CNC Plastic Processing Design: How Plastics Behave at the Cutter

• 1
  Why CNC plastic processing design differs from metal
• 2
  Wall thickness and rib design in CNC plastic processing design
• 3
  Radii, corners and internal geometry
• 4
  What tolerance plastic actually holds
• 5
  Undercuts, cavities and when to split the part
• 6
  Machining or molding: choosing by part and volume

Metal and plastic fail in opposite ways at the cutter. Aluminum conducts heat away and holds its shape; plastic stores heat locally and softens. A 6 mm end mill running 3,000 rpm in 6061 stays cool. The same tool in ABS at the same speed can rub, melt and weld chips back onto the flute.

The second difference is stiffness. PEEK has an elastic modulus near 3.6 GPa, roughly one eighteenth of aluminum. Push it with a 12 mm cutter and the wall deflects before the edge shears the chip. The tool takes a lighter bite than the feed rate assumes, rubs instead of cutting, and the surface turns cloudy.

The third difference is recovery. Plastic springs back under the clearance face of the tool, so the finished wall can measure larger than the cutter path. Bore a Ø20 H7 hole in POM and it may close by 0.02–0.05 mm within a day. Metal does not do this.

So the design rules for plastic are not the metal rules with smaller numbers. They come from low thermal conductivity, low stiffness and time-dependent recovery. Every recommendation below traces back to one of those three.

One practical consequence: the same part in two plastics is two different jobs. Acetal machines cleanly at moderate speed. PMMA chips well but cracks at sharp internal corners. Polycarbonate is tough enough to grab a small cutter and climb it. Match the grade to the geometry before you set the drawing.

This is also why we ask for the material on the RFQ. The tolerance we can hold, the radii we can cut and the wall we can leave all shift with the resin and with how much glass or carbon fiber is in it.

Thin walls are the most common reason a plastic part fails on the machine. Below roughly 1.5 mm, cutting force pushes the wall away from the tool. The cutter skips, the surface tears, and the operator has to slow the feed until the tool rubs.

A useful starting point for machined plastic: 2 mm minimum for unfilled grades, 3 mm for glass-filled. These are not absolute. A 1 mm wall in a 10 mm tall boss behaves fine because it is short and stiff. The same 1 mm wall standing 40 mm tall will chatter.

Stiffness scales with the cube of thickness and inversely with the cube of unsupported length. Doubling wall thickness makes a wall eight times stiffer. Halving the free length does the same. When a wall chatters, adding a temporary support rib often costs less than adding material.

Ribs should not be as thick as the wall they stiffen. Keep rib thickness at 0.5 to 0.6 of the main wall and add a draft of 0.5° to 1°. This avoids a thick mass that cools unevenly and pulls the plate out of flat.

If the function allows it, add a fillet at the rib root instead of a sharp corner. A 0.5 mm root radius spreads stress and reduces the chance of a crack starting during clamping or deburring.

Long thin plates warp after machining even when the cut is perfect. Stress built into the extruded sheet releases when you remove material from one side. Rough the part, let it rest, then finish. For a 200 mm plate, we often leave 0.5 mm and take it in a second setup.

Sharp internal corners concentrate stress and trap heat. In plastic, the corner is also where the cutter cannot clear chips. A 6 mm end mill leaves a 3 mm corner radius whether you drew one or not, so drawing a 3 mm radius is honest and drawing a 0.5 mm radius is not.

Rule of thumb: internal corner radius at least one third of the pocket depth, and never smaller than the radius of the smallest cutter you are willing to pay for. A 3 mm cutter can reach a 1.5 mm corner but breaks easily and needs slow passes.

External corners tolerate tighter radii. A 0.5 mm edge break is easy on a profile. What is not easy is a knife edge. A sharp feather edge on plastic chips, cracks and cuts the operator during handling. Add a 0.3–0.5 mm chamfer or radius on every exposed edge.

Deep pockets need a different strategy. A pocket 40 mm deep and 8 mm wide is a 5:1 ratio. Tool deflection grows with the cube of the length-to-diameter ratio, so a 6 mm cutter at that depth will push off the wall and leave taper. Wider pockets, or pockets with a drafted wall, machine far better.

Threads in plastic are workable but fragile. A tapped M4 in acrylic strips at low torque. Use coarse threads, keep thread depth at 1.5 times diameter, and consider a metal insert for anything assembled more than a few times.

Blind holes should end in a drill point or a flat with a small radius. A truly flat-bottomed blind hole requires a flat end mill and a corner radius, and the last 0.2 mm is often left as a witness mark.

Plastic moves after machining. A part measured at the machine at 20 °C can measure differently after a day, after a week, or after a shift in humidity. Nylon absorbs moisture and grows. Acetal and PEEK are more stable but still move.

That is why a blanket ±0.005 mm callout on a plastic drawing usually fails, and not because the machine is inaccurate. We can hold ±0.005 mm on a 6061 aluminum feature. On plastic we hold ±0.005 mm when the feature is small, stiff and measured in a controlled room. On a 300 mm plastic plate, ±0.05 mm is a realistic target.

Set tolerances per feature, not per drawing. A bore that receives a bearing needs a tight band and a defined material. A clearance slot needs nothing better than ±0.2 mm. A cosmetic surface needs a finish callout, not a size callout.

Thermal expansion matters at size. Unfilled nylon expands about 80 × 10⁻⁶ per °C, roughly eight times more than steel. A 200 mm nylon part that warms 10 °C grows about 0.16 mm. If it mates with a metal frame, the fit must absorb that.

Moisture is the other variable. PA6 can pick up 2 to 3 percent water by weight in humid air, which changes both dimensions and stiffness. For a dimension-critical nylon part, specify the conditioning state and measure after it stabilizes.

Finish and tolerance are separate purchases. A tight tolerance on a glossy surface costs more than the same tolerance on an as-machined surface, because the finishing pass has to be light and slow to avoid marks.

An undercut is any feature the tool cannot reach in a straight line from one direction. Three-axis machining handles undercuts by stopping and re-fixturing, which costs setup time and adds a position error each time the part moves.

Five-axis machining reaches undercuts by tilting the tool. We run 16 simultaneous 5-axis centers with a Ø400 mm rotary table, and that is usually the cheaper route for a re-entrant contour on a part that also needs tight position between features.

Not every undercut is worth a tilt. A small internal groove can often be replaced by a cross-hole, a two-piece assembly or a slot open to one side. Redesign is frequently cheaper than a fifth setup.

Cavities deserve their own check. A closed internal cavity cannot be machined at all unless the part is split. If the cavity is functional, design it as two halves with a joint face, dowel pins and screws. If it is only for weight, remove material from the outside instead.

Draft helps everywhere. Even on a machined part, a 1° wall draft reduces tool rubbing, improves chip evacuation and lets the finishing pass run at a consistent radial engagement. It costs nothing in function for most brackets and housings.

Finally, think about how the part will be held. A thin, tall housing with no flat surface is hard to clamp without distortion. Adding a sacrificial boss or a small flat pad gives the operator something to grip without touching a cosmetic face.