CNC Processing Polycarbonate: What the Material Allows

• 1
  Why CNC processing polycarbonate behaves differently at the spindle
• 2
  Tooling and parameters for CNC processing polycarbonate
• 3
  Fixture and stock-removal sequence that keeps parts flat
• 4
  When polycarbonate is the wrong choice for CNC processing
• 5
  Polycarbonate against the plastics we machine most
• 6
  What tolerance you can actually hold on polycarbonate

Polycarbonate is amorphous. It has no crystal melting point, so it does not soften gradually the way POM or PA do. Below roughly 145 °C it stays glassy and stiff. Above that it turns rubbery fast, and the window between rubbery and degraded is narrow. A cutter that is dull or a feed that is too slow puts heat into the chip instead of lifting it, and the chip welds back onto the flank face within a few seconds.

That weld is what operators call built-up edge. On steel it usually means a rougher surface. On polycarbonate it means a torn surface, because the welded lump drags material instead of shearing it. The fix is not more coolant. It is a sharper edge, a higher surface speed and a feed that keeps the tool engaged.

Thermal expansion is the second mechanism. Polycarbonate expands about 65–70 × 10⁻⁶ per °C, roughly six times more than aluminum and ten times more than steel. A 200 mm plate that warms 10 °C during roughing grows about 0.13 mm. If you measure it hot and adjust the offset, the part shrinks back after cooling and the finish pass cuts undersize.

The third mechanism is stress. Extruded plate carries internal stress from the cooling rolls. Remove one side of a stressed blank and the remaining material relaxes toward the cut side. A flat plate bows. A bored hole goes oval. This is not a machine problem, and no amount of tightening the fixture removes it. Only stress-relieved stock or a balanced stock-removal sequence does.

Moisture matters less than it does for nylon, but it is not zero. Polycarbonate takes up roughly 0.2–0.3% water at room conditions. For a 300 mm frame with tight hole spacing, drying at 120 °C for 2–4 hours before the finishing pass removes most of the dimensional drift.

Transparency adds a constraint that metals do not have. Any scratch on a clear part is permanent and visible. Any chip left on the table re-cuts the surface on the next pass. So the workholding, the air blast and the table cleaning all become part of the process, not housekeeping.

Use polished single-flute or two-flute end mills made for aluminum. Uncoated carbide with a sharp, high-rake geometry works well. Coated tools are usually a mistake: the coating rounds the edge slightly and the coating itself has a lower thermal conductivity than the carbide under it, so heat stays in the work.

Spindle speed for a 6 mm cutter runs 12,000–18,000 rpm in our shop, which lands the surface speed around 250–350 m/min. Feed per tooth is 0.05–0.15 mm. The number that matters more than any single value is chip load: if the chip is powdery or the tool sounds like it is rubbing, the feed is too low and you are generating heat instead of removing it.

Roughing should leave 0.3–0.5 mm of radial stock for finishing. Climb milling gives a better edge on the exit side. Never dwell in the cut. A pause of even half a second at 15,000 rpm glazes the surface and starts the weld.

Cooling is a choice, not a default. Compressed air or a mist of clean air plus a small amount of water-soluble fluid handles most jobs. Flood coolant can work, but polycarbonate absorbs water slowly and clear parts can show a milky edge near a flooded cut. For optical parts we run dry with high-pressure air and accept lower depth of cut.

Drilling needs a modified point. A standard 118° twist drill grabs on breakthrough and can crack a thin wall. Use 90–120° point with a low helix, feed 0.08–0.15 mm/rev, and reduce feed by half in the last 2 mm. For holes under Ø3 mm, peck drill with a 0.5 × D peck.

Tapping polycarbonate works up to about M6. Beyond that, thread milling is safer because it does not wedge the material. Expect thread flanks to spring back 0.02–0.05 mm, so cut the pitch diameter slightly small if the screw must seat by hand.

Hold the part on the largest face you can, with soft jaws or a vacuum plate. Point contact from a few clamps concentrates stress and marks the surface. If the part is clear, put a protective film on the clamping face and remove it after the last operation.

For flat plates, machine both faces. Take an equal depth from each side in alternating passes, roughly 0.5 mm per side, until the plate is at size. This balances the residual stress layer and keeps bow under control. A single-sided cut on a 10 mm plate commonly bows 0.15–0.4 mm over 200 mm.

Rough, then rest. Leave the part on the bench for 2–4 hours, or stress relieve at 120–125 °C for 1–2 hours and cool slowly. Then take the finish pass. The rest period costs a day on the schedule and saves a scrapped batch.

For thin walls, support the back with a machined wax or low-melt fixture compound. Bulk removal first, then step down to a light finish pass of 0.1–0.2 mm radial engagement. Wall thickness below 1.0 mm is possible but the part becomes a handling problem, not a machining problem.

Deburr with a sharp blade or a fine file, not a deburring wheel. A wheel generates heat and smears the edge. For clear parts, finish the edge with progressively finer abrasive film, 400 then 800 then 1200 grit, wet.

Vapor polishing and flame polishing improve clarity but they round sharp edges and change the surface chemistry slightly. If the part has to bond or print later, keep the polished faces masked.

Polycarbonate is not a high-temperature material. Continuous service above about 115–120 °C is outside its range, and a part that sees 130 °C under load will creep. If the application runs hot, PEEK or a machined metal part is the honest answer, even though polycarbonate is cheaper and easier to cut.

It is also sensitive to some solvents and to alkaline cleaners. Machined parts that will be cleaned in an aggressive degreaser can craze within weeks. Stress from machining makes this worse, so a stress-relieved part survives longer in the same chemical environment.

If the requirement is true optical transmission with no visible ripple, CNC alone rarely gets there. A diamond-turned surface or a molded lens is the right process. We can machine the housing and the mounting features and leave the optical surface to the process that owns it.

Finally, if the part is a thin, flat cover with no functional features, thermoforming or laser cutting will beat milling on cost. CNC processing polycarbonate earns its place when there are pockets, threads, bores, tight positions or a mix of features in one setup.