CNC Router Speeds, Feeds & Materials The complete guide for custom projects
Getting speeds and feeds dialled in separates clean, repeatable results from expensive frustration — and expensive is doing a lot of work in that sentence. This guide breaks down chip load, material-by-material parameters, and the tool geometry decisions that determine whether you get a good part or a ruined workpiece.
Speed is your spindle RPM. Feed is your feed rate — how fast the machine moves the cutter through the material. These two numbers are inseparable. Getting the balance wrong costs you in three distinct ways: tool breakage, rough finish from heat, or both simultaneously.
The goal is to hit the sweet spot where the cutter is removing material cleanly rather than rubbing against it. That sweet spot is defined by chip load — the thickness of material each cutting edge removes per revolution.
Chip Load = Feed Rate (mm/min) ÷ (RPM × Number of Flutes)
Running at 18,000 RPM with a 2-flute 6mm end mill at 2,160 mm/min: chip load = 2,160 ÷ (18,000 × 2) = 0.06mm per tooth — squarely in range for timber.
Target chip load: 0.05–0.10mm per tooth. Forgiving range — good starting point for dialling in a new setup.
Target chip load: 0.04–0.08mm per tooth. Pull back slightly from softwood settings — grain matters here.
Target chip load: 0.05–0.10mm per tooth. Single-flute O-flute bit essential — heat is the enemy, not force.
Target chip load: 0.08–0.15mm per tooth. Push feed rates harder — HDPE sheds heat easily.
Target chip load: 0.02–0.05mm per tooth. Conservative range — lubrication and rigidity are non-negotiable.
Target chip load: 0.01–0.025mm per tooth. Fragile tool — feeds under 600 mm/min, very shallow passes only.
Wood is relatively forgiving, but it has its quirks. MDF cuts cleanly and consistently until you see the dust volume — proper extraction is not optional. Fine MDF dust packs into the cut, ruins the finish, and presents a genuine respiratory hazard.
Typical Parameters (MDF)
- Spindle: 18,000–20,000 RPM
- Feed rate: 2,000–3,000 mm/min
- Depth of cut: 4–6mm per pass (6mm bit)
- Hardwoods: pull feed back ~20% from these
Common Issues
- Burn marks → feed too slow; increase feed rate first
- Chip-out on edges → wrong tool; use compression or downcut
- Fuzzy surface → dull bit rubbing, not cutting; replace it
- Plywood face chip-out → compression spiral, both faces clean
For NZ hardwoods like rimu or macrocarpa — common in custom joinery work — pull the feed back about 20% and consider a compression spiral bit for sheet goods. It cuts upward from the bottom and downward from the top simultaneously, giving clean edges on both faces.
Acrylic is where beginners most reliably go wrong. The intuition is to increase RPM for a cleaner finish. It achieves the opposite. High heat melts acrylic back onto the tool, rewelding chips directly into the cut and destroying the edge.
Cast Acrylic — Preferred
- Spindle: 16,000–18,000 RPM
- Feed rate: 2,500–3,500 mm/min
- Depth: 2–3mm per pass
- Single-flute O-flute bit only
HDPE / Polyethylene
- Push feed rates harder than acrylic
- Handles aggressive chip loads well
- Sheds heat easily — forgiving material
- Sharp tooling essential to avoid gumming
Polycarbonate is a different beast — tougher than acrylic, more prone to stress cracking, and it melts at lower temperatures than expected. Keep depth of cut shallow and introduce air cooling wherever possible. Do not run polycarbonate the same way as cast acrylic.
Routing aluminium on a CNC router demands respect. You are working at the edge of what a router spindle was designed to do. With the right setup — rigidity, chip clearance, lubrication — it is entirely achievable. At GeoSaffer in Auckland, 6061 is machined regularly for brackets, panels, and enclosures.
Parameters (6061, 6mm 2-flute)
- Spindle: 12,000–16,000 RPM (lower = more torque)
- Feed rate: 800–1,500 mm/min
- Depth of cut: 0.5–1.0mm per pass
- Finishing pass: 0.1–0.2mm for surface quality
Non-Negotiable Rules
- Never dry-cut without air blast — welds to carbide instantly
- Climb milling on finishing passes for surface quality
- Keep depth conservative — chatter snaps small tools
- 3mm end mills: under 600 mm/min, very shallow only
Cutting fluid or isopropyl alcohol mist applied continuously — not occasionally — is the difference between a clean part and a welded mess. The alloy matters too: 6061-T6 cuts cleanly, 5052 builds up on the tool edge, and 1000-series is best avoided entirely on a router.
Flute count, helix angle, and coating all influence the result. Choosing the wrong tool geometry for the material negates everything else in the setup.
General-purpose wood and plastics. Good chip evacuation, pulls chips up and out of the cut. Best for pocketing and profiling where top surface finish is not critical.
Clean top-surface finish in wood. Poor chip evacuation — do not go deep. Use on final passes where visible face quality matters most.
Best of both worlds — upcut from bottom, downcut from top simultaneously. The right choice for plywood and laminated sheet goods where both faces need to be clean.
Acrylics, soft plastics, and some foams. The large chip clearance evacuates material before heat can accumulate. More flutes means more heat in plastics — the opposite of intuitive.
Aluminium and harder materials. TiAlN coating reduces heat transfer to the tool. Change two variables at once and you learn nothing — adjust feed rate or depth of cut, not both simultaneously.
GeoSaffer’s CNC routing in Auckland spans architectural timber components, custom aluminium panels, and plastic fabrication for small manufacturers throughout New Zealand. If you are optimising your own setup or need a precision fabrication partner — we have made the expensive mistakes already and are happy to help you avoid them.
Get a quote or talk through your project →