CNC Feeds and Speeds for Wood: A Calculator That Won't Burn Your Bits

July 19, 2026  ·  by CabiAI  ·  about 8 min read

Pick your material, bit and diameter below and you'll get a starting range for chipload, RPM, feed, plunge and depth of cut. Every number is calculated server-side from published manufacturer chipload tables — not a rule of thumb someone typed into a forum in 2011.

Why "just slow down" is the mistake that breaks bits

Every woodworker's instinct, when a cut sounds wrong, is to back off the feed. That is exactly the wrong move. When you slow the feed without touching RPM, each flute takes a smaller bite — it contacts the wood more often and carves less each time. Instead of cutting a chip, it rubs. Rubbing means heat, and heat burns the wood and the carbide both.

It feels backwards, and the tool manufacturers say the same thing: a chip the size of dust simply can't carry enough heat out of the cut. The right way to be conservative is not to slow the feed — it's to take a shallower pass, or drop RPM slightly so chipload stays in range. That's the whole principle behind this calculator: it keeps chip thickness where it belongs.

The four numbers, and how they relate

Everything comes from one equation. Get it and you'll never need to memorize a chart again:

Feed rate = RPM × number of flutes × chipload

• Chipload — thickness each edge removes per revolution. The real variable. Everything else is downstream.
• RPM — spindle speed. Comes from the material and gets reduced for large diameters (rim speed rises with diameter, and rim speed is what burns).
• Feed rate (IPM) — how fast the machine travels through the cut. The output of the equation, not an independent choice.
• Plunge rate — Z speed entering the material, roughly 30–50% of feed. Plunging at full feed rate is how you snap small bits.

Depth of cut: the number that depends on what you're doing

This is where most published rules of thumb quietly mislead you. "Never exceed 1× diameter" is a slotting rule — and slotting is a specific case where the cutter is buried, fully engaged on both sides, carrying double the load.

Cutting a part free from a sheet is a different operation. There the cutter is engaged on one side only, and 1×–2× diameter is routine: a 3/8" compression bit cuts 3/4" plywood in a single pass, every day, in every cabinet shop running a router. That's 2× diameter and it's correct.

Bit type shifts it too. Compression and upcut clear chips and can go deep. Downcut packs chips down into the cut (heat builds), and straight bits are less rigid — the calculator lowers depth for both automatically. Switch the tool type above and you'll see the number move.

Drills are a completely different animal

A drill doesn't work on per-flute chipload, and its numbers here come from real field tables, not from the metal-cutting surface-speed formula — a common error that produces numbers several times too low. A 5 mm dowel drill runs fast, around 3,500–6,000 RPM. A 35 mm hinge cup bit runs far slower on a single spindle (from 600 on a drill press) so it doesn't scorch the door.

One note from the field worth understanding: on an industrial drill bank (Biesse, SCM and the like) the head runs at a fixed RPM, typically 4,000–6,000 — and that same speed drives every bit, including the 35 mm. That's why the top of the RPM range for large diameters converges on bank speed rather than staying slow. If your RPM is fixed, use it, and let the calculator guide you on the plunge rate instead. In hardwood, drop RPM (~40%) so you don't burn.

Note the drill diameters above are metric, and that's deliberate — cabinet hardware is metric worldwide. Your 5 mm system holes and 35 mm hinge cups are 5 mm and 35 mm in Ohio exactly as they are in Munich.

The honest part: where the numbers come from, and what they aren't

These ranges are built on the well-known chipload tables from the tooling manufacturers (Onsrud and Freud among them), cross-referenced against each other. Three things you should know to trust them correctly:

• This is a starting point, not a law of physics. The manufacturers say the same in their own documents — "start here and tune." No calculator can give you a final number without seeing your cut.
• Brand doesn't change the numbers. A cheap import and a premium bit of the same geometry get the same starting point. What differs is how long the edge stays sharp — the cheap one dulls sooner and then starts rubbing. Watch for that, but don't change your settings because of it.
• The verified range has limits. The tables cover real cabinet tooling: router bits to 3/4" and drills to 35 mm. Past that you're into surfacing bits and insert heads with their own specs — the calculator won't guess a number for those, it'll point you to the manufacturer's chart. "No answer" beats a wrong answer when the answer feeds a machine.

From dimensions straight to machine files

This calculator helps you with a single tool. Real work is a longer chain: break the piece into parts, assign the router and drill operations to each one, place the holes and hardware, nest it onto sheets, and export a DXF or NC file the machine can actually run. That's the part that eats hours.

That's what CabiAI does in seconds: describe the piece in plain language and the system works out every part, hole and piece of hardware, nests it onto sheets, and hands you a cut-ready file — no drafting, no spreadsheet.