CNC Acrylic Cutting Guide

• 1
  Why acrylic cuts differently from metal
• 2
  Cast versus extruded acrylic stock
• 3
  Tool geometry for CNC acrylic cutting
• 4
  Speeds, feeds and heat control
• 5
  Clamping, drilling and stress relief
• 6
  Where CNC acrylic cutting fits and where it does not
• 7
  Which cutting process for which acrylic part

Acrylic, or PMMA, has a thermal conductivity around 0.19 W/m·K. Aluminium 6061 is roughly 1,000 times more conductive. Heat generated at the cutting edge has nowhere to go, so it stays in the chip and in the workpiece. Once the local temperature passes the glass transition range near 105 °C, the polymer softens, the chip welds back onto the flute, and the surface turns cloudy.

PMMA is also brittle. Its notch sensitivity means a sharp internal corner concentrates stress and can crack days after the part leaves the machine, especially if it later sees solvent or thermal cycling. Radii are not cosmetic on acrylic parts. A 1 mm corner radius can be the difference between a part that ships and a part that splits during assembly.

• 1
  Low conductivityCoolant and air blast matter more than on metals.
• 2
  Notch sensitiveInternal corners need a radius, not a sharp tool path.
• 3
  Thermally softAbove roughly 105 °C the surface smears instead of cutting.

Cast PMMA is polymerized in a mold between glass plates. It has a higher molecular weight, better optical clarity, and lower internal stress. It machines to a cleaner edge and takes a flame or vapor polish well. It is also more expensive and available in fewer thicknesses.

Extruded PMMA is pushed through a die. It is cheaper, more uniform in thickness, and easier to bend. It also carries more residual stress from the extrusion process, which shows up as crazing around drilled holes or after solvent bonding. For a flat display panel with a laser-cut outline, extruded is fine. For a thick machined lens holder or a part that will be annealed, cast is the safer choice.

• 1
  CastBetter clarity, lower stress, cleaner machined edges.
• 2
  ExtrudedLower cost, tighter thickness tolerance, more residual stress.
• 3
  Optical gradeRequires slower feed and more attention to chip evacuation.

A single-flute router bit with a high helix, often called an O-flute, is the standard starting point. One flute gives a large chip gullet, so the chip leaves the cut instead of rubbing. Two-flute tools work for finishing passes at lower chip load, but they pack the gullet faster on deep pockets.

Edge geometry matters as much as flute count. A polished, razor-sharp cutting edge with a high rake angle slices the polymer. A dull or honed edge pushes it, which is where the white stress marks around a hole come from. Solid carbide lasts longer than high-speed steel, but the coating is a trade-off. Uncoated carbide is usually the right call for PMMA because some coatings have a higher friction coefficient against plastic.

• 1
  O-fluteBest chip evacuation on pockets and deep cuts.
• 2
  High rake angleSlices rather than pushes the polymer.
• 3
  Uncoated carbideLower friction than many coated tools on PMMA.
• 4
  Sharp, not honedA polished edge reduces stress marks.

The goal is to cut fast enough to keep the tool in the material and slow enough to avoid melting. On a 6 mm single-flute carbide router at 18,000 rpm, a feed of 2,500–3,500 mm/min gives a chip load around 0.15–0.20 mm per tooth. That is a starting point, not a recipe. Increase feed before you increase speed if the edge is smearing.

Depth of cut should stay light. For a 6 mm tool, 3–4 mm axial depth and 50% radial engagement is a reasonable pass. Climb milling is the default on acrylic because it starts the cut at maximum chip thickness, which reduces rubbing and heat. Conventional milling on a finishing pass can leave a better edge on some cast grades, so test both on scrap.

Air blast is often enough. A cold-air gun at -10 °C to -20 °C keeps the chip clear and the edge cool without the cleanup that flood coolant creates. If you do use coolant, use a mist or a water-soluble fluid compatible with acrylic, and dry the part afterward. Trapped moisture can cause crazing on some grades.

Acrylic cracks under point loads. Standard metal vises and toe clamps will mark the surface and can split a thin panel. Vacuum tables with a spoilboard, or double-sided tape on a flat fixture, distribute the load. For thin sheets under 3 mm, a sacrificial MDF backing plate supports the material at the exit of the cut.

Drilling is where most acrylic parts fail. A standard 118° twist drill grabs and pulls through the bottom of the hole, which chips the exit edge. Use a 60–90° point angle, reduce the feed as the drill breaks through, and peck if the hole is deeper than one diameter. A 0.2–0.5 mm chamfer on entry and exit removes the sharp edge that would otherwise initiate a crack.

Annealing is the step most shops skip. A cast PMMA part machined from stock and then heated to 80 °C for one hour per 3 mm of thickness, followed by a slow ramp down, relieves the stress that machining introduced. It costs cycle time. It also prevents the part from crazing three weeks later in a customer's solvent bath.

• 1
  Vacuum or tapeAvoid point loads from vises and clamps.
• 2
  Back the exitSacrificial plate prevents breakout on thin sheet.
• 3
  Chamfer holesRemoves the sharp edge that starts a crack.
• 4
  Anneal after machining80 °C, one hour per 3 mm, slow cool.

CNC routing wins on thickness. Once a part is over 8–10 mm thick, or has a three-dimensional profile such as a curved display cover or a machined lens holder, a router is often the only practical process. It also holds tighter tolerances than laser on thick stock, because the laser kerf widens and the edge angle changes as the beam defocuses through the material.

Laser cutting is faster and cheaper for flat parts under about 6 mm with simple outlines. It leaves a slightly tapered edge and a heat-affected zone that can craze under stress. Waterjet cuts thick acrylic without heat, but the abrasive slurry leaves a matte edge and the process is slower on small parts. For a flat 3 mm sign panel, laser is usually the right call. For a 20 mm machined manifold block, it is not.

• 1
  CNC routingThick stock, 3D profiles, tight tolerances, threaded features.
• 2
  LaserFlat parts under roughly 6 mm, fast turnaround, tapered edge.
• 3
  WaterjetThick stock, no heat, matte edge, slower on small parts.