How to Use a CNC Machine for Woodworking
A step-by-step guide for engineers and shop owners who need to cut wood parts on a CNC machine for woodworking. We cover tooling, feeds and speeds, workholding, dust control, and the cases where a router is the wrong choice.
What matters before you cut
What a CNC machine for woodworking actually does
A CNC machine for woodworking follows G-code from a CAD/CAM file and moves a spinning cutter along a programmed path. The operator does not steer the tool. That single change is why the same part comes off the table the same way on Monday and on Friday.
The work splits into three stages. Design happens in CAD, where you model the finished part and any fixtures it needs. CAM turns that model into toolpaths with a chosen cutter, stepover and depth of cut. The machine then executes the code. Errors in any stage show up as scrap, not as a warning light.
Wood behaves differently from aluminium or steel. Grain direction changes cutting force. Moisture content changes dimensions after machining. A panel that measures 18.2 mm in the morning can measure 18.0 mm the next day in a dry shop.
That is why a woodworking router is usually a gantry machine with a large bed, not a vertical mill. Travel matters more than spindle taper. GreatLight runs 127 high-precision CNC machines for metal and plastic work, and we quote wood parts when the geometry calls for tight tolerance rather than panel size.
Cutter selection for wood, MDF and plywood
Most wood routing uses carbide upcut or downcut spiral bits in 3.175 mm, 6 mm or 12.7 mm shank. Upcut spirals lift chips out of the kerf and suit through cuts. Downcut spirals push chips down and leave a clean top face, which matters on veneered plywood.
Flute count sets chip clearance. Two flutes give a large gullet for softwood and MDF. Three or four flutes give a better finish on hard hardwood but need a slower feed to avoid packing the kerf. Packed chips rub, and rubbing burns the edge.
Compression bits solve the tear-out problem on double-sided veneer. The upcut section at the tip and the downcut section above it pull material toward the middle of the panel. They cost more and only work at one depth range, so reserve them for visible edges.
Do not run coated metal cutters on MDF. The abrasive resin wears the coating in minutes and the edge temperature climbs. A sharp uncoated carbide bit is cheaper and lasts longer in panel products.
Feeds, speeds and depth of cut
Start with chip load, not spindle speed. For a 6 mm two-flute carbide bit in hardwood, a feed per tooth of 0.2–0.3 mm is a safe range. At 18,000 rpm that gives a feed rate of roughly 7,200–10,800 mm/min. If the machine cannot reach that feed, lower the rpm instead of starving the cutter.
Depth of cut depends on cutter diameter and rigidity. A rule that holds up in practice: axial depth no more than one times the cutter diameter for roughing, and radial engagement no more than half the diameter. A 6 mm bit then takes a 6 mm deep pass at 3 mm stepover.
MDF cuts faster than hardwood because it has no grain and consistent density. Plywood sits in between, but glue lines deflect the cutter. Reduce feed by 20–30 percent when you cross a glue line at full depth.
Listen to the cut. A clean shearing sound means the chip load is right. A high-pitched squeal means the cutter is rubbing. A heavy thud means you are asking for more than the spindle or the fixture can hold.
Holding the part and controlling dust
Flat panels go on a vacuum table. A bleeder board under the part spreads the vacuum and lets you cut through without hitting the table. Vacuum holds well on parts larger than about 150 × 150 mm. Below that, the surface area is too small for the clamping force you need.
Small parts and 3D shapes need mechanical workholding. Tabs leave 0.8–1.5 mm of material connecting the part to the stock, and you cut them free with a flush trim bit or a knife. Screws into waste areas work when the part has a solid region you can drill later.
Dust extraction is not optional. Wood dust is a health hazard and an explosion hazard. A shoe around the cutter connected to a 100 mm duct captures most of the chip volume. Fine dust from MDF needs a cyclone or a cartridge filter rated for the particle size.
Fire risk rises with dwell time. If a toolpath pauses in one spot, the cutter rubs and the dust ignites. Keep the tool moving, and never leave a wood job running unattended without a fire watch routine.
Step by step: from file to finished part
- 11. Model the part and its fixtureModel the finished geometry in CAD at true scale. Add locating features for the fixture if the part is not flat. Check that every internal corner has a radius at least equal to the cutter radius.
- 22. Choose the stock and check moistureMeasure thickness at four points. For solid wood, let the stock sit in the shop for 24 hours so it reaches equilibrium. Allow 2–3 mm of extra thickness for face machining.
