How to Choose a CNC Router Bit
Three things decide the bit: the material (does it splinter, melt or crumble?), the job (cut right through, clear a flat pocket, carve a V or a curved surface?) and the machine (how much load can it take before it flexes?).
The picker works through those three in that order. The job sets the shape of the bit, the material sets the flute style, and the machine sets the size and number of flutes. It then hands you on to the feeds and speeds calculator with the bit filled in, because the right bit at the wrong feed still burns or breaks.
The Main Bit Types
| Bit | What it does | Best for |
|---|---|---|
| Upcut spiral | Lifts chips up and out of the cut. Can fray the top face. | Solid wood, MDF, deep slots, pockets, general cutting |
| Downcut spiral | Pushes fibres down for a clean top edge. Packs chips into the slot. | Plywood and veneered faces, shallow pockets, inlay clearing |
| Compression | Upcut at the tip, downcut above it: clean top and bottom faces. | Plywood, melamine and veneered board cut right through |
| Single-flute O-flute | One big polished flute that throws large chips and carries heat away. | Acrylic, HDPE, PVC foam, aluminium on light machines |
| V-bit | Cuts wider as it goes deeper, so it can draw sharp corners and varying widths. | Signs, lettering, chamfers, V-carve inlays |
| Ball nose (straight or tapered) | Rounded tip that follows curved surfaces in small steps. | 3D reliefs, carving, rounded grooves |
| Surfacing bit | Wide, flat cutter that skims a big area level. | Spoilboards, slabs, river tables |
Rules of Thumb Behind the Picks
Diameter
Use the biggest bit that fits the smallest inside corner (the corner comes out with the bit's radius). Stiffness rises steeply with diameter, so a 6 mm bit deflects far less than a 3 mm one. Light desktop machines usually run 1/8" (3.175 mm) bits; hobby and rigid machines 1/4" or 6 mm.
Flutes
Feed ÷ (rpm × flutes) is the chip each tooth takes. Routers spin fast and hobby machines feed slowly, so fewer flutes keep the chip thick enough to carry heat away. That is why one or two flutes are the norm, and three only on rigid machines that can feed fast.
Cutting length
Choose a cutting length just over the material thickness, and keep the shank deep in the collet. Every extra millimetre of stick-out makes the bit bend and chatter more.
Shank
The shank must match the collet exactly: a 1/4" (6.35 mm) bit is not a 6 mm bit. ER11 collets on desktop machines take up to 7 mm, ER20 up to 13 mm, and trim routers usually 1/4", 6 mm or 8 mm depending on the model and country.
Worked Example
Cutting 18 mm birch ply shelf parts on a WorkBee-style hobby machine
- Job: profile cut, through the sheet. Material: plywood, with show faces on both sides.
- Pick: compression spiral, 2 flute, 6 mm or 1/4". The upcut tip keeps the bottom face clean, the downcut body keeps the top face clean.
- Catch: the first pass must go deeper than the upcut section at the tip, or the top can still fray. Check the maker's drawing for that length.
- Next: the "Feeds and speeds for this bit" button opens the calculator set to a hobby machine, plywood, a compression bit, 2 flutes and 6.35 mm, ready for your router's speed range.
- On a light 3018 the picker switches to a 1/8" downcut instead, because a light machine cannot take the deep first pass a compression bit needs.
Practical Tips
- Start with a few good bits. A 1/4" upcut, a 1/4" downcut or compression, a 60° and a 90° V-bit and a 1/8" ball nose cover most hobby work.
- Carbide, not HSS. Solid carbide holds an edge far longer in MDF and plywood glue, which blunt steel quickly.
- Watch the chips. Good chips are flakes, not dust. Dust and burn marks usually mean the chip is too thin: feed faster or slow the spindle.
- Check the finish on curves. For a 3D relief, the cusp height calculator shows how stepover and ball size set the ridges between passes.
- Turning photos into carvings? The image to V-carve G-code tool makes V-bit carvings straight from a picture.
- Safety. Wear eye and ear protection, use dust extraction (MDF dust is especially fine), and never reach in while the spindle turns.
Frequently Asked Questions
Use an upcut when chip clearing matters most: deep cuts, solid wood and MDF. Use a downcut when the top face must stay crisp: plywood, veneers and shallow pockets. If both faces of a sheet show, a compression bit gives you both in one cut.
A single-flute O-flute upcut. Its single large flute makes thick chips that carry the heat away, so the acrylic does not melt and re-weld behind the bit. Cast acrylic machines more cleanly than extruded acrylic, which softens at a lower temperature.
A 90° V-bit cuts wider and shallower for a given depth, so it suits larger lettering and signs. A 60° bit goes deeper for the same width, which shows smaller text and fine detail better. For very fine detail, 30° and engraving bits go narrower still.
Yes, with light passes and the right cutter. Use a sharp carbide end mill made for aluminium, single flute on most hobby machines, with a polished or ZrN finish rather than AlTiN. Clear chips with an air blast or a little mist, and use ramping or adaptive toolpaths. Light desktop machines can only manage thin sheet and shallow cuts.
Match it to the machine. Around 1 inch (25 mm) suits most trim-router hobby machines, smaller on light desktop machines, and 1-1/2 to 2 inches on rigid machines with a spindle. Check the shank fits your collet, take shallow passes, and tram the router first or the passes leave ridges.
These are common starting points, not rules. Bits from different makers vary in geometry and coatings, so read the maker's recommendations, make test cuts in scrap, and wear eye and ear protection.