Acrylic CNC processing parameters: how to cut PMMA without melting or cracking
This page covers the acrylic CNC processing parameters that actually decide part quality: spindle speed, feed per tooth, depth of cut, tool geometry, workholding, and chip removal. It is written for engineers and buyers who need clear optical edges and stable dimensions, not just a cut part.
Why acrylic is not machined like aluminium
PMMA cuts easily on paper. In practice it fails differently: heat stays in the cut, chips weld to the tool, and the edge crazes.
Thermal and mechanical limits of PMMA
Acrylic (PMMA) is a glass-like thermoplastic. It has good optical clarity and impact resistance, but it is brittle and has a low melting point compared with metals. Cutting forces that would be trivial in 6061 aluminium can chip a thin acrylic wall or leave a cloudy edge.
The main enemy is heat. PMMA softens near 100 °C and starts to degrade well before that at the tool tip, where friction is concentrated. Once the chip softens, it smears instead of shearing, and the surface turns opaque. The second problem is stiffness. Acrylic is roughly 30 times less rigid than steel, so any vibration from the tool or fixture shows up directly in the cut.
This is why acrylic CNC processing parameters are not just a speed and feed lookup. They are a heat budget and a vibration plan. Get both right and the part comes off the machine with a transparent edge. Get one wrong and you spend the afternoon polishing out a melted line.
- 1HeatSoftening and smearing at the cutting edge if feed is too low or dwell is too long.
- 2VibrationChatter marks and chipping on thin walls and long unsupported sections.
- 3StressCrazing and tiny cracks near holes, slots, and sharp internal corners.
Core acrylic CNC processing parameters
The four numbers that matter most are spindle speed, feed per tooth, depth of cut, and stepover. They are linked. High spindle speed alone creates heat; it only works when the feed is high enough to take a real chip and carry that heat away. In acrylic, the chip is the cooling system.
For most end mills from 3 mm to 12 mm, a surface speed around 300 to 600 m/min is a reasonable starting point. That translates to high rpm on small tools and moderate rpm on large ones. Feed per tooth is usually 0.05 to 0.15 mm for roughing and lower for finishing where surface quality drives the decision.
Depth of cut should be conservative on the first pass. Acrylic grabs a cutter when the engagement is too light, so a very small depth can be worse than a moderate one. Radial engagement of 30 to 50 percent of tool diameter gives the tool something to bite. Full-width slotting is possible but only with good chip evacuation and a rigid setup.
Cooling is debated. Many shops run acrylic dry with strong air blast because coolant can stain or stress-crack the part. Compressed air aimed at the cutter removes chips and carries heat away without a liquid. Where coolant is used, it should be a clean, compatible fluid and the part must be dried properly afterward.
Parameter ranges for common acrylic operations
Values are starting points for rigid setups. Adjust to the specific tool and part.
| Operation | Surface speed | Feed per tooth | Notes |
|---|---|---|---|
| Roughing, 6 mm end mill | 300–500 m/min | 0.08–0.15 mm | Air blast, 30–50% stepover |
| Finishing, 6 mm end mill | 400–600 m/min | 0.03–0.08 mm | Sharp tool, light depth |
| Slotting, 3 mm end mill | 300–450 m/min | 0.05–0.10 mm | Chip evacuation is critical |
| Drilling, 5 mm bit | 60–120 m/min | 0.10–0.20 mm/rev | Peck to clear chips |
| Deep pocket, 10 mm end mill | 250–400 m/min | 0.10–0.15 mm | Rigid holder, short flute length |
Tool geometry and edge preparation for PMMA
Tool choice matters as much as the numbers. A cutter that is sharp and polished will leave a clear edge; a dull one will rub and melt. For acrylic, two flutes is usually the best compromise. It leaves enough room for chip clearance while keeping the tool stiff enough to resist deflection.
Coatings are often unnecessary and can be counterproductive. Bare, polished carbide with a high rake angle and a sharp cutting edge is the standard choice for transparent parts. Aluminium-specific coatings designed to reduce built-up edge can also help on longer runs, but they must be applied to a properly ground tool.
For finishing cuts that need optical clarity, a single-flute or two-flute tool with a large helix removes chips quickly and reduces the chance of recutting. The trade-off is feed rate. Fewer flutes means the table has to move faster to maintain the same chip load, which puts more demand on the machine and the fixture.
- 1Flute countTwo flutes for general work; single flute for deep pockets and fast chip evacuation.
- 2Helix angleHigher helix pulls chips up and out, but increases axial force.
- 3SharpnessA fresh edge cuts cooler. Replace or resharpen before the edge rubs.
Workholding and chip management
Acrylic is soft enough to mark and brittle enough to crack. Clamping force has to be light and spread over a wide area. Vacuum fixtures work well on flat plates. For thin walls, a support material or a sacrificial backing plate prevents deflection and breakout.
Chip management is not optional. A chip that stays in the cut gets recut, and recutting is what generates the heat that ruins the finish. Air blast, vacuum extraction, or a combination keeps the cut clear. On deep pockets, pecking and retracting helps, even if it costs cycle time.
Asking the design for a small change also pays off. A sharp internal corner forces a small tool with low stiffness. Adding a radius that matches the cutter diameter lets a larger, stiffer tool do the same job with fewer passes and less risk. The same logic applies to deep, narrow slots.
Questions engineers ask about acrylic machining
Can acrylic be machined dry?
Yes, and many shops prefer it. Compressed air at the cutter removes chips and carries heat away without introducing a liquid that might stain or stress-crack the part.
Where coolant is used, it should be clean and compatible with PMMA, and the part must be dried properly before inspection or packing.
Why does my acrylic part come out cloudy instead of clear?
A cloudy edge usually means the tool rubbed instead of cutting. Common causes are a dull cutter, too low a feed per tooth, or chips left in the cut to be recut.
A sharp two-flute tool, a higher feed per tooth, and strong air blast usually restore clarity. The finish also depends on the stepover used on the final pass.
What tolerance is realistic for acrylic CNC machining?
On a rigid setup with controlled temperature, ±0.005 mm is achievable on critical features. Acrylic moves with heat and moisture, so the measurement matters as much as the cut.
Thin walls and long unsupported sections are the hard cases. They deflect under cutting force and can creep after machining, so the drawing should allow for that.
Should acrylic parts be annealed after machining?
Annealing relieves internal stress and reduces the risk of crazing, especially on parts with holes, slots, or machined pockets. It is common for medical and optical parts.
The decision depends on the service environment and the amount of material removed. A stress-relief cycle is worth discussing with the machine shop before the run starts.
How do acrylic and polycarbonate compare for CNC parts?
Acrylic is clearer and harder, which makes it better for optical parts and display components. Polycarbonate is tougher and less likely to crack, but it scratches more easily and is harder to polish.
For a part that will be handled or impacted, polycarbonate is often the safer choice. For a part that must stay transparent and dimensionally stable, acrylic usually wins.
What file format do you need for an acrylic quote?
A STEP or IGES file with a 2D drawing showing tolerances and surface finish is ideal. For simple parts, a dimensioned PDF is often enough.
We review the file for tool access, wall thickness, and corner radii, and we send a DFM note with the quote so any changes are agreed before cutting starts.
Send us your acrylic part and we will review the parameters
We quote and return a free DFM analysis within 12 hours, and we machine from one prototype to 10,000+ parts with 100% inspection before shipment.
12-hour quoteFree DFM analysis100% inspection±0.005 mm tolerance
