CNC Routing Timber: Basics of Startup

• 1
  What happens at the cutter in CNC routing timber
• 2
  From CAD file to machine path: the startup chain
• 3
  Router bits and the materials they suit
• 4
  Feeds and speeds that keep the cut clean
• 5
  Holding wood still while the tool cuts it
• 6
  Wood movement, grain, and moisture
• 7
  What a startup shop needs beyond the machine
• 8
  CNC routing timber compared with other wood processes

CNC routing timber is a subtractive process. A rotating cutter moves along a programmed path while the wood stays fixed to the table. The cutting edge shears fibers ahead of the tool, then lifts the chip out of the groove. The wood does not bend or flow. It fractures along the grain if the tool pushes too hard or enters from the wrong side.

The router spins the tool fast, often between 12,000 and 24,000 rpm on a 6 mm to 12 mm cutter. Feed rate has to keep up with that rotation. If the chipload per tooth drops too low, the edge rubs instead of cutting. Heat builds, the edge dulls in minutes, and the surface turns fuzzy. A typical chipload for hardwood sits near 0.1 mm to 0.3 mm per tooth, depending on tool diameter and spindle power.

Direction matters more in wood than in metal. Cutting with the grain gives a clean sheared edge. Cutting against it lifts fibers and tears them. On a CNC router you control this by choosing climb or conventional direction relative to the grain, not by hand feel. The same part cut with the wrong direction will show tearout that no sanding step fully hides.

The machine has no feel for the material. It follows coordinates. Every defect you see on a routed wood part traces back to a number in the CAM file, a clamp position, or a tool that no longer cuts clean. That is the useful part of the process. Once you know the cause, you can repeat the fix.

Startup work is mostly information work. A vector or solid model defines the shape. CAM software turns that shape into toolpaths and posts G-code the controller reads. The controller then moves three or more axes along those coordinates. Any error introduced early gets cut into the wood later.

Draw the part at finished size, then add tool radius compensation in CAM rather than in the drawing. A 6 mm cutter cannot enter a 4 mm internal corner. If the drawing shows a sharp inside corner, the CAM operator has to leave a radius or plan a smaller tool for a rest pass. Decide this before the first cut, not after.

Toolpath type changes the result. A profile path cuts the outline. A pocket path clears material inside a boundary. A V-carve path varies depth with width to produce lettering and inlays. Raster paths clear large areas in parallel lines and leave a scalloped floor you may need to sand or accept as finish.

Post-processor settings decide how the machine interprets the path. Units, arc handling, and safe retract height are common startup mistakes. G21 sets millimeters and G20 sets inches. An arc told to run in the wrong plane will alarm out or, worse, cut through the part. Run the first program in air with the spindle off, then with the tool a few millimeters above the stock, before committing to a full depth cut.

Solid carbide upcut and downcut spirals cover most routing work. An upcut spiral lifts chips out of the groove and suits through cuts and deep pockets. A downcut spiral pushes chips down, leaves a cleaner top edge, and helps hold thin veneered sheet in place. A compression spiral combines both: downcut at the tip, upcut above, so both faces stay clean on double-sided sheet.

Straight flute bits cut fast and cheap but leave a rougher wall. They suit roughing passes and softwoods where finish is not critical. V-bits cut lettering, chamfers, and inlays. Ball nose bits produce curved surfaces and are the standard choice for 3D relief carving. Their stepover controls the scallop height you will see on the finished surface.

Cutter diameter sets the smallest internal radius and the achievable depth of cut. A rule of thumb is to keep depth of cut under one times the tool diameter for roughing in hardwood, and under two times diameter for softwood with a rigid setup. Push past that and the tool deflects, the wall tapers, and the cut wanders.

Coatings matter less in wood than in metal, but they still help. A bare carbide edge works for most jobs. A coated edge lasts longer in abrasive sheet goods such as MDF and particleboard, where glue and mineral content dull the tool quickly. Track cut length per tool and replace on schedule rather than on failure.

Three numbers drive the cut: spindle speed, feed rate, and chipload per tooth. They are linked. Chipload equals feed rate divided by spindle speed times number of flutes. Fix two and the third follows. Most startup problems appear because the feed is too slow for the spindle speed, not the other way around.

