CNC Plastic Processing WI: How Plastic Parts Are Actually Cut

• 1
  Why plastic behaves differently under a cutter
• 2
  Which plastics machine well, and which fight back
• 3
  Cutting parameters that keep a plastic part in tolerance
• 4
  Features that machine cleanly and features that do not
• 5
  How a plastic job actually moves through the shop
• 6
  Plastic material, machinability and best use

Metal cutting is mostly about shear. A carbide edge shears a chip off steel and the heat leaves with the chip. Plastic does not work that way. The material is soft, it conducts heat poorly, and it springs back under the edge. So the same toolpath that gives a clean finish on 6061 aluminium will smear a polycarbonate face.

Three things then decide the result: heat, chip evacuation and support. Heat softens the material at the cut, so a dull edge drags instead of shearing. Chips that are not cleared are re-cut, and re-cut chips score the finished wall. A thin wall that is not supported will deflect away from the cutter and spring back, which shows up later as a taper you cannot measure on the bench.

The practical consequence is that feed and speed cannot be copied from a metal job card. Plastics want a sharp, polished flute, a higher surface speed and a feed high enough to cut rather than rub. Rubbing is the enemy. A tool that rubs generates heat, and heat is what melts an edge, welds a chip to the flute and burns a mark into the part.

There is also a thermal memory effect. A plastic part machined fast and hot will keep moving after it leaves the machine. Measure it cold, hours later, and the numbers shift. That is why we rough, then let the part rest, then finish. It costs one setup, and it saves the argument about whether the part was in tolerance when it shipped.

POM, often sold as Delrin, is the friendliest engineering plastic on a mill. It cuts clean, holds a thread, and resists the fuzz that plagues softer grades. ABS and PC behave well with the right edge geometry. PMMA, acrylic, machines to an optical finish but cracks if you clamp it hard or let a chip weld to the cutter.

PA, nylon, is tough and wears well, but it absorbs moisture and moves after machining. Parts that must hold a tight number should be conditioned first. PP and HDPE are chemically excellent and mechanically soft. They machine, but holding ±0.005 mm on a thin PP wall is not realistic, and we will say so before quoting.

PEEK and carbon-fibre-filled grades sit at the other end. PEEK is abrasive, expensive and needs sharp tooling and generous coolant or air blast. Carbon fibre composite is worse for tool life and worse for your lungs, so it gets sealed enclosure work and dust extraction. It is doable at ±0.005 mm on a rigid setup, but it is not a cheap part.

A useful rule for the design table: if the part is a bracket, a housing, a cover or a fixture, almost any of these will work. If it is a bearing surface, a seal land or a snap fit that must cycle 100,000 times, the material choice is doing the engineering, not the machining.

On a 5-axis or 3-axis machine, plastic generally takes a spindle speed in the 8,000–20,000 rpm range with a two- or three-flute carbide tool. Depth of cut stays light, often 0.5–2 mm in roughing, because a heavy radial engagement pushes the wall and heats the chip. Finishing passes run shallow and fast with a constant feed, never a dwell.

Cooling matters more than most people expect. Compressed air is the default. It clears chips from a deep pocket and keeps the edge from welding. Mist or flood coolant is used on PEEK and on long roughing cycles, then the part is dried and inspected. Water-based coolant left on a nylon part will be absorbed, so it gets wiped and bagged.

Clamping is where the tolerance is usually lost, not at the cutter. Soft jaws machined to the part profile, vacuum plates for flat panels, and light pressure on the vise are standard. A plastic part squeezed hard will relax overnight and the flatness you measured at 4 pm is gone by 9 am.

For a part held to ±0.005 mm, the sequence is rough, stress relief or rest, semi-finish, rest, then finish and inspect. For a part held to ±0.05 mm, one setup will do. The process window widens as the tolerance loosens, and quoting reflects that.

Sharp internal corners are the first thing to fix. A cutter has a radius, so a square pocket corner needs a relief or an EDM-style undercut that plastic machining will not give you cheaply. Add a corner radius of at least 1 mm, ideally equal to the tool radius, and the pocket finishes in one pass with no chatter.

Threads hold well in POM, PEEK and PC, and poorly in PP and HDPE. For plastics, coarse threads with a larger minor diameter cut cleaner than fine threads. Thread milling beats tapping on a deep hole, because the chip clears and the tool does not bind. Inserts are the better answer for any thread that will be assembled more than a few times.

Thin walls are the second limit. Below roughly 1 mm on an unsupported wall, deflection and vibration show up in the finish. Ribbing, a machined support web, or splitting the part into two pieces will often cost less than trying to hold a 0.6 mm wall in one hit.

Living hinges, snap fits and press fits all depend on material strain, not on the machine. We can cut the geometry to ±0.005 mm, but whether the snap survives 1,000 cycles is a material modulus question. Give us the mating part and the cycle count, and the design review is worth more than a tighter tolerance.

It starts with the file and the intent. A STEP file gives geometry, not function. So we ask what the part touches, what holds it, and which dimension is the one that must not move. Those three answers usually cut a program from twelve operations to five.

A DFM review goes back within 12 hours, often with a marked-up model. Typical notes: open a deep pocket with a larger tool, add a corner radius, change a fine thread to a coarse one, or move a datum. None of this costs the customer anything, and it removes the scrap risk before a single chip is made.

Then the setup is built. Soft jaws or a vacuum plate, a probe check on the stock, and a first-article cut. On a tolerance-critical plastic part we inspect the first article fully, adjust the cutter compensation, and only then run the batch. Production can start within 24 hours of the go-ahead on a simple part.

Finishing follows if the drawing calls for it. Bead blasting gives a uniform matte on ABS and PC. Laser marking needs a minimum character height of 1.5 mm to stay legible. Vapor polishing and painting are outside work, so they add days, not hours. Shipment on a standard plastic job runs 3–5 days after that.