CNC Polycarbonate PC: How the Material Behaves on a Machine

• 1
  What Polycarbonate Does Under a Cutter
• 2
  Feeds, Speeds and Tooling for CNC Polycarbonate PC
• 3
  Why Machined PC Parts Move After the Cut
• 4
  What Tolerance and Surface Finish to Expect
• 5
  When CNC Polycarbonate PC Beats Other Plastics
• 6
  Polycarbonate vs Nearby Machinable Plastics

Polycarbonate is an amorphous thermoplastic built around carbonate groups in the polymer chain. Those bulky groups stop the chains from packing into a crystal lattice, so the material stays glassy and transparent instead of turning milky. In practice that means high notched impact strength, good stiffness, and very low creep under a steady load. It also means no sharp melting point. The resin softens gradually, which is exactly why it behaves the way it does at the tool tip.

Cutting generates heat. Because PC has no crystalline phase to absorb that heat, the chips stay soft and tend to weld back onto the machined face. That smearing is the single most common defect on a CNC polycarbonate PC job. A sharp, polished two-flute cutter running at 8,000–16,000 rpm keeps the chip thin and carries heat away before the surface reaches its softening range. Dull tools do the opposite and leave a torn, cloudy wall.

The material is also notch sensitive. A sharp internal corner concentrates stress and can crack weeks after the part is shipped, especially near a press-fit hole. Design corner radii of at least 0.5 mm, and 1 mm if the part sees repeated load. Threads hold up better with a coarse pitch; fine threads in thin walls strip easily.

Moisture matters more than most shops admit. PC absorbs water from the air, and a wet blank will show bubbles, streaks and dull patches after machining. Dry the stock before the first cut, and keep it dry between operations.

• 1
  Amorphous, no melting pointSoftens gradually, so heat control decides surface quality.
• 2
  Notch sensitiveSize internal radii from the load, not from the tool corner.
• 3
  HygroscopicDry the blank or accept bubbles and cloudiness.
• 4
  Low creepHolds dimensions under long static load better than many plastics.

The usual rule for plastics is high spindle speed and high feed per tooth, and polycarbonate follows it, but with a narrower window than POM or ABS. Cutting speeds land around 200–500 m/min for finishing and 100–250 m/min for roughing. Chipload sits at 0.05–0.15 mm per tooth on a two-flute cutter. Go below that and the tool rubs; the edge heats, the chip welds, and the finish turns milky.

Roughing should remove material in light axial steps. A 0.5–1.5 mm depth of cut with a 40–60% stepover keeps the cutter engaged and the heat spread out. Plunging straight into the part with a flat end mill is a bad habit on PC; ramp in at 2–3° instead. Climb milling gives a cleaner wall on the finishing pass.

Cooling is where shops differ. Flood coolant with a clean water-soluble fluid carries heat away well and keeps chips from recirculating, but the part must be dried and the fluid must be compatible with PC. Many shops run dry with high-pressure air and get good results on simple geometry. Compressed air alone can fail on deep pockets, where chips pack and rub.

Finishing tools should be uncoated carbide or polished. Diamond-like coatings help on long runs, but a coating that flakes will leave hard particles embedded in the surface. Keep the flute count low. Two flutes give the chip room to clear; four flutes on a deep pocket is a recipe for chip welding.

Drilling and tapping follow the same logic. Use 118° or 90° point drills with a slow feed and peck deep holes to clear chips. For tapped holes, form taps work in thicker walls, cut taps in thin ones. Add a small countersink at each hole entry so the thread does not lift the surface.

• 1
  Roughing0.5–1.5 mm depth of cut, 40–60% stepover, ramp entry.
• 2
  Finishing200–500 m/min, 0.05–0.15 mm per tooth, two flutes.
• 3
  CoolingFlood coolant or high-pressure air; dry air fails in deep pockets.
• 4
  HolesPeck drill, countersink the entry, coarse pitch for threads.

Extruded PC sheet and rod carry internal stress from the manufacturing process. When you remove material from one side, that balance breaks and the part bows. A 10 mm plate milled down to 4 mm on one face can move 0.1–0.3 mm across a 200 mm length. That is far more than the ±0.005 mm tolerance we hold on metal, and no amount of machine accuracy fixes it.

The answer is sequence. Rough both sides, leave 0.5–1 mm of stock, then anneal before finishing. Annealing PC means heating it slowly to a temperature below its softening range and cooling it slowly enough that the inside and outside stay close in temperature. A controlled oven cycle is the only reliable way to do this; a heat gun is not. After annealing, take the finishing cuts and the part stays flat.

