CNC Machining Plastic Parts: What Actually Sets Your Tolerance

• 1
  Why cnc machining plastic parts behave differently under a cutter
• 2
  Material choice decides the achievable tolerance
• 3
  Which part geometry fits milling and turning
• 4
  What tolerance is realistic on a plastic part
• 5
  Where the cost actually comes from
• 6
  Plastic material selection for cnc machining plastic parts

Metal removes heat with the chip. Plastics do not. Thermal conductivity of a typical engineering plastic sits in the range of 0.2–0.3 W/m·K, roughly a thousand times lower than aluminium. The heat generated at the cutting edge has nowhere to go except into the workpiece, the tool and the air. That single fact drives most of the differences between machining steel and cnc machining plastic parts.

The second difference is stiffness. Young's modulus for ABS is around 2 GPa, for POM about 3 GPa, for PEEK roughly 4 GPa. Aluminium 6061 is near 69 GPa. A plastic part therefore deflects under a cutting load that a metal part would barely notice. Push a 12 mm end mill through a 6 mm ABS wall at metal feeds and the wall bends away from the tool. The cutter does not cut where you programmed it. It cuts where the material happened to be at that instant.

The third difference is recovery. Plastics are viscoelastic. They spring back after the tool passes, and the amount depends on temperature, depth of cut and how long the material was loaded. A slot cut at 0.5 mm radial engagement springs back less than the same slot taken in one 3 mm pass. This is why a shop that only machines aluminium will often miss tolerance on a first plastic job even with a correct drawing.

• 1
  Low conductivityHeat stays in the part and the tool, not the chip.
• 2
  Low modulusCutting force bends thin walls before it cuts them.
• 3
  SpringbackThe finished dimension differs from the tool path.

Not every plastic machines well. The ones that do share two traits: decent stiffness and a low tendency to smear. POM, PC, PEEK, ABS, PMMA and PA fall into the workable group. PP and HDPE sit at the other end. They are soft, they have a low melting point, and they tend to drag rather than shear. PP can be machined, but expect to hold ±0.05 mm at best on a good day, not ±0.005 mm.

POM is the workhorse. It is dimensionally stable, it chips cleanly, and it holds ±0.01 mm without heroics. PC is stiffer and tougher but generates more heat and needs sharper tools and lower feed. PEEK machines like a light metal, holds tight tolerance well, and costs several times more per kilogram. PMMA gives an optical finish if you keep the feed steady and flood the cut.

ABS is the most common request because it is cheap and easy to prototype. It also creeps under sustained load. A clamp or a snap-fit made from ABS will relax over months. If the part carries a load for years, POM or PA is the better call, even at the higher material cost.

Carbon-fibre-filled grades are a separate case. The fibres make the material stiffer and cut the thermal expansion, but they are abrasive. Tool life drops sharply and the cut edge can fray. Design for a slightly larger edge radius and plan a finishing pass with a fresh tool.

• 1
  POM, PC, PEEK, ABS, PMMA, PAMachine cleanly; tight tolerance is realistic.
• 2
  PP, HDPESoft and gummy; expect ±0.05 mm and rougher edges.
• 3
  Carbon-fibre gradesStiff but abrasive; budget more tool changes.

A plastic part with a thick, closed cross-section and generous walls is easy. A thin housing with 1.5 mm walls and a deep pocket is hard, and no machine choice fixes that. The limit is the material, not the spindle. As a working rule, a wall thinner than 1 mm per 20 mm of unsupported length will deflect during roughing and chatter during finishing.

Sharp internal corners are the other common problem. A cutter leaves a radius equal to its own corner radius, and a small cutter that fits a sharp corner has to run slow and shallow. Adding a corner radius of at least 0.5 mm, ideally 1 mm, lets a larger tool run at a productive feed. The corner also stops stress concentrating in service.

Deep holes follow the same logic. A depth-to-diameter ratio above 5:1 in plastic needs a peck cycle, a through-tool coolant if the machine has it, and a drill with a high helix and polished flutes to clear the chip. Chips that stay in the hole rub, melt, and weld to the wall.

Thin, flat parts are the hardest of all. A 1 mm plate 150 mm across will lift off the fixture under cutter pressure. The fix is support, not a slower feed: vacuum fixturing, a sacrificial backing plate, or tabs that hold the part until the last pass.

• 1
  Wall thicknessKeep above 1 mm per 20 mm of unsupported span.
• 2
  Internal cornersAdd 0.5–1 mm radius so a larger cutter can run.
• 3
  Hole depthAbove 5:1 needs peck cycles and chip clearing.

A tolerance callout is a claim about a process, not a wish. On a stable material like POM or PEEK, in a part with walls above 3 mm, our shop holds ±0.005 mm on critical features and inspects 100% before shipment. That is the tight end. It applies to the feature, not to the whole part.

Across a 200 mm plastic part, thermal expansion does the talking. POM expands about 100 × 10⁻⁶ per °C. A 10 °C shop swing over a 200 mm span moves the part 0.2 mm. No machine can hold ±0.005 mm over that distance if the part is measured at a different temperature than it was cut. For long plastic parts, we quote a wider band and say why.

The practical answer is to split the drawing. Mark the features that matter, usually a bore, a mating face, a bearing seat, and give those a tight callout. Let the rest of the part sit at ±0.1 mm. A drawing with ±0.005 mm on every dimension costs more and buys nothing, because the part cannot meet it anyway.

Surface finish follows the same rule. As-machined plastic sits at Ra 1.6–3.2 μm. A finishing pass with a sharp tool and a light depth of cut reaches Ra 0.8–1.6 μm. Below that, you are polishing, and polishing soft plastic rounds edges and moves dimensions.

• 1
  Critical features only±0.005 mm on bores and seats, not the whole part.
• 2
  Long spansThermal expansion, not the machine, sets the limit.
• 3
  FinishRa 0.8–1.6 μm from a light finishing pass.

Plastic stock is cheap next to aluminium. What makes a plastic part expensive is time on the machine and the risk of scrapping it late. A part that needs three setups, a custom soft jaw and a vacuum plate will cost more than a part that drops out of bar stock in one op, even if the material bill is identical.

Fixture design is the hidden line item. Plastics mark easily, so a hardened steel vise jaw leaves a print on a visible face. We cut aluminium or POM soft jaws to match the part profile. That is extra programming and extra setup, but it stops the scrapping that comes from clamping too hard.

Tool choice also shows up in the price. Two-flute and three-flute end mills with polished flutes and a high helix clear plastic chips better than the four-flute tools used on steel. A shop that runs plastic often keeps that tooling on the shelf. A shop that runs steel will substitute, and the finish and the tolerance will show it.

The last cost driver is temperature control. On a long roughing cycle the part can climb 20 °C or more. If the finishing pass happens before the part cools, the final dimension is wrong. Adding a cool-down between roughing and finishing costs machine time but is often the cheapest way to hit tolerance on a plastic part.

• 1
  SetupsEach additional setup adds programming and risk.
• 2
  Soft jawsStop clamp marks and over-compression.
• 3
  Cool-downRough, wait, then finish to hit tolerance.