CNC Router Speeds & Feeds for Wood and Plastic A practical troubleshooting guide
Getting speeds and feeds right is one of the harder skills to develop on a CNC router — not because the maths is complicated, but because several variables interact at once and the consequences of getting it wrong are immediate and expensive. What does stay consistent is the logic underneath it all — and once that clicks, troubleshooting stops feeling like guesswork.
RPM, feed rate, and chip load. Most operators focus on the first two and ignore the third — but chip load is the one that matters most. Too low, and you’re rubbing rather than cutting. The tool generates heat instead of chips, and heat destroys both tooling and workpieces.
The Core Formula
- Chip Load = Feed Rate ÷ (RPM × Flutes)
- Feed Rate = Chip Load × RPM × Flutes
- Too low chip load → rubbing → heat → burn
- Too high chip load → overload → breakage
Target Chip Loads (6mm bit)
- Softwood (pine, macrocarpa): 0.05–0.10 mm
- Hardwood (rimu, tōtara): 0.04–0.08 mm
- MDF / particle board: 0.04–0.08 mm
- Acrylic (cast): 0.05–0.10 mm
- HDPE / polyethylene: 0.08–0.15 mm
- Aluminium composite: 0.02–0.05 mm
Treat these as starting points. Where you land in practice depends on your specific machine, tooling condition, and how rigid the workholding is. A machine with any flex in it needs to run more conservatively than the tables suggest.
Most hobby and prosumer routers sit between 10,000 and 30,000 RPM. A lot of operators set it to maximum and forget about it. That’s usually where problems start. Higher RPM means more heat — particularly dangerous with plastics and hardwoods.
18,000–22,000 RPM with a matched feed rate. These tolerate higher speeds but need the feed rate to keep up — don’t run fast spindle with slow feed.
16,000–20,000 RPM. Let chip load do the work, not spindle speed. NZ natives (rimu, tōtara) behave like medium hardwoods; macrocarpa is more forgiving.
16,000–18,000 RPM — err lower. Heat causes chips to re-weld in the kerf. If that happens, increase feed rate before dropping RPM.
12,000–16,000 RPM. Among the most heat-sensitive materials you’ll work with. Low RPM, fast feed, sharp tooling.
14,000–18,000 RPM with sharp, uncoated carbide. Dibond cuts well but the aluminium skins require reasonable rigidity in the machine.
Bit geometry has just as much influence on cut quality as your speeds and feeds. The three types you’ll use most in NZ workshop conditions:
For MDF — the most common NZ workshop material — a single-flute or two-flute upcut in solid carbide is the sensible default. MDF dust is genuinely abrasive and destroys cheaper tooling faster than almost anything else. Don’t try to save money on bits here.
Starting points for a hobby-to-prosumer CNC — Shapeoko Pro, WorkBee, 6040, or equivalent. Industrial machines can push considerably harder. Start here, get a clean result, then push gradually until quality slips, and back off 10%.
Wood & Sheet Materials
- Softwood: 2-flute upcut, 20k RPM, 3,000–4,000 mm/min, 3mm DOC
- Hardwood (rimu, oak): 2-flute upcut, 18k, 2,500–3,000, 3mm DOC
- MDF: 2-flute upcut, 20k, 3,000–4,500, 4mm DOC
- Baltic birch ply: compression, 18k, 2,500–3,500, full depth
Plastics & Composites
- Cast acrylic: O-flute, 17k, 3,500–4,500 mm/min, 3–4mm DOC
- HDPE: O-flute, 13k, 4,500–6,000, 4mm DOC
- Polycarbonate: O-flute, 16k, 3,000–4,000, 3mm DOC
- Aluminium composite: 2-flute upcut, 16k, 2,000–2,500, 1.5mm DOC
One deliberate change at a time. Listen to the cut — a clean result sounds even and consistent. A struggling cut chatters, screams, or occasionally goes quiet in a way that means something is about to break.
Almost always chip load too low — feed rate too slow, RPM too high, or both. A dull bit rubs before it cuts. Fix: increase feed rate first. If burns persist, bring RPM down. If both fail, the bit is past its useful life.
Upcut bit pulling fibres on top face, climb cutting, or depth of cut too aggressive. Fix: switch to downcut or compression for veneered materials. Use conventional milling. Take shallower passes.
Multi-flute bits can’t clear chips fast enough — they re-melt in the cut. Fix: use an O-flute or single-flute bit. Push feed rate up meaningfully. Compressed air or a small fan aimed at the cut zone helps considerably.
Usually depth of cut too aggressive, climb milling, or workpiece movement. Fix: keep DOC at or below 50% of tool diameter. Check workholding — any movement eventually breaks a tool. Check collet for runout; even 0.05mm shortens tool life noticeably.
Chip load too high, worn tooling, or machine vibration from loose mechanical components. Fix: drop feed rate by 20% and check whether finish improves. If the machine is vibrating, check gantry bolts and eccentric nuts before changing parameters.
GeoSaffer’s CNC routing work runs across hardwood joinery components, custom acrylic panels, and aluminium composite signage. If you’re working with an unusual material and can’t find reliable parameters, or you have a job that’s outpacing what your current machine can handle cleanly — we’re happy to talk through it, whether that means advice or just taking the job on.
Discuss your routing job with GeoSaffer →