CNC Router Speeds and Feeds for Wood: Complete Setup Guide

Why Wood Is Different from Metal

Metal is isotropic — its mechanical properties are the same in every direction. A piece of 6061 aluminum cuts the same whether you're milling along the grain or across it (because aluminum doesn't have a grain). Wood is anisotropic. Its strength, hardness, and cutting behavior change dramatically depending on whether you're cutting with the grain, across the grain, or into end grain.

Cutting with the grain (ripping) produces long, clean fibers that evacuate easily. Cutting across the grain (crosscutting) shears the fibers and is more likely to cause tear-out on the exit side. Cutting into end grain is the hardest cut — the tool is splitting fibers apart rather than shearing them, which requires more force and generates more heat.

The second major difference is heat sensitivity. Metals can tolerate hundreds of degrees at the cutting edge without permanent damage (the heat colors steel but doesn't destroy it). Wood combusts. The ignition temperature of most hardwoods is around 400-500°F, and the friction temperature at a rubbing cutting edge can easily reach that. This is why burn marks happen — the wood is literally scorching at the cut surface.

The third difference is chip evacuation. Metal chips are dense and fall away by gravity. Wood chips are light, fluffy, and tend to pack into the cut. A clogged flute generates friction, which generates heat, which causes burning. Effective dust collection is not optional for CNC wood routing — it's part of the cutting system.

Finally, wood contains moisture. Green lumber can be 30%+ moisture content, and even kiln-dried lumber is typically 6-8%. Moisture affects cutting forces, chip formation, and the tendency for the workpiece to move during machining. Wet wood gums up cutters and produces fuzzy surfaces. Stable, properly dried wood machines cleanly.

Chip Load Calculation for CNC Router Bits

The chip load formula for wood routing is identical to metal milling: Chip Load (inches per tooth) = Feed Rate (IPM) ÷ (RPM × number of flutes). What differs is the target chip load range and the consequences of getting it wrong.

For CNC router bits in wood, typical chip load ranges are: 1/4" diameter bit: 0.003 to 0.006 IPT. 3/8" diameter bit: 0.005 to 0.010 IPT. 1/2" diameter bit: 0.007 to 0.015 IPT. 3/4" diameter bit: 0.010 to 0.020 IPT. These ranges are wider than metal because wood is more forgiving of chip load variation — but the extremes (too light or too heavy) cause specific, identifiable problems.

Chip load too low (rubbing): The bit rubs instead of cutting. Friction generates heat. You get burn marks on the wood surface, especially in hardwoods like maple, cherry, and oak. The tool edge dulls rapidly from the heat. The surface may look polished (from friction) but discolored (from heat). Solution: increase feed rate.

Chip load too high (overfeeding): The tool tries to take too big a bite. You get rough surfaces, splintering, chip-out on edges, and possibly deflection of the bit (which causes inaccurate cuts). On thin material, the bit can pull the workpiece out of the hold-down. Solution: decrease feed rate or increase RPM.

The sweet spot: A proper chip load produces clean chips (not dust and not chunks), a smooth cut surface with no burn marks, minimal fuzz, and consistent dimensions. The chips should look like small flakes, not powder. If you're producing powder instead of chips, your chip load is too low.

Router RPM Settings: Finding the Right Speed

CNC routers spin much faster than metalworking mills. A typical CNC router spindle runs 8,000 to 24,000 RPM, while a VMC metalworking spindle tops out at 8,000 to 15,000 RPM. This high RPM is necessary because router bits have fewer flutes (usually 1, 2, or 3) and the soft material allows higher surface speeds without excessive tool wear.

Trim routers (Makita, DeWalt, etc.): These are common on hobby and light-commercial CNC routers like the Shapeoko, X-Carve, and similar machines. They typically run 10,000 to 30,000 RPM with speed dial settings rather than precise RPM control. The relationship between dial setting and RPM varies by brand and must be calibrated with a tachometer. A Makita RT0701C on dial setting 1 runs about 10,000 RPM; on dial 6, about 30,000 RPM.

VFD-controlled spindles (1.5 kW, 2.2 kW, etc.): These are common on mid-range and commercial CNC routers. They provide precise RPM control via the VFD (Variable Frequency Drive). Typical operating range is 8,000 to 24,000 RPM. The VFD allows the controller to set RPM automatically via G-code (S command), which is important for tool changes where different bit diameters need different speeds.

