How to Use a CNC Wood Machine: Setup, Feeds and Cut Order
Wood behaves nothing like 6061 or POM, so the same machine needs a different plan. This guide walks through workholding, tool choice, feed and speed ranges, and the checks that keep edges clean. It is written for engineers and buyers who already run metal and are adding wood parts.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
- 8
Key takeaways
What Makes Wood Different on a CNC Wood Machine
A CNC wood machine removes material the same way a mill does, but the material pushes back differently. Wood is anisotropic: strength and cut quality change with grain direction. A pass that climbs cleanly on one face can blow out the far edge on the next.
Density varies inside a single board. Earlywood cuts like a soft plastic, latewood rings cut like a hard one. Feeds that work in the middle of the board may burn on a knot ten millimeters away.
Wood also moves. A board that measured 19.0 mm in the morning may read 18.7 mm after a day in a dry shop. That is why a wood job rarely holds the ±0.005 mm we quote on metal parts.
The machine itself does not change. The same 5-axis centers, the same controllers, the same probing. What changes is the tool, the workholding and the cut order. Get those three right and the rest follows.
One more difference matters for scheduling. Wood dust is flammable and abrasive. It loads filters, dulls carbide faster than aluminum does, and needs extraction at the cutter, not at the far end of the table.
Choosing Tooling for Wood on a CNC Wood Machine
Start with flute count. Two flutes give the chip room to leave the cut. A three or four flute tool built for aluminum has less gullet volume, so chips recirculate, heat builds and the edge burns. Use 2-flute upcut or compression tools.
Upcut spirals pull chips out of the cut and give a clean top edge, but they lift the part off the table. Downcut spirals push down, which protects a veneered face, yet they pack chips in the slot. On double-sided melamine or plywood, a compression bit solves both.
Solid carbide lasts longer than high-speed steel in abrasive hardwood and MDF. Coatings help. A diamond-like coating on a 6 mm compression bit is a normal choice for long MDF runs.
Diameter follows the smallest inside corner in the part. A 3 mm bit reaches a 1.5 mm corner radius, but it deflects. Keep the cutting length as short as the part allows; a long 3 mm tool will chatter in a 19 mm deep pocket.
Keep a separate set of tools for wood and never run them on aluminum without cleaning. Pitch and resin from softwood will gall the flutes and change the cut within a few meters.
Workholding and Zero Setting
Wood is light and stiff, which sounds helpful until the cutter lifts it. The most common failure on a first wood job is a part that moves mid-cut. Screw, clamp or vacuum it down before you touch the spindle.
For sheet goods, a vacuum table with a bleeder board is fast and leaves no holes. For solid stock, screw through the waste board into the underside of the part, or leave tabs in the profile. Tabs 0.8–1.5 mm thick hold the part and snap off with a chisel.
Set X and Y from a hard reference such as a fence or a corner you machined, not from a sawn edge. Sawn edges are rarely square and can be 0.5 mm off over 300 mm.
For Z, touch off on the top face at the point where you will cut. Wood surfaces are not flat. Cupping of 0.3 mm across a 200 mm board is normal, and a zero taken at one corner will cut too deep at the other.
If the part has two setups, machine a locating feature in the first setup and use it as the datum for the second. Re-probing a sawn edge for flip operations is where most scrap comes from.
Feeds, Speeds and Depth of Cut
Chip load drives the cut, not spindle speed. For a 6 mm 2-flute carbide bit in hardwood, a starting range is 12,000–16,000 rpm at 2,500–4,000 mm/min, giving roughly 0.08–0.15 mm per tooth. Softwood tolerates the higher end.
Depth of cut should stay between 0.5 and 1× the tool diameter for roughing. A 6 mm bit takes 3–6 mm passes. Going deeper loads the tool, deflects it and leaves a stepped wall you cannot sand out without losing the profile.
Adaptive or trochoidal toolpaths let you go deeper because the radial engagement is small. On a 6 mm bit, a 10 mm depth at 10 percent radial width is realistic and keeps heat down.
Finishing passes should remove 0.2–0.4 mm of radial stock. Less than that and the tool rubs instead of cutting, which burns the surface. More than that and the finish pass carries the load of a roughing cut.
Climb milling gives the cleaner edge in solid wood and plywood. Conventional milling is worth considering on veneered faces where the top ply is thin, because it pushes the fibers down at the entry instead of lifting them.
Listen to the cut. A healthy cut is steady and loud. A squeal means too many rpm for the feed. A dull thud with fine dust instead of chips means the tool is rubbing.
After the Cut: Tabs, Sanding and Moisture
Cut the part free with a knife, not pliers. Pliers crush the tab area and pull fibers out of the face. Trim close, then sand flush with a block, keeping the block flat so you do not round the edge.
Wood dust left on the surface will show under any finish. Blow it off with dry compressed air and wipe with a tack cloth. Do not use a wet rag on raw wood; it raises the grain.
If the part carries a finish, sanding sequence matters more than grit choice. On hardwood, 120 then 180 then 220 grit is enough for most industrial parts. Going past 220 closes the pores and can hurt adhesion.
Let the part sit in the shop for a day before final inspection if the drawing has a tight tolerance. It will move as it equalizes with the room. Measure after that, not before.
For parts we machine at GreatLight, inspection happens before shipment and reports are available on request. Wood parts get the same treatment: dimensions checked against the drawing, edges checked for tear-out.
