Guide to the Process: CNC Plastic Machining Step by Step

• 1
  Key takeaways
• 2
  What this guide to the process covers
• 3
  Choosing the right plastic for the cut
• 4
  Tooling geometry that actually clears chips
• 5
  Feeds, speeds and depth of cut
• 6
  Workholding and fixture design for soft parts
• 7
  Stress relief, finishing and inspection
• 8
  When this guide to the process does not apply
• 9
  Step by step: from stock to finished part
• 10
  Machinability and realistic tolerance by plastic

CNC plastic machining removes material from a plastic blank with a rotating cutter. The machine motion is the same as for aluminum: three linear axes, sometimes a fourth or fifth, sometimes a mill-turn spindle. What changes is the physics at the cutting edge. Plastics are soft, springy and poor at carrying heat away. That single fact drives tool choice, feed rates, workholding and finishing.

This guide to the process is written for engineers who already know what a face mill does. We skip the history of CNC and go straight to the decisions that decide whether a plastic part comes off the machine on size or ends up in the scrap bin. Each section ends with the failure mode to watch for.

You will find the same sequence we use on the floor: pick stock, pick tooling, set the cut, hold the part, relieve stress, finish the surface, then measure. Skip any step and the next one gets harder.

• 1
  ScopeRigid and semi-rigid thermoplastics: ABS, PC, PMMA, POM, PA, PEEK, PP, HDPE.
• 2
  Not coveredElastomers and foams, which need different tool geometry and cold fixturing.
• 3
  Best fitPrototypes, bridge tooling, low-to-mid volume runs and parts with undercuts.

Start with the datasheet, then check the machining behavior. POM (Delrin) is the benchmark: it cuts clean, holds ±0.02 mm on a stable machine, and produces small chips that evacuate well. ABS and PC are close behind, though PC needs slower surface speeds to avoid gumming. PMMA cuts like glass and will chip at the exit edge unless you back the cut with a support board.

PA (nylon) absorbs moisture from the air. A plate that measures 50.00 mm today can grow 0.10 mm after a week in a humid shop. Dry the stock, machine it, then measure after 24 hours. PEEK and PEI hold their shape better but cost far more, so use them only where temperature or chemical resistance demands it.

Soft polyolefins are the hard case. PP and HDPE deflect away from the cutter, so the tool rubs instead of slicing. Expect fuzzy edges, poor finish, and dimensions that need a spring pass to settle. If your part can be made in POM or ABS instead, do that.

• 1
  POM / DelrinBest all-round machinability, tight tolerances, low chip welding.
• 2
  PC / PMMAOptical and impact parts; slow the spindle and support thin edges.
• 3
  PA / PEEKHigh strength and temperature; dry the stock and anneal after cutting.
• 4
  PP / HDPEChemical resistance at the cost of finish and tolerance control.

Use two-flute carbide end mills with polished flutes and a high helix. The open flute form gives chips room to leave the cut before they melt and weld to the edge. Four-flute tools run faster on steel, but in plastic they pack the flute and rub. A dull tool is worse than a slow one: it heats the material, smears the wall, and pulls the part out of the vise.

For finishing passes, a single-flute or O-flute router bit leaves a cleaner wall on acrylic and polycarbonate. For drilling, use 118° point drills with a slow peck cycle and retract fully to clear the stringy chip. Countersinks and chamfer tools should be sharp and run at reduced feed, because the tip engages a lot of material at once.

Coating matters less than sharpness. Uncoated polished carbide works for most plastics. Diamond coating helps on abrasive filled grades such as glass-filled PA or carbon fibre, where the tool edge wears in minutes.

• 1
  RoughingTwo-flute carbide, high helix, 10–12 mm diameter for most pockets.
• 2
  FinishingSingle-flute or O-flute router bit for a clean wall on clear plastics.
• 3
  Drilling118° point, peck cycle, full retract to break the chip.
• 4
  Filled gradesDiamond-coated tooling to survive abrasive glass or carbon fill.