RPM selection principle: The surface speed (SFM) at the cutting edge determines how fast the material is moving past the cutting edge. SFM = π × diameter × RPM ÷ 12. For wood, target SFM is typically 300-800 for softwoods and 400-600 for hardwoods. A 1/4" bit at 18,000 RPM produces SFM = 3.14 × 0.25 × 18,000 ÷ 12 = 1,178 SFM — which is on the high side but acceptable for softwoods with sharp tooling.

In practice, most CNC router operators run 16,000 to 18,000 RPM for general-purpose cutting with 1/4" bits, and 12,000 to 16,000 RPM for larger bits (1/2" and up). The key is balancing RPM against feed rate to achieve the target chip load. If you increase RPM, you must increase feed rate proportionally to maintain chip load.

Tool Selection: Upcut, Downcut, and Compression Bits

The helix direction of a router bit determines how chips are evacuated and whether the top or bottom surface gets the cleaner cut. This is one of the most important and least understood aspects of CNC wood routing.

Upcut bits: The flute helix pulls chips upward, out of the cut. This is excellent for chip evacuation, especially in deep slots and pockets. But the upward pulling action also lifts the fibers on the top surface, causing tear-out and fuzzy edges on the upper face. Upcut bits produce a cleaner bottom surface and a rougher top surface. Use them for: pocketing operations, through-cuts where the top surface will be hidden, and any cut where chip evacuation is the priority.

Downcut bits: The flute helix pushes chips downward into the cut. This pushes fibers down on the top surface, producing a clean, splinter-free edge on top. But chips are packed into the cut instead of evacuated, which generates heat and can cause burning in deep cuts. Downcut bits produce a cleaner top surface and a rougher (or burned) bottom surface. Use them for: shallow profiling and dadoes where the top surface must be clean, lettering and inlay work, and laminated or veneered materials where the top veneer must not tear out.

Compression bits: These combine upcut geometry on the bottom portion and downcut geometry on the top portion. The upcut section clears chips from the bottom while the downcut section presses fibers down on the top. The result is a clean surface on both top and bottom, making compression bits ideal for through-cutting plywood, melamine, and laminated sheet goods. The trade-off is that they only work correctly when the depth of cut is at least deep enough to engage the downcut section (typically 3/4" DOC or deeper for a standard compression bit).

Straight flute bits: No helix angle. They cut without pulling or pushing fibers in either direction. They produce less tear-out than upcut bits and less heat than downcut bits, but they also evacuate chips less effectively. Good for: soft materials like foam, soft plastics, and very soft woods where tear-out isn't a concern.

Material-Specific Starting Parameters

These are starting parameters for a 1/4" (6.35mm) 2-flute carbide upcut bit. Adjust proportionally for other diameters using the chip load formula. All values assume sharp tooling and adequate dust collection.

Softwoods (pine, cedar, spruce, fir): RPM: 16,000-18,000. Feed rate: 100-150 IPM. Chip load: 0.003-0.004 IPT. DOC: up to 1x diameter (0.250"). Softwoods are forgiving. You can run fast and aggressive. The main risk is fuzzy surfaces from the soft grain — sharp tooling and proper chip load minimize this.

Hardwoods (oak, maple, cherry, walnut): RPM: 16,000-18,000. Feed rate: 80-120 IPM. Chip load: 0.003-0.004 IPT. DOC: 0.5x to 1x diameter. Hardwoods are denser and generate more heat. Burn marks on maple and cherry are the classic sign of too-slow feed rate. Keep the chip load in the sweet spot and don't dwell (pause) with the bit in the cut.

Plywood (Baltic birch, construction ply): RPM: 16,000-18,000. Feed rate: 100-140 IPM. Chip load: 0.003-0.004 IPT. DOC: up to full thickness for through-cuts. Use compression bits for through-cuts. The alternating grain layers make plywood prone to delamination if chip load is wrong. Baltic birch (many thin layers) is more forgiving than construction plywood (few thick layers).

