CNC Feeds & Speeds Calculator

How it works

The calculator looks up a starting cutting speed for the material and tool, turns it into a spindle speed, and then sets the feed from the chip load. It uses the same speed ranges and chip loads as the Speeds & Feeds guide.

V_c is cutting speed, z the number of flutes, f_z the chip load per tooth, a_e the stepover and a_p the axial depth. Chip load is read from a table at 3, 6 and 12 mm for aluminum, mild steel and stainless steel, and interpolated for the diameter you enter. Other materials use these rows with a factor (brass 0.8 × aluminum, plastics 1.2 × aluminum, cast iron the same as mild steel, 4140 steel and titanium 0.8 × mild steel and stainless steel) and HSS end mills use 0.75 × the carbide value. “Conservative” and “Aggressive” also scale the chip load by 0.8 and 1.2. Those factors are estimates, so treat them as a starting point.

Worked example

A 10 mm, four-flute carbide end mill side-milling mild steel with a 1 mm stepover (10%), at a typical speed. Carbide in mild steel runs 75–150 m/min, so the typical value is 101 m/min. Spindle speed = 1000 × 101 ÷ (π × 10) = 3 223 RPM. The chip load for a 10 mm tool is 0.067 mm. The stepover is under half the diameter, so chip thinning applies: 10 ÷ (2 × √(10 × 1 − 1)) = 1.67, which gives a corrected chip load of 0.112 mm. Feed rate = 3 223 × 4 × 0.112 = 1 448 mm/min. With a 10 mm axial depth, the removal rate is 1 × 10 × 1 448 ÷ 1000 = 14.5 cm³/min. For drilling a 12.7 mm (1/2 in) hole in mild steel with an HSS drill at a typical speed, the calculator gives 714 RPM and a feed of 0.250 mm/rev.

Things to know

These are starting values. Real limits depend on your machine’s rigidity, the tool stick-out, the coolant, the exact alloy and the tool’s coating. Start at “Conservative” on a new tool or setup and work up.

Use the tool maker’s chart first. If your end mill’s manufacturer publishes speeds and feeds, those beat any general table.

The spindle limit changes the answer. Many hobby mills and routers top out at 6 000 to 24 000 RPM. When the ideal speed is higher, the tool runs slower than ideal but the feed drops with the RPM, so the chip load is right.

Burning and squealing usually mean the feed is too slow (a rubbing cut), not too fast. Raise the feed before you slow it down.

Deep cuts. The chip load is for axial depths up to about the diameter. Cut it by around 25% as the depth reaches twice the diameter.

Drilling. Feed per revolution grows with drill size and is lower in hard or tough materials. Pilot large holes and peck deep ones.

Safety. Always check the work holding and the tool’s maximum rated speed before running at the calculated RPM.

Common questions

What is chip load?

The thickness of material each cutting tooth removes on each pass. It is the key number to protect: too small and the tool rubs and wears, too large and it can chip or break.

Why is my feed rate higher with a small stepover?

With a light stepover each tooth only cuts for a short arc, so the real chip is thinner than the programmed chip load. The tool applies a correction (chip thinning) to bring it back to the right thickness.

Can I use this for routers and wood?

Not directly. Wood, MDF and similar materials are not in the list. See the Speeds & Feeds guide for router chip loads, which differ from metal values.

How do I choose between Conservative, Typical and Aggressive?

Conservative picks the low end of the speed range and feeds, good for new tools, small machines and long tool stick-out. Aggressive uses the upper-middle of the range and suits rigid machines with short tools and good chip evacuation.

Sources

• University of Pennsylvania, ME Design Lab, Feeds and Speeds guide (carbide end mill chip loads).
• Starrett, twist drill feed tables.
• Sandvik Coromant and Machining Doctor references for cutting speed ranges and the chip-thinning factor.

Last reviewed: November 2, 2026