CNC Cutting Plexiglass: Tips and Checks for Clean Edges
This guide is for engineers and machinists who cut PMMA on a mill or router and keep getting melted edges, crazing, or cracks near the clamps. It covers tool choice, spindle and feed ranges, workholding, chip clearance, and the checks we run before a plastic job goes on the machine.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
- 8
Key takeaways
Why plexiglass behaves differently from aluminum
PMMA is about one-third the density of aluminum and roughly 30 times lower in thermal conductivity. Heat does not leave the cut zone through the chip the way it does in metal. It stays in the wall of the part and softens the material right behind the flute. Once the edge softens, the cutter rubs instead of shearing, and the finish turns cloudy or stringy.
The second difference is brittleness. Acrylic has low elongation at break, so it does not absorb clamping load or tool pressure. A vise tightened to the torque you would use on 6061 will leave stress marks or start a crack at a drilled hole. Stress cracks can appear hours after machining, so a part that looks fine at the machine can fail during shipping.
Grade matters as much as the setup. Cast sheet has higher molecular weight and better chemical resistance than extruded sheet, which machines with a consistent chip and resists crazing around holes and pockets. Extruded sheet is cheaper and flatter, and it works for thin signage panels. On deep pockets or tapped holes, the difference shows up quickly.
- 1Heat stays in the partLow thermal conductivity means the cut zone needs air, not just speed.
- 2Low elongationPMMA will not yield under clamp pressure. It cracks or crazes.
- 3Cast vs extrudedCast for pockets and threads, extruded for flat panels and light trim.
Picking the right cutter for CNC cutting plexiglass
Use a single-flute or two-flute up-cut O-flute router bit made for plastics. The wide, polished flute lifts chips out of the slot without packing them against the wall. A 4-flute end mill designed for aluminum has too little chip room and too much flute contact, so it generates friction with every revolution. That is the most common cause of a melted edge.
Tool diameter follows the feature size. A 6 mm cutter handles pockets, profiles, and most edges. Drop to 3 mm for small internal corners and keep the axial depth of cut conservative, because a slender tool deflects and rubs. For face passes on thick sheet, a 10 mm or 12 mm O-flute runs a wide, clean path and leaves fewer witness lines.
Sharpness is not something you can inspect by eye at the machine. A cutter that has already run a few sheets of PMMA will have a slightly rounded edge, and rounded edges burnish instead of cut. Keep a dedicated set of plastic tools and track the cutting distance. When the edge finish starts to dull, change the tool before you chase the problem with feeds and speeds.
- 1O-flute, up-cutWide polished flute, high rake, sharp edge. One or two flutes only.
- 2Avoid metal end millsAluminum chips embedded in acrylic make black marks that cannot be polished out.
- 3Dedicate the toolKeep plastic cutters separate and log the cutting distance.
Spindle speed and feed ranges that work
A practical starting point for a 6 mm single-flute O-flute in cast PMMA is 12,000 to 18,000 rpm with a chipload of 0.10 to 0.20 mm per tooth. At 15,000 rpm and one flute, that is 1,500 to 3,000 mm/min. Start near the middle, watch the chip, and adjust. The chip tells you more than the numbers do.
A healthy chip is a small, opaque curl that comes off the cutter freely. Fine powder means you are rubbing. Long strings or a welded ribbon mean the edge is too hot. Adjust feed first, not RPM. Doubling the feed per tooth while holding RPM usually clears the cut and drops the edge temperature, which is the opposite of what most people expect.
Depth of cut stays modest. Rough with 0.5 to 1.0 mm axial depth in multiple passes rather than one heavy pass. Radial engagement around 40 to 50 percent of the cutter diameter keeps the flute loaded without burying it. On finishing passes, take 0.2 mm radial and run the full depth to avoid a visible step where the passes meet.
- 1Roughing0.5–1.0 mm axial, 40–50 percent radial engagement, 12,000–18,000 rpm.
- 2Finishing0.2 mm radial, full depth, single pass for a consistent edge.
- 3Read the chipCurl is good. Powder or ribbon means heat, not cutting.
Workholding without leaving marks or cracks
Clamp on the waste border, never on a finished face. A machinist vise with serrated jaws will imprint acrylic at very low torque. Use soft jaws machined to the sheet thickness, or a vacuum table with a spoil board when the part has enough flat area. Vacuum holds evenly, which is what acrylic needs.
Support the full underside of the sheet. If the part has unsupported spans near a cut, the material will chatter and the edge will chip. A sacrificial backing board of MDF or PVC keeps the cutter from pushing the sheet down and gives the bottom edge something to shear against.
When a fixture must contact the part, use a light film of protective tape and keep the pressure low. Release the clamp slowly. Snapping a clamp open puts a shock load into the sheet and can start a crack at the nearest hole or corner radius.
- 1Soft jaws or vacuumEven pressure across the sheet, no point loads on finished faces.
- 2Back the sheetMDF or PVC spoil board controls chatter and protects the bottom edge.