Fixturing pressure is the second source of movement. PC is soft compared with aluminum, so vise jaws bite into the surface and leave marks, and over-tightening bows a thin plate before the cutter even touches it. Use soft jaws machined to the part profile, or vacuum fixtures for flat panels. Support the underside across the full area, not just at two points.

Thin walls deserve a separate conversation. Below about 1.5 mm, the cutter pushes the wall away instead of cutting it, and you get chatter and a wavy surface. If the design needs a thin rib or a snap-fit arm, cut it last, use a smaller cutter with a short flute length, and accept a slower feed.

Transparent parts add one more constraint. Every tool mark shows. A polished cutter, a clean coolant flow and a steady feed matter more on a clear cover than on a hidden bracket. If the part must stay optically clear, plan a vapor polish or a fine bead blast as a finishing step and budget for the extra handling.

• 1
  Rough then annealLeave 0.5–1 mm stock, stress relieve, then finish.
• 2
  Soft jaws or vacuumAvoid jaw marks and bowing on thin plates.
• 3
  Thin wallsBelow 1.5 mm expect chatter; cut ribs last.
• 4
  Clear partsTool marks show; plan polishing into the process.

Metals machined in our shop hold ±0.005 mm. Polycarbonate does not, and quoting it that way would be dishonest. Thermal expansion is roughly 65–70 × 10⁻⁶ per °C, about ten times that of steel. A 100 mm PC part moving 10 °C changes length by roughly 0.07 mm. On a shop floor with no climate control, that alone is larger than a tight metal tolerance.

A realistic band for machined PC is ±0.05 mm on a stable feature measured at 20 °C, and ±0.1 mm on parts with long unsupported sections. Holes that will take a press-fit insert need a pilot check, because the interference that works in aluminum will crack a PC boss. Design a slightly looser fit and add a chamfer.

Surface finish is where PC rewards good practice. As-machined faces land at Ra 1.6–3.2 μm. A careful finishing pass with a polished cutter reaches Ra 0.8–1.6 μm, which is what most cover and lens-housing parts need. Going below Ra 0.8 μm on a machined face is possible on flat geometry but is not a general promise; polishing is usually the cheaper route.

Measurement deserves a note. Touch probes and micrometer anvils apply pressure, and PC deflects. Use low-force gauging, measure at a controlled temperature, and record the timing. A part measured one minute after the cut and again after a day will read differently while it settles.

Where the part must be both clear and dimensionally tight, split the job. Machine to ±0.05 mm with an Ra 0.8–1.6 μm finish, then polish. Trying to hit both at the cutter raises cost and scrap rate for a gain the application rarely needs.

• 1
  Practical band±0.05 mm on stable features at 20 °C.
• 2
  Long spansAllow ±0.1 mm and add support ribs.
• 3
  FinishRa 0.8–1.6 μm with a polished cutter; polish below that.
• 4
  GaugingUse low-force measurement at controlled temperature.

Pick PC when the part needs impact resistance, transparency, or dimensional stability under a long static load. Machine guards, electrical enclosures, lens housings, manifold blocks, jigs and fixtures all fit this pattern. The material absorbs a dropped tool without cracking, and it keeps its shape under a bolted joint.

Do not pick PC when the part sees repeated flexing at a sharp corner, or when it will sit in contact with certain solvents. Polycarbonate stress-cracks in the presence of some cleaning agents, fuels and hydraulic fluids. A stressed, molded-in or machined-in corner plus the wrong fluid is a classic field failure. If the part will be wiped down regularly, confirm the chemical list first.

Compare it with the nearby options before you commit. POM is stiffer, machines more easily and holds tighter tolerances, but it is opaque and notched impact strength is lower. PMMA is clearer and cheaper to polish, but it is brittle and chips at the edges. PEEK survives higher temperatures and aggressive chemicals, at several times the material cost.

There is no single winner. A clear cover that gets bumped belongs in PC. A precision gear that runs dry belongs in POM. A part that sits at 150 °C belongs in PEEK. Write the service condition down first, then match the polymer to it.

• 1
  Choose PCImpact, clarity, low creep, moderate temperature.
• 2
  Avoid PCSharp corners under cyclic load, solvent contact.
• 3
  POM alternativeBetter stiffness and tolerance, opaque, less impact.
• 4
  PEEK alternativeHigher temperature and chemical resistance, higher cost.