Processing plastics on CNC machines: how the material decides the method
This page explains what happens when a cutter meets a polymer, and why the same program behaves differently in ABS and in PEEK. It is written for design and process engineers who need to choose a plastic, set a tolerance, and know when machining is the wrong route.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
Why processing plastics differs from cutting metal
Metals pull heat away from the cutting zone fast. Polymers do not. Thermal conductivity in unfilled plastics sits roughly a thousand times lower than aluminium, so the heat generated by the tool stays near the surface. The chip carries off very little. The workpiece, not the tool, absorbs most of the energy.
That single fact explains most of what goes wrong when processing plastics. The material expands as it warms, the cutter keeps removing material along the programmed path, and the finished part measures oversize once it cools. A hole drilled at 20 °C can close by several hundredths of a millimetre after the part returns to room temperature.
Softening makes it worse. Above the glass transition temperature, the polymer loses stiffness quickly, so the cutting force that was fine at the start of the pass starts pushing the wall away from the tool. The cutter rubs instead of shearing. Rubbing raises temperature further, and the cycle feeds itself.
Chip evacuation is the second half of the problem. Long stringy chips wrap around the tool and re-cut, which doubles the heat going into the part. Everything below follows from these two constraints: keep the heat low, and get the chip out.
Which plastics machine well and which ones fight back
Amorphous plastics such as ABS, PC and PMMA soften gradually. They cut cleanly, hold a good surface, and tolerate a wider window of speeds and feeds. They also creep under load and are sensitive to solvent attack, which matters if the part will see cleaning fluids or fuel.
Semi-crystalline plastics behave differently. POM, PA and PEEK have a sharp melting point and a narrow window between cutting well and smearing. Below that window the material is too brittle and chips at the edges. Above it, the surface turns waxy and the cutter pulls material instead of cutting it.
Filled grades change the rules again. Carbon fibre and glass-filled nylon are abrasive, so tool wear accelerates and carbide grades matter more than geometry. They also conduct heat better than the base resin, which helps, but the fibre ends up in the chip and can irritate skin.
Some plastics are simply awkward on a mill. Soft PP and HDPE deflect under clamping pressure and spring back after the cut, so wall thickness and support matter more than the toolpath. Very thin sections in any polymer will chatter unless they are backed up.
Speeds, feeds and tooling for polymer cutting
Spindle speed for plastics runs high, often 8,000 to 24,000 rpm on small tools, because the chip load per tooth must stay high enough to shear rather than rub. A two-flute cutter at 12,000 rpm and 0.05 mm per tooth removes material cleanly in POM. Drop to 0.01 mm per tooth and the same cutter polishes the surface until it burns.
Rake angle matters more than coating. Sharp, polished flutes with a high positive rake cut polymers well. Aluminium-specific geometry usually works. Tools coated for steel do not help here and can add friction, so uncoated carbide or a thin diamond coating is the better choice for abrasive filled grades.
Cooling is a balance. Flood coolant removes heat and flushes chips, but some polymers absorb moisture or stain. Compressed air at 0.4–0.6 MPa handles most cases and keeps the part dry. For PEEK and other high-temperature grades, air plus a lower surface speed is usually enough.
Roughing leaves stock for a reason. A 0.3–0.5 mm finishing allowance lets the part reach thermal equilibrium before the last pass, so the final dimensions are cut into a stable workpiece rather than one that is still cooling.
Holding the part without deforming it
Clamping pressure that would be normal on steel will crush or bow a plastic part. Vacuum chucks, soft jaws machined to the part profile, and low-pressure vises spread the load. For thin walls, supporting the back side with a machined nest or a potting compound keeps the wall from moving during the cut.
Datum choice matters as much as clamping. Pick faces that will not be machined later, and machine all critical features from one setup where possible. Every re-fixture adds a small offset, and in plastics those offsets accumulate faster than in metal because the material moves.
Measurement needs the same care. A part measured hot will read large. Let it stabilise, then measure at the same temperature the drawing assumes, usually 20 °C. For tight features, a coordinate measuring machine with low contact force gives more reliable numbers than a micrometer pressed against a soft wall.
Surface finish targets should match the material. Ra 0.8–1.6 μm is realistic on most engineering plastics with a sharp tool. Chasing Ra 0.2–0.8 μm on a soft, gummy grade usually costs more than the function requires.
What tolerance is realistic in a polymer
±0.005 mm is achievable on plastics, but it belongs to specific conditions: a stable grade, a rigid part, controlled temperature, and a finishing pass after the part has cooled. Broad statements about tolerance ignore the fact that the material moves after the machine stops.
Thermal expansion drives most of the error. A 100 mm PC part warming by 10 °C grows about 0.07 mm before any cutter force is applied. If the drawing calls for ±0.02 mm across that length, the temperature window during machining and inspection has to be controlled, not assumed.
