Plexiglass CNC Cutting Guide

• 1
  Why acrylic behaves differently from aluminum
• 2
  Tool geometry and speeds for plexiglass CNC cutting
• 3
  Clamping, support and the risk of crazing
• 4
  What tolerance plexiglass CNC cutting can actually hold
• 5
  Thickness range and when to pick another process
• 6
  Material choice for transparent and structural parts

Acrylic is a thermoplastic, not a metal. It has no useful thermal conductivity, so heat generated at the cutting edge has nowhere to go except into the chip and into the part. Aluminum pulls heat away through the workpiece; PMMA stores it at the surface until the material softens. That single fact drives every parameter choice in plexiglass CNC cutting.

The practical result is a narrow window. Cut too slow or dwell in one spot and the chip welds back onto the flute, then the edge smears and turns cloudy. Cut too aggressively on a small tool and the cutter grabs, because acrylic is brittle under point load and has a low modulus compared to metals.

Acrylic also absorbs moisture. Sheet that has been stored in a humid room will machine slightly differently from dry sheet, and cast sheet behaves differently from extruded sheet. Cast PMMA machines more predictably; extruded sheet is cheaper and more prone to stress cracking around holes and sharp internal corners.

One more property matters: internal stress from the extrusion or casting process. Every cut releases some of it. Thin webs, long slots and asymmetric pockets will move after clamping is released, even when the cut itself was dimensionally correct.

• 1
  Heat stays in the cutNo conduction path, so coolant air or mist does the work.
• 2
  Chips weld fastA dwelling flute turns into a scraper within one or two revolutions.
• 3
  Stress releasesThin sections move after unclamping, not during the cut.

Use two-flute cutters with a high helix or a single-flute O-flute cutter. Two flutes give enough chip room without the rubbing that four flutes cause in a soft material. An O-flute has a wide polished channel that lifts a continuous stringy chip out of the slot, which is exactly the chip acrylic produces.

Keep the cutter sharp and uncoated, or use a polished diamond-like coating. Standard TiAlN coatings are too rough on the rake face and raise cutting temperature. For edge quality that matters optically, a finishing pass with a sharp two-flute cutter at 0.2–0.3 mm radial engagement leaves a transparent edge.

Spindle speed on small tools runs 12,000–18,000 rpm for cutters from 3 mm to 6 mm. Feed per tooth is the number to watch. For a 6 mm two-flute cutter, 0.05–0.10 mm per tooth keeps the chip thick enough to carry heat. Below about 0.02 mm per tooth the tool rubs instead of cutting.

Depth of cut depends on tool diameter. Roughing at 0.5 × diameter axial depth is safe in cast sheet; finishing at 0.1–0.2 mm radial with full depth works well on walls. If the spindle load meter climbs while the sound stays flat, the chip is not clearing and the tool is re-cutting.

• 1
  Flute countTwo flutes or one O-flute; avoid four.
• 2
  Surface speedRoughly 300–500 m/min for small-diameter carbide.
• 3
  Chip load0.05–0.10 mm per tooth on a 6 mm cutter.

Acrylic scratches if you look at it wrong. Never clamp directly on a finished face. Use soft jaws, sacrificial MDF or a vacuum table with a rubber gasket. Vacuum is the cleanest option because it spreads load across the whole sheet instead of concentrating it at three points.

Support the part under the cut. A sheet spanning an open area will deflect downward as the cutter pushes through, which changes the effective depth of cut and leaves a step on the wall. Back the work with a flat sacrificial board and keep the sheet fully supported within 50 mm of every toolpath.

Crazing is the network of fine cracks that appears around holes, sharp corners and drilled edges. It comes from localized stress plus residual solvent or moisture. Drill pilot holes at 50 percent of final diameter, then open them with a helical toolpath rather than a plunge. Keep internal corners at a minimum radius of one third of the cutter diameter.

Annealing helps when a part will see load or solvent exposure. A controlled heat soak below the glass transition temperature relieves the stress that cutting introduced. It takes hours, so plan it before the finish pass, not after the part has been packed.

• 1
  Vacuum or soft jawsSpread the load; never clamp on a finished face.
• 2
  Back the cutA sacrificial board stops wall steps and breakout.
• 3
  Corner radiusAt least one third of the cutter diameter.

Plexiglass CNC cutting holds ±0.005 mm on a machined metal reference, but not on every acrylic feature. The material moves with temperature and humidity, so a tight tolerance only means something when the inspection temperature is stated. On a 300 mm acrylic part, a 5 °C shop swing is worth more than the machining tolerance itself.

Thin walls are the second limit. A wall under 1.5 mm thick in PMMA will deflect under normal cutting forces and spring back when the tool passes. Expect ±0.10 mm on a 1 mm wall, and design the wall thicker if the fit matters.

Edge finish is easier to control than dimension. A sharp two-flute cutter with a light finishing pass reaches Ra 0.8–1.6 μm on the cut face, which reads as a matte-polished edge. To get a truly transparent edge you need flame polishing or vapor polishing after machining, and both soften sharp corners.

Holes are the classic failure point. A drilled hole in acrylic is usually 0.05–0.10 mm oversize because of elastic recovery, and the entry lip chips if the drill breaks through without backing. Bore critical holes with a helical path and leave 0.1 mm for a reaming pass.

• 1
  State the temperatureTolerance without a temperature is not a tolerance.
• 2
  Thin walls driftBelow 1.5 mm, expect ±0.10 mm.
• 3
  Holes run oversizeAllow 0.05–0.10 mm for elastic recovery.

Acrylic sheet from 0.5 mm to over 100 mm can be machined, but thickness is not the real constraint. Part geometry and the required tolerance decide feasibility. A 3 mm sheet with a 40 mm deep pocket is harder than a 40 mm block with an open profile, because the thin sheet flexes while the tool pushes.

Very thin sheet, under about 1 mm, needs a different approach: bond the sheet to a rigid carrier with a low-tack adhesive, cut through both, then release. Cutting free-standing 0.5 mm acrylic on a router table usually ends in vibration marks or a torn edge.

When the part is flat, simple and produced in volume, laser cutting or waterjet is faster and cheaper than milling. Routing wins when you need a 3D contour, a counterbore, a thread or a tight tolerance on a pocket wall. For a single prototype, milling is also the only option that lets you change a dimension without a new setup.

If the part must carry structural load, hold a thread under repeated fastening, or survive high temperature, acrylic is the wrong material. Aluminum or stainless will do the job with a known and stable tolerance. We machine PMMA, PC, POM and PEEK on the same machines, so the material call is a design decision, not a capacity limit.

• 1
  Geometry beats thicknessA deep pocket in thin sheet is the hard case.
• 2
  Flat and simpleLaser or waterjet is usually cheaper in volume.
• 3
  Load-bearingSwitch to aluminum or stainless.