Start conservative and listen to the cut. A clean cut sounds steady and produces chips, not dust. Fine powder means the edge is rubbing. A high-pitched scream usually means the tool is chattering. Chips that look like small shavings with a slight sheen indicate the chipload is in range. Adjust feed in steps of 10 percent and watch the chip, not the numbers on the screen.

Depth of cut and stepover control tool load. For a 6 mm compression spiral in 18 mm plywood, a common starting point is 4 mm to 6 mm depth per pass at 3,000 mm/min to 5,000 mm/min, with the spindle at 18,000 rpm. These are starting points, not universal values. Spindle power, machine rigidity, and hold-down quality shift the numbers.

Wood is not uniform. Knots, resin pockets, and density changes along the grain will alter the load mid-cut. A feed rate tuned in clear straight grain can stall in a knot. Keep spindle load under about 80 percent of rated power so the controller has margin to push through hard spots without losing position.

A router pushes sideways as well as down. If the part shifts even a fraction of a millimeter, the cut wanders and the edge shows a step. Workholding on a router table is therefore a rigidity problem, not just a convenience. Vacuum tables, clamps, and tape-and-glue methods each suit different part shapes.

Vacuum holding suits flat sheet and thin panels. It leaves the top face clear, so you can cut around the outline without moving clamps. The limit is porosity. Open-grain and porous woods bleed air and lose grip. Sealing the edges or using a bleeder board and higher vacuum flow helps, but very porous stock may need tabs or mechanical clamps as backup.

Tabs are small uncut bridges that hold the part to the sheet until the job ends. They are the simplest fix for parts that would otherwise come loose at the last pass. Place them in low-visibility areas and cut them by hand after the program finishes. A 3 mm to 5 mm tab is usually enough for a panel part.

For solid timber blocks, mechanical clamps and a spoilboard give the most control. Clamp outside the cut path and check clearance in CAM. A clamp that sits 2 mm inside the toolpath will be hit. On thin or delicate parts, double-sided tape or a glue-down to a spoilboard spreads the load without crushing the workpiece.

Wood moves with moisture. It swells and shrinks mostly across the grain, far more than along it. A board that measures 200 mm wide at 12 percent moisture content can change several millimeters when the shop humidity shifts. Routed parts that must fit together need to be designed with that movement in mind, not cut to a fixed number and assumed stable.

Grain direction also sets edge quality. Routing parallel to the grain leaves a clean edge. Routing across the end grain tends to lift fibers and produce fuzz, especially on softwoods. A sharp downcut or compression bit reduces this, and a light finishing pass with a new edge helps more than slowing the feed.

Moisture content at the time of cutting matters for the finished part. Kiln-dried stock in the 6 percent to 8 percent range is easier to hold to size than green or air-dried stock. If the part will see a humid environment, seal all faces, including the routed edges, to slow moisture exchange.

Plywood and MDF behave differently from solid timber. Plywood has cross-grain layers that resist movement, but the internal voids and glue lines can chip the cutter. MDF is uniform and machines cleanly, yet the dust is fine and abrasive. Both need strong dust extraction at the cutter, not just at the table edge.

The machine is one part of the system. A startup also needs dust extraction, a flat and rigid table, a spoilboard that can be resurfaced, a tool setting method, and a way to measure results. Without those, the best router still produces inconsistent parts.

Dust extraction protects the cut and the operator. Chips left in a groove get recut and dull the tool. Fine dust from MDF and hardwood is a health hazard. A hood at the cutter plus a cabinet or cyclone handles most of it. Check airflow at the tool, not at the far end of the duct.

A resurfaceable spoilboard is the reference surface. Face it flat with a large flycutter or surfacing bit, then record the new Z zero. Every time you change the setup, this surface sets the depth relationship between the tool and the stock. A worn or uneven spoilboard shows up as inconsistent cut depth.

Measurement closes the loop. Calipers on the finished part, a quick check of cut depth and wall straightness, and a note on which tool and feed produced the result. Over a few jobs, those notes become the shop's process library. That is how a startup turns one successful cut into a repeatable capability.