Why Is My Acrylic Melting When I Cut It?

Why melting happens

Acrylic (PMMA) softens at around 160°C. A router bit generates heat two ways: by shearing material, and by rubbing against it. Shearing is efficient — most of the heat leaves with the chip. Rubbing is not — that heat goes straight into the workpiece and the tool.

When each flute takes too small a bite, the cutting edge stops slicing and starts burnishing. Fine dust replaces solid chips, that dust holds no heat away, and the temperature at the cut face climbs until the acrylic goes plastic. It then flows back into the kerf behind the bit and re-hardens, which is the glossy bead or blobbed edge you are looking at.

This is why the instinctive reaction — slowing the feed down because the cut looks rough — makes melting worse. Slower feed means thinner chips means more rubbing.

The number that matters: chipload

Chipload is the thickness of material each flute removes per revolution:

Chipload = Feed rate (IPM) ÷ (RPM × number of flutes)

A worked example. Say you are running 18,000 RPM, 50 IPM, with a 2-flute bit:

50 ÷ (18,000 × 2) = 0.0014″ per flute — less than a seventh of what a 1/4″ bit in acrylic should be taking. That bit is polishing the plastic, not cutting it.

Corrected, at the same 18,000 RPM with a single-flute 1/4″ bit targeting 0.011″: 18,000 × 1 × 0.011 = 198 IPM. If that number looks alarming, that reaction is exactly why so much acrylic gets melted.

Target chiploads for acrylic

These are LMT Onsrud's own published application figures for solid carbide O-flute tooling in acrylic — the same data behind our Cut Doctor and feed rate calculator, and listed per size on each bit's product page.

Why flute count matters more in plastic than in wood

Every flute you add divides the chipload at the same feed and speed. A 2-flute bit at 100 IPM and 18,000 RPM produces 0.0028″ chips. A single-flute bit at the identical settings produces 0.0056″ — double the chip thickness, double the heat carried away, with no change to your program.

That is why plastic-cutting bits are usually single-flute, and why the flute is polished and deeply scooped: the O-flute profile gives the chip somewhere to go and a slick surface to slide along, so it evacuates instead of packing into the kerf and re-melting.

Fixing it, in order

1. Calculate your actual chipload. Use the formula above, or the feed rate calculator. Most melting problems are diagnosed right here.
2. Raise the feed rate until you land in the band for your bit diameter. This is the single most effective change.
3. If your machine cannot feed fast enough, drop the RPM instead. Chipload depends on the ratio, so 12,000 RPM at 132 IPM gives the same 0.011″ as 18,000 RPM at 198 IPM.
4. Switch to a single-flute O-flute if you are running a 2-flute or a general-purpose wood bit.
5. Limit depth per pass to roughly one bit diameter, so chips clear rather than recirculate.
6. Add air blast if you have it. Cooling the chip is far more effective than cooling the workpiece.
7. Check the bit is sharp. A dull edge rubs no matter what the arithmetic says. Acrylic is not abrasive, so a bit that melts from the first cut is more likely mis-fed than worn.

Bits that cut acrylic cleanly

Acrylic is a hard plastic, which matters when choosing: Onsrud's soft-plastic series (63-750, 62-750) are ground for materials like HDPE and polypropylene and are the wrong tool here. These three are the hard-plastic O-flutes, all solid carbide, all single-flute, each carrying per-size feeds and speeds on its product page.

Browse the full range in CNC router bits for acrylic & plastics, or use the Bit Finder to match a bit to your material thickness and finish requirements.

Upcut or downcut for acrylic?

Upcut is the default. It pulls chips up and out of the cut, which is exactly what you want when heat evacuation is the whole problem. The trade-off is that it can lift thin sheet, so hold-down matters.

Downcut presses the top surface down and leaves a slightly crisper top edge, at the cost of pushing chips into the kerf — where they can re-melt. Use it for shallow engraving and profiling on show faces, not for deep through-cuts.

Compression bits, which are the right answer for plywood and melamine, offer no advantage in acrylic: plastic does not have face veneers to protect and does not chip out the way laminates do.

Common questions

Should I use coolant or lubricant on acrylic?

Air blast is preferable to liquid. It cools the chip and clears the kerf without leaving residue that has to be cleaned off a clear part. Liquid coolant can also stress-craze some cast acrylics.

Why does my edge melt only on the second pass?

Because chips from the first pass are still in the slot. The bit is re-cutting its own debris, which generates heat with no fresh material to carry it away. Clear the slot, use an upcut bit, and keep depth per pass at or below one bit diameter.

Cast or extruded acrylic — does it change the settings?

Cast acrylic machines more forgivingly and takes a better edge. Extruded acrylic is softer and more prone to melting, so it benefits even more from single-flute geometry and a healthy chipload. The chipload targets above apply to both; start extruded at the upper end of the range.

Can I polish a melted edge instead of recutting?

Flame or buff polishing can improve a slightly hazy edge, but it cannot fix re-welded material or a wavy kerf. It is faster to correct the parameters and recut than to rescue a badly melted part.

Chipload ranges reflect manufacturer application data for solid carbide tooling across our catalogue. Start conservative, verify on scrap, and adjust for your machine's rigidity and hold-down. Every bit we sell lists its own recommended feeds and speeds on its product page.