Chip clearance and edge cooling
Air blast is the default for PMMA. A nozzle aimed at the cut, roughly 2 to 4 bar, clears the chip and carries heat away from the edge. Coolant works, but it wets the sheet, and some coolants leave a residue that shows under the polished surface. Mist is a middle option when the cut is deep and the air alone cannot keep up.
Chip recutting is the quiet killer. A chip trapped under the flute rubs the wall twice and leaves a dull band. If you see a repeated mark at the same depth on every pass, the slot is not clearing. Increase air pressure, reduce axial depth, or switch to a single flute so there is more room in the groove.
Keep the toolpath moving. A dwell, a pause for a tool change, or a slow lead-in gives the edge time to heat. Ramp into the cut at the same feed you use for cutting, and avoid plunging straight down into a pocket floor.
- 1Air at 2–4 barDirected at the cut, not across the whole table.
- 2No dwellConstant motion keeps the edge below the softening point.
Step by step: setting up a plexiglass job
Run these in order. Each step catches a problem before it reaches the part.
- 1Confirm the grade and thickness
- 2Fit a fresh plastic cutter
- 3Mount on soft jaws or vacuum
- 4Set zero on the top face
- 5Start at 15,000 rpm and 0.15 mm per tooth
- 6Finish with a 0.2 mm radial pass
- 7Deburr with a scraper, not sandpaper
- 8Anneal if the part sees solvent or stress
Which setup fits your plexiglass part
Match the cut to the feature. The wrong column is how edges melt and parts crack.
| Feature | Tool and setup | Starting parameters | Watch for |
|---|---|---|---|
| Straight profile on 3–6 mm sheet | 6 mm single-flute O-flute, vacuum table | 16,000 rpm, 0.15 mm/tooth, 1.0 mm axial | Chatter at unsupported edges |
| Deep pocket, cast PMMA | 6 mm O-flute, soft jaws, air blast | 14,000 rpm, 0.12 mm/tooth, 0.5 mm axial | Chip packing in the slot |
| Small internal corner under 4 mm | 3 mm O-flute, reduced gauge length | 18,000 rpm, 0.08 mm/tooth, 0.3 mm axial | Tool deflection and rub marks |
| Tapped or threaded hole | Cast sheet, form tap, slow spindle | 400–600 rpm, peck to clear chips | Crazing around the hole |
| Face pass for clarity | 10–12 mm O-flute, single direction | 12,000 rpm, 0.20 mm/tooth, 0.2 mm radial | Witness lines between passes |
| Thin panel, 2 mm or less | Vacuum table, low clamp pressure | 16,000 rpm, 0.10 mm/tooth, light axial | Lift and vibration at the center |
Common questions about CNC cutting plexiglass
Why does my acrylic edge come out cloudy or white?
A cloudy edge is a rubbing mark, not a cutting mark. The usual causes are a dull cutter, too little feed per tooth, or a slot that is not clearing chips. The flute contacts the wall more than once and burnishes it.
Check the chip first. Powder means rubbing. Raise the feed per tooth, confirm the tool is sharp, and add air at the cut. If the finish improves but does not clear, take a 0.2 mm radial finishing pass at full depth.
Can I cut acrylic with the aluminum end mill already in the spindle?
It will cut, but the result is usually poor. A metal end mill has more flutes and less chip room, so it rubs and heats the sheet. Aluminum residue on the flutes also transfers into the acrylic and leaves dark marks that cannot be polished out.
Keep a separate set of sharp O-flute tools for plastics. The change takes two minutes and saves the part.
Do I need coolant when CNC cutting plexiglass?
Most jobs run dry with an air blast at 2 to 4 bar. Air clears the chip and carries heat away without wetting the sheet or leaving a residue on a polished face.
Mist is useful on deep pockets where air alone cannot keep up. Flood coolant works but needs a wash and dry step before the part is packed.
How do I stop cracks starting at holes and corners?
Cracks start where stress concentrates and the material cannot yield. Clamping on a finished face, a sharp internal corner, and a hole drilled with a blunt bit are the three usual sources.
Use cast sheet for structural parts, add a corner radius where the design allows, peck-drill with a sharp bit and low pressure, and clamp on waste only. For parts that will see solvent, a stress-relief oven cycle reduces the risk.
What tolerance can we hold on machined PMMA?
On a stable setup with cast sheet and controlled temperature, we hold ±0.005 mm on critical features and inspect 100 percent before shipment. Acrylic moves with temperature, so tight tolerances should be called out on the drawing and measured at a defined temperature.
The bigger risk on plastic is not the machined size. It is stress cracking days later, which is why the tool, the clamp, and the annealing step matter as much as the numbers.
How thin a sheet can be machined without vibration?
Down to about 1.5 mm with a vacuum table and a backing board. Below that, the sheet lifts between the vacuum grooves and the cut edge chips.
Hold thin panels flat with a full-coverage fixture or a light spray adhesive on a spoil board. Reduce axial depth and keep the cutter sharp.
Send your PMMA drawing and we will quote it
Upload the file and we return a quotation plus a free DFM analysis within 12 hours. No minimum order quantity, from one prototype to a 10,000-part run.
12-hour quote100% inspectionNDA on request
More machining notes from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
