Short answer: For CNC routing, the usual choice is a sharp solid-carbide O-flute bit made for plastics: single-flute on lighter machines, two-flute on rigid ones, upcut for chip clearance. The key setting is chip load (feed ÷ (rpm × flutes)): too low and the bit rubs and melts the acrylic. Onsrud's formula and charts put typical chip loads for plastics in roughly the 0.002 to 0.010 in. range depending on diameter. For hand routers, the Plexiglas manual calls for 10,000 to 20,000+ rpm, sharp carbide bits 5/16 to 1/2 in. in diameter, and a steady feed.
Key facts
- Bit: solid carbide, polished O-flute ("single-edge O" or "two-flute O") designed for plastics.
- Chip load: chip load = feed rate ÷ (rpm × number of cutting edges). Onsrud's charts for hard plastics mostly run from about 0.002 to 0.016 in. per tooth, rising with diameter.
- Depth: Onsrud reduces chip load 25% at a depth of 2× the bit diameter and 50% at 3×.
- Melting: Onsrud's fix for chips re-welding is to increase the feed rate or switch to a single-edge tool.
- Hand routers: Plexiglas recommends at least 10,000 rpm (20,000 to 25,000 preferred), carbide bits 5/16 to 1/2 in. diameter, back clearance about 10°, rake up to 15°.
- Cast vs extruded: cast routes cleaner; extruded softens sooner and needs better chip clearing.
Why does acrylic melt when routing?
Acrylic softens a little above 200 °F. A router bit that is spinning fast but moving slowly takes a chip so thin that it rubs and generates heat instead of cutting. The chips soften, stick to the flute, and get dragged back through the cut, smearing the edge. The cure is usually counterintuitive: feed faster or slow the spindle so each tooth takes a real chip, and get the chips out of the cut. Onsrud's technical data puts it plainly: when chips re-weld while cutting plastic, increase the feed rate or go to a single-edge tool.
What router bit should I use for acrylic?
| Bit type | Use it for | Notes |
|---|---|---|
| Single-flute O-flute, upcut | Most CNC routing on hobby and mid-size machines | Biggest chip per tooth at a given feed; large flute clears chips |
| Two-flute O-flute, upcut | Rigid machines that can run high feeds | Smoother finish when the feed is high enough |
| O-flute downcut | Thin sheet that lifts off the table | Holds sheet down; packs chips, so watch heat |
| Straight two- or three-flute carbide | Hand-held and table routers, edge trimming | What the Plexiglas manual specifies for manual routing |
| Spiral bit | Thick sections | Always has an edge in contact, so less chatter (Plexiglas) |
Plastics-specific O-flute bits are made by Onsrud, Amana, and others. A common example is a 1/4 in. single-flute O-flute such as Amana's 51404-K, which ToolsToday demonstrates at 18,000 rpm and 100 in./min with 1/8 in. per pass on acrylic. Treat that as one machine's starting point, not a rule.
Note that the Plexiglas manual, which is written for manual routers, says not to use single-fluted cutters at all. That advice is about hand-fed tools at modest feeds. On a CNC that holds a constant, high feed, single-flute O-flute bits are the standard choice for plastics.
How do I set feeds and speeds for acrylic?
- Start from the bit maker's chart for "hard plastic" (cast acrylic) or "soft plastic" (extruded) at your diameter.
- Calculate the feed: feed (in./min) = rpm × flutes × chip load. Example: 18,000 rpm × 1 flute × 0.005 in. = 90 in./min.
- Lower the rpm if your machine can't reach the feed the chip load calls for. Slower spindle, same chip.
- Limit depth per pass to about 1× the bit diameter at full chip load, and cut chip load 25% at 2× depth.
- Clear chips with an air blast or vacuum right at the cutter. Recut chips melt.
- Make a finishing pass: rough to within about 0.010 in., then take a light full-depth pass for a cleaner edge.
- Hold the sheet flat and still. Vibration chips edges; vacuum tables or tabs keep parts from moving at breakthrough.
Look at the chips: clean curls or flakes mean you're cutting; fine dust or stringy, melted strands mean the chip load is too low or the bit is dull.
Hand router tips
The Plexiglas manual recommends a router of at least 10,000 rpm with no load (higher is better), sharp carbide straight-flute bits 5/16 to 1/2 in. in diameter, about 10° back clearance and up to 15° positive rake, and a smooth, constant feed of 10 to 25 ft/min to avoid local heating. Avoid low-power routers, which bog down and tear chunks out, and bits under 5/16 in., which clog and break. Use a template or straightedge, and take light passes on thick sheet.
What edge does a router leave?
A sharp bit at the right chip load leaves a smooth, satin edge with fine tool marks. It's square and low in stress, so it's the best edge for solvent cementing. For a clear edge, it needs flame or diamond polishing or buffing; see how to polish acrylic edges and laser-cut vs router-cut edges. We route 3/4 and 1 in. sheet and anything that needs a machined edge; see thick acrylic cutting or price parts in the instant quote.
Questions
Can I use a wood router bit on acrylic?
A sharp carbide straight bit works for hand routing. Wood spiral bits with tight flutes tend to pack with melted chips on a CNC; plastic O-flute bits clear much better.
Should I use coolant when routing acrylic?
Usually an air blast is enough and keeps things clean. Mist coolant can help on deep cuts, but use only water-based coolants known to be compatible with acrylic; some cutting emulsions can craze it.
What is the smallest router bit for acrylic?
Bits down to 1/16 in. are used on CNCs with light depth per pass, but they break easily and leave inside corners with at least that radius. For fine detail, a laser is better; see smallest detail in laser-cut acrylic.