How to Use a CNC Wood Machine: Step by Step
- 11. Pick the stock and let it settleChoose a board 1–2 mm thicker than the finished thickness so you can face both sides. Let it sit in the shop for 24 hours before machining. Check for cupping with a straightedge; more than 0.5 mm across 300 mm and you should face it first.
- 22. Decide grain direction and rotate the partLook at the grain on the top face. Put it so the cutting edge exits along the fibers, not into the end grain. On plywood, run the finish pass along the face veneer direction.
- 33. Build the CAM setup with the right toolSet a 2-flute upcut or compression bit. Roughing at 12,000–16,000 rpm, 0.08–0.15 mm per tooth, 0.5–1× diameter depth of cut. Leave 0.2–0.4 mm radial stock for finishing. Add tabs 0.8–1.5 mm thick on profile cuts.
- 44. Fix the stock to the tableVacuum for sheets, screws through the waste board for solid stock. Never rely on double-sided tape for a cut deeper than 3 mm. Confirm the part cannot move by pushing it sideways with your hand.
- 55. Set X, Y and Z from real datumsUse a machined corner or fence for X and Y. Touch off Z on the top face at the highest point of the board. Record the offsets; a flip setup needs them again.
- 66. Run a dry pass firstRun the toolpath 10 mm above the stock and watch the whole path. Check that clamps and screws are outside the tool envelope. This takes two minutes and saves a board.
- 77. Cut the roughing, then the finishing passKeep the same tool if the geometry allows, and change only the stepover. Climb mill for solid wood. Watch the chips: they should be warm and shaped, not dust.
- 88. Free the part and deburrCut tabs with a knife, sand flush with a flat block, blow off dust. Let the part rest a day before final measurement if the tolerance is tight.
Starting Parameters by Material and Tool
Ranges for a 6 mm 2-flute carbide upcut bit. Reduce feed by 20 percent on the first part and adjust from the chips.
| Material | Spindle speed | Feed | Depth of cut |
|---|---|---|---|
| Softwood (pine, fir) | 16,000–18,000 rpm | 3,500–4,500 mm/min | 1× D |
| Hardwood (oak, maple) | 12,000–16,000 rpm | 2,500–4,000 mm/min | 0.5–0.8× D |
| MDF and particleboard | 14,000–18,000 rpm | 3,000–5,000 mm/min | 1× D |
| Plywood (12–18 mm) | 12,000–16,000 rpm | 2,500–3,500 mm/min | 0.5–0.8× D |
| Veneered panel (top cut) | 14,000–16,000 rpm | 3,000–4,000 mm/min | 0.5× D |
| Dense plastic (POM, PC) | 10,000–14,000 rpm | 1,500–2,500 mm/min | 0.5× D |
When Wood Is the Right Call
Wood suits fixtures, panels, prototypes and non-structural parts where moisture is controlled and tolerances are looser than ±0.1 mm. If the drawing needs ±0.005 mm or the part sees load, use aluminum or a filled plastic instead. Send us the model and we will tell you which one fits.
Common Questions
Can the same CNC machine cut wood and aluminum?
Yes, the machine does not care about the material. What changes is the tool, the workholding and the parameters. Keep separate tool sets and clean the table between materials, because wood dust and aluminum chips do not mix well in a coolant system.
If you switch often, keep a dedicated spoilboard for wood. Aluminum chips embedded in a wood board will scratch the next part.
Why does my wood part burn along the edge?
Burning is almost always too many rpm for the feed rate, or a dull tool. The cutting edge rubs instead of slicing, and friction cooks the lignin. Raise the feed by 20 percent and check the chips. If they come out as fine dust, the tool is done.
A second cause is a finishing pass that removes too little stock. Below 0.2 mm radial, the tool rubs. Increase to 0.2–0.4 mm.
How do I stop tear-out on plywood?
Use a compression bit or a downcut spiral for the top face, and put a sacrificial board under the part. Score the outline first with a 0.5 mm deep pass, then cut through. That pre-cuts the fibers and stops them from lifting.
Grain direction still matters. Run the finish pass so the tool exits along the face veneer, not across it.
What tolerance can I expect on wood parts?
On stable sheet goods in a controlled shop, ±0.1 mm is realistic. On solid hardwood, expect ±0.2 mm or looser because moisture and internal stress move the part after machining.
That is well outside the ±0.005 mm we hold on metal parts. If your drawing needs metal tolerances, the part should probably not be wood.
Do I need a vacuum table?
Not for one-off parts. Screws into a waste board and tabs are cheaper and hold harder. A vacuum table pays off when you cut many flat sheets and want to skip the screwing step.
For small parts under 100 mm square, vacuum alone is often not enough. Add tabs or use a fixture that traps the part.
How deep can I cut in one pass?
Up to 1× the tool diameter with a standard toolpath, and deeper with adaptive roughing at low radial engagement. A 6 mm bit can take 10 mm in one adaptive pass at 10 percent radial width.
Do not push a long, small-diameter tool. A 3 mm bit at 19 mm depth will deflect and leave a tapered wall, no matter what the feed rate is.
Send Us Your Wood or Metal Part
Upload a STEP file and we return a quotation with a free DFM analysis within 12 hours. Production can start within 24 hours, and every part is inspected before shipment.
12-hour quote100% inspectionNo minimum order quantity
More Machining Notes
We publish setup notes, tooling trials and inspection data from the factory floor.
