Kerfwise CNC Feeds & Speeds Calculator

What it is for

Every new bit, material or cut raises the same question: how fast should the spindle turn and how fast should the machine move? Too slow a feed and the bit rubs, burns the edge and dulls quickly. Too fast and it deflects, chatters or snaps. The calculator gives you a sensible first setting before the first test cut.

You choose a material, the cutter diameter and the number of flutes, and either your spindle speed or a cutting speed. The tool looks up the chip load per tooth in a published router-bit chart for hardwood, softwood, plywood, MDF and particle board, acrylic, hard plastics and aluminium. It then adjusts for deep cuts and narrow side cuts and returns rpm, feed, removal rate and, where a specific cutting energy is known, the spindle power. Metric and imperial both work.

The numbers are starting values, not guarantees.

Worked example

The built-in example is a 6 mm two-flute compression bit in MDF at 18 000 rpm, slotting 6 mm deep. The chart range at 6 mm is 0.305–0.381 mm per tooth, and the middle value is 0.3431 mm. The result:

18000 rpm, feed 12352 mm/min at 0.3431 mm per tooth; removal rate 444.7 cm³/min. Estimated spindle power 0.4632 kW.

That feed is high on purpose: MDF wants big chips. If your machine cannot reach 12 m/min, lower the rpm rather than the chip load.

A second case is a finishing pass in hardwood with a 6.35 mm bit at 16 000 rpm, 12.7 mm deep and 1.5 mm wide. The 12.7 mm depth is 2 × D, so the chart value of 0.254 mm drops by 25 % to 0.1905 mm. The narrow 1.5 mm cut thins the chip, so the calculator raises the programmed chip load by a factor of 1.177 to 0.2242 mm. The feed comes out at 7176 mm/min. Hardwood has no built-in cutting energy, so no power is shown unless you enter one.

How to read the result

• Spindle speed and cutting speed: if you enter a cutting speed, rpm = Vc × 1000 / (π × D). Otherwise your rpm is used and the resulting cutting speed is shown.
• Chip load table: the chart range, the value you chose, the depth factor, the target chip thickness, the chip-thinning factor and the programmed chip load.
• Feed rate: rpm × flutes × programmed chip load. This is the number for your CAM or controller.
• Removal rate and power: width × depth × feed. Power uses a specific cutting energy, built in for MDF (0.05 J/mm³) and aluminium (0.7 J/mm³).
• Chart table: every built-in material's range at your diameter.

Tips and common mistakes

• Start at the low end of the range on a light hobby machine, then raise the feed until the finish suffers and back off by about 10 %.
• Leave the radial engagement empty for slots and profile cuts. Enter it only for real side cuts, otherwise the chip thinning raises the feed for nothing.
• If the spindle maximum caps the rpm, the feed drops with it. The warning tells you when that happens.
• In Kerfwise, use Feeds… next to an end mill in the CNC tool library to put the rpm and feed straight into the tool.

FAQ

Where do the chip loads come from?

From a widely published router-bit chart for solid-carbide spiral bits, as printed in tool makers' catalogues. Values between the 1/8, 1/4, 3/8 and 1/2 inch columns are interpolated.

Why does a narrow cut need a higher feed?

When less than half the cutter is engaged, each tooth takes a thinner chip than the feed per tooth. Raising the feed keeps the chip thick enough to cut instead of rub.

Can I use it for drills?

No. It is for end mills and router bits cutting sideways; drilling follows different rules.

Why is there no power for plywood or acrylic?

No published specific cutting energy is built in for those materials. Enter a value from your tool maker or your own measurement and the power appears.