Plastic machining runs fast and light. Spindle speed for a 10 mm two-flute cutter in POM sits around 8,000–12,000 rpm. Feed per tooth lands between 0.05 and 0.15 mm, which puts the table feed near 1,500–3,000 mm/min. Cut depth for roughing is typically 1–2 mm axial with 40–50% radial engagement. These are starting numbers; listen to the cut and watch the chip color.

Chip color is the best feedback you have. White or light chips mean the cut is cool and the tool is sharp. Brown edges mean friction heat is building; reduce spindle speed or increase feed. If the chip comes off as a continuous string, the material is too warm and the tool is rubbing rather than cutting.

Finishing passes should remove 0.2–0.5 mm radially at full depth. A spring pass with no additional offset cleans up wall deflection on thin ribs. For PP and HDPE, drop the feed by 20–30% and expect to accept a looser tolerance window.

• 1
  Spindle speed8,000–12,000 rpm for a 10 mm cutter in POM or ABS.
• 2
  Feed per tooth0.05–0.15 mm, higher for POM, lower for PC and PMMA.
• 3
  Roughing depth1–2 mm axial, 40–50% radial engagement.
• 4
  Finishing0.2–0.5 mm radial at full depth, plus one spring pass.

Plastic clamps like a spring. Tighten a vise the way you would on steel and the part bows, then springs back after the cut. Light clamping pressure spread over a large area is the rule. Soft jaws machined to the part profile hold better than flat jaws and leave fewer marks.

For thin plates and covers, use a vacuum table or a sacrificial backing board. Double-sided tape works for flat prototypes but creeps under side load. When a part has no good clamping surface, machine it from a tabbed blank and cut the tabs by hand at the end.

Support the exit edge of every through cut. A backing board of MDF or acrylic stops the cutter from pushing material out and chipping the far wall. This single habit removes most edge defects on PMMA and PC.

• 1
  Soft jawsMachined to profile, spread the load and reduce witness marks.
• 2
  Vacuum tableBest for thin flat plates and covers with no clampable edge.
• 3
  Backing boardMDF or acrylic behind the part stops exit-edge chipping.
• 4
  TabsLeave 2–3 mm tabs on parts with no clamping surface, cut by hand later.

Annealing is the step most shops skip and most customers notice later. A roughed part carries internal stress from the blank and from the cut itself. Left alone, it can move 0.1–0.3 mm over a few days, especially in PA and PC. A two-hour soak at 80–120 °C followed by slow cooling inside the oven removes most of that risk.

Surface finish depends on the tool path, not on polishing alone. A clean finishing pass at Ra 0.8–1.6 μm is normal for POM and ABS. Clear PMMA and PC need a single-flute finish pass, then flame or vapor polishing if the part is optical. Bead blasting gives a uniform matte look but hides fine detail below about 0.5 mm.

Inspection follows the drawing. Measure critical features with a micrometer or CMM, check wall thickness at the thinnest section, and verify flatness after the part has rested. For medical and automotive work we inspect 100% before shipment and keep reports on request.

• 1
  Annealing80–120 °C for 2 hours, slow cool in the oven for PA, PEEK and PC.
• 2
  As-machined finishRa 1.6–3.2 μm for most plastics with a sharp two-flute cutter.
• 3
  Fine finishRa 0.8–1.6 μm with a single-flute pass on clear plastics.
• 4
  InspectionCMM or micrometer on critical features after a 24-hour rest.

CNC plastic machining is not always the right answer. If you need 50,000 identical small parts with no undercuts, injection molding will beat it on unit cost every time. If the part is a hollow shell with uniform 1 mm walls and no critical features, vacuum casting or 3D printing may be faster to first article.

CNC wins when the geometry is complex, the volume is low to mid, or the material is one that molds poorly. It also wins when the design is still moving. A machined blank can be revised in hours; a steel mold cannot.

The honest test: if your part has tight tolerances, undercuts, or a material with a short shelf life in molding, machine it. If it is a simple high-volume commodity, do not.

• 1
  Choose CNCPrototypes, bridge tooling, undercuts, tight tolerances, low-to-mid volume.
• 2
  Choose moldingHigh volume, simple geometry, no critical tolerances.
• 3
  Choose printingHollow shells, very fast first article, non-critical surfaces.