (in)

The cutting diameter of the tool in inches. Use the cutting diameter, not the shank, which can be a different size on reduced-shank tools.

Number of Flutes

The number of cutting flutes. Fewer flutes clear chips better in soft metals; more flutes give a finer finish in harder ones and allow a faster feed at the same chip load.

Chip Load per Tooth (in/tooth)

The thickness of the chip each tooth removes per revolution, in inches per tooth, from the tool maker's chart. Too low a value makes the tool rub instead of cut; too high can break it.

Worked example: a 1/2 inch end mill in aluminum

A 0.50 in, 3-flute carbide end mill is cutting 6061 aluminum. A conservative starting point from the tool chart is 600 SFM and a chip load of 0.004 in per tooth. What spindle speed and feed rate should be programmed?

Worked by hand:

1. Spindle speed. RPM = SFM × 12 ÷ (π × diameter) = 600 × 12 ÷ (π × 0.50) = 4,584 RPM. (The shop shortcut RPM ≈ 3.82 × SFM ÷ D gives 4,584.)
2. Feed rate. IPM = RPM × flutes × chip load = 4,584 × 3 × 0.004 = 55.0 in per minute.
3. Sanity check. The tool advances 3 × 0.004 = 0.012 in per revolution, and each of its 3 teeth takes a 0.004 in chip, which is what the chart asked for.

Program about 4,584 RPM and 55 IPM as a starting point. The spindle speed is within the range of most machines, but a smaller tool at the same SFM needs much more: a 1/4 in cutter would call for about 9,167 RPM, which may be above what a machine can turn. Halving the chip load would halve the feed to 27.5 IPM, and a 4-flute cutter at the same chip load would feed at 73.3 IPM.

Reading the result: starting values, not final ones

The published SFM and chip load are recommendations for a rigid setup and a fully engaged cut, and the numbers here are exactly as good as the values you feed in. They are a starting point to adjust by sound, chip shape and tool wear.

• Machine limits come first. A small tool can demand an RPM the spindle cannot reach, and a slow spindle then caps the feed. When the RPM is capped, the true chip load falls below what you intended.
• Light radial cuts need faster feeds. When the radial depth of cut is less than about half the diameter, the chip is thinner than the nominal chip load, and the feed can be raised to compensate (radial chip thinning).
• Rigidity limits everything. A long stick-out, a flexible workpiece or a weak fixture calls for lower speeds and a lighter cut than a chart assumes.
• Coolant and chip evacuation matter, especially in aluminum and deep slots, where chips packing into the flutes break tools long before the speed is wrong.

Notes & limitations

• Recommended SFM and chip load values come from tooling manufacturers' cutting data for a specific tool coating and material — this calculator turns those numbers into machine settings, it doesn't supply the SFM/chip-load numbers themselves.
• Running well below recommended parameters isn't automatically "safer" — too light a chip load can cause a tool to rub rather than cut cleanly, which paradoxically increases heat and wear rather than reducing it.

Common mistakes

• Using the maximum spindle speed as a default. The correct speed depends on the material and tool, not on what the machine can reach.
• Confusing chip load per tooth with feed per revolution. Feed per revolution is chip load times the number of flutes.
• Entering the shank diameter, which is not the cutting diameter on a reduced-shank tool.
• Copying values for a different material. Steel, stainless and aluminum differ by factors of several in surface speed.
• Trusting the numbers over the cut. If the tool squeals, chatters or packs with chips, back off regardless of what the calculation says.

Frequently asked questions

Papers worth reading

On the art of cutting metals Taylor, F. W. (1906), Transactions of the ASME. The experiments that tied cutting speed to tool life, the relationship behind every speeds-and-feeds recommendation since.