Acrylic CNC Processing Service Guide

PMMA machines more like a soft metal than like a brittle glass. It cuts with a continuous chip, holds a sharp edge, and takes a drilled and tapped thread without cracking if the tool geometry is right. That combination is what makes a machining route practical for optics housings, fluidic manifolds, and clear covers that would be expensive to mold at low volume.

Cast sheet and extruded sheet behave differently on the machine. Cast PMMA has a higher molecular weight, machines cleaner, and polishes to near-optical clarity. Extruded sheet is cheaper and more uniform in thickness, but it can stress-crack around tight radii and releases more internal stress when you remove material from one side.

Thermal expansion matters more than most people expect. PMMA moves roughly 70 × 10⁻⁶ per °C, about eight times that of aluminum. A 300 mm part measured in a cold inspection room and then installed on a warm machine can drift several tenths of a millimeter. Check the part at the temperature it will actually run at.

• 1
  Cast sheetBest for optical clarity and deep polished edges; higher cost.
• 2
  Extruded sheetGood for flat panels and brackets; watch stress near tight corners.
• 3
  Annealed stockReduces internal stress before machining thin walls.
• 4
  Sheet thicknessThin stock flexes under clamping; support it or switch to plate.

Acrylic wants a sharp, polished flute with a high rake angle. Two-flute carbide end mills made for aluminum work well, but the edge must be fresh. A dull cutter rubs instead of shearing, and the heat that follows leaves a cloudy band along the cut and can weld chips back onto the wall.

Spindle speed and feed have to be balanced so the chip carries heat away. Run too slow and the tool rubs; run too fast with a light chip load and the same thing happens. On a 6 mm cutter in cast PMMA we typically run in the 12,000 to 18,000 rpm range with a chip load around 0.05 to 0.1 mm per tooth, then trim for the finish the part needs.

Chip evacuation is not optional. PMMA chips are light, they cling, and they pack into a slot fast. Air blast beats flood coolant here because coolant can leave marks and, on some grades, promote crazing. Clear the pocket between passes and never let the cutter recut a chip.

• 1
  Rake angleHigh positive rake shears cleanly and lowers cutting force.
• 2
  Flute countTwo flutes clear chips best in deep pockets.
• 3
  Tool coatingUncoated or DLC; avoid thick coatings that round the edge.
• 4
  CoolantAir blast or mist; avoid flooding where marks matter.

Acrylic scratches if you look at it wrong, and it deflects under point loads. Vacuum tables with a soft gasket spread the force across a face and leave no marks. Where you need mechanical clamps, use soft jaws or a sacrificial MDF or PVC backing plate and keep the clamp pressure low.

Thin walls are the main source of scrap. A 1.5 mm wall on a 50 mm tall pocket will chatter no matter how good your cutter is. Add ribs, thicken the wall, or split the part so the wall is machined in a second operation when there is more material to hold.

Rough and finish in separate passes, and leave 0.3 to 0.5 mm of stock for the finish cut. A light finishing pass removes the stressed skin left by roughing and gives the wall a chance to spring back before the final dimension is set. On tight-tolerance features, take a spring pass with no radial engagement change.

Keep inside corners rounded. A sharp internal corner concentrates stress and becomes the crack origin when the part is bolted down or dropped. A corner radius of at least one third of the cutter diameter costs nothing and removes that risk.

Avoid threads in thin sections. A tapped M3 hole in a 3 mm wall has very little material around it and will strip or craze. Thread milling gives a cleaner result, or better, use a through-hole with a nut or an insert on the back side.

Be realistic about tolerances. We hold ±0.005 mm on metal parts, but PMMA moves with temperature and relaxes after machining, so a general tolerance of ±0.1 mm on plastic features is usually the honest number. Reserve tight tolerances for features that mate with metal and check them at a controlled temperature.

Plan the finish before you cut. A flame-polished edge and a machined edge are different operations with different lead times. If the part is a light guide or a sight window, say so on the drawing so the finish pass is scheduled with the right tool and the right edge treatment.

• 1
  Corner radiiAt least one third of the cutter diameter.
• 2
  Wall thicknessKeep above 1.5 mm where the part is unsupported.
• 3
  Hole depthBlind holes no deeper than 3× diameter without a pilot.
• 4
  DraftNot needed for machining, but helps assembly.

Acrylic is not a structural material. If the part carries a bending load, sees repeated impact, or is a safety cover, polycarbonate is the better call even though it scratches more easily and costs more. PC takes roughly 200 times the impact energy of PMMA at the same thickness.

Solvent contact is another limit. Many cleaning agents, adhesives, and cutting fluids will craze PMMA over time. If the part will be wiped down with alcohol or exposed to fuel, test the specific grade first or move to a different plastic such as PEEK or PP.

Very high volumes change the math too. Above roughly 10,000 identical small parts, injection molding usually beats machining on unit cost. Between one and a few thousand, machining is the faster and cheaper route because there is no tooling to cut.