CNC Plastics Processing Guide

• 1
  Why CNC Plastics Processing Is Not Milling Aluminum
• 2
  Machining Behavior of Common CNC Plastics
• 3
  Tool Geometry, Speed and Cooling in CNC Plastics Processing
• 4
  Tolerance, Finish and Measurement Reality
• 5
  Step by Step: From Drawing to Finished Plastic Part
• 6
  CNC Plastics Processing: Material and Parameter Comparison

Plastic removes heat badly. Thermal conductivity of unfilled POM sits near 0.3 W/m·K, while 6061 aluminum is around 167 W/m·K. The heat a cutter generates has almost nowhere to go, so it collects at the cutting edge and in the chip. If the tool dwells in one spot, the material softens, smears, and then re-solidifies on the flank. That built-up edge is the root cause of most bad plastic parts.

The second difference is stiffness. Plastics have an elastic modulus roughly 2 to 10 percent of aluminum. A part that feels rigid on the bench will deflect under cutting force, and a vise tightened by feel will bow the middle of a thin wall. Cutting force therefore becomes a fixture problem more than a spindle problem.

Chips behave differently too. Aluminum chips curl and break. Many plastics produce continuous strings that wrap the tool and recut the surface. Others, like PMMA and PC, fracture into dust that packs into flutes. Chip evacuation has to be designed, not assumed.

Put together, these three facts drive every parameter choice in CNC plastics processing. Higher surface speed, sharper positive geometry, lower feed per tooth, and air blast instead of flood coolant. Once you know the mechanism, the numbers stop looking arbitrary.

• 1
  Heat stays at the edgeLow conductivity means short engagements and air cooling
• 2
  Part flexes before the tool doesSupport the workpiece, not just clamp it

Acetal (POM) is the friendliest grade for tight work. It chips cleanly, holds ±0.005 mm on stable features, and takes a fine finish without polishing. It also has low moisture uptake, so dimensions stay put after machining. Watch for its low melting point: a dull cutter will polish the surface instead of cutting it.

ABS and PC are the workhorses for enclosures and brackets. ABS machines softly and tends to burr; a light chamfer or a deburr pass is usually built into the plan. PC is tougher and more notch-sensitive, so avoid sharp internal corners and use generous radii. Both are prone to stress whitening if you take aggressive depths of cut.

PMMA (acrylic) gives the best optical result but cracks under stress. Use sharp tooling, climb milling, and a slow exit from the cut. Never cool it with liquid; thermal shock crazes the surface. Nylon (PA) is the opposite: it absorbs moisture, moves after machining, and produces stringy chips that need air blast and pecking.

PEEK and carbon-fibre-filled grades sit at the hard end. PEEK needs high spindle speed and carbide or diamond-coated tooling; it also needs higher part temperature stability because its cost makes scrapping painful. Filled materials are abrasive and will wear a cutter fast.

• 1
  POM and ABSGood first choice for functional prototypes
• 2
  PC and PMMAEnclosures, lenses and covers
• 3
  PASliding parts, but plan for moisture growth
• 4
  PEEK and CF gradesHigh temperature or high stiffness, higher tool wear

Two flutes is the usual starting point for plastic. Fewer flutes means more chip room, and chip room is what keeps the tool from recutting. For slotting and deep pockets, a single-flute cutter on a router-style spindle clears better still. Where surface finish matters more than evacuation, three flutes with polished flutes can work.

Use high rake angles, typically 10 to 20 degrees, and a sharp edge with no honing. A cutter that has already run aluminum will have a worn edge that rubs plastic rather than shearing it. Keep a separate set of tooling for plastics and track its life; the cost is small compared with rework.

Spindle speed should be high, often 10,000 to 24,000 rpm on small tools, with a moderate feed per tooth. The goal is to cut fast enough that heat leaves with the chip. If you see a polished, glossy smear on POM rather than a matte cut surface, the feed is too low or the tool is dull.

Cooling is usually compressed air or a cold-air gun. Flood coolant helps on PEEK and other hot-running grades, but it must be dried properly afterwards. For PMMA and some PC parts, dry cutting with air is the safer route because liquid coolant can leave marks and stress cracks.

• 1
  Rule of thumbMore chip room beats more flutes
• 2
  Keep plastics tooling separateDo not share with aluminum jobs
• 3
  Finish tells you the truthGlossy smear means rubbing, not cutting

CNC plastics processing can reach ±0.005 mm on a well-supported feature in a stable material such as POM. That number depends on the feature, not the shop. A 30 mm bore in a thick block is a different problem from a 150 mm long, 2 mm thick rib. Quote the critical dimensions and let the rest run loose.

Thermal expansion works against you. Plastics expand several times more than steel per degree, so a part measured warm will read larger than the same part at 20 °C. For tight features, let the part stabilize before final inspection. This is not a paperwork step; it changes the measured number.

Surface finish follows tooling and rigidity. As-machined plastic typically lands around Ra 1.6–3.2 μm; with a finishing pass and sharp tooling, Ra 0.8–1.6 μm is realistic, and Ra 0.2–0.8 μm is achievable on grades that polish well. Filled materials will always read rougher because the filler tears out at the surface.

Inspection at GreatLight runs across the whole order: incoming material check, in-process monitoring and a final pass before shipment, with reports on request. For plastic parts, we also record the room temperature during critical measurement so the numbers can be compared later.

• 1
  Specify critical featuresNot every dimension needs a tight callout
• 2
  Let parts stabilizeMeasure at 20 °C for tight work
• 3
  Filler raises roughnessExpect a duller surface on CF grades