- 33. Build the toolpath in CAMRough with a 6 mm two-flute upcut at 1× diameter axial depth and 50 percent stepover. Finish with a 3 mm bit at 0.5 mm stepover. Add tabs every 150–200 mm on the profile cut.
- 44. Set the datum and tool lengthTouch off X and Y against a known corner, then set Z on the top of the stock. Re-check tool length after every tool change. A 0.2 mm error in Z shows up as a visible step in the floor of a pocket.
- 55. Dry run above the partRun the program with Z offset 20 mm high and the feed override at 100 percent. Watch for rapid moves that cross a clamp. This step catches most crashes before they happen.
- 66. Cut the first part at reduced feedRun at 60–70 percent feed override and listen. Increase to full feed once the sound is steady. Measure the first part before running the batch.
- 77. Cut tabs and finish edgesRemove the part, cut the tabs with a flush trim bit, and sand or chamfer edges. Deburr inside corners by hand; a cutter cannot reach a sharp internal corner.
- 88. Record the parameters that workedWrite down cutter, rpm, feed, depth and material batch. The next job in the same material then starts from a known point instead of a guess.
Which machine for which wood job
| Job type | Best machine | Why | Watch out for |
|---|---|---|---|
| Flat panel, nested parts | 3-axis router with vacuum table | Large bed, fast positioning | Small parts lift off the vacuum |
| 2.5D pockets and profiles | 3-axis router | Simple setup, low cost per part | Deep narrow pockets need long reach |
| Angled and undercut faces | 4-axis or 5-axis | One setup, compound angles | Hourly rate is higher |
| Curved furniture components | 5-axis with rotary table | Continuous tool contact, better finish | Programming time grows quickly |
| Tight tolerance inserts | Metal-cutting VMC | Rigid frame, ±0.005 mm capability | Bed size limits panel work |
The short version
A router with the right cutter, a real fixture and dust extraction will hold ±0.1 mm on wood all day. If your drawing says ±0.005 mm, the material is wrong, not the machine.
Common questions
Can a metal-cutting CNC machine be used for wood?
Yes, but the setup changes. A vertical mill has a small bed and a closed enclosure that fills with dust. You need a dust shoe, a chip tray and a spindle speed high enough for wood, often 12,000–24,000 rpm.
The bigger issue is workholding. A machine vise marks softwood. Use soft jaws, spoil boards and light clamping pressure. For panel work, a gantry router is the better tool.
What tolerance can I expect on wood parts?
On a rigid router with a sharp cutter and stable stock, ±0.1 mm is repeatable on flat profiles. Humidity moves the part after machining, so a part that measures 50.00 mm today may measure 49.85 mm in a dry room next week.
If the drawing calls for ±0.005 mm, wood is the wrong material. That tolerance belongs on metal or engineering plastic, and GreatLight machines those on 5-axis centers with 100 percent inspection.
Why does my plywood tear out on the top face?
The cutter pushes fibers upward as it exits. Switch to a downcut or compression spiral, reduce the feed per tooth by about 20 percent, and make sure the panel is fully supported underneath.
A blunt cutter makes it worse. Carbide edges in MDF and plywood lose sharpness after roughly 4–8 hours of cutting time, depending on the resin content.
How do I stop small parts from moving?
Use tabs. A 0.8–1.5 mm tab every 150–200 mm holds the part without letting it shift. Cut the tabs after the profile pass, not during it.
For very small parts, cut them from a larger blank held in a fixture, or add a sacrificial base plate and screw through the waste area.
Does dust extraction affect cut quality?
Yes. Chips left in the kerf get re-cut, which heats the cutter and dulls it faster. A dust shoe that surrounds the cutter keeps the kerf clear and gives a cleaner edge.
Fine MDF dust also clogs the machine rails and screws. Extraction protects the machine as much as the operator.
When should I send a wood part to a machine shop instead?
When the geometry has compound angles, thin walls, or metal inserts pressed into the wood. Also when the part needs a certified finish or a documented inspection report.
GreatLight machines wood, plastic and metal in the same shop. We quote the part, run a free DFM analysis within 12 hours, and ship in 3–5 days.
Send us the part, not just the drawing
Upload a STEP or DXF file and we return a quotation with a free DFM analysis within 12 hours. No minimum order quantity, from one prototype to 10,000+ part runs.
12-hour quote100% inspection±0.005 mm on metal
More from GreatLight
We publish setup notes, tooling trials and inspection data from the factory floor.