Moisture is the slower problem. PA and POM take up water from the air, and a part that measures correctly on Tuesday can be out of tolerance on Friday. For moisture-sensitive grades, either machine from dried stock and keep it dry, or accept a looser tolerance and specify the conditioning state.
Where the fit is not critical, do not pay for precision. Cosmetic covers, ducts and housings rarely need better than ±0.1 mm. Spending the budget on flatness, wall uniformity and a clean surface usually serves the assembly better than a tighter number on a drawing.
Boundaries: when machining plastics is the wrong choice
Machining wins for prototypes, low and mid volumes, tight features and parts where the material grade is fixed by a specification. It also wins when the geometry has undercuts, deep pockets or moulded-in details that would need expensive tooling. No minimum order quantity means one part is a valid order.
Injection moulding wins once the annual volume justifies a tool. If the same part runs in the tens of thousands per year and the geometry is stable, the per-part cost gap is large enough to absorb tooling. Machining a moulded part forever is an expensive habit.
Some shapes are effectively impossible to cut. Long thin tubes, complex internal channels and parts with a wall under about 0.5 mm in a soft grade will deflect or break. For those, moulding, 3D printing or vacuum casting are the honest answers, not a clever fixture.
The practical test is feature count against volume. Few complex features and a high annual volume point to moulding. Many features, tight tolerances and an uncertain design point to machining, because the design can still change without scrapping a tool.
Plastic families and what they are good for
Ranges reflect typical shop practice, not guaranteed limits.
| Family | Typical parts | Main risk |
|---|---|---|
| ABS, PC, PMMA | Enclosures, covers, lenses | Creep and solvent attack |
| POM, PA | Gears, bushings, slides | Smearing at high rpm |
| PEEK, PEI | Seals, insulators, implants | Cost and tool wear |
| Carbon / glass filled | Brackets, housings | Abrasion and edge fraying |
| PP, HDPE | Tanks, liners, ducts | Deflection and poor finish |
The short version
Pick machining when the design is still moving, when the volume is low, or when the tolerance is tight on a stable grade; pick moulding when the geometry is frozen and the annual volume is high. For soft, thin or gummy parts, change the material or the design before you change the fixture.
Questions engineers ask next
Can you hold ±0.005 mm on every plastic?
No, and any shop that says yes is not describing the material honestly. ±0.005 mm is realistic on stable, rigid grades such as POM, PEEK or filled nylon when the part is thick enough, the temperature is controlled, and a finishing pass runs after the part cools.
On soft or moisture-sensitive grades, expect ±0.05 mm or looser unless the drawing justifies the extra control steps. We will tell you which category your part falls into during the DFM review, before the first chip is cut.
How do you stop a plastic part from warping after machining?
Most warping comes from residual stress in the stock, not from the cut. Stress-relieved or annealed stock behaves far better. Where that is not available, take lighter roughing passes, leave 0.3–0.5 mm of finishing stock, and let the part rest before the final pass.
Clamping is the other half. A part held under heavy pressure will spring back when released, so soft jaws and vacuum workholding are standard for thin-walled parts.
Does coolant help or hurt?
It depends on the polymer. Flood coolant removes heat and flushes chips, which helps on deep pockets and abrasive filled grades. But some plastics absorb moisture or stain, and a wet chip is harder to clear from a deep cavity.
Compressed air at 0.4–0.6 MPa covers most jobs and keeps the part dry. For high-temperature grades such as PEEK, air plus a moderate surface speed is usually enough.
Which plastics are the hardest to machine?
Soft, gummy grades such as PP and HDPE are the most difficult in practice. They deflect under clamping, smear instead of shearing, and hold a poor surface unless the tool is very sharp and the chip load is high.
Very thin sections in any polymer come second, because chatter and deflection are hard to fixture away. Filled grades are abrasive rather than difficult, and tool wear is the main cost.
How does part size affect the process?
Our work envelope reaches 4,000 mm in the largest travel configuration, with smaller 750 × 1,150 × 550 mm and 500 × 500 × 450 mm machines for compact work. Large plastic parts are mainly a fixturing and thermal problem, since a long part grows and shrinks more with temperature.
Small, high-feature parts suit the 5-axis centres, where one setup can reach five faces and avoid the offset stacking that comes from re-fixturing.
What information do you need to quote a plastic part?
A 3D file, the material grade with any filler or colour requirement, the tolerance callouts that matter, the surface finish target, and the quantity. Tell us which features are functional and which are cosmetic, and the DFM notes will be more useful.
Uploads are kept confidential. An NDA is available on request, and quotation plus a free DFM analysis comes back within 12 hours.
Send the file and get a DFM answer
Upload your model and we will review material, tolerance and fixturing, then return a quotation with a free DFM analysis within 12 hours.
12-hour quote100% inspectionNDA on request
Follow GreatLight
We publish setup notes, tooling trials and inspection data from the factory floor.