MDF (Medium Density Fiberboard): RPM: 16,000-18,000. Feed rate: 100-150 IPM. Chip load: 0.003-0.005 IPT. DOC: up to 1x diameter. MDF machines very cleanly because it has no grain direction. The main concern is dust — MDF dust is extremely fine and hazardous. Excellent dust collection is mandatory. MDF also dulls tools faster than solid wood because of the resin binders.

Hardboard/HDF: Similar to MDF but denser. Reduce feed rate by about 10% compared to MDF. Very abrasive to tooling due to high resin content.

Melamine/Laminate: RPM: 14,000-16,000. Feed rate: 80-100 IPM. Chip load: 0.003-0.004 IPT. Always use compression bits to prevent chipping the laminate layer. The laminate surface is essentially a thin layer of hard plastic over particleboard — it chips easily if the bit pulls upward on the top face.

Depth of Cut and Stepover Guidelines

Axial depth of cut (DOC): This is how deep the bit plunges per pass. For CNC routers, the general guideline is DOC should not exceed 1x the bit diameter for softwoods and 0.5x the bit diameter for hardwoods. A 1/4" bit should take no more than 0.250" deep in pine and 0.125" deep in maple. Exceeding these guidelines causes deflection, poor surface finish, and increased risk of tool breakage.

For slotting (full-width cuts), reduce DOC to 0.5x diameter regardless of material. Slotting puts maximum load on the tool because both sides of the flute are engaged simultaneously. For profiling (single-side engagement), you can run deeper because the tool is only loaded on one side.

Radial stepover (for pocketing): When machining a pocket, each pass overlaps the previous one. The stepover is the distance between adjacent passes. For roughing, use 40-60% of the bit diameter. For finishing, use 5-15% of the bit diameter. Smaller steovers produce smoother surfaces but take more time.

At very small stepovers (below 10% of diameter), chip thinning applies just as it does in metal milling. The effective chip load drops because the bit is only engaged over a small arc. You need to increase the feed rate to compensate. Most CAM software handles this automatically with adaptive or trochoidal toolpaths.

Plunge rate: Router bits are not designed to plunge straight down like a drill. Use a ramping or helical entry to start each pocket or profile. A ramp angle of 2-5 degrees is typical. For bits that can plunge (spiral bits with center-cutting geometry), limit the plunge feed rate to about 50% of the horizontal feed rate.

Troubleshooting Burn Marks and Chip-Out

Burn marks: Burn marks are the #1 complaint in CNC wood routing. They appear as dark discoloration on the cut surface, most commonly in hardwoods like maple, cherry, and oak. The cause is always excessive heat at the cut surface, which has only three sources: (1) chip load too low (rubbing), (2) dull tool, or (3) dwell time (bit sitting in one place while spinning).

Solutions: (1) Increase feed rate to achieve proper chip load. This is the most common fix. (2) Replace the bit. Carbide router bits stay sharp for 500-2,000 linear feet of cutting in hardwood, depending on the material and bit quality. After that, they rub instead of cut. (3) Eliminate dwells in your toolpath. In CNC programming, corners are a common dwell point — the machine decelerates to change direction, and the bit sits in the corner generating heat. Using corner rounding (G64 tolerance mode on many controllers) or dog-bone fillets eliminates this problem.

Chip-out / tear-out: Chip-out occurs when fibers are pulled out of the surface instead of being cleanly sheared. It most commonly occurs on the top surface with upcut bits, on the bottom surface with downcut bits, and at edges where the bit exits the material. Plywood is especially prone because of the cross-grain layers.

Solutions: (1) Switch bit type. Use downcut for clean top surfaces, compression for clean top and bottom. (2) Use a scoring pass. Run a very shallow (0.020") pass at reduced feed to score the surface fibers before the full-depth cut. (3) Apply masking tape to the surface before cutting. The tape holds fibers in place during cutting. This is a standard technique for clean cuts in veneered and laminated materials. (4) Reduce chip load slightly — heavy chip loads increase exit-side tear-out.

Fuzzy surfaces: Soft woods (pine, poplar, cedar) often produce fuzzy surfaces regardless of feed settings. This is caused by the soft, flexible wood fibers bending out of the way instead of being cleanly sheared. Solutions: use a downcut bit (pushes fibers into the surface), use a very sharp bit (dull edges push fibers instead of cutting them), and take a light finishing pass (0.010-0.020" radial engagement) at a higher